ANSYS Explicit Dynamics Analysis Guide PDF [PDF]

Zitiervorschau

ANSYS Explicit Dynamics Analysis Guide

ANSYS, Inc. Southpointe 2600 ANSYS Drive Canonsburg, PA 15317 [email protected] http://www.ansys.com (T) 724-746-3304 (F) 724-514-9494

Release 2019 R2 May 2019 ANSYS, Inc. and ANSYS Europe, Ltd. are UL registered ISO 9001: 2015 companies.

Copyright and Trademark Information © 2019 ANSYS, Inc. Unauthorized use, distribution or duplication is prohibited. ANSYS, ANSYS Workbench, AUTODYN, CFX, FLUENT and any and all ANSYS, Inc. brand, product, service and feature names, logos and slogans are registered trademarks or trademarks of ANSYS, Inc. or its subsidiaries located in the United States or other countries. ICEM CFD is a trademark used by ANSYS, Inc. under license. CFX is a trademark of Sony Corporation in Japan. All other brand, product, service and feature names or trademarks are the property of their respective owners. FLEXlm and FLEXnet are trademarks of Flexera Software LLC.

Disclaimer Notice THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE SECRETS AND ARE CONFIDENTIAL AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. The software products and documentation are furnished by ANSYS, Inc., its subsidiaries, or affiliates under a software license agreement that contains provisions concerning non-disclosure, copying, length and nature of use, compliance with exporting laws, warranties, disclaimers, limitations of liability, and remedies, and other provisions. The software products and documentation may be used, disclosed, transferred, or copied only in accordance with the terms and conditions of that software license agreement. ANSYS, Inc. and ANSYS Europe, Ltd. are UL registered ISO 9001: 2015 companies.

U.S. Government Rights For U.S. Government users, except as specifically granted by the ANSYS, Inc. software license agreement, the use, duplication, or disclosure by the United States Government is subject to restrictions stated in the ANSYS, Inc. software license agreement and FAR 12.212 (for non-DOD licenses).

Third-Party Software See the legal information in the product help files for the complete Legal Notice for ANSYS proprietary software and third-party software. If you are unable to access the Legal Notice, contact ANSYS, Inc. Published in the U.S.A.

Table of Contents 1. Explicit Dynamics Analysis Guide Overview ........................................................................................... 1 2. Explicit Dynamics Workflow ................................................................................................................... 3 2.1. Introduction ..................................................................................................................................... 3 2.2. Create the Analysis System ................................................................................................................ 4 2.3. Define Engineering Data ................................................................................................................... 4 2.4. Attach Geometry .............................................................................................................................. 4 2.5. Define Part Behavior ......................................................................................................................... 6 2.6. Define Connections .......................................................................................................................... 7 2.6.1. Spot Welds in Explicit Dynamics Analyses ................................................................................. 8 2.6.2. Body Interactions in Explicit Dynamics Analyses ....................................................................... 9 2.6.2.1. Properties for Body Interactions Folder ........................................................................... 11 2.6.2.1.1. Contact Detection ................................................................................................. 11 2.6.2.1.2. Formulation .......................................................................................................... 13 2.6.2.1.3. Sliding Contact ..................................................................................................... 14 2.6.2.1.4. Manual Contact Treatment .................................................................................... 14 2.6.2.1.5. Shell Thickness Factor and Nodal Shell Thickness ................................................... 14 2.6.2.1.6. Body Self Contact .................................................................................................. 17 2.6.2.1.7. Element Self Contact ............................................................................................. 17 2.6.2.1.8. Tolerance .............................................................................................................. 17 2.6.2.1.9. Pinball Factor ........................................................................................................ 18 2.6.2.1.10. Time Step Safety Factor ....................................................................................... 18 2.6.2.1.11. Limiting Time Step Velocity ................................................................................. 18 2.6.2.1.12. Edge on Edge Contact ......................................................................................... 18 2.6.2.2. Interaction Type Properties for Body Interaction Object .................................................. 19 2.6.2.2.1. Frictionless Type ................................................................................................... 19 2.6.2.2.2. Frictional Type ...................................................................................................... 19 2.6.2.2.3. Bonded Type ........................................................................................................ 20 2.6.2.2.4. Reinforcement Type .............................................................................................. 24 2.6.2.3. Identifying Body Interactions Regions for a Body ............................................................ 25 2.6.3. Manual Contact Regions in Explicit Dynamics Analyses ........................................................... 25 2.6.3.1. Manual Contact Region Behavior for Proximity Based Contact and Trajectory Contact with Discrete Sliding or Manual Contact Treatment set to Lumped ............................................. 26 2.6.3.2. Manual Contact Region Behavior for Trajectory Contact with Connected Surface Sliding and Manual Contact Treatment set to Pairwise .......................................................................... 28 2.6.4. Joints in an Explicit Dynamics Analysis .................................................................................... 30 2.6.4.1. Joint Solver ................................................................................................................... 30 2.6.4.2. Scoping to geometry ..................................................................................................... 32 2.6.4.3. Initial Conditions ........................................................................................................... 33 2.6.4.4. Boundary Conditions ..................................................................................................... 33 2.6.4.5. Using Contact with Joints .............................................................................................. 35 2.6.4.6. Postprocessing .............................................................................................................. 35 2.7. Setting Up Symmetry ...................................................................................................................... 35 2.7.1. Explicit Dynamics Symmetry .................................................................................................. 35 2.7.1.1. General Symmetry ......................................................................................................... 35 2.7.1.2. Global Symmetry Planes ................................................................................................ 36 2.7.2. Symmetry in an Euler Domain ................................................................................................ 36 2.8. Define Remote Points ..................................................................................................................... 37 2.8.1. Explicit Dynamics Remote Points ............................................................................................ 37 2.8.2. Explicit Dynamics Remote Boundary Conditions ..................................................................... 38 2.8.3. Initial Conditions on Remote Points ........................................................................................ 38 Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

iii

Explicit Dynamics Analysis Guide 2.8.4. Constraints and Remote Points ............................................................................................... 39 2.9. Apply Mesh Controls/Preview Mesh ................................................................................................ 40 2.10. Establish Analysis Settings ............................................................................................................. 41 2.10.1. Analysis Settings for Explicit Dynamics Analyses ................................................................... 45 2.10.1.1. Explicit Dynamics Step Controls ................................................................................... 45 2.10.1.2. Explicit Dynamics Solver Controls ................................................................................. 50 2.10.1.3. Explicit Dynamics Euler Domain Controls ..................................................................... 53 2.10.1.4. Explicit Dynamics Damping Controls ............................................................................ 54 2.10.1.5. Explicit Dynamics Erosion Controls ............................................................................... 55 2.10.1.6. Explicit Dynamics Output Controls ............................................................................... 56 2.10.1.7. Explicit Dynamics Data Management Settings .............................................................. 60 2.10.1.8. Recommendations for Analysis Settings in Explicit Dynamics ........................................ 61 2.10.2. Body Control ........................................................................................................................ 65 2.11. Define Initial Conditions ................................................................................................................ 67 2.12. Apply Loads and Supports ............................................................................................................ 67 2.12.1. Impedance Boundary ........................................................................................................... 69 2.12.2. Detonation Point .................................................................................................................. 72 2.12.3. Activation/Deactivation of Loads in Explicit Dynamics ........................................................... 75 2.12.4. Importing External Loads ..................................................................................................... 77 2.13. Solve ............................................................................................................................................ 77 2.13.1. Solving from Time = 0 ........................................................................................................... 77 2.13.2. Resume Capability for Explicit Dynamics Analyses ................................................................. 78 2.13.2.1. Load and Constraint Behavior when Extending Analysis End Time ................................ 79 2.13.3. Explicit Dynamics Performance in Parallel ............................................................................. 79 2.14. Postprocessing ............................................................................................................................. 80 2.14.1. Solution Output ................................................................................................................... 80 2.14.2. Result Trackers ..................................................................................................................... 81 2.14.2.1. Point Scoped Result Trackers for Explicit Dynamics ....................................................... 81 2.14.2.2. Body Scoped Result Trackers for Explicit Dynamics ....................................................... 84 2.14.2.3. Spring Result Trackers for Explicit Dynamics ................................................................. 86 2.14.2.4. Viewing and Filtering Result Tracker Graphs for Explicit Dynamics ................................. 86 2.14.2.5. Force Reaction Result Trackers for Explicit Dynamics ..................................................... 87 2.14.3. Review Results ..................................................................................................................... 88 2.14.4. Eroded Nodes in Explicit Dynamics Analyses ......................................................................... 89 2.14.5. Euler Domain in Explicit Dynamics Analyses .......................................................................... 91 2.14.6. User Defined Results for Explicit Dynamics Analyses .............................................................. 93 3. Transforming an Implicit Model to run in Explicit Dynamics ................................................................ 99 3.1. When Implicit Models Can be Run in Explicit .................................................................................... 99 3.2. When to Consider an Explicit Analysis ............................................................................................ 100 3.2.1. Incorrect Model Setup .......................................................................................................... 100 3.2.2. Large Deformations .............................................................................................................. 101 3.2.3. Large Contact Models ........................................................................................................... 102 3.2.4. Rigid Body Deformations ...................................................................................................... 103 3.3. Setting up the Explicit Dynamics Analysis ...................................................................................... 104 3.3.1. Attaching an Explicit Dynamics System to an Existing Static Structural System ....................... 104 3.3.2. Materials .............................................................................................................................. 105 3.3.3. Meshing ............................................................................................................................... 105 3.3.3.1. Uniform Mesh Works Best ............................................................................................ 106 3.3.3.2. Midside Nodes not Used .............................................................................................. 106 3.3.3.3. Hex/Rectangular Mesh Elements most Effective ........................................................... 107 3.3.4. Contact/Connections ........................................................................................................... 107 3.3.4.1. Contacts Tab ................................................................................................................ 107

iv

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Explicit Dynamics Analysis Guide 3.3.4.2. Body Interactions Tab .................................................................................................. 108 3.3.5. Boundary Conditions ............................................................................................................ 108 3.3.5.1. Adjusting Load Cases for Reasonable Run Times ........................................................... 108 3.3.5.2. Missing Boundary Conditions from Explicit Dynamics ................................................... 109 3.3.5.3. Avoiding Conflicting Boundary Conditions ................................................................... 109 3.3.5.4. Initial Conditions ......................................................................................................... 111 3.4. Analysis Settings ........................................................................................................................... 111 3.4.1. Analysis Setting Preference ................................................................................................... 111 3.4.2. Step Controls ....................................................................................................................... 111 3.4.2.1. End Time ..................................................................................................................... 112 3.4.2.2. Timestep Controls ........................................................................................................ 112 3.4.2.3. Restarting an Analysis .................................................................................................. 114 3.4.3. Solution Stability .................................................................................................................. 114 3.4.3.1. Mass Scaling ................................................................................................................ 114 3.4.3.2. Erosion ........................................................................................................................ 115 3.4.3.3. Damping .................................................................................................................... 116 3.4.4. Output Controls ................................................................................................................... 116 3.5. Solution Information ..................................................................................................................... 117 3.6. Postprocessing ............................................................................................................................. 118 3.6.1. Result Trackers ..................................................................................................................... 119 3.6.2. Result Sets ........................................................................................................................... 119 3.6.3. Improving your Simulation ................................................................................................... 120 4. Applying Pre-Stress Effects for Explicit Analysis ................................................................................ 121 4.1. Recommended Guidelines for Pre-Stress Explicit Dynamics ............................................................ 121 4.2. Pre-Stress Object Properties .......................................................................................................... 123 5. Using Explicit Dynamics to Define Initial Conditions for Implicit Analyses ........................................ 125 5.1. Transfering Explicit Results to MAPDL ............................................................................................ 125 6. Explicit Dynamics Theory Guide ......................................................................................................... 129 6.1. Why use Explicit Dynamics? ........................................................................................................... 129 6.2. What is Explicit Dynamics? ............................................................................................................ 129 6.2.1. The Solution Strategy ........................................................................................................... 130 6.2.2. Basic Formulations ............................................................................................................... 130 6.2.2.1. Implicit Transient Dynamics ......................................................................................... 131 6.2.2.2. Explicit Transient Dynamics .......................................................................................... 131 6.2.3. Time Integration ................................................................................................................... 132 6.2.3.1. Implicit Time Integration .............................................................................................. 132 6.2.3.2. Explicit Time Integration .............................................................................................. 132 6.2.3.3. Mass Scaling ................................................................................................................ 134 6.2.4. Wave Propagation ................................................................................................................ 134 6.2.4.1. Elastic Waves ............................................................................................................... 135 6.2.4.2. Plastic Waves ............................................................................................................... 135 6.2.4.3. Shock Waves ................................................................................................................ 135 6.2.5. Reference Frame .................................................................................................................. 136 6.2.5.1. Lagrangian and Eulerian Reference Frames .................................................................. 136 6.2.5.2. Eulerian (Virtual) Reference Frame in Explicit Dynamics ................................................ 138 6.2.5.3. Key Concepts of Euler (Virtual) Solutions ...................................................................... 140 6.2.5.3.1. Multiple Material Stress States ............................................................................. 140 6.2.5.3.2. Multiple Material Transport ................................................................................. 142 6.2.5.3.3. Supported Material Properties ............................................................................. 142 6.2.5.3.4. Known Limitations of Euler Solutions ................................................................... 142 6.2.6. Explicit Fluid Structure Interaction (Euler-Lagrange Coupling) ............................................... 142 6.2.6.1. Shell Coupling ............................................................................................................. 144 Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

v

Explicit Dynamics Analysis Guide 6.2.6.2. Sub-cycling ................................................................................................................. 144 6.3. Analysis Settings ........................................................................................................................... 145 6.3.1. Step Controls ....................................................................................................................... 145 6.3.2. Damping Controls ................................................................................................................ 146 6.3.3. Solver Controls ..................................................................................................................... 150 6.3.4. Erosion Controls ................................................................................................................... 158 6.4. Model Size Limitations in Explicit Dynamics ................................................................................... 159 6.5. References .................................................................................................................................... 160 7. Material Models Used in Explicit Dynamics Analysis .......................................................................... 163 7.1. Introduction ................................................................................................................................. 163 7.2. Explicit Material Library ................................................................................................................. 165 7.3. Density ......................................................................................................................................... 171 7.4. Linear Elastic ................................................................................................................................. 171 7.4.1. Isotropic Elasticity ................................................................................................................ 171 7.4.2. Orthotropic Elasticity ............................................................................................................ 172 7.4.3. Viscoelastic .......................................................................................................................... 172 7.5. Test Data ....................................................................................................................................... 173 7.6. Hyperelasticity .............................................................................................................................. 173 7.7. Plasticity ....................................................................................................................................... 178 7.7.1. Bilinear Isotropic Hardening ................................................................................................. 179 7.7.2. Multilinear Isotropic Hardening ............................................................................................ 179 7.7.3. Bilinear Kinematic Hardening ............................................................................................... 180 7.7.4. Multilinear Kinematic Hardening .......................................................................................... 180 7.7.5. Johnson-Cook Strength ........................................................................................................ 180 7.7.6. Cowper-Symonds Strength ................................................................................................... 182 7.7.7. Steinberg-Guinan Strength ................................................................................................... 183 7.7.8. Zerilli-Armstrong Strength .................................................................................................... 184 7.8. Brittle/Granular ............................................................................................................................. 186 7.8.1. Drucker-Prager Strength Linear ............................................................................................ 186 7.8.2. Drucker-Prager Strength Stassi ............................................................................................. 187 7.8.3. Drucker-Prager Strength Piecewise ....................................................................................... 188 7.8.4. Johnson-Holmquist Strength Continuous ............................................................................. 189 7.8.5. Johnson-Holmquist Strength Segmented ............................................................................. 191 7.8.6. RHT Concrete Strength ......................................................................................................... 193 7.8.7. MO Granular ........................................................................................................................ 198 7.9. Equations of State ......................................................................................................................... 199 7.9.1. Background ......................................................................................................................... 199 7.9.2. Bulk Modulus ....................................................................................................................... 200 7.9.3. Shear Modulus ..................................................................................................................... 200 7.9.4. Ideal Gas EOS ....................................................................................................................... 200 7.9.5. Polynomial EOS .................................................................................................................... 201 7.9.6. Shock EOS Linear .................................................................................................................. 203 7.9.7. Shock EOS Bilinear ................................................................................................................ 204 7.9.8. JWL EOS ............................................................................................................................... 206 7.10. Porosity ...................................................................................................................................... 208 7.10.1. Porosity-Crushable Foam .................................................................................................... 208 7.10.2. Compaction EOS Linear ...................................................................................................... 210 7.10.3. Compaction EOS Non-Linear .............................................................................................. 211 7.10.4. P-alpha EOS ....................................................................................................................... 213 7.11. Failure ......................................................................................................................................... 216 7.11.1. Plastic Strain Failure ............................................................................................................ 218 7.11.2. Principal Stress Failure ........................................................................................................ 218

vi

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Explicit Dynamics Analysis Guide 7.11.3. Principal Strain Failure ........................................................................................................ 219 7.11.4. Stochastic Failure ............................................................................................................... 220 7.11.5. Tensile Pressure Failure ....................................................................................................... 221 7.11.6. Crack Softening Failure ....................................................................................................... 222 7.11.7. Johnson-Cook Failure ......................................................................................................... 224 7.11.8. Grady Spall Failure .............................................................................................................. 225 7.12. Strength ..................................................................................................................................... 226 7.13. Thermal Specific Heat .................................................................................................................. 227 7.14. Rigid Materials ............................................................................................................................ 227 7.15. References .................................................................................................................................. 227 8. Using Workbench LS-DYNA for an Explicit Dynamics Analysis ........................................................... 229 8.1. How to Load Workbench LS-DYNA ................................................................................................ 229 8.2. How to use Workbench LS-DYNA ................................................................................................... 229 8.3. Using the Workbench LS-DYNA Extension ..................................................................................... 230 8.3.1. Licensing Requirements ....................................................................................................... 231 8.3.2. Running a Distributed Solution ............................................................................................. 231 8.3.3. Setting up a Project .............................................................................................................. 231 8.3.3.1. Defining Materials ....................................................................................................... 231 8.3.3.2. Attaching Geometry .................................................................................................... 231 8.3.3.3. Defining Part Behavior ................................................................................................. 232 8.3.3.3.1. Adaptive Region ................................................................................................. 232 8.3.3.4. Defining Connections .................................................................................................. 232 8.3.3.5. Defining Mesh Settings ................................................................................................ 233 8.3.3.6. Defining Analysis Settings ............................................................................................ 233 8.3.4. Defining Initial Conditions .................................................................................................... 234 8.3.5. Defining Boundary Conditions .............................................................................................. 234 8.3.5.1. Rigid Body Tools .......................................................................................................... 235 8.3.5.2. Airbag or Simple Pressure Volume ................................................................................ 235 8.3.5.3. Input File Include Constraint ...................................................................................... 237 8.3.5.4. Keyword Snippet (LS-DYNA) Constraint ..................................................................... 238 8.3.5.5. Bolt Pretension ............................................................................................................ 238 8.3.5.6. Dynamic Relaxation ..................................................................................................... 239 8.3.6. Accessing Results ................................................................................................................. 242 8.3.7. Special Analysis Topics .......................................................................................................... 244 8.3.7.1. Importing the Results of a Thermal Analysis .................................................................. 244 8.3.8. Restarting a Workbench LS-DYNA Analysis ............................................................................ 244 8.3.8.1. Performing a Simple Restart ......................................................................................... 246 8.3.8.2. Performing a Small Restart ........................................................................................... 247 8.3.8.3. Performing a Full Restart .............................................................................................. 250 8.3.9. Additional LS-DYNA Analysis Tools ....................................................................................... 251 8.4. LS-DYNA Keywords used by Workbench LS-DYNA .......................................................................... 252 8.4.1. Input File Header .................................................................................................................. 252 8.4.2. Database Format .................................................................................................................. 252 8.4.3. Control Cards ....................................................................................................................... 253 8.4.4. Part Setup ............................................................................................................................ 260 8.4.5. Engineering Data Materials and Equations of State ................................................................ 267 8.4.6. Mesh Definition .................................................................................................................... 281 8.4.7. Coordinate Systems .............................................................................................................. 284 8.4.8. Components and Named Selections ..................................................................................... 285 8.4.9. Remote Points and Point Masses ........................................................................................... 285 8.4.10. Contacts and Body Interactions .......................................................................................... 289 8.4.10.1. Keywords Created from the Contact Properties Object ............................................... 293 Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

vii

Explicit Dynamics Analysis Guide 8.4.11. Magnitude and Tabular Data ............................................................................................... 295 8.4.12. Acceleration and Gravity ..................................................................................................... 295 8.4.13. Supports ............................................................................................................................ 296 8.4.14. Loads ................................................................................................................................. 297 8.4.15. Discrete Connections .......................................................................................................... 298 8.4.16. Other Supports .................................................................................................................. 299 8.4.17. Environment Temperature .................................................................................................. 300 8.4.18. ASCII Files ........................................................................................................................... 300 8.4.19. Database Output Settings ................................................................................................... 303 8.4.20. End of Input File ................................................................................................................. 304 8.5. Material Models Available in Workbench LS-DYNA ......................................................................... 304 8.5.1. Introduction ......................................................................................................................... 304 8.5.1.1. Equation of State ......................................................................................................... 304 8.5.1.2. Material Strength Model .............................................................................................. 304 8.5.1.3. Material Failure Model ................................................................................................. 305 8.5.2. Density ................................................................................................................................ 305 8.5.3. Linear Elastic ........................................................................................................................ 305 8.5.3.1. Isotropic Elasticity ........................................................................................................ 305 8.5.3.2. Orthotropic Elasticity ................................................................................................... 305 8.5.3.3. Anisotropic Elasticity ................................................................................................... 305 8.5.4. Test Data ............................................................................................................................. 305 8.5.5. Hyperelasticity ..................................................................................................................... 305 8.5.5.1. Blatz-Ko Hyperelasticity ............................................................................................... 306 8.5.5.2. Mooney-Rivlin ............................................................................................................. 306 8.5.5.3. Polynomial .................................................................................................................. 306 8.5.5.4. Yeoh ............................................................................................................................ 306 8.5.5.5. Ogden ........................................................................................................................ 306 8.5.6. Plasticity .............................................................................................................................. 306 8.5.6.1. Bilinear Isotropic Hardening ......................................................................................... 307 8.5.6.2. Multilinear Isotropic Hardening .................................................................................... 307 8.5.6.3. Bilinear Kinematic Hardening ....................................................................................... 308 8.5.6.4. Johnson-Cook Strength ............................................................................................... 308 8.5.6.5. Cowper-Symonds Power Law Hardening ...................................................................... 308 8.5.6.6. Rate Sensitive Power Law Hardening ............................................................................ 309 8.5.6.7. Cowper-Symonds Piecewise Linear Hardening ............................................................. 310 8.5.6.8. Modified Cowper-Symonds Piecewise Linear Hardening ............................................... 310 8.5.7. Forming Plasticity ................................................................................................................. 311 8.5.7.1. Bilinear Transversely Anisotropic Hardening ................................................................. 311 8.5.7.2. Multilinear Transversely Anisotropic Hardening ............................................................ 311 8.5.7.3. Bilinear FLD Transversely Anisotropic Hardening .......................................................... 312 8.5.7.4. Multilinear FLD Transversely Anisotropic Hardening ..................................................... 313 8.5.7.5. Bilinear 3 Parameter Barlat Hardening .......................................................................... 313 8.5.7.6. Exponential 3 Parameter Barlat Hardening ................................................................... 314 8.5.7.7. Exponential Barlat Anisotropic Hardening .................................................................... 314 8.5.8. Foams .................................................................................................................................. 315 8.5.8.1. Rate Independent Low Density Foam .......................................................................... 315 8.5.9. Eulerian ................................................................................................................................ 315 8.5.9.1. Vacuum ...................................................................................................................... 315 8.5.10. Rigid Materials ................................................................................................................... 315 8.5.11. Equations of State .............................................................................................................. 316 8.5.11.1. Background ............................................................................................................... 316 8.5.11.2. Bulk Modulus ............................................................................................................. 316

viii

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Explicit Dynamics Analysis Guide 8.5.11.3. Shear Modulus ........................................................................................................... 316 8.5.11.4. Polynomial EOS ......................................................................................................... 316 8.5.11.5. Shock EOS Linear ....................................................................................................... 316 8.5.11.6. Shock EOS Bilinear ..................................................................................................... 317 8.5.12. Failure ................................................................................................................................ 317 8.5.12.1. Plastic Strain Failure ................................................................................................... 317 8.5.12.2. Principal Stress Failure ................................................................................................ 318 8.5.12.3. Principal Strain Failure ................................................................................................ 318 8.5.12.4. Johnson-Cook Failure ................................................................................................. 319 8.5.13. Thermal Properties ............................................................................................................. 319 8.6. Customizing Workbench LS-DYNA using ACT ................................................................................. 319 8.6.1. CreateMaterial ...................................................................................................................... 322 8.6.2. CreateMaterial ...................................................................................................................... 322 8.6.3. CreateNewElement .............................................................................................................. 322 8.6.4. GetNewPartId ...................................................................................................................... 323 8.6.5. LSDynaSolverExtension.KeyWords.Part.Part CreateNewPart .................................................. 323 8.6.6. CreateSection ...................................................................................................................... 324 8.6.7. GetComponent .................................................................................................................... 324 8.6.8. GetContactId ....................................................................................................................... 324 8.6.9. GetContactTargetId .............................................................................................................. 325 8.6.10. GetCoordinateSystemSolverId ............................................................................................ 325 8.6.11. GetEndTime ....................................................................................................................... 325 8.6.12. GetMaterialSolverId ............................................................................................................ 325 8.6.13. GetNamedSelectionLSDYNAId ............................................................................................ 326 8.6.14. GetNewContact .................................................................................................................. 326 8.6.15. GetNewCurveId .................................................................................................................. 326 8.6.16. GetNewElementId .............................................................................................................. 326 8.6.17. GetNewElementType .......................................................................................................... 326 8.6.18. GetNewNodeId .................................................................................................................. 327 8.6.19. GetNewVectorId ................................................................................................................. 327 8.6.20. GetRemotePointNodeId ..................................................................................................... 327 8.6.21. GetSolverUnitSystem .......................................................................................................... 327 8.6.22. ContainsDynamicRelaxation ............................................................................................... 327 8.6.23. CurrentStep ........................................................................................................................ 328 8.6.24. MaxElementId .................................................................................................................... 328 8.6.25. MaxElementType ................................................................................................................ 328 8.6.26. MaxNodeId ........................................................................................................................ 328 8.7. References .................................................................................................................................... 328 9. Using the Drop Test Wizard ................................................................................................................. 329 9.1. What is the Drop Test Wizard ......................................................................................................... 329 9.2. Loading and Opening the Drop Test Wizard ................................................................................... 329 9.3. Preparing the Geometry for Use in the Drop Test Wizard ................................................................ 329 9.4. Setting up the Drop Parameters .................................................................................................... 330 9.5. Complete the Analysis ................................................................................................................... 332 9.6. The Rotate Geometry Object ......................................................................................................... 332 9.7. Current Limitations ....................................................................................................................... 333 Index ........................................................................................................................................................ 335

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

ix

x

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

List of Figures 2.1. Interaction of Lumped Manual Contact Regions .................................................................................... 27 2.2. Treatment of Friction for Lumped Manual Contact ................................................................................. 28 2.3. Interaction of Pairwise Manual Contact Regions .................................................................................... 29 2.4. Treatment of Friction for Pairwise Manual Contact ................................................................................. 29 3.1. Different applications of the two solvers with respect to velocity ........................................................... 99 3.2. Example Model Run with Explicit Dynamics Showing Problem Area (right) ........................................... 101 3.3. Comparison between the implicit (left) and the explicit (right) solvers for maximum deformation values ........................................................................................................................................................... 102 3.4. Model Setup Showing Contact (left) and Boundary Conditions (right) .................................................. 102 3.5. Final Stress Values Comparison Between the Explicit (left, 3.4E10 Pa) and Implicit (right, 3.7E10 Pa) Solvers ............................................................................................................................................................ 103 3.6. The Clip Model Setup in the Implicit Solver with Final Deformation Values (right) ................................. 103 3.7. The Clip Model Setup in Explicit Dynamics with Final Deformation Values (right) .................................. 104 3.8. Choices for information sharing between cells of implicit and explicit systems ..................................... 104 3.9. Meshing options menu - physics preference ........................................................................................ 106 3.10. Meshing options menu - Defaults ...................................................................................................... 107 3.11. Body Interactions Object under Connections ..................................................................................... 108 3.12. Initial Conditions Object .................................................................................................................... 111 3.13. Analysis Settings - Step Controls ........................................................................................................ 113 3.14. Default Solution Information display during solve with the estimated time remaining highlighted in yellow ...................................................................................................................................................... 113 3.15. Example of Eroded Material in a Model Simulating a Bullet going Through a Vase (eroded elements colored red) .............................................................................................................................................. 115 3.16. Analysis Settings - Output Controls .................................................................................................... 116 3.17. Graph of Energy Conservation for an Explicit Simulation .................................................................... 118 3.18. Deformation Graph (with respect to simulation time) and Results Table .............................................. 120 6.1. Conditions at a Moving Shock Front .................................................................................................... 136 6.2. Example energy conservation graph for model with symmetry plane and erosion ................................ 145 6.3. Comparison of pressure solution at a shock wave discontinuity a) using no artificial viscosity b) using the default artificial viscosity ........................................................................................................................... 146 6.4. Effects of artificial viscosity on the solution .......................................................................................... 147 6.5. Comparison of results of a Taylor test solved using SCP, ANP and NBS Tetrahedral elements. Results using NBS and ANP tetrahedral elements compare more favorably with experimental results than results using SCP (see table below). ............................................................................................................................... 153 6.6. Example bending test using SCP (1), ANP (2), NBS tetrahedral (3), and hex (4) elements.The displacement of the beam with NBS tetrahedral elements is the most similar to the beam meshed with hexahedral elements as it does not exhibit shear locking. ........................................................................................................... 154 6.7.Taylor test: Iron cylinder impacting rigid wall at 221m/s. Good correlation between ANP and Hex element results is obtained ..................................................................................................................................... 154 6.8. Example pull out test simulated using both hexahedral elements and ANP tetrahedral elements. Similar plastic strains and material fracture are predicted for both element formulations used. .............................. 155 7.1. Drucker-Prager Strength Linear ........................................................................................................... 187 7.2. Drucker-Prager Strength Stassi ............................................................................................................ 187 7.3. Drucker-Prager Strength Piecewise ...................................................................................................... 188 7.4. Johnson-Holmquist Strength Model ................................................................................................... 189 7.5. Johnson-Holmquist Damage Model .................................................................................................... 190 7.6. Johnson-Holmquist Strength Segmented ............................................................................................ 192 7.7. RHT Representation of Compressive Meridian ...................................................................................... 194 7.8.Third invariant dependence ................................................................................................................. 195 7.9. Bi-linear strain hardening function ...................................................................................................... 195 Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

xi

Explicit Dynamics Analysis Guide 7.10. RHT Elastic, Fracture and Residual Failure Surfaces ............................................................................. 196 7.11. Fit to Shock Velocity-Particle Velocity Relationship ............................................................................. 205 7.12. Pressure as function of density for the JWL equation of state .............................................................. 206 7.13. Loading-Unloading Behavior for a Porous Solid .................................................................................. 210 7.14. Mott Distribution for Varying Values of Gamma .................................................................................. 220 8.1. Discrete and Cable Controls when the Option is set to Discrete Beam ................................................... 262 8.2. Discrete and Cable Controls when the Option is set to Cable ................................................................ 263

xii

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

List of Tables 2.1. Example: Drop Test onto Reinforced Concrete Beam .............................................................................. 24 6.1. Characteristic Element Dimensions ..................................................................................................... 133 6.2. Typical stress strain curves for a ductile metal ...................................................................................... 135 6.3. Comparison of the performance of SCP, ANP, NBS and hex elements in a model involving bending.The displacement of the beam with NBS tetrahedral elements is the most similar to the beam meshed with hexahedral elements as it does not exhibit shear locking as is seen in the beams solved using SCP and ANP tetrahedral elements. ................................................................................................................................ 153 7.1. Input Data .......................................................................................................................................... 173 7.2. Input Data .......................................................................................................................................... 184 7.3. Input Data .......................................................................................................................................... 185 7.4. Input Data .......................................................................................................................................... 187 7.5. Input Data .......................................................................................................................................... 188 7.6. Input Data .......................................................................................................................................... 188 7.7. Input Data .......................................................................................................................................... 190 7.8. Input Data .......................................................................................................................................... 192 7.9. Input Data .......................................................................................................................................... 197 7.10. Input Data ........................................................................................................................................ 199 7.11. Input Data ........................................................................................................................................ 201 7.12. Input Data ........................................................................................................................................ 202 7.13. Input Data ........................................................................................................................................ 204 7.14. Input Data ........................................................................................................................................ 205 7.15. Input Data ........................................................................................................................................ 207 7.16. Input Data ........................................................................................................................................ 209 7.17. Input Data ........................................................................................................................................ 216 7.18. Input Data ........................................................................................................................................ 219 7.19. Input Data ........................................................................................................................................ 221 7.20. Input Data ........................................................................................................................................ 221 7.21. Input Data ........................................................................................................................................ 224 7.22. Input Data ........................................................................................................................................ 225 7.23. Input Data ........................................................................................................................................ 226 8.1. Solverdata Methods ............................................................................................................................ 321 8.2. Properties ........................................................................................................................................... 322 8.3. Properties ........................................................................................................................................... 322 8.4. Properties ........................................................................................................................................... 323 8.5. Properties ........................................................................................................................................... 323 8.6. Properties ........................................................................................................................................... 324 8.7. Properties ........................................................................................................................................... 324 8.8. Properties ........................................................................................................................................... 325 8.9. Properties ........................................................................................................................................... 325 8.10. Properties ......................................................................................................................................... 325 8.11. Properties ......................................................................................................................................... 326 8.12. Properties ......................................................................................................................................... 326 8.13. Properties ......................................................................................................................................... 327

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

xiii

xiv

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 1: Explicit Dynamics Analysis Guide Overview ANSYS Explicit Dynamics is a transient explicit dynamics Workbench application that can perform a variety of engineering simulations, including the modeling of nonlinear dynamic behaviour of solids, fluids, gases and their interaction. Additionally, the Workbench LS-DYNA extension is available to analyze a model using the LS-DYNA solver. A typical simulation consists of setting up the model, interactions and the applied loads, solving the model's nonlinear dynamic response over time for the loads and interactions, then examining the details of the response with a variety of available tools. The Explicit Dynamics application has objects arranged in a tree structure that guide you through the different steps of a simulation. By expanding the objects, you expose the details associated with the object, and you can use the corresponding tools and specification tables to perform that part of the simulation. Objects are used, for example, to define environmental conditions such as contact surfaces and loadings, and to define the types of results you want to have available for review. The following sections describe in detail how to use the Explicit Dynamics application to set up and run a simulation: • Explicit Dynamics Workflow (p. 3) • Transforming an Implicit Model to run in Explicit Dynamics (p. 99) • Applying Pre-Stress Effects for Explicit Analysis (p. 121) • Using Explicit Dynamics to Define Initial Conditions for Implicit Analyses (p. 125) • Explicit Dynamics Theory Guide (p. 129) • Material Models Used in Explicit Dynamics Analysis (p. 163) The following section discusses how to solve an Explicit Dynamics analysis using the LS-DYNA solver: • Using Workbench LS-DYNA for an Explicit Dynamics Analysis (p. 229)

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

1

2

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 2: Explicit Dynamics Workflow To learn how to perform an analysis, see Create Analysis System in the Mechanical User's Guide. Note that the features available may differ from one solver to another. To perform analyses that are beyond those available using Workbench, you can insert a Commands object in the tree. This chapter contains the following topics: 2.1. Introduction 2.2. Create the Analysis System 2.3. Define Engineering Data 2.4. Attach Geometry 2.5. Define Part Behavior 2.6. Define Connections 2.7. Setting Up Symmetry 2.8. Define Remote Points 2.9. Apply Mesh Controls/Preview Mesh 2.10. Establish Analysis Settings 2.11. Define Initial Conditions 2.12. Apply Loads and Supports 2.13. Solve 2.14. Postprocessing

2.1. Introduction You can perform a transient Explicit Dynamics analysis in the Mechanical application using an Explicit Dynamics system. Additionally, the Workbench LS-DYNA ACT Extension is available to analyze a model using the LS-DYNA solver. Unless specifically mentioned otherwise, this section addresses both the Explicit Dynamics system and Workbench LS-DYNA. Special conditions for Workbench LS-DYNA are noted where pertinent. An Explicit Dynamics analysis is used to determine the dynamic response of a structure due to stress wave propagation, impact or rapidly changing time-dependent loads. Momentum exchange between moving bodies and inertial effects are usually important aspects of the type of analysis being conducted. This type of analysis can also be used to model mechanical phenomena that are highly nonlinear. Nonlinearities may stem from the materials, (for example, hyperelasticity, plastic flows, failure), from contact (for example, high speed collisions and impact) and from the geometric deformation (for example, buckling and collapse). Events with time scales of less than 1 second (usually of order 1 millisecond) are efficiently simulated with this type of analysis. For longer time duration events, consider using a Transient analysis system. The time step used in an Explicit Dynamics analysis is constrained to maintain stability and consistency via the CFL condition (p. 132); that is, the time increment is proportional to the smallest element dimension in the model and inversely proportional to the sound speed in the materials used. Time increments are usually on the order of 1 microsecond and therefore thousands of time steps (computational cycles) are usually required to obtain the solution. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

3

Explicit Dynamics Workflow An Explicit Dynamics analysis typically includes many different types of nonlinearities including large deformations, large strains, plasticity, hyperelasticity, material failure etc. An Explicit Dynamics analysis can contain both rigid and flexible bodies. For rigid/flexible body dynamic simulations involving mechanisms and joints you may wish to consider using either the Transient Structural Analysis or Rigid Dynamics Analysis options.

Note The intent of this document is to provide an overview of an Explicit Dynamics analysis. Consult our technical support department to obtain a more thorough treatment of this topic.

2.2. Create the Analysis System For general information about creating an analysis system see Create Analysis System in the Mechanical User's Guide. From the Toolbox drag an Explicit Dynamics or a Workbench LS-DYNA template to the Project Schematic.

Note You need to load (p. 229) the Workbench LS-DYNA ACT extension before you see the template in the toolbox. Explicit Dynamics analyses only support the mm, mg, ms solver unit system (see Explicit Dynamics Solver Controls (p. 50) for supported units in a Workbench LS-DYNA analysis). The Explicit Dynamics solver is double precision (a Workbench LS-DYNA analysis can use single or double precision).

2.3. Define Engineering Data For general information about defining Engineering Data, see Define Engineering Data in the Mechanical User's Guide. Material properties can be linear elastic or orthotropic. Many different forms of material nonlinearity can be represented including hyperelasticity, rate and temperature dependent plasticity, pressure-dependent plasticity, porosity, material strength degradation (damage), material fracture/failure/fragmentation. For a detailed discussion on material models used in Explicit Dynamics, refer to Material Models Used in Explicit Dynamics Analysis (p. 163). Density must always be specified for materials used in an Explicit Dynamics analysis. Data for a range of materials is available in the Explicit material library.

2.4. Attach Geometry For general information about attaching a geometry to a system, see Attach Geometry/Mesh in the Mechanical User's Guide.

4

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Attach Geometry Solid, Surface, and Line bodies can be present in an Explicit Dynamics analysis. Only symmetric cross sections are supported for line bodies in Explicit Dynamics analyses, except those using the Workbench LS-DYNA ACT extension. The following cross sections are not supported: T-Sections, L-Sections, Z-Sections, Hat sections, Channel Sections. For I-Sections, the two flanges must have the same thickness. For rectangular tubes, opposite sides of the rectangle must be of the same thickness. For Workbench LS-DYNA all available cross sections in DesignModeler will be exported for analysis with the LS-DYNA solver. However, there are some limitations in the number of dimensions that the LS-DYNA solver supports for the Z, Hat and Channel cross sections. For more information consult the LS-DYNA Keywords manual. To prevent the generation of unnecessarily small elements (and long run times) try using DesignModeler or SpaceClaim to remove unwanted "small" features or holes from your geometry. Thickness can be specified for selected faces on a surface body by inserting a thickness object. Constant, tabular, and functional thickness are all supported. Stiffness Behavior Flexible behavior can be assigned to any body type. Rigid behavior can be applied to Solid, Surface, and Line bodies. Coordinate System Local Cartesian coordinate systems can be assigned to bodies. These will be used to define the material directions when using the Orthotropic Elasticity property in a material definition. The material directions 1, 2, 3 will be aligned with the local x, y and z axes of the local coordinate system.

Note Cylindrical coordinate systems assigned to bodies are not supported for Explicit Dynamics systems. Cylindrical coordinate systems are only supported to define rotational displacement or velocity constraints. Cylindrical coordinate systems are not supported with Workbench LS-DYNA. Reference Temperature This option defines the initial (time=0.0) temperature of the body. Reference Frame Available for solid bodies when an Explicit Dynamics system is part of the solution; the user has the option of setting the Reference Frame to Lagrangian (default) or Eulerian (Virtual). If Stiffness Behavior is defined as Rigid, Eulerian is not a valid setting. The reference Frame is not supported for Workbench LS-DYNA. Rigid Materials For bodies defined to have rigid stiffness, only the Density property of the material associated with the body will be used. For Explicit Dynamics systems all rigid bodies must be discretized with a Full Mesh

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

5

Explicit Dynamics Workflow or the Rigid Body Behavior must be defined as Dimensionally Reduced. The Full Mesh option will be specified by default for the Explicit meshing physics preference. The mass and inertia of the rigid body will be derived from the elements and material density for each body. By default, a kinematic rigid body is defined and its motion will depend on the resultant forces and moments applied to it through interaction with other Parts of the model. Elements filled with rigid materials can interact with other regions via contact. Constraints can only be applied to an entire rigid body. For example, a fixed displacement cannot be applied to one edge of a rigid body, it must be applied to the whole body.

Note • 2-D Explicit Dynamics analyses are supported for Plane Strain and Axisymmetric behaviors. 2D analyses are Beta in Workbench LS-DYNA. • Only symmetric cross-sections are supported for line bodies. • Flexible and rigid bodies cannot be combined in Multi-body Parts. Bonded connections can be applied to connect rigid and flexible bodies. • The Thickness Mode and Offset Type fields for surface bodies are not supported for Explicit Dynamics systems. Offset Type is supported for Workbench LS-DYNA. • Initial over-penetrations of nodes/elements of different bodies should be avoided or minimized if sliding contact is to be used. There are several methods available in Workbench to remove initial penetration.

2.5. Define Part Behavior For general information about defining parts, see Define Part Behavior in the Mechanical User's Guide. Nonlinear effects are always accounted for in Explicit Dynamics analysis. Parts may be defined as rigid or flexible. In the solver, rigid parts are represented by a single point that carries the inertial properties together with a discretized exterior surface that represents the geometry. Rigid bodies should be meshed using similar Method mesh controls as those used for flexible bodies. The inertial properties used in the solver will be derived from the discretized representation of the body, and the material density and hence may differ slightly from the values presented in the properties of the body in the Mechanical application GUI. At least one flexible body must be specified when using the Explicit Dynamics solver. The solver requires this in order to calculate the time-step increments. In the absence of a flexible body, the time-step becomes underdefined. The boundary conditions allowed for the rigid bodies with Explicit Dynamics are: • Connections – Contact Regions: Frictionless, Frictional and Bonded.

6

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections – Body Interactions: Frictionless, Frictional and Bonded. Bonded body interactions are not supported for Workbench LS-DYNA. – In Explicit Dynamics systems, rigid bodies may not be bonded to other rigid bodies. • Initial Conditions: Velocity, Angular Velocity • Supports: Displacement, Fixed Support and Velocity. • Loads: Pressure and Force. Force is not supported for Explicit Dynamics analyses. For an Explicit Dynamics analysis, the following postprocessing features are available for rigid bodies: • Results and Probes: Deformation only - that is, Displacement, Velocity. • Result Trackers: Body average data only. If a multibody part consists only of rigid bodies, all of which share the same material assignment, the part will act as a single rigid body, even if the individual bodies are not physically connected.

2.6. Define Connections For general information about defining connections, see Define Connections in the Mechanical User's Guide. Line body to line body contact is possible subject to the following: • Contact Detection is set to Proximity Based in the Body Interactions Details view. • Edge on Edge is set to Yes in the Body Interactions Details view. • The Interaction Type is defined as Frictional or Frictionless. • Workbench LS-DYNA uses the *CONTACT_AUTOMATIC_GENERAL and *CONTACT_AUTOMATIC_SINGLE_SURFACE keywords when a friction or frictionless Body Interaction is scoped to geometry that contains line bodies. The keywords handle contacts between line bodies only, and line bodies to other body types respectively. In the case where the Body Interaction is scoped to only line bodies, then only the *CONTACT_AUTOMATIC_GENERAL keyword is used. Reinforcement body interaction should be supported in the case when only line bodies are scoped to a Body Interaction of Type = Reinforcement. The line bodies will then be tied to any solid body that they intersect. Reinforcement body interactions are not supported for 2D Explicit Dynamics analyses. However utilizing Keyword Snippets under Contact Region objects should provide a suitable alternative. Body Interactions (p. 9), Contact (p. 25) and Spot Welds are all valid in Explicit Dynamics analyses. Frictional, Frictionless and Bonded body interactions and contact options are available. Conditionally bonded contact can be simulated using the breakable property of each bonded region. Spot Welds can also be made to fail using the breakable property. Joints and Beam connections are not supported for Explicit Dynamics analyses. Springs are not supported for Workbench LS-DYNA analyses. The Contact Tool is also not applicable to Explicit Dynamics analyses. For Workbench LS-DYNA, bonded body interactions are not supported. Also, Contact Region objects with Auto Asymmetric Behavior or just Asymmetric Behavior are treated the same. Symmetric Be-

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

7

Explicit Dynamics Workflow havior will create a _SURFACE_TO_SURFACE keyword for the contact and an Asymmetric Behavior will create a _NODES_TO_SURFACE keyword. Bonded contact is not supported in an Explicit Dynamics analysis for bodies that have their Reference Frame set to Eulerian (Virtual). A solver warning is shown to let the user know that such bodies will be ignored for bonds. Bonded contact is not support in a 2D Explicit Dynamics analysis. To avoid hourglassing problems, remote points can be used if there are only a few nodes active in the bond definition. Bonds are not recommended for joining tetrahedral meshes. Use multibodied parts or remote points instead. By default, a Body Interaction object will be automatically inserted in the Mechanical application tree and will be scoped to all bodies in the model. This object activates frictionless contact behavior between all bodies that come into proximity during the analysis.

2.6.1. Spot Welds in Explicit Dynamics Analyses Spot welds provide a mechanism to rigidly connect two discrete points in a model and can be used to represent welds, rivets, bolts, etc. The points usually belong to two different surfaces and are defined on the geometry (see DesignModeler or SpaceClaim help). During the solver initialization process, the two points defining each spot weld will be connected by a rigid beam element. Additionally, rigid beam elements will be generated on each surface to enable transfer of rotations at the spot weld location (see figure below). If the point of the spot weld lies on a shell body, both translational and rotational degrees of freedom will be linked at the connecting point. If the point of the spot weld lies on a surface of a solid body, additional rigid beam elements will be generated to enable transfer of rotations at the spot weld location. Spot welds can be released during a simulation using the Breakable Stress or Force option. If the stress criteria is selected the user will be asked to define an effective cross sectional area. This is used to convert the defined stress limits into equivalent force limits. A spot weld will break (release) if the following criteria is exceeded: (2.1)

Where: fn and fs are normal and shear interface forces Sn and Ss are the maximum allowed normal and shear force limits n and s are user defined exponential coefficients Note that the normal interface force f

n

is non-zero for tensile values only.

After failure of the spot weld the rigid body connecting the points is removed from the simulation. Spot welds of zero length are permitted. However, if such spot welds are defined as breakable the above failure criteria is modified since local normal and shear directions cannot be defined. A modified criteria is used with global forces:

8

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections

(2.2) Where,

are the force differences across the spot weld in the global coordinate system.

Note A spot weld is equivalent to a rigid body and as such multiple nodal boundary conditions cannot be applied to spot welds.

2.6.2. Body Interactions in Explicit Dynamics Analyses Within an Explicit Dynamics analysis, the body interaction feature represents contact between bodies and includes settings that allow you to control these interactions. If the geometry you use has two or more bodies in contact, a Body Interactions object folder appears by default under Connections in the tree. Included in a Body Interactions folder are one or more Body Interaction objects, with each object representing a contact pair. You can also manually add these two objects: • To add a Body Interactions folder, highlight the Connections folder and choose Body Interactions from the Connect group in the Context tab. A Body Interactions folder is added and includes one Body Interaction object. • To add a Body Interaction object to an existing Body Interactions folder, highlight the Connections folder, the Body Interactions folder, or an existing Body Interaction object, and choose Body Interaction from the Connect group in the Context tab. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

9

Explicit Dynamics Workflow

General Notes Each Body Interaction object activates an interaction for the bodies scoped in the object. With body interactions, contact detection is completely automated in the solver. At any time point during the analysis any node of the bodies scoped in the interaction may interact with any face of the bodies scoped in the interaction. The interactions are automatically detected during the solution. The default frictionless interaction type that is scoped to all bodies activates frictionless contact between any external node and face that may come into contact in the model during the analysis. To improve the efficiency of analyses involving large number of bodies, you are advised to suppress the default frictionless interaction that is scoped to all bodies, and instead insert additional Body Interaction objects which limit interactions to specific bodies. The union of all frictional/frictionless body interactions defines the matrix of possible body interactions during the analysis. For example, in the model shown below: • Body A is traveling towards body B and we require frictional contact to occur. A frictional body interaction type scoped only to bodies A and B will achieve this. Body A will not come close to body C during the analysis so it does not need to be included in the interaction. • Body B is bonded to body C. A bonded body interaction type, scoped to bodies B and C will achieve this. • If the bond between bodies B and C breaks during the analysis, we want frictional contact to take place between bodies B and C. A frictional body interaction type scoped only to bodies B and C will achieve this.

A bonded body interaction type can be applied in addition to a frictional/frictionless body interaction. A reinforcement body interaction type be can be applied in addition to a frictional/frictionless body interaction. Object property settings are included in the Details view for both the Body Interactions folder and the individual Body Interaction objects. Refer to the following sections for descriptions of these properties. 2.6.2.1. Properties for Body Interactions Folder 2.6.2.2. Interaction Type Properties for Body Interaction Object 2.6.2.3. Identifying Body Interactions Regions for a Body

10

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections

2.6.2.1. Properties for Body Interactions Folder All properties for the Body Interactions folder are included in an Advanced category and define the global properties of the contact algorithm for the analysis. These properties are applied to all Body Interaction objects and to all frictional (p. 19) and frictionless (p. 19) manual contact regions. This section includes descriptions of the following properties for the Body Interactions folder: 2.6.2.1.1. Contact Detection 2.6.2.1.2. Formulation 2.6.2.1.3. Sliding Contact 2.6.2.1.4. Manual Contact Treatment 2.6.2.1.5. Shell Thickness Factor and Nodal Shell Thickness 2.6.2.1.6. Body Self Contact 2.6.2.1.7. Element Self Contact 2.6.2.1.8.Tolerance 2.6.2.1.9. Pinball Factor 2.6.2.1.10.Time Step Safety Factor 2.6.2.1.11. Limiting Time Step Velocity 2.6.2.1.12. Edge on Edge Contact

2.6.2.1.1. Contact Detection The available choices are described below.

Trajectory The trajectory of nodes and faces included in frictional or frictionless contact are tracked during the computation cycle. If the trajectory of a node and a face intersects during the cycle a contact event is detected. The trajectory contact algorithm is the default and recommended option in most cases for contact in Explicit Dynamics analyses. Contacting nodes/faces can be initially separated or coincident at the start of the analysis. Trajectory based contact detection does not impose any constraint on the analysis time step and therefore often provides the most efficient solution. Note that nodes which penetrate into another element at the start of the simulation will be ignored for the purposes of contact and thus should be avoided. To generate duplicate conforming nodes across a contact interface: 1. Use the multibody part option in DesignModeler and set Shared Topology to Imprint. 2. For meshing, use Contact Sizing, the Arbitrary match control or the Match mesh Where Possible option of the Patch Independent mesh method.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

11

Explicit Dynamics Workflow

Proximity Based The external faces, edges and nodes of a mesh are encapsulated by a contact detection zone. If during the analysis a node enters this detection zone, it will be repelled using a penalty based force.

Note • An additional constraint is applied to the analysis time step when this contact detection algorithm is selected. The time step is constrained such that a node cannot travel through a fraction of the contact detection zone size in one cycle. The fraction is defined by the Time Step Safety Factor (p. 18) described below. For analyses involving high velocities, the time step used in the analysis is often controlled by the contact algorithm. • The initial geometry/mesh must be defined such that there is a physical gap/separation of at least the contact detection zone size between nodes and faces in the model. The solver will give error messages if this criteria is not satisfied. This constraint means this option may not be practical for very complex assemblies. • Proximity Based Contact is not supported in 2D Explicit Dynamics analyses.

12

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections

2.6.2.1.2. Formulation This property is available if Contact Detection is set to Trajectory. The available choices are described below.

Penalty If contact is detected, a local penalty force is calculated to push the node involved in the contact event back to the face. Equal and opposite forces are calculated on the nodes of the face in order to conserve linear and angular momentum. Trajectory based penalty force,

Proximity based penalty force, Where: D is the depth of penetration M is the effective mass of the node (N) and face (F) Δt is the simulation time step

Note • Kinetic energy is not necessarily conserved. You can track conservation of energy in contact using the Solution Information object, the Solution Output, or one of the energy summary result trackers. • The applied penalty force will push the nodes back towards the true contact position during the cycle. However, it will usually take several cycles to satisfy the contact condition.

Decomposition Response All contacts that take place at the same point in time are first detected. The response of the system to these contact events is then calculated to conserve momentum and energy. During this process, forces are calculated to ensure that the resulting position of nodes and faces does not result in further penetration at that time point.

Note • The decomposition response algorithm cannot be used in combination with bonded contact regions. The formulation will be automatically switch to penalty if bonded regions are present in the model. • The decomposition response algorithm is more impulsive (in a given cycle) than the penalty method. This can give rise to large hourglass energies and energy errors.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

13

Explicit Dynamics Workflow

2.6.2.1.3. Sliding Contact This option is available if Contact Detection is set to Trajectory. When a contact event is detected part way through a cycle and the contact node has a tangential velocity relative to the face it has made contact with, the node needs to slide along the face for the remainder of the cycle. If the node should slide to the edge of the face before the end of the cycle, it is necessary to determine whether the node needs to begin to slide along an adjacent face. Two options described below are available for determining which (if any) face the node needs to slide to.

Discrete Surface When a node slides to the edge of a face, the next face the node needs to slide on is determined using the contact detection algorithm. This option is the default and will provide the most time efficient solution. However, penetrations of nodes may be seen in situations where the faces that the nodes are sliding on are experiencing large deformations or rotations. When such penetrations occur, it is recommended the user switches to the Connected Surface option.

Connected Surface When a node slides to the edge of a face, the next face the node needs to slide on is determined using the mesh connectivity.

2.6.2.1.4. Manual Contact Treatment This option is available if Sliding Contact is set to Connected Surface. It determines how combinations of manual contact regions and body interactions are handled in the Explicit Dynamics solver. Options are Pairwise and Lumped. When Lumped is selected, all regions that are scoped to a manual contact region are free to contact with each other. When Pairwise is selected, contact can only occur between a node and a face if the node appears in the contact scoping and the face in the target scoping of the same manual contact region. This is explained further in Manual Contact Regions in Explicit Dynamics Analyses (p. 25).

2.6.2.1.5. Shell Thickness Factor and Nodal Shell Thickness These properties are available if the geometry includes one or more surface bodies and if Contact Detection is set to Trajectory. The Shell Thickness Factor allows you to control the effective thickness of surface bodies used in the contact. The value of the factor must be between 0.0 and 1.0, and determines the amount of the shell thickness that is taken into account for the interaction distance. Typically, a value of 0.0 or 1.0 should be chosen. Interaction in the solver is always taking place between a node and a face (contact surface). You can enable two (complementary) algorithms to take the shell thickness into account: 1. Shell thickness for the faces which will offset the faces 2. Shell thickness for the nodes which creates a "sphere" around the node In order to use one or both of these thickness algorithms you can: 1. Set the shell thickness factor to a value other than zero to activate the shell thickness algorithm for the faces

14

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections 2. Enable nodal shell thickness to activate the shell thickness algorithm for the nodes, in addition to shell thickness for the faces Interaction Behavior with Shell Thickness Setting the factor to a value other than zero means that the contact surface is positioned at (0.5 x shell thickness x factor) on both sides of the shell mid plane. A factor of 0.0 means that the shell has no contact thickness and the contact surface is positioned at the shell mid plane. Note that with this setting the nodal shell thickness can not be activated separately. The contact area of a node depends on the setting for Nodal Shell Thickness. If it is set to No, the node is always located at the mid-surface of the shell (Situation I (p. 15)). If it is set to Yes, the node is located at a spherical distance of half the thickness away from the physical node location (Situation II (p. 15)). Situation I Two shell parts with thickness δ1 and δ2 will not contact at a distance of (δ1/2 + δ2/2), but at a distance which is half of the largest shell thickness as is depicted below.

Note that for shell node on solid face impacts, the node will be able to get to within zero distance of the solid face; the thickness for the shell nodes will not be taken into account. The solid nodes will, however, find the shell faces at contact distance. Situation II By enabling the nodal shell thickness, two shell parts will contact at a distance of (δ1/2 + δ2/2). From a physical point of view this is correct, as can be seen in the picture below.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

15

Explicit Dynamics Workflow

Note Care should be taken for nodes that are on or close to a free edge of the shell surface because the node may find contact in an unexpected manner due to the spherical contact around these nodes. This is shown below in a 2D manner, where for example node 1 and 2 have an additional contact area which extends beyond the geometry.

When set to Program Controlled, the behavior of nodal shell thickness is determined by the Analysis Settings Preference Type (p. 61).

16

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections

2.6.2.1.6. Body Self Contact When set to Yes, the contact detection algorithm will check for external nodes of a body contacting with faces of the same body in addition to other bodies. This is the most robust option since all possible external contacts should be detected. When set to No, the contact detection algorithm will only check for external nodes of a body contacting with external faces of other bodies. This setting reduces the number of possible contact events and can therefore improve efficiency of the analysis. This option should not be used if a body is likely to fold onto itself during the analysis, as it would during plastic buckling for example. When set to Program Controlled, the behavior of self contact is determined by the Analysis Settings Preference Type (p. 61). Presented below is an example of a model that includes self impact.

2.6.2.1.7. Element Self Contact When set to Yes, automatic erosion (removal of elements) is enabled when an element deforms such that one of its nodes comes within a specified distance of one of its faces. In this situation, elements are removed before they become degenerated. Element self contact is very useful for impact penetration examples where removal of elements is essential to allow generation of a hole in a structure. Element removal through Element Self Contact is only activated when one of the erosion options under Erosion Controls is also set to Yes.

When set to Program Controlled, the behavior of self contact is determined by the Analysis Settings Preference Type (p. 61).

2.6.2.1.8. Tolerance This property is available if Contact Detection is set to Trajectory and Element Self Contact is set to Yes. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

17

Explicit Dynamics Workflow Tolerance defines the size of the detection zone for element self contact when the trajectory contact option is used (see Element Self Contact (p. 17)). The value input is a factor in the range 0.1 to 0.5. This factor is multiplied by the smallest characteristic dimension of the elements in the mesh to give a physical dimension. A setting of 0.5 effectively equates to 50% of the smallest element dimension in the model.

Note The smaller the fraction the more accurate the solution.

2.6.2.1.9. Pinball Factor This property is available if Contact Detection is set to Proximity Based. The pinball factor defines the size of the detection zone for proximity based contact. The value input is a factor in the range 0.1 to 0.5. This factor is multiplied by the smallest characteristic dimension of the elements in the mesh to give a physical dimension. A setting of 0.5 effectively equates to 50% of the smallest element dimension in the model.

Note The smaller the fraction the more accurate the solution. The time step in the analysis could be reduced significantly if small values are used (see Time Step Safety Factor (p. 18)).

2.6.2.1.10. Time Step Safety Factor This property is available if Contact Detection is set to Proximity Based. For proximity based contact, the time step used in the analysis is additionally constrained by contact such that in one cycle, a node in the model cannot travel more than the detection zone size, multiplied by a safety factor. The safety factor is defined with this property and the recommended default is 0.2. Increasing the factor may increase the time step and hence reduce runtimes, but may also lead to missed contacts. The maximum value you can specify is 0.5.

2.6.2.1.11. Limiting Time Step Velocity This property is available if Contact Detection is set to Proximity Based. For proximity based contact, this setting limits the maximum velocity that will be used to compute the proximity based contact time step calculation.

2.6.2.1.12. Edge on Edge Contact This property is available if Contact Detection is set to Proximity Based.

18

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections By default, contact events in Explicit Dynamics are detected by nodes impacting faces. Use this option to extend the contact detection to include discrete edges impacting other edges in the model.

Note This option is numerically intensive and can significantly increase runtimes. It is recommended that you compare results with and without edge contact to make sure this feature is required. A model with edge on edge contact cannot be run in parallel.

2.6.2.2. Interaction Type Properties for Body Interaction Object This section includes descriptions of the interaction types for the Body Interaction object: 2.6.2.2.1. Frictionless Type 2.6.2.2.2. Frictional Type 2.6.2.2.3. Bonded Type 2.6.2.2.4. Reinforcement Type

2.6.2.2.1. Frictionless Type Setting Type to Frictionless activates frictionless sliding contact between any exterior node and any exterior face of the scoped bodies. Individual contact events are detected and tracked during the analysis. The contact is symmetric between bodies (that is, each node will belong to a master face impacted by adjacent slave nodes; each node will also act as a slave impacting a master face).

Supported Connections Explicit Dynamics Connection Geometry

Volume

Shell

Line

Volume

Yes

Yes

Yes

Shell

Yes

Yes

Yes

Line

Yes

Yes

*Yes

*Only for Contact Detection = Proximity Based and Edge on Edge Contact = Yes (This option switches on contact between ALL lines / bodies / edges; that is, there is no dependence on the scoping selection of body interactions.) Workbench LS-DYNA Connection Geometry

Volume

Shell

Line

Volume

Yes

Yes

No

Shell

Yes

Yes

No

Line

No

No

No

2.6.2.2.2. Frictional Type Setting Type to Frictional activates frictional sliding contact between any exterior node and any exterior face of the scoped bodies. Individual contact events are detected and tracked during the simulation.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

19

Explicit Dynamics Workflow The contact is symmetric between bodies (that is, each node will belong to a master face impacted by adjacent slave nodes, each node will also act as a slave impacting a master face). Friction Coefficient: A non-zero value will activate Coulomb type friction between bodies (F = μR). The relative velocity (ν) of sliding interfaces can influence frictional forces. A dynamic frictional formulation for the coefficient of friction can be used. (2.3) where = friction coefficient = dynamic coefficient of friction β = exponential decay coefficient ν = relative sliding velocity at point of contact Non-zero values of the Dynamic Coefficient and Decay Constant should be used to apply dynamic friction.

Supported Connections Explicit Dynamics Connection Geometry

Volume

Shell

Line

Volume

Yes

Yes

Yes

Shell

Yes

Yes

Yes

Line

Yes

Yes

*Yes

*Only for Contact Detection = Proximity Based and Edge on Edge Contact = Yes (This option switches on contact between ALL lines / bodies / edges; that is, there is no dependence on the scoping selection of body interactions.) Workbench LS-DYNA Connection Geometry

Volume

Shell

Line

Volume

Yes

Yes

No

Shell

Yes

Yes

No

Line

No

No

No

2.6.2.2.3. Bonded Type Descriptions of the following properties are also addressed in this section: • Maximum Offset • Breakable – Stress Criteria

20

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections → Normal Stress Limit → Normal Stress Exponent → Shear Stress Limit → Shear Stress Exponent External nodes of bodies included in bonded interactions will be tied to faces of bodies included in the interaction if the distance between the external node and the face is less than the value defined by the user in Maximum Offset. The solver automatically detects the bonded nodes/faces during the initialization phase of the analysis. Note that it is important to select an appropriate value for the Maximum Offset. The automatic search will bond everything together which is found within this value. During the analysis the nodes are kept at the same relative position on the face to which they are bonded. This is done by means of penalty forces which are either dependent on the mass of the nodes/faces or the stiffness of the material. The stiffness is weighted based on materials on either side of the bond. In models with mass scaling the penalty method is chosen based on the mass scaling setting: • Mass scaling off: Penalty method based on harmonic mass in the bonded pair. • Mass scaling on: Penalty method based on harmonic stiffness in the bonded pair. Origin of Model

Mass Scaling Off

Mass Scaling On

Any Workbench project opened in R18.0 or later

Harmonic Mass

Harmonic Stiffness

Note The stiffness weighted penalty method is typically superior to a mass weighted penalty and increases the robustness of (offset) bonds. By switching on mass scaling and still using a small target timestep (eg 1e-20) no mass will be added, but the penalty method will be switched to harmonic stiffness. When large material stiffness occurs between two materials that are bonded, it is recommended that you use an asymmetric definition where the contact scope (nodes to be bonded) refers to the soft material and the target scope (faces to bond to) refers to the stiffer material. Use the custom variable BOND_STATUS to check bonded connections in Explicit Dynamics. The variable records the number of nodes bonded to the faces on an element during the analysis. This can be used not only to verify that initial bonds are generated appropriately, but also to identify bonds that break during the simulation. The automatic search algorithm for bonded regions will search for the minimum distance to any of the faces. If this minimum distance falls within the maximum offset value, the bond pair will be established. In order to compute the proper distance to a face the algorithm will determine if the perpendicular projection to the face falls within the face. If that is not the case, the perpendicular projection to the face edges is considered. If that is not the case, the distance to one of the face nodes is considered. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

21

Explicit Dynamics Workflow This algorithm guarantees that a minimum distance is always found and can be properly compared against the value input for Maximum Offset. Verification of the initialized bonds can be done by inspection of the prt file. A summary is given which lists the number of candidate nodes for bonding and the actual number of nodes that were bonded. If the percentage of nodes to be bonded is 0% it means none of the nodes are actually bonded. You should consider increasing the Maximum Offset in this case.

Maximum Offset defines the tolerance used at initialization to determine whether a node is bonded to a face. Breakable = No implies that the bond will remain throughout the analysis. Breakable = Stress Criteria implies that the bond may break (or be released) during the analysis. The criteria for breaking a bond is defined as: (2.4) where = Normal Stress Limit n = Normal Stress Exponent = Shear Stress Limit m = Shear Stress Exponent The Behavior option can be used as described in Behavior. 22

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections Auto Asymmetric behavior is dependent on the type of scoping: • Bonded connections with only faces scoped will behave symmetrically. • All other bonded connections (if the Contact or Target is scoped to a vertex or edge) will behave asymmetrically. Note that there are two distinguishing factors during initialization based on behavior: Internal out-of-plane tolerance • For symmetric bond behavior the perpendicular projection of a node to a face has to fall within the face bounds otherwise the bond pair is disregarded a candidate. • For asymmetric bond behavior the perpendicular projection of a node to a face does not have to fall within the face bounds in order to be considered as a candidate. • For both types of behavior the Maximum offset is always taken into account. • If needed, a symmetric bond definition can also be changed to search out-of-plane by taking the following steps: – Set the definition to Asymmetric in order to search out-of-plane – Duplicate the definition of the bond object (right-click operation) – Subsequently "flip" Contact and Target (right-click operation) Effectively, you have created a symmetric definition (Contact->Target, Target->Contact) and bonds will be searched out of plane. Bond definitions referring to a single part • Symmetric bonds are disregarded for definitions that scope to a single part. • Asymmetric bonds are considered for definitions that scope to a single part. The Trim Contact option is ignored by the Explicit solver.

Supported Connections Explicit Dynamics See Supported Contact Types for more information.

Note Bonded body interactions and contact are not supported for 2D Explicit Dynamics analyses. Workbench LS-DYNA* Connection Geometry

Volume

Shell

Line

Volume

Yes

Yes

No

Shell

Yes

Yes

No

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

23

Explicit Dynamics Workflow Connection Geometry Line

Volume

Shell

Line

Yes

Yes

No

*The above matrix is valid only for Contact Regions. Bonded body interactions are not supported at all.

2.6.2.2.4. Reinforcement Type This body interaction type is used to apply discrete reinforcement to solid bodies. All line bodies scoped to the object will be flagged as potential discrete reinforcing bodies in the solver. On initialization of the solver, all elements of the line bodies scoped to the object which are contained within any solid body in the model will be converted to discrete reinforcement. Elements which lie outside all volume bodies will remain as standard line body elements. The reinforcing beam nodes will be constrained to stay at the same initial parametric location within the volume element where they reside during element deformation. Typical applications involve reinforced concrete or reinforced rubber structures like tires and hoses. If the volume element to which a reinforcing node is tied is eroded, the beam node bonding constraint is removed and becomes a free beam node. On erosion of a reinforcing beam element node, if inertia is retained the node will remain tied to the parametric location of the volume element. If inertia is not retained, the node will also be eroded.

Note Volume elements that are intersected by reinforcement beams, but do not contain a beam node, will not be experiencing any reinforced beam forces. Good modeling practice is therefore to have the element size of the beams similar or less than that of the volume elements. Table 2.1: Example: Drop Test onto Reinforced Concrete Beam

Note that the target solid bodies do not need to be scoped to this object – these will be identified automatically by the solver on initialization.

24

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections

Supported Connections Explicit Dynamics Connection Geometry

Volume

Shell

Line

Volume

No

No

*Yes

Shell

No

No

No

Line

*Yes

No

No

*Only the line body needs to be included in the scope. The Explicit Dynamics solver automatically detects which volume bodies that the line body passes through.

Note Reinforcement body interactions are not supported for 2D Explicit Dynamics analyses. Workbench LS-DYNA Connection Geometry

Volume

Shell

Line

Volume

No

No

*Yes

Shell

No

No

No

Line

*Yes

No

No

*Only the line body needs to be included in the scope. The Explicit Dynamics solver automatically detects which volume bodies that the line body passes through.

Note Reinforcement body interactions are not supported for 2D Workbench LS-DYNA analyses.

2.6.2.3. Identifying Body Interactions Regions for a Body See the description for Body Interactions for Selected Bodies in the section Correlating Tree Outline Objects with Model Characteristics in the Mechanical User's Guide.

2.6.3. Manual Contact Regions in Explicit Dynamics Analyses In addition to Body Interaction (p. 9) objects, contact regions can be defined in an Explicit Dynamics analysis using manual Contact Regions. They can be used when the Contact Detection method is set to either Trajectory or Proximity Based. This section describes how manual contact regions are treated in the Explicit Dynamics solver. It does not apply to the Workbench LS-DYNA solver. In addition to the rules governing the scoping for manual contact regions in other analysis types, there are some additional rules for the scoping supported in an Explicit Dynamics analysis. These rules depend on the overall contact settings defined in the Body Interactions object and are described in section Manual Contact Region Behavior for Proximity Based Contact and Trajectory Contact with Discrete Sliding or Manual Contact Treatment set to Lumped (p. 26) and Manual Contact Region Behavior for Trajectory Contact with Connected Surface Sliding and Manual Contact Treatment set to Pairwise (p. 28).

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

25

Explicit Dynamics Workflow Manual contact regions are additive to any contact defined through Body Interaction objects; they do not override the behavior defined in Body Interaction objects. The Explicit Dynamics solver handles manual contact regions based on the options selected in the Body Interactions object. Note that the discussion that follows is about manual Contact Region behavior, but the settings that affect the behavior are found in the Body Interactions object. If no Body Interactions object is present, the default options for Body Interactions are used. The different behaviors are described in the following sections. 2.6.3.1. Manual Contact Region Behavior for Proximity Based Contact and Trajectory Contact with Discrete Sliding or Manual Contact Treatment set to Lumped 2.6.3.2. Manual Contact Region Behavior for Trajectory Contact with Connected Surface Sliding and Manual Contact Treatment set to Pairwise

2.6.3.1. Manual Contact Region Behavior for Proximity Based Contact and Trajectory Contact with Discrete Sliding or Manual Contact Treatment set to Lumped The behavior described below is expected for contact detection in the following scenarios: • Contact Detection set to Proximity Based • Contact Detection set to Trajectory and either: – Sliding Contact set to Discrete Surface – Sliding Contact set to Connected Surface and Manual Contact Treatment set to Lumped The scoping supported with these contact settings are: • The Contact scoping and the Target scoping are both of type Face. • The Contact scoping and the Target scoping are both of type Body. All faces and nodes in the scoping of any manual contact region or any Body Interaction object are all able to find contact with one another. Therefore, a node in the scoping of one contact region may find contact with a face in the scoping of a different contact region. See Figure 2.1: Interaction of Lumped Manual Contact Regions (p. 27) for further explanation.

26

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections Figure 2.1: Interaction of Lumped Manual Contact Regions

Manual contact regions are defined A) between the lower face of Body 1 and the upper face of Body 3; B) between the lower face of Body 2 and the upper face of Body 3; C) between the rightmost face of Body 1 and the leftmost face of Body 2. In this scenario the Explicit Dynamics solver will also search for contact events between the upper face of Body 3 and the rightmost face of Body 1 and the leftmost face of Body 2 even though those interactions have not been explicitly defined with manual contact regions. The Symmetry Behavior option and Trim Contact option of all manual contact regions are ignored. Friction coefficients are stored per pairs of bodies in the solver, and not per pair of contact scopings. Therefore, if a manual contact region has Contact scoped to faces on Body A, and the Target is scoped to faces on Body B, the friction coefficient defined for this manual contact region will be use for any contact between Body A and Body B. Care should be taken when defining friction coefficients, and a warning message will be issued if any manual contact region overwrites the friction coefficients set by another manual contact region or by a Body Interaction object. See Figure 2.2: Treatment of Friction for Lumped Manual Contact (p. 28) for further explanation.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

27

Explicit Dynamics Workflow Figure 2.2: Treatment of Friction for Lumped Manual Contact

In this example consisting of two parts (the ball and the slide), three contact regions are defined. Contact Region 1 is frictionless, but Contact Region 2 and Contact Region 3 are frictional. As friction is only stored in Explicit Dynamics per pair of parts and not per contact region, all the contact events detected during the solve will be treated as frictional. This includes the contact events detected between the scoping in Contact Region 1 which was defined as frictionless. Frictional forces are computed as described in Frictional Type (p. 19).

2.6.3.2. Manual Contact Region Behavior for Trajectory Contact with Connected Surface Sliding and Manual Contact Treatment set to Pairwise The behavior described here is expected when the Contact Detection is set to Trajectory, the Sliding Contact is set to Connected Surface, and the Manual Contact Treatment is set to Pairwise. The scoping supported with these contact settings are: • The Target scoping must be either of type Face or type Body. • The Contact scoping may be of types Vertex, Edge, Face, or Body. The detected contact events respect the pairwise nature of the manual contact regions. Therefore if a node is in the scoping of the Contact of one manual contact region, and a face is in the scoping of the Target of a different manual contact region, but not in the first manual contact region, then the node will not find contact with the face. See Figure 2.3: Interaction of Pairwise Manual Contact Regions (p. 29) for further explanation.

28

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections Figure 2.3: Interaction of Pairwise Manual Contact Regions

Manual contact regions are defined A) between the lower face of Body 1 and the upper face of Body 3; B) between the lower face of Body 2 and the upper face of Body 3; C) between the rightmost face of Body 1 and the leftmost face of Body 2. In this scenario the Explicit solver will not search for contact events between the upper face of Body 3 and the rightmost face of Body 1 and the leftmost face of Body 2. Note that this is in contrast to the treatment described in Figure 2.1: Interaction of Lumped Manual Contact Regions (p. 27). The Symmetry Behavior option is respected, but the Trim Contact option of all contact regions is ignored. Friction coefficients are stored per contact region and per Body Interaction object in the solver. Therefore, the model described in Figure 2.4: Treatment of Friction for Pairwise Manual Contact (p. 29) will behave from a friction perspective as defined in the model setup. A solver setup error message is issued if conflicting friction coefficients are defined between any pair of nodes and faces in all of the scopings to manual contact regions and Body Interaction objects in the model. Figure 2.4: Treatment of Friction for Pairwise Manual Contact

In this example a frictional manual contact region is defined between the ball and slide. In addition, a Body Interaction is created which is scoped to all bodies and is frictionless. In this scenario the Explicit solver will issue a solver setup error because two different types of friction behavior have been defined between the surface of the ball and the surface of the slide.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

29

Explicit Dynamics Workflow Frictional forces are computed as described in Frictional Type (p. 19).

Note The Pairwise option for Manual Contact Treatment is not fully supported in the Autodyn user interface. If a model with the above settings is transferred to Autodyn, limited pre-processing will be available.

2.6.4. Joints in an Explicit Dynamics Analysis In an Explicit Dynamics analysis joint definitions between bodies can be taken into account by means of an abstraction. General information about joints is described here Joints. This section describes Joint information specific to an Explicit Dynamics analysis. A video demonstrating the capabilities of Joint modeling in an Explicit Dynamics system can be found here.

2.6.4.1. Joint Solver Models that are setup to run with the Explicit Dynamics solver often contain mechanisms that we refer to as joint systems. These systems consist of rigid bodies and remote points that are connected by joint definitions on rigid or flexible body geometry. There are two types of remote points, which will always behave rigidly in the Explicit Dynamics solver.

• Internal Remote Points: – Defined through a Remote Attachment. – These Internal Remote Points can be promoted to User-defined Remote Points.

30

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections

• User defined Remote Points: – The properties are defined by a Remote Point object in the tree. There is no difference in terms of Explicit solver behavior between Internal and User-defined Remote Points: they effectively create a group of rigid nodes which together act as a normal Rigid Body. If the group of nodes is already part of a Rigid Body, the definitions will be merged into one single rigid body while keeping the associated boundary conditions. Without employing any joint definition, a simple system can be modeled with a remote displacement, which is effectively a body-grounded joint with a number of free and fixed (or prescribed) displacements. These remote displacements are always grounded, and as such are limited in their usage. In practice it is possible to model joints by means of contact definition between parts. It must be noted that this will employ a penalty method and may not always simulate the desired behavior. Especially when prescribing rotations, the faceting of the contact surface can cause sticking between the two surfaces. By using joint definitions between different geometric parts, it is possible to alleviate these limitations since the solver will fulfill the kinematic constraints exactly by solving them implicitly during the timestep. For example, a dropping rotating shaft can be modelled with joints without the need of defining a contact between contact and target surface of the shaft. An Explicit model containing joints can be created by: • Setting the behavior of any geometry object to either Flexible or Rigid. • Connecting these geometry objects using Joint definitions, which will create (internal) Remote Points. The scoped surfaces of flexible bodies will behave rigidly and the scoped surfaces of rigid bodies will merge into the actual rigid body.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

31

Explicit Dynamics Workflow • The rest of the body will have flexible behavior and is as such suitable for a full Explicit investigation. • It should be noted that a pinball region on the Remote Scope can be used to limit the extent of the rigid surface that will be created on a flexible body. Multiple disconnected systems may be defined in a single model, where each system is solved separately, and the systems interact either through contact or through internal forces of the flexible elements. In practice it is valuable to create a fully rigid system in order to establish correct behaviour of the modeled mechanism. This can be done by: • Setting the behavior of all geometry to Rigid. • Connecting these rigid geometry objects using Joint definitions. • Defining a maximum timestep. Typically you need about 1000 to 10000 timesteps to solve the system with sufficient robustness. For example: – Endtime = 1.5 seconds – Maximum timestep ~ 1e-4 seconds In this case, the solution will effectively be a Rigid Body Dynamics solution.

2.6.4.2. Scoping to geometry • Joint mechanisms can be scoped to either flexible or rigid parts (see Stiffness Behavior). – If the parts are considered Rigid, the scope of the joint (reference and/or mobile) will merge with the Rigid Body that is created. – If the parts are considered Flexible, a Remote Point will be created for the scoped nodes. • Multiple joints scoped to the same geometry (essentially overlapping Remote Points) are allowed by the Explicit solver. The solver will merge the underlying nodes in the scope into a single rigid body. • In theory, the mesh of Rigid Bodies can be defined as dimensionally reduced. However it is important that the scope of the joints to these Rigid Bodies is passed on to the solver. This means the scope needs to be meshed with elements. This can be accomplished by defining contact surfaces on the scope. – Note that non interpenetrating meshes are needed to warrant frictionless behaviour. – If a part is not meshed at all the following error will be given:

This can be resolved by meshing a part of the geometry with elements.

32

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Connections

2.6.4.3. Initial Conditions You can apply initial conditions to rigid bodies that are involved in joint systems. Care should be taken that the condition satisfies the free motion of the system at the start; in other words, it is possible to apply an initial velocity in the direction of a fixed degree of freedom, but the solver will cancel out the initial motion at the start of the solution.

2.6.4.4. Boundary Conditions There are two considerations when applying boundary conditions in a model with rigid bodies joint systems. 1. In all joint systems (not limited to the Explicit Dynamics solver) it cannot be guaranteed that applied boundary conditions result in a converged solution. Consider a simple swing under gravity which solves correctly:

Alternatively, instead of inducing motion through gravity, the horizontal bar can be given a velocity boundary condition. This is done by defining a planar body-grounded joint on the horizontal bar and defining a velocity joint load in the local X-direction.

The boundary condition can be satisfied up to the point that the horizontal bar reaches the far left motion of the swing.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

33

Explicit Dynamics Workflow

After that point the solution will not be correct anymore, even though a solution will be provided.

Caution Be aware that the explicit dynamics solver will not issue a warning when boundary conditions are not satisfied.

2. There is another important consideration for Explicit Dynamics systems. When joints are used in the model, you should use joint loads for all the necessary kinematic boundary conditions. Take care evaluating results when using the following boundary conditions on rigid bodies when a model has joint systems defined: • Fixed support • Displacement

34

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting Up Symmetry • Remote Displacement • Velocity The above boundary conditions can always be applied by means of a Joint Load as well. It may be necessary to define an additional (body-grounded) joint with sufficient free degrees of freedom in order to setup the model correctly.

2.6.4.5. Using Contact with Joints The contact algorithm in the Explicit Dynamics solver is active by default. Therefore, contact forces will be computed during the timestep, including on the scoped geometry of a joint definition. When geometries are not smoothly meshed (and interpenetrate) these joints may exhibit unexpected behavior due to additional contact forces in the direction of the free DOF. Typically it is good practice to model the joints with sufficient offset between the surfaces to be scoped.

2.6.4.6. Postprocessing • All Joint probe variables are available after the simulation has been run. • Values for acceleration ((angular/translational) will be zero at cycle 0 due to the nature of the solution algorithm.

2.7. Setting Up Symmetry For general information about setting up symmetry see Defining Symmetry in the Mechanical User's Guide.

2.7.1. Explicit Dynamics Symmetry Symmetry regions can be defined in Explicit Dynamics analyses. Symmetry objects should be scoped to faces of flexible bodies defined in the model. All nodes lying on the plane defined by the selected face are constrained to give a symmetrical response of the structure.

Note • Anti-symmetry, periodicity, and anti-periodicity symmetry regions are not supported in Explicit Dynamics systems. • Symmetry cannot be applied to rigid bodies. • Only the General Symmetry interpretation is used by the solver in 2D Explicit Dynamics analyses.

Symmetry conditions can be interpreted by the solver in two ways: 2.7.1.1. General Symmetry 2.7.1.2. Global Symmetry Planes

2.7.1.1. General Symmetry In general, a symmetry condition will result in degree of freedom constraints being applied to the nodes on the symmetry plane. For volume elements, the translational degree of freedom normal to the sym-

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

35

Explicit Dynamics Workflow metry plane will be constrained. For shell and beam elements, the rotational degrees of freedom in the plane of symmetry will be additionally constrained. For nodes that have multiple symmetry regions assigned to them (for example, along the edge between two adjacent faces), the combined constraints associated with the two symmetry planes will be enforced.

Note • Symmetry regions defined with different local coordinate systems may not be combined, unless they are orthogonal with the global coordinate system. • General symmetry does not constrain eroded nodes. Thus, if after a group of elements erodes, a "free" eroded node remains, the eroded node will not be constrained by the symmetry condition. This can be resolved in certain situations via the special case of Global symmetry, described in the next section.

2.7.1.2. Global Symmetry Planes If a symmetry object is aligned with the Cartesian planes at x=0, y=0 or z=0, and all nodes in the model are on the positive side of x=0, y=0, or z=0, the symmetry condition is interpreted as a special case termed Global symmetry plane. In addition to general symmetry constraints: • If a symmetry plane is coincident with the YZ plane of the global coordinate system (X=0), and no parts of the geometry lie on the negative side of the plane, then a symmetry plane is activated at X=0. This will prevent any nodes (including eroded nodes) from moving through the plane X=0 during the analysis. • If a symmetry plane is coincident with the ZX plane of the global coordinate system (Y=0), and no parts of the geometry lie on the negative side of the plane, then a symmetry plane is activated at Y=0. This will prevent any nodes (including eroded nodes) from moving through the plane Y=0 during the analysis. • If a symmetry plane is coincident with the XY plane of the global coordinate system (Z=0), and no parts of the geometry lie on the negative side of the plane, then a symmetry plane is activated at Z=0. This will prevent any nodes (including eroded nodes) from moving through the plane Z=0 during the analysis.

Note Global symmetry planes are only applicable to 3D Explicit Dynamics analyses.

2.7.2. Symmetry in an Euler Domain There are additional considerations if an Euler Domain is defined for an analysis. For symmetry to be applied to an Euler Domain, symmetry will have to be defined with the global coordinate system, not a local one, and it will need to be applied on geometry faces which lie on the global coordinate system planes. • If the symmetry is not defined with the global coordinate system, it is ignored and a warning is shown in the messages window saying that such symmetry will be ignored but the analysis continues to solve. • If the symmetry is not applied on faces which lie on the global coordinate system planes then an error is shown and the solution is terminated.

36

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Remote Points In the case where symmetry is valid for use with Euler Domains, if the boundary of the Euler Domain which is parallel to the symmetry plane is below the symmetry plane, then that boundary will be moved to lie on the symmetry plane if the following conditions are true: • The Euler Domain Size Definition option in the Analysis settings is set to Program Controlled. • The Euler body is on the positive side of the global coordinate axis.

2.8. Define Remote Points The algorithm in the Explicit Dynamics solver is different from the Implicit solver in the way it handles rigid bodies. For general information about how to use remote points, see Specifying Remote Points and Remote Boundary Conditions in the Mechanical User's Guide. The following topics describe the use of remote points and boundary conditions for the explicit solvers: 2.8.1. Explicit Dynamics Remote Points 2.8.2. Explicit Dynamics Remote Boundary Conditions 2.8.3. Initial Conditions on Remote Points 2.8.4. Constraints and Remote Points

2.8.1. Explicit Dynamics Remote Points A remote point in Explicit Dynamics consists of a: • Location - The point in space from which a remote boundary condition can be applied. • Scoped region - The area of geometry the remote point is scoped to. The nodes of this scoping form a group of rigid body nodes along with a further node created at the remote point location. • Boundary condition (optional) - The Remote Displacement and Remote Force boundary conditions are currently available as remote boundary conditions. The Explicit Dynamics solver does not support Deformable Behavior when using remote points. The group of rigid body nodes which is created is treated as a regular rigid body by the Explicit Dynamics solver. For example, if the scoped region of the remote point consists of two faces from two separate parts, the solver will determine the center of mass and the inertial properties for all the nodes, with all the nodes making up a combined group of rigid body nodes. This calculation creates a rigid connection between the two parts. In the solution, the forces acting on the group of rigid body nodes are summed at each time step. This calculation determines the rigid body motion of the nodes belonging to the remote point. Due to the mandatory rigid behavior of Remote Points, the group of rigid body nodes are unable to deform, even if the elements of the parts used have flexible behavior. The group of rigid body nodes are, however, free to translate and rotate. Due to this restriction it is important to maintain a sufficient number of nodes in the scoped area of a remote point when scoped to a flexible solid part.

Note When using Remote Points in Explicit Dynamics analyses: • The Behavior field must be set to Rigid. If it is set to Deformable the solution will terminate and an error will be generated.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

37

Explicit Dynamics Workflow • Only the remote displacement and remote force boundary conditions are supported for Remote Points in Explicit Dynamics analyses. • Commands are not supported for Remote Points in Explicit Dynamics analyses. • Remote Points and boundary conditions are not supported for 2D Explicit Dynamics analyses.

2.8.2. Explicit Dynamics Remote Boundary Conditions The remote boundary conditions available in the Explicit Dynamics solver are Remote Displacement and Remote Force. The Explicit Dynamics solver treats a Remote Displacement as follows: • The geometry that the Remote Displacement boundary condition is scoped to becomes a group of rigid body nodes, determining its mass and inertial properties, and preventing these nodes from deforming. If this group of rigid body nodes spans multiple parts, then these parts will be rigidly connected. • Displacements and/or rotations at the remote point and the group of rigid body nodes are tracked and converted into velocities and angular velocities for use by the solver. • The actual translation and rotation of the remote point are a combination of the imposed boundary constraints of the Remote Displacement definition and the forces acting on the group of nodes scoped to the Remote Point. Therefore, the translation and rotation of the Remote Point and the group of rigid body nodes are determined simultaneously and enforced with the use of a single corrective force and moment. The Explicit Dynamics solver treats a Remote Force as follows: • The geometry that the Remote Force boundary condition is scoped to becomes a group of rigid body nodes, determining its mass and inertial properties, and preventing these nodes from deforming. If this group of rigid body nodes spans multiple parts, then these parts will be rigidly connected. • The force specified is applied to the node representing the remote point, which is rigidly attached to the group of rigid body nodes. • The force is applied to the scoped group of nodes specified by the remote point. • The motion of the remote point is determined by a combination of the loads applied to the remote point, the mass and inertial properties of the group of rigid body nodes, and the properties of the parts the group of rigid body nodes are attached to.

Note Remote Force is not supported for Workbench LS-DYNA.

2.8.3. Initial Conditions on Remote Points Initial conditions are scoped to geometric parts in the model. Effectively this means that the initial condition is scoped to a set of elements. However, remote points are scoped to the underlying nodes in the model. This may result in different initial conditions on the same node in a remote point definition. This section describes the behavior in such instances.

38

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Define Remote Points Initial condition on a flexible part: Initial conditions can be scoped to a subset of or all elements in a flexible part. It is not necessary to scope an initial condition to all the nodes in the remote point definition, as long as there is only one initial condition defined for the nodes that participate in the remote point definition. Initial condition on a rigid body part: The remote point definition will automatically include all the nodes in a rigid part. Therefore the initial condition (or multiple identical initial conditions) should be scoped to all the elements in the rigid part. The scoped nodes of the remote point will follow the initial condition of the scoped rigid body. If the flexible scoped nodes of the remote point contain their own initial condition, this will be ignored.

2.8.4. Constraints and Remote Points When applying constraints to a model that includes remote points, it is important to ensure that the model is not over-constrained. Since the Explicit Dynamics solver treats the remote point and its scoped region as a single rigid body, the model could be over-constrained in the following two examples: • Two remote points share common nodes in their scoped regions. This is an over-constraint because each remote point generates its own rigid body and rigid bodies cannot share nodes.

Example of an overconstrained model caused by two remote points scoped to adjacent faces. • A velocity boundary condition applied to some or all of the nodes in a remote point scoping, and a remote displacement applied to the remote point.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

39

Explicit Dynamics Workflow Example of an overconstrained model caused by a constraining boundary condition such as a fixed support applied to a face which is adjacent to a remote point scoping with a remote displacement applied. This list of examples is not exhaustive and a setup error will be issued to the user on solve if any such over-constraints occur.

2.9. Apply Mesh Controls/Preview Mesh For general information about how to apply mesh controls and preview the mesh, see Apply Mesh Controls and Preview Mesh in the Mechanical User's Guide All mesh methods available in the Workbench meshing application can be utilized in Explicit Dynamics systems. • Swept Volume Meshing • Patch Dependant Volume Meshing • Hex Dominant Meshing • Patch Independent Tetrahedral Meshing • Multizone Volume Meshing • Patch dependant shell meshing • Patch independent shell meshing A smooth uniform mesh should be sought in the regions of interest for the analysis. Elsewhere, coarsening of the mesh may help to reduce the overall size of the problem to be solved. Use the Explicit meshing preference (set by default) to auto-assign the default mesh controls that will provide a mesh well suited for Explicit Dynamics analyses. This preference automatically sets the Rigid Body Behavior mesh control to Full Mesh. The Full Mesh setting is only applicable to Explicit Dynamics analyses. Other physics preferences can be used if better consistency is desired between implicit and explicit models. Consideration should be given to the number of elements in the model and the quality of the mesh to produce larger resulting time steps and therefore more efficient simulations. A coarse mesh can often be used to gain insight into the basic dynamics of a system while a finer mesh is required to investigate nonlinear material effects and failure. The Mesh Metric option allows you to view mesh metric information and thereby evaluate the mesh quality. A very useful mesh metric is the Characteristic Length: it is primarily used to determine the timestep for an element. Swept/multi-zone meshes are preferred in Explicit Dynamics analyses so geometry slicing, combined with multibody part options in DesignModeler, are recommended to facilitate hexahedral meshing. Alternatively, use the patch independent tetrahedral meshing method to obtain more uniform element sizing and take advantage of automatic defeaturing. Define the element size manually to produce more uniform element size distributions especially on surface bodies. Midside nodes should be dropped from the mesh (set Element Order to Linear) for all elements types (solids, surface and line bodies). Error/warning messages are provided if unsupported (higher order) elements are present in the mesh. 40

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Establish Analysis Settings Pyramid elements are not supported in Explicit Dynamics analyses. Any elements of this type are converted into two tetrahedral elements, and will warrant a warning in the message window of the Mechanical application. An Explicit Dynamics model with fewer elements than the number of slave processes specified cannot be run in parallel. For Workbench LS-DYNA, only the element types listed below are supported (partly due to LS-DYNA limitations). Any parts with a mesh containing unsupported elements will be excluded from the exported mesh. A warning is displayed specifying excluded parts. • Shells – 1st Order: triangles, quadrilaterals – 2nd Order: none • Solids – 1st Order: tetrahedrons, pyramids, wedges, hexahedrons, beams – 2nd Order: tetrahedrons • LS-DYNA supports Thick Shell elements. Please refer here in the meshing documentation for information on how to create these elements.

Note Pyramids are not recommended for LS-DYNA. A warning is issued if such elements are present in the mesh. When performing an implicit static structural or transient structural analysis to an Explicit Dynamics analysis, the same mesh is required for both the implicit and explicit analysis and only low order elements are allowed. If high order elements are used, the solve will be blocked and an error message will be issued.

2.10. Establish Analysis Settings For general information about how to establish analysis settings, see Establish Analysis Settings in the Mechanical User's Guide. The basic analysis settings for Explicit Dynamics analyses (p. 45) are: • Step Controls - The required input for step control is the termination time for the analysis. This should be set to your best estimate of the solution time required to simulate the event being modeled. You should normally allow the solver to determine its own time step size based on the smallest CFL condition (p. 132) in the model. The efficiency of the solution can be increased with the help of mass scaling options. Use this feature with caution; too much mass scaling can give rise to non-physical results. An Explicit Dynamics solution may be started, interrupted and resumed at any point in time. For example, an existing solution that has reached its End Time may be extended to continue to review the progression of the mechanical phenomena simulated. The Resume From Cycle option enables you to select which Restart file you would like to use to resume the analysis. See Resume Capability for Explicit Dynamics Analyses (p. 78) for more information. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

41

Explicit Dynamics Workflow Step Control options: – Number of Steps (option not available in Workbench LS-DYNA) – Current Step Number (option not available in Workbench LS-DYNA) – Resume from cycle (option not available in Workbench LS-DYNA) – Maximum Number of Cycles – Reference energy cycle (option not available in Workbench LS-DYNA) – The Maximum Element Scaling and Update frequency (options not available in Workbench LSDYNA) • Solver Controls – These advanced controls allow you to control a range of solver features including element formulations and solution velocity limits. The defaults are applicable to wide range of applications. – Shell thickness update, shell inertia update, density update, minimum velocity, maximum velocity and radius cutoff options can only be set in the Explicit Dynamics system. – A selectable Unit System is available only in Workbench LS-DYNA. • Euler Domain Controls – There are three sets of parameters that are necessary to define the Euler Domain: the size of the whole domain (Domain Size Definition), the number of computational cells in the domain (Domain Resolution Definition), and the type of boundary conditions to be applied to the edges of the domain.

Note Euler capabilities are not supported for Workbench LS-DYNA. The domain size can be defined automatically (Domain Size Definition = Program Controlled) or manually (Domain Size Definition = Manual). For both the automatic and manual options, the size is defined from a 3D origin point and the X, Y, and Z dimensions of the domain. For the automatic option, specify the Scope of the Domain Size Definition so that the origin and X, Y, and Z dimensions are set to create a box large enough to include all bodies in the geometry (Scope = All Bodies) or the Eulerian Bodies only (Scope = Eulerian Bodies Only). The automatically determined domain size can be controlled with three scaling parameters, one for each direction (X Scale Factor, Y Scale Factor, Z Scale Factor). The size of the domain is affected by the scale factors according to the following equations: (2.5) (2.6) (2.7) where lx, ly, lz are the lengths of the unscaled domain in the x, y, and z directions respectively. These parameters are obtained automatically from the mesh. l'x, l'y, l'z are the lengths of the scaled domain in the x, y, and z directions respectively. 42

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Establish Analysis Settings Fx, Fy, Fz are the scale factors for the x, y, and z directions respectively. For the Manual option of the Domain Size Definition, specify the origin of the Euler Domain (Minimum X Coordinate, Minimum Y Coordinate, Minimum Z Coordinate) and the dimension in each direction (X Dimension, Y Dimension, Z Dimension). The domain resolution specifies how many cells should be created in the X, Y, and Z directions of the domain. Use the Domain Resolution Definition field to specify how to determine the resolution: either the cell size (Cell Size), the number of cells in each of the X, Y, and Z directions (Cells per Component), or the total number of cells to be created (Total Cells). – For the Cell Size option, specify the size of the cell in the Cell Size parameter. The value specified is the dimension of the cell in each of the X, Y, and Z directions. The units used for the cell size follow the ones specified in the Mechanical application window and are displayed in the text box. The number of the cells in each direction of the domain are then determined from this cell size and the size of the domain with the following equations: (2.8) (2.9) (2.10) where Nx, Ny, Nz are the number of cells in the X, Y, and Z directions respectively. D is the dimension of the cell in each direction (this is the same in all directions). – For the Cells per Component option, enter the number of cells required in each of the X, Y, and Z directions (Number of Cells in X, Number of Cells in Y, Number of Cells in Z). – For the Total Cells option, specify Total Cells (the default is 250,000). The size of the cells will depend on the size of the Euler Domain. The size of the cell is calculated from the following equation: (2.11) where Ntot is the total number of cells in the domain. If any bodies are defined as Eulerian (Virtual), when Analysis Settings is selected in the outline view, the Euler domain bounding box is displayed in the graphics window. The Euler domain resolution is indicated by black node markers along each edge line of the Euler domain. The visibility of this can be controlled by the Display Euler Domain option in the Analysis Settings. You can set boundary conditions on each of the faces of the Euler Domain. The faces are labeled Lower X Face, Lower Y Face, Lower Z Face (which correspond to the faces with the minimum X, Y, and Z coordinates) and Upper X Face, Upper Y Face, and Upper Z Face (which correspond to the

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

43

Explicit Dynamics Workflow faces with the maximum X, Y, and Z coordinates). The values of the boundary conditions that can be set for each face are: – Flow Out Use the Flow Out boundary condition to flow out material through cell faces. The boundary condition makes the material state of the dummy cell outside the Euler domain the same as that of the cell adjacent to the Flow Out boundary, thus setting the gradients of velocity and stress to zero over the boundary. This approach simulates a far field solution at the boundary, but is only exact for outflow velocities higher than the speed of sound and is an approximation for lower velocities. Therefore, the Flow Out boundary condition is approximate in many cases, and should be placed as far as possible from region of interest and best at a location where the gradients are small. – Impedance The Impedance boundary condition acts exactly the same as the Flow Out boundary condition and provides the same results. – Rigid Use the Rigid boundary condition to prevent flow of material through cell faces. The cell faces are closed for material transport and act as rigid non-slip walls. The Rigid boundary condition takes the material state of the dummy cell outside the Euler domain as a mirrored image of the cell adjacent to the Wall boundary, thus setting the normal material velocity at the rigid wall to zero and leaving the tangential velocity unaffected. Euler Tracking is currently only By Body, which scopes the results to Eulerian bodies in the same manner as Lagrangian bodies. • Damping Controls – Damping is used to control oscillations behind shock waves and reduce hourglass modes in reduced integration elements. These options allow you to adapt the levels of damping, and formulation used for the analysis being conducted. Elastic oscillations in the solution can also be automatically damped to provide a quasi-static solution after a dynamic event. For Hourglass Damping, only one of either the Viscous Coefficient or Stiffness Coefficient, is used for the Flanagan Belytschko option - when running an Explicit Dynamics analysis using the LS-DYNA solver, LS-DYNA does not allow for two coefficients to be entered in *CONTROL_HOURGLASS. Thus the non-zero coefficient determines the damping format to be either "Flanagan-Belytschko viscous" or "Flanagan-Belytschko stiffness", accordingly. If both are non-zero, the Stiffness Coefficient will be used.

Note Linear Viscosity in Expansion options are not supported for Workbench LS-DYNA. Hourglass damping in LS-DYNA is standard by default; in the Explicit Dynamics System the same control is Autodyn Standard.

• Erosion Controls – Erosion is used to automatically remove highly distorted elements from an analysis and is required for applications such as cutting and impact penetration. In an Explicit Dynamics analysis, erosion is a numerical tool to help maintain large time steps, and thus obtain solutions in appropriate time scales. Several options are available to initiate erosion. The default settings will erode elements which experience 44

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Establish Analysis Settings geometric strains in excess of 150%. The default value should be increased when modeling hyperelastic materials. Geometric strain limit and material failure criteria are not present in LS-DYNA. • Output Controls – Solution output is provided in several ways: – Results files which are used to provide nodal and element data for contour and probe results such as deformation, velocity, stress and strain. Note that probe results will provide a filtered time history of the result data due to the relatively infrequent saving of results files. – Restart files should be stored less frequently than results files and can be used to resume an analysis. – Tracker data is usually stored much more frequently than results or restart data and thus is used to produce full transient data for specific quantities. – Output controls to save result tracker and solution output are not available for LS-DYNA. – When performing an implicit to explicit analysis, for a nonlinear implicit analysis, the Strain Details view property must be set to Yes because plastic strains are needed for the correct results.

2.10.1. Analysis Settings for Explicit Dynamics Analyses The following sections describe the available properties for the Analysis Settings folder in an Explicit Dynamics analysis. In addition to describing each setting, it is noted whether the setting is available for 2D analyses, and whether it is available on restart (applies to 2D and 3D analyses).

Note Explicit Dynamics settings are not step aware except for the Static Damping Coefficient and Output Controls. No Workbench LS-DYNA settings are step aware. 2.10.1.1. Explicit Dynamics Step Controls 2.10.1.2. Explicit Dynamics Solver Controls 2.10.1.3. Explicit Dynamics Euler Domain Controls 2.10.1.4. Explicit Dynamics Damping Controls 2.10.1.5. Explicit Dynamics Erosion Controls 2.10.1.6. Explicit Dynamics Output Controls 2.10.1.7. Explicit Dynamics Data Management Settings 2.10.1.8. Recommendations for Analysis Settings in Explicit Dynamics

2.10.1.1. Explicit Dynamics Step Controls Field

Options

Description

Number of Steps

See Defining Multiple Analysis Steps and Activation/Deactivation of Loads in Explicit Dynamics (p. 75) for more information.

Current Step Number

Shows the step ID for the current load step End Time. The currently selected step is also highlighted in the bar at the bottom of the Graphics window. Note that Explicit analysis settings are not step aware except for the Static Damping Coefficient.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

2D

Restart

45

Explicit Dynamics Workflow Field

Options

Description

2D

Restart

End Time

(Required input) The maximum length of Yes time (starting from time zero) to be simulated by the explicit analysis. You should enter a reasonable estimate to cover the phenomena of interest.

Yes

Resume From Cycle

Allows you to select the integration cycle from which to start the solution upon selecting Solve. A cycle of zero (default setting) indicates the solution will clear any previous progress and start from time zero. A non-zero cycle, on the other hand, allows you to revisit a previous solution and extend it further in time. A solution obtained from a non-zero cycle is considered to have been "resumed" or "restarted".

Yes

Yes

Maximum Number of Cycles

The maximum number of cycles allowed Yes during the analysis. The analysis will stop once the specified value is reached. Enter a large number to have the analysis run to the defined End Time.

Yes

Maximum Energy Error

Energy conservation is a measure of the Yes quality of an Explicit Dynamics analysis. Large deviations from energy conservation usually imply a less than optimal model definition. This parameter allows you to automatically stop the solution if the deviation from energy conservation becomes unacceptable. Enter a fraction of the total

Yes

Note that the list will only contain non-zero selections if a solve was previously executed and restart files have been generated. When resuming an analysis, changes to analysis settings will be respected where possible. For example, you may wish to resume an analysis with an extended termination time. Changes to any other features in the model (geometry suppression, connections, loads, and so on) will prevent restarts from taking place. See Resume Capability for Explicit Dynamics Analyses (p. 78) for more information. This field is not available for Workbench LS-DYNA.

46

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Establish Analysis Settings Field

Options

Description

2D

Restart

system energy (measured at the Reference Energy Cycle) for which you want the analysis to stop. For example, the default value of 0.1 will cause the analysis to stop if the energy error exceeds 10% of the energy at the reference cycle. For Workbench LS-DYNA this field requires a percentage to be entered. Thus the field name changes to Maximum Energy Error (%). Reference Energy Cycle

The cycle at which you want the solver to Yes calculate the reference energy, against which it will calculate the energy error. Usually this will be the start cycle (cycle = 0). You may need to increase this value if the model has zero energy at cycle = 0 (for example if you have no initial velocity defined).

Yes

This field is not available for Workbench LS-DYNA. Initial Time Step

Enter an initial time step you want to use, Yes or use the Program Controlled default. If left on Program Controlled, the time step will be automatically set to ½ the computed element stability time step. The Program Controlled setting is recommended.

Yes

This field is not available for Workbench LS-DYNA. Minimum Time Step

Enter the minimum time step allowed in the Yes analysis, or use the Program Controlled default. If the time step drops below this value the analysis will stop. If set to Program Controlled, the value will be chosen as 1/10th the initial time step.

Yes

This field is not available for Workbench LS-DYNA. Maximum Time Step

Enter the maximum time step allowed in the Yes analysis, or use the Program Controlled default. The solver will use the minimum of this value or the computed stability time step during the solve. The Program Controlled setting is recommended.

Yes

Time Step Safety Factor

A safety factor limit is applied to the computed stability time step to help keep the solution stable. The default value of 0.9 should work for most analyses.

Yes

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Yes

47

Explicit Dynamics Workflow Field

Options

Description

2D

Restart

Characteristic Dimension

Diagonals (default setting)

The characteristic dimension (p. 132) used to determine the time-step for hex elements will be calculated as the volume of the element divided by the square of the longest element diagonal and then scaled by sqrt(2/3).

Yes

No

This field is not available for Workbench LS-DYNA. Opposing Face

The characteristic dimension used to determine the time-step for hex elements will be based on the minimum distance between opposing faces. Select this option to obtain the optimal time step for hex solid elements. Experience to date has shown that this option can significantly improve the efficiency of 3D Lagrange simulations. However, in certain circumstances when cells become highly distorted, instabilities have been observed causing the calculation to terminate with high energy errors. The correct choice of erosion strain can reduce these problems. It is therefore recommended that users only utilize this option if efficiency is critical. This field is not available for Workbench LS-DYNA.

Nearest Face

The characteristic dimension used to determine the time-step for hex elements will be based on the minimum distance between neighboring faces. Experience to date has shown that this option can significantly improve the efficiency of 3D Lagrange simulations. However, in certain circumstances when cells become highly distorted, instabilities have been observed causing the calculation to terminate with high energy errors. The correct choice of erosion strain can reduce these problems. It is therefore recommended that users only utilize this option if efficiency is critical. This field is not available for Workbench LS-DYNA.

48

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Establish Analysis Settings Field

Options

Automatic Mass Scaling Minimum CFL Time Step

Description

2D

Restart

If set to Yes, activates automatic mass scaling and exposes the following options.

Yes

Yes

The time step that you want to achieve in the analysis.

Yes

Yes

Yes

Yes

Yes

Yes

Allows you to control the frequency at which Yes the mass scaling will be calculated during the solve. The frequency equates to the increment in cycles at which the mass scale factor will be recomputed, based on the current shape of the elements. The default of 0 is recommended and means that the mass scale factor is only calculated once, at the start of the solve.

Yes

Caution Mass scaling introduces additional mass into the system to increase the computed CFL time step (p. 132). Introducing too much mass can lead to non-physical results.

Note Employ User Defined Results MASS_SCALE (ratio of scaled mass/physical mass) and TIMESTEP to review the effects of automatic mass scaling on the model. Maximum Element Scaling

This value limits the ratio of scaled mass/physical mass that can be applied to each element in the model. This field is not available for Workbench LS-DYNA.

Maximum Part Scaling

This value limits the ratio of scaled mass/physical mass that can be applied to an individual body. If this value is exceeded, the analysis will stop and an error message is displayed. This field is not available for Workbench LS-DYNA.

Update Frequency

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

49

Explicit Dynamics Workflow Field

Options

Description

2D

Restart

Description

2D

Restart

All model inputs will be converted to this set of units during the solve. Results from the analysis will be converted back to the user units system in the GUI. For Explicit Dynamics systems, this setting is always mm, mg, ms.

Yes

No

Bending

Any line bodies will be represented as beam No elements including a full bending moment calculation.

No

Truss

Any line bodies will be represented as truss elements. No bending moments are calculated.

Post cycle 0 adjustment will only take place for solid elements (excluding ANP and NBS tetrahedra). In parallel solutions the update frequency is always set to 0. This field is not available for Workbench LS-DYNA.

2.10.1.2. Explicit Dynamics Solver Controls Field

Options

Solve Units

For Workbench LS-DYNA this field is termed Unit System and six systems are available for selection: nmm; μmks; Bft; Bin; mks; cgs. Beam Solution Type

Beam Time Step Safety Factor

An additional safety factor you may apply No to the stability time step calculated for beam elements. The default value ensures stability for most cases.

No

Exact

Provides an accurate calculation of element volume, even for warped elements.

No

No

1pt Gauss

Approximates the volume calculation and is less accurate for elements featuring warped faces. This option is more efficient.

Shell Sublayers

The number of integration points through No the thickness of an isotropic shell. The default of 3 is suitable for many applications; however, this number can be increased to achieve better resolution of through thickness plastic deformation and/or flow.

No

Shell Shear Correction Factor

The transverse shear in the element No formulation is assumed constant over the thickness. This correction factor accounts for

No

Hex Integration Type

50

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Establish Analysis Settings Field

Options

Description

2D

Restart

the replacement of the true parabolic variation through the thickness in response to a uniform transverse shear stress. Using a value other than the default is not recommended. Shell BWC Warp Correction

Shell Thickness Update

Nodal

The Belytschko-Lin-Tsay element formulation No becomes inaccurate if the elements are warped. To overcome this, the element formulation has an optional correction to include warping. Setting this correction to Yes is recommended.

No

Changes in shell thickness are calculated at the nodes of shell elements.

No

No

The tetrahedral element formulation includes No an average nodal pressure integration. This formulation does not exhibit volumetric locking, and can be used for large deformation, and nearly incompressible behavior such as plastic flow or hyperelasticity. This formulation is recommended for the majority of tetrahedral meshes.

No

This field is not available for Workbench LS-DYNA. Elemental

Changes in shell thickness are calculated at the element integration points. This field is not available for Workbench LS-DYNA.

Tet Integration

Average Nodal Pressure

Constant Pressure Uses the constant pressure integrated tetrahedral formulation. This formulation is more efficient than Average Nodal, however it suffers from volumetric locking under constant bulk deformation. Nodal Strain

When Tet Integration is set to Nodal Strain the Puso Stability Coefficient, field is shown. For NBS models exhibiting zero energy modes, the Puso coefficient can be set to a non-zero value. A value of 0.1 is recommended. See Solver Controls (p. 150) for more information.

Shell Inertia Update

Recompute

The principal axes of rotary inertia are by default recalculated each cycle.

No

No

This field is not available for Workbench LS-DYNA Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

51

Explicit Dynamics Workflow Field

Options

Description

2D

Restart

Rotate

Rotates the axes, rather than recomputing each cycle. This option is more efficient; however, it can lead to numerical instabilities due to floating point round-off for long running simulations.

Yes

No

Yes

Yes

Yes

Yes

At the start of your calculation, if a node is Yes within the specified radius of a symmetry plane, it will be placed on the symmetry plane. If a node is outside the specified radius from a symmetry plane at the start of your calculation, it will not be allowed to come closer than this radius to the symmetry plane as your calculation proceeds.

Yes

This field is not available for Workbench LS-DYNA. Density Update

Program Controlled

The solver decides whether an incremental update is necessary based on the rate and extent of element deformation. This field is not available for Workbench LS-DYNA.

Incremental

Forces the solver to always use the incremental update. This field is not available for Workbench LS-DYNA.

Total

Forces the solver to always recalculate the density from element-volume and mass. This field is not available for Workbench LS-DYNA.

Minimum Velocity

The minimum velocity you want to allow in the analysis. If any model velocity drops below this Minimum Velocity, it will be set to zero. The default is recommended for most analyses. This field is not available for Workbench LS-DYNA.

Maximum Velocity

The maximum velocity you want to allow in the analysis. If any model velocity rises above the Maximum Velocity, it will be capped. This can improve the stability/robustness of the analysis in some instances. The default is recommended for most analyses. This field is not available for Workbench LS-DYNA.

Radius Cutoff

52

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Establish Analysis Settings Field

Options

Description

2D

Restart

This field is not available for Workbench LS-DYNA. Minimum Strain Rate Cutoff

The minimum strain rate you want to allow Yes in the analysis. If any model strain rate drops below this value, it will be set to zero. The default is recommended for most analyses. For low speed or quasi-static analyses, it may be necessary to decrease this value.

Yes

This field is not available for Workbench LS-DYNA.

2.10.1.3. Explicit Dynamics Euler Domain Controls Field

Options

Description

2D

Restart

Domain Size Definition

Program Controlled

Set Domain Size Definition to automatic.

No

No

Manual

Set Domain Size Definition to manual. Toggles visibility of the annotation of the Euler domain in the graphics window.

No

No

All Bodies

Euler domain is sized to include all bodies.

No

No

Eulerian Bodies Only

Euler domain is sized to include Euler bodies only.

Display Euler Domain Scope

X Scale factor, Y Scale factor, Z Scale Factor

User defined scaling factors for the automatically determined X, Y, and Z sizes .

No

No

Minimum X Coordinate, Minimum Y Coordinate, Minimum Z Coordinate

X, Y, Z coordinates for the Euler domain origin for the Manual option.

No

No

X Dimension, Y Dimension, Z Dimension

Euler domain X, Y, Z dimensions for the Manual option.

No

No

Total Cells

Set Domain Resolution Definition by specifying the total number of cells in the Euler domain.

No

No

Cell Size

Set Domain Resolution Definition by specifying the size of the cells in the Euler domain.

No

No

Domain Resolution Definition

Cells per Compon- Set Domain Resolution Definition by ent specifying the number of cells in each dimension in the Euler domain. Total Cells

Total number of cells that the Euler domain should contain if Domain Resolution Definition is Total Number of Cells.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

53

Explicit Dynamics Workflow Field

Options

Description

2D

Restart

Cell Size

Dimension of the cell in each of the X, Y, and No Z directions if Domain Resolution Definition is Cell Size.

No

Number of Cells in X, Number of Cells in Y, Number of Cells in Z

Number of cells required in the X, Y, and Z directions if Domain Resolution Definition is Number of Cells by Component.

No

No

No

No

No

No

Lower X Face, Lower Y Face, Lower Z Face, Upper X Face, Upper Y Face, Upper Z Face

Flow Out (Default setting)

Specify the boundary condition of the selected Euler domain face to be Flow Out.

Impedance

Specify the boundary condition of the selected Euler domain face to be Impedance.

Rigid

Specify the boundary condition of the selected Euler domain face to be Rigid.

Euler Tracking

By Body

Results may be scoped to Eulerian bodies in the same way as for Lagrangian bodies.

If any bodies are defined as Eulerian (Virtual), when Analysis Settings is selected in the outline view the Euler domain bounding box is displayed in the graphics window, as shown below.

The Euler domain resolution is indicated by black node markers along each edge line of the Euler domain. The visibility of this can be controlled by the Display Euler Domain option in the Analysis Settings.

2.10.1.4. Explicit Dynamics Damping Controls Field

Options

Description

2D

Restart

Linear Artificial Viscosity

A linear coefficient of artificial viscosity. This Yes coefficient smooths out shock discontinuities over the mesh. Using a value other than the default is not recommended.

Yes

Quadratic Artificial Viscosity

A quadratic coefficient of artificial viscosity. Yes This coefficient damps out post shock discontinuity oscillations. Using a value other than the default is not recommended.

Yes

54

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Establish Analysis Settings Field

Options

Linear Viscosity in Expansion

Description

2D

Artificial viscosity is normally applied to Yes materials in compression only. This option allows you to apply the viscosity for materials in compression and expansion.

Restart Yes

This field is not available for Workbench LS-DYNA. Artificial Viscosity for Shells

Apply artificial viscosity to all shell elements in addition to solid elements.

No

Yes

The method of hourglass damping to be used with solid hexahedral elements. The AUTODYN Standard option is available For 2D analyses only.

Yes

Yes

Stiffness Coefficient

The Stiffness Coefficient for Flanagan Belytschko hourglass damping in solid hexahedral elements.

No

Yes

Viscous Coefficient

The viscous coefficient for hourglass damping used in hexahedral solid elements and quadrilateral shell elements.

Yes

Yes

Static Damping

A static damping constant may be specified which changes the solution from a dynamic solution to a relaxation iteration converging to a state of stress equilibrium. For optimal convergence, the value chosen for the damping constant, R, may be defined by: R = 2*timestep/T where timestep is the expected average value of the timestep and T is longest period of vibration for the system being analyzed. The Static Damping is step aware. This allows the solution to be damped during a step in the solution.

Yes

Yes

Description

2D

Restart

If set to Yes, elements will automatically erode if the geometric strain in the element exceeds the specified limit.

Yes

Yes

This field is not available for Workbench LS-DYNA. Hourglass Damping

AUTODYN Standard Flanagan Belytschko

2.10.1.5. Explicit Dynamics Erosion Controls Field On Geometric Strain Limit

Options

This field is not available for Workbench LS-DYNA.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

55

Explicit Dynamics Workflow Field

Options

Geometric Strain Limit

Description

2D

Restart

The geometric strain limit for erosion. Recommended values are in the range from 0.75 to 3.0. The default value is 1.5.

Yes

Yes

If set to Yes, elements will automatically Yes erode if a material failure property is defined in the material used in the elements, and the failure criteria has been reached. Elements with materials including a damage model will also erode if damage reaches a value of 1.0.

Yes

This field is not available for Workbench LS-DYNA. On Material Failure

This field is not available for Workbench LS-DYNA. On Minimum Element Time Step

If set to Yes, elements will automatically Yes erode if their calculated time step falls below the specified value.

Yes

Minimum Element Time Step

The minimum controlling time step (p. 112) that an element can have. If the element time step drops below the specified value, the element will be eroded.

Yes

Yes

Retain Inertia of Eroded Material

If all elements that are connected to a node in the mesh erode, the inertia of the resulting free node can be retained if this option is set to Yes. The mass and momentum of the free node is retained and can be involved in subsequent impact events to transfer momentum in the system.

Yes

No

2D

Restart

If set to No, all free nodes will be automatically removed from the analysis.

2.10.1.6. Explicit Dynamics Output Controls Field Step-aware Output Controls

56

Options

Description Set to No by default. If set to Yes the frequency of Results, Restart, and Result Tracker data is made step-aware; that is the values represent the frequency per step and

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Establish Analysis Settings Field

Options

Description

2D

Restart

During the solve of an Explicit Dynamics system, results are saved to disk at a frequency defined through this control. The following settings are available.

Yes

Yes

Save results files after a specified increment in the number of cycles. Exposes a Cycles field where you enter the increment in cycles.

Yes

Yes

the Output Controls are displayed in the Worksheet.

Note When setting this to Yes, for an analysis with 3 steps in it and Save Results/Restart Files on set to Equally Spaced points, the frequency of Results/Restart Files would become 3 times the original value. Therefore, it is worth resetting these values per step if needed when turning on this feature. This field is not available for Workbench LS-DYNA. Save Results on

Cycles

This setting is not available for Workbench LS-DYNA. Time

Save results file after a specified increment in time. Exposes a Time field where you enter a time increment.

Yes

Yes

Equally Spaced Points

(Default) Save a specified number of result files during the analysis. The frequency is defined by the termination time / number of points. Exposes a Number of Points field where you enter the number of results files required.

Yes

Yes

During the solve of an Explicit Dynamics system, restart files are saved to disk at a frequency defined through this control. The following settings are available.

Yes

Yes

Save restart files after a specified increment in the number of cycles. Exposes a Cycles field where you enter the increment in cycles.

Yes

Yes

Save Restart Files on

Cycles

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

57

Explicit Dynamics Workflow Field

Options

Description

2D

Time

Save restart files after a specified increments Yes in time. Exposes a Time field where you enter a time increment.

Restart Yes

This setting is not available for Workbench LS-DYNA. Equally Spaced Points

Save Result Tracker Data on

(Default) Save a specified number of restart files during the analysis. The frequency is defined by the termination time / number of points. Exposes a Number of Points field where you enter the number of restart files required.

Yes

Yes

Use this control to define the frequency at which result tracker data and solution output is saved to disk.

Yes

Yes

(Default) Save results tracker and solution Yes output data after a specified increment in the number of cycles. Exposes a Cycles field where you enter the increment in cycles. The default value is 1.

Yes

Result tracker data objects are scoped to specific regions in a model. Solution output provides a summary of the state of the solution as the solve proceeds. This is shown when Solution Information is highlighted in the project tree. This setting applies to all the selectable views in the Solution Output drop down list located in the Solution Information Details view. This field is not available for Workbench LS-DYNA. Cycles

If a number less than or equal to 10 is entered for Cycles, then the following plots available from the Solution Output drop down will be updated every 10 cycles unless overall progress has increased by 5% since the last data point (in which case, the plots will be updated at a frequency as close to the entered cycle increment as possible). Results trackers are excluded from this limitation. • Time Increment • Energy Conservation

58

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Establish Analysis Settings Field

Options

Description

2D

Restart

Yes

Yes

No

Yes

• Momentum Summary • Energy Summary The Solver Output view from the Solution Output drop down will be updated at the entered cycle increment. Cycle zero and the final cycle will always be displayed even if it is not a multiple of the cycles entered. Time

Save result tracker and solution output data after a specified increment in time. Exposes a Time field where you enter a time increment. Although time based, the frequency of Solution Output update is limited to no more than every 10 cycles. If a time equating to 10 cycles or less is chosen, then the following plots available from the Solution Output drop down will be updated every 10 cycles, unless overall progress has increased by 5% since the last data point (in which case, the output will be updated at a frequency as close to the entered time increment as possible). Results trackers are excluded from this limitation. • Time Increment • Energy Conservation • Momentum Summary • Energy Summary The Solver Output view from the Solution Output drop down will be updated every cycle.

Output Contact Forces

Use this control to define the frequency that contact forces are written out to file. • Contact forces information is written to the solution directory into ASCII files named extfcon_*.cfr, where * is the cycle number.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

59

Explicit Dynamics Workflow Field

Options

Description

2D

Restart

• Each file contains forces in the global x, y and z directions for nodes on external faces, where the forces are non-zero. • Contact forces are not written for Line bodies or Eulerian (Virtual) bodies. • Contact forces are only written for 3D analyses. • A separate line pair exists for each node in the following format: Node number Contact Force X

Contact Force Y

Contact Force Z

• These text files may be used by ACT to visualize the contact pressure between bodies.

Note Output Contact Forces are not step-aware. Off

(Default) Disable output of contact forces.

No

Yes

Cycles

Write contact forces to a file after a specified No increment in the number of cycles. Exposes a Cycles field where you enter the increment in cycles.

Yes

Time

Write contact forces to a file after a specified No increment in time. Exposes a Time field where you enter a time increment.

Yes

Equally Spaced Points

Write a specified number of contact force No files during the analysis. The frequency is defined by the termination time/ number of points. Exposes a Number of Points field where you enter the number of contact force files required.

Yes

2.10.1.7. Explicit Dynamics Data Management Settings Note that these settings cannot be changed from the Details panel. Field

Description

Solver Files Directory

The permanent location for all the files generated during a solve. This is a read-only field provided for information.

Scratch Solver Files Directory

A temporary location for all files generated during a solve. These files are then moved to the Solver Files Directory for completed

60

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Establish Analysis Settings Field

Description solves. This is a read-only field provided for information. See Analysis Data Management in the Mechanical User's Guide for more information. This field is not available for Workbench LS-DYNA.

2.10.1.8. Recommendations for Analysis Settings in Explicit Dynamics Explicit Dynamics may be used for a wide range of applications, and a default set of Analysis Settings designed to provide the most robust solution are not necessarily suited to every application. Therefore, the Type setting allows the selection of particular defaults depending on the requirements of the solution. The following options are available: • Program Controlled – This is the default setting with a priority for a robust solution. • Low Velocity – Recommended for low deformation/velocity (100m/s) analyses. • Efficiency – Settings for minimum runtime. In some cases, this may have an effect on robustness and accuracy. • Quasi-static – Recommended for quasi-static analyses. • Drop Test – Recommended for drop test analyses. The exact Analysis Settings values for each of the Analysis Settings Preference Types are shown in the table below. Switching the Type property will update all of the items displayed in the table as indicated. If any of these settings are subsequently changed, then the Type will be indicated as Custom. Program Efficiency Low Controlled Velocity Default Setting (Robustness)for minimum run time (also minimum robustness and accuracy in some cases)

High Velocity

Quasi-Static Drop Test

Recommended Recommended Recommended Recommended setting for high setting setting for low deformation/velocity for for drop deformation/velocity simulationsquasi-static test simulations (>100m/s) simulationsanalyses (Impedance Boundary. 2. Define the Scoping Method.

Details View Properties The selections available in the Details view are described below. Category

Fields/Options/Description

Scope

Scoping Method: Options include: • Geometry Selection: Default setting, indicating that the boundary condition is applied to a geometry or geometries, which are chosen using a graphical selection tools. – Geometry: Visible when the Scoping Method is set to Geometry Selection. Displays the type of geometry (Body, Face, etc.) and the number of geometric entities (for example: 1 Body, 2 Edges) to which the boundary has been applied using the selection tools. • Named Selection: Indicates that the geometry selection is defined by a Named Selection. – Named Selection: Visible when the Scoping Method is set to Named Selection. This field provides a drop-down list of available user-defined Named Selections.

Definition

Type: Read-only field that describes the object - Impedance Boundary. Material Impedance: Program Controlled or input value. Reference Velocity: Program Controlled or input value. Reference Pressure: Program Controlled or input value. Suppressed: Include (No - default) or exclude (Yes) the boundary condition.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

71

Explicit Dynamics Workflow

2.12.2. Detonation Point You can detonate an explosive by various methods of delivering energy to it. However whether an explosive is dropped, thermally irradiated, or shocked, either mechanically or through a shock from an initiator (of a more sensitive explosive), initiation of an explosive always goes through a stage in which a shock wave is an important feature. It is assumed that, on initiation, a detonation wave travels away from the initiation point with constant detonation velocity, being refracted around any inert obstacles in the explosive without moving the obstacle, maintaining a constant detonation velocity in the refracted zone and detonating each particle of explosive on arrival at that particle.

Analysis Types Detonation Point is available for an Explicit Dynamics analysis only.

Common Characteristics This section describes the characteristics of the boundary condition, including the application requirements, support limitations, and loading definitions and values. Dimensional Types • 3D Simulation: Supported. • 2D Simulation: Not Supported.

Note Detonation Points are not available for Workbench LS-DYNA.

Boundary Condition Application 1. Click the Loads drop-down menu from the Context tab and select Detonation Point. Or, right-click the Environment tree object or the Geometry window and select Insert → Detonation Point. 2. Specify Location. Multiple detonation points can be added to an analysis. The location of the selected detonation point and the detonation time are displayed in the annotation on the model.

Details View Properties The selections available in the Details view are described below. Category

Fields/Options/Description

Definition

Burn Instantaneously: When set to Yes, results in initiation of detonation for all elements with an explosive material at the start of the solve. Detonation Time: User can enter the time for initiation of detonation. [Only visible if Burn Instantaneously is set to No.]

72

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Apply Loads and Supports Category

Fields/Options/Description Suppressed - Include (No - default) or exclude (Yes) the boundary condition.

Location

Enter detonation point coordinates: • X Coordinate • Y Coordinate • Z Coordinate Location: User can interactively select detonation location using the vertex/edge/face selection tools: • Select Vertex: Sets X/Y/Z location to vertex location. • Select Edge: Sets X/Y/Z location to centre of edge. • Select Face: Sets X/Y/Z location to centre of face.

Theory The Detonation analysis method used is Indirect Path detonation. Detonation paths are computed by finding either a direct path through explosive regions or by following straight line segments connecting centers of cells containing explosives. Either: Detonation paths will be computed as the shortest route through cells that contain explosive. Or... Detonation paths are computed by finding the shortest path obtained by following straight line segments connecting the centers of cells containing explosive. The correct detonation paths will automatically be computed around wave-shapers, obstacles, corners, etc. Detonation points must lie within the grid. Paths cannot be computed through multiple Parts. If a detonation point is placed in one Part, the detonation from this point cannot propagate to another Part. If this is required, you must place one or more detonation points in the second Part with the appropriate initiation times set to achieve the required detonation. The following illustration outlines the detonation process:

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

73

Explicit Dynamics Workflow

• Detonation is initiated at a node or plane (user defined) • Detonation front propagates at the Detonation Velocity, D • Cell begins to burn at time T1 • Burning is complete at time T2 • Chemical energy is released linearly from T1 to T2; burn fraction increases from 0.0 to 1.0 over this time The result DET_INIT_TIME can be used to view the initiation times of the explosive material. For example, in the image below, the body on the left side has a detonation point with instantaneous burn defined, and so the entire material has a detonation initiation time of 1x10-6 ms. The second body has a detonation point defined in the lower X, lower Y, lower Z corner, and the detonation time can be seen to vary from 0 ms (in other words, instantaneous detonation) to a value of 0.19555 ms in the corner of the body furthest away from the detonation point. Once detonation is initiated in an element, a value of zero is shown for DET_INIT_TIME.

74

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Apply Loads and Supports

The result ALPHA can be used to view the progress of the detonation wave through the material. This corresponds to the burn fraction, which will be a value between zero (no detonation) and one (detonation complete). For the same example, looking at values of alpha at a later stage in the calculation, the detonation wave can clearly be seen in the body on the right as the spherical band of contours showing the value of alpha changing from zero to one. The body on the left has a value of one for the entire body, as it detonated instantaneously.

2.12.3. Activation/Deactivation of Loads in Explicit Dynamics You can activate or deactivate a load (which includes it in, or excludes it from, the analysis) within the time span of a step. For most loads (for example, pressure or force) deleting the load is the same as

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

75

Explicit Dynamics Workflow setting the load value to zero. But for certain loads, such as a specified displacement, this is not the case.

Note Changing the method of how a multiple-step load value is specified (such as Tabular to Constant), the Activation/Deactivation state of all steps resets to the default, Active. To activate or deactivate a load in a stepped analysis: 1.

Highlight the load within a step in the Graph or a specific step in the Tabular Data window.

2.

Click the right mouse button and choose Activate/Deactivate at this step!.

Note For displacements and remote displacements, it is possible to deactivate a selection of degrees of freedom within a step.

Supported Constraints • Acceleration • Standard Earth Gravity • Pressure • Force • Remote Force • Line Pressure • Joint Load (displacement/velocity/acceleration/force/moment) • Displacement • Remote Displacement • Velocity • Nodal Force • Nodal Displacement Step deactivation is (by design) not applicable for: • Hydrostatic Pressure • Detonation Point • Fixed support • Impedance Boundary

76

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Solve

Application of Load Steps Here are some example scenarios where load deactivation is useful: • Springback of a cantilever beam after a plasticity analysis. • Locking a joint or remote point in a certain location by setting the velocities to zero. • Specifying different initial velocities for different parts in an Explicit Dynamics analysis during the analysis by activating an acceleration during a load step. • Multistep type of analysis to keep track of loads in a logical way.

Caution Reactivation of translational and rotational displacement boundary conditions is not allowed. The explicit solver is not able to fulfill such a constraint in one cycle when the boundary condition becomes active. This will result in an error message: Boundary condition contains a load step which has been reactivated after being deactivated. The constraint cannot be fulfilled because it would cause very large displacements in one solver cycle. Instead use a velocity based boundary condition. In the following example the nodes would be free to move during load step 2. Adhering to the constraint at the start of load step 3 would cause the deformations to become too large. This restriction does not apply for non-displacement type of boundary conditions.

2.12.4. Importing External Loads The External Data system allows you to import external loads into an explicit dynamics analysis. Currently, the only load supported for explicit dynamics analyses is Imported Pressure.

2.13. Solve For general information about solving, see Solve in the Mechanical User's Guide

2.13.1. Solving from Time = 0 Solving from Time = 0, which is from Cycle=0, is the typical way to start an analysis. This cycle value is the default setting in the Resume From Cycle field located in the Step Controls (p. 45) section of the Analysis Settings (p. 41). The analysis will run until either the user-defined Maximum Number of Cycles or End Time is reached. The following restriction applies: Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

77

Explicit Dynamics Workflow • An Explicit Dynamics solve can only be performed if the model contains at least one Initial Condition (Translational or Rotational velocity), a non-zero constraint (displacement or velocity), or a valid load. If you are using RSM for the solution, the Remote Solve Manager can be used to monitor the analysis and obtain any solution related output. Another way of monitoring the progress of the solve is to view the Solution Information (p. 80) while the solve is running, where you can view the estimated run time remaining. A running analysis can be interrupted; for example, to review results part way through the analysis. An interrupted analysis can be resumed (p. 78) to continue to the end. Similarly, a successfully ended analysis can be extended beyond its current end time or cycle.

2.13.2. Resume Capability for Explicit Dynamics Analyses If an Explicit Dynamics analysis has partially or totally completed, you can resume the analysis from a non-zero time step (cycle). You may want to do this in order to: • Extend an analysis that has successfully completed beyond its current end time or cycle. • Complete an analysis that has been interrupted. For example you may wish to interrupt an analysis in order to review results part way through a longer simulation. • Continue an analysis that has stopped part way through. For example, if an analysis has terminated prematurely due to the time-step size being too small, you can make adjustments to mass scaling, and restart the calculation. • Adjust the frequency of restart file, result file or other output information. For example, you may wish to resolve part of an analysis that is of interest with more frequent results. • Adjust damping or erosion controls. You may resume an analysis from any cycle that has a restart file by first selecting the cycle in the Resume From Cycle field located in the Step Controls (p. 45) section of the Analysis Settings (p. 45), then making any other required analysis changes and selecting Solve. The frequency of restart file output is controlled in the Analysis Settings Output Controls (p. 56). There is no limit to the number of times an analysis may be resumed. The following restrictions apply: • Changes made to any feature of the model outside of the Analysis Settings will prevent a resume from taking place. • Changes made to any of the (Analysis Settings) Solver Controls, except for Minimum Velocity, Maximum Velocity and Radius Cutoff, will prevent a resume from taking place. • Changes made to the Retain Inertia of Eroded Material field will prevent a resume from taking place.

78

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Solve • Changes to all other Erosion Controls, Damping Controls, and Output Controls are valid and will not prevent a resume from taking place.

Note You cannot edit the Static Damping and Output Controls for load steps with End Time values smaller than the Restart Time corresponding to the Restart Cycle.

• To use Automatic Mass Scaling under Analysis Settings, Step Controls), it must be enabled from the start of the calculation. You cannot change the Automatic Mass Scaling property for a restart calculation. If Automatic Mass Scaling is active, the other Mass Scaling properties may be changed part way through a calculation. • Analyses with non-zero Displacement constraints defined may not be resumed.

2.13.2.1. Load and Constraint Behavior when Extending Analysis End Time For a model with loads and constraint, when using the resume capability to extend the end time of an analysis, the following points should be considered. • Loads and constraints may not be modified after cycle zero. • If an analysis end time has been increased, then it is possible that the analysis time may fall outside the defined region of a time-dependent load or constraint. If this is the case, no load or constraint will be applied. • Time-dependent data for loads and supports can be defined for times greater than the end time of the analysis, and these will become valid if the end time is then extended for a resumed analysis. • The solver representation of loads and constraints may be verified by looking at admodel.prt in the Solver Files directory.

2.13.3. Explicit Dynamics Performance in Parallel For general information about solving in parallel with the Mechanical Application see Understanding Solving in the Mechanical User's Guide Parallel processing is not supported for 2D Explicit Dynamics models. Explicit Dynamics 3D solutions default to using up to two cores with shared-memory parallelism. MPI parallel processing support for 3D Explicit Dynamics models is described in the following table. Windows

Linux

Local Parallel

Distributed Parallel

Windows HPC Jobscheduler

Local Parallel

Distributed Parallel

Parallel Jobschedulers

IBM Platform MPI, INTEL MPI, Microsoft MPI

IBM Platform MPI, INTEL MPI

N/A

IBM Platform MPI

IBM Platform MPI

N/A

You can use the additional command line arguments field as described in Using Solve Process Settings in the Mechanical User's Guide to specify the information necessary to run an Explicit Dynamics solution in parallel.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

79

Explicit Dynamics Workflow The MPI software used in a distributed parallel simulation can be specified using the -mpi option. The available options are: ibmmpi (IBM), intelmpi (Intel), and msmpi (Microsoft). The default option is IBM MPI (ibmmpi) and will be used if the -mpi option is not specified in the additional command line options. IBM MPI is the only mpi option that is supported for Linux machines. The machines used in a distributed parallel analysis can be specified using the -machines option. The machines argument should be specified as: -machines machineName1:N1,MachineName2:N2

where machineName1 will be started with N1 slave executables and MachineName2 will be started with N2 slave executables. The machine name and number of slaves should be separated by a colon and each pair of machine name\number of slaves should be separated by a comma. If spaces are added then the -machines argument should be enclosed in double quotes: -machines "machineName1 : N1 , MachineName2 : N2"

Note When running Explicit Dynamics using IBM MPI, the MPI files used are the IBM MPI files included with the ANSYS installation. It is possible to specify a different location for the MPI files by setting the environment variable EXD_MPI_ROOT; for example: EXD_MPI_ROOT = "C:\Program Files (x86)\IBM\Platform-MPI"

The following capabilities of the explicit solver are not supported for a parallel environment: • Line body to line body contact using Proximity Based interaction in combination with the Edge on Edge option. • Trajectory contact with the Decomposition Response formulation.

Note When a model contains a capability that is not supported for a parallel environment, the analysis will automatically run in serial mode.

2.14. Postprocessing You can review the Solution Information object and the Result Trackers to analyze your solution quality. Result trackers must be defined before you start the solution.

2.14.1. Solution Output The Solution Information object provides a summary of the solution time increments and progress is continuously updated in the solution output. For distributed analyses, the parallel load balancing is also displayed. This is calculated for each slave as the CPU time taken on the slave divided by the average CPU time taken on all the slaves. For a perfectly balanced solution, all slaves will have a load balancing of one. Histograms of time step, energy and momentum are also available for real time monitoring of solution progress.

80

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing You can monitor the quality of the solution by reviewing momentum and energy conservation graphs in the solution output. Low energy errors (0 - eroded (will not be displayed). EPS_RATE

Effective Plastic Strain Rate.

Element Nodal

F_AXIAL

Beam axial force.

Element Nodal

INT_ENERGYALL

Internal energy of the material.

Element Nodal

MASSALL

Mass of material in an element.

Element Nodal

MATERIAL

Material index. The material index as defined in the Explicit solver. There is not always a direct one-to-one correlation with materials defined in Engineering Data and those used in the Explicit solver.

Elemental

For layered section shells, the MATERIAL for individual layers can be shown by using the Layer property in the results details view. MOM_TOR

Beam rotation inertia.

Element Nodal

POROSITY

Material Porosity:

Elemental

Porosity, α = ρSolid/ρ PRESSURE

Pressure.

PRES_BULK

Dilation pressure for the Johnson-Holmquist brittle strength model. Elemental

RB_CONTACT_ENERGY Energy in Rigid Body contact.

94

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Element Nodal Element Nodal

Postprocessing Expression

Description

Type

SOUNDSPEED

Material soundspeed.

Element Nodal

STATUS

Material Status:

Elemental

1 – elastic. 2 – undergoing plastic flow. 3 – failed due to effective criteria (with healing). 4 – failed due to effective criteria. 5 – failed due to stress/strain in principal direction 1. 6 – failed due to stress/strain in principal direction 2. 7 – failed due to stress/strain in principal direction 3. 8 – failed due to shear stress/strain in principal direction 12. 9 – failed due to shear stress/strain in principal direction 23. 10 – failed due to shear stress/strain in principal direction 31. For layered section shells, the STATUS for individual layers can be shown by selecting the Layer number in the results details view. STOCH_FACT

Stochastic factor applied when the stochastic property as defined in the material failure model.

Elemental

STRAIN_XX

Total strain XX.

Element Nodal

STRAIN_YY

Total strain YY.

Element Nodal

STRAIN_ZZ

Total strain ZZ.

Element Nodal

STRAIN_XY

Total strain XY. These are tensor shear strains, and not engineering Element shear strains. Nodal

STRAIN_YZ

Total strain YZ. These are tensor shear strains, and not engineering Element shear strains. Nodal

STRAIN_ZX

Total strain ZX. These are tensor shear strains, and not engineering Element shear strains. Nodal

TASK_NO

Assigned task number for parallel processing.

Elemental

TEMPERATUREALL

Material Temperature.

Element Nodal

THICKNESS

Shell Thickness.

Element Nodal

TIMESTEP

Element computational time step.

Element Nodal

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

95

Explicit Dynamics Workflow Expression TYPE

Description Element category (element number returned):

Type Elemental

HEX: 100-101. PENTA: 102. TET: 103-104,106. PYRAMID: 105. QUAD: 107. TRI: 108. SHL: 200-202, 204. BEAM: 203. VISC_PRES

Viscous pressure due to artificial viscosity. No results will display for an Eulerian part.

Element Nodal

VTXX

Viscoelastic stress XX.

Element Nodal

VTYY

Viscoelastic stress YY.

Element Nodal

VTZZ

Viscoelastic stress ZZ.

Element Nodal

VTXY

Viscoelastic stress XY.

Element Nodal

VTYZ

Viscoelastic stress YZ.

Element Nodal

VTZX

Viscoelastic stress ZX.

Element Nodal

For Euler (Virtual) Analyses The following results are multi-material variables: • EFF_PL_STN • INT_ENERGY • MASS • COMPRESS • DET_INIT_TIME • ALPHA • DAMAGE • TEMPERATURE

96

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing For each Eulerian (Virtual) body in the analysis, a separate component will be available, which will allow the user to plot the result for the particular material associated with that body. The component name will be derived from the body name. There will also be an “ALL” component, which displays results for all materials. Results for Lagrangian bodies can be viewed by selecting this “ALL” component. For a purely Lagrangian analysis, only the “ALL” component will be available to the user. For example, an analysis has two Eulerian (Virtual) bodies (Solid, Solid) and a Lagrangian Body (Surface Body), as shown in the image of the Outline View below.

In the User Defined Result Expression Worksheet, there are three components available for the multimaterial results named SOLID, SOLID_2, and ALL.

Note It may be necessary to delete and reinsert multi-material results in order to view result for databases created prior to Release 13.0

For NBS Tetrahedral Elements The element variables listed below can be used to visualize the variable values at the nodes. The variable values presented in the element are a volume weighted average of those at the nodes. • TEMPERATURE • SOUNDSPEED • DENSITY • COMPRESS • STRAINS (NORMAL AND SHEAR) • EFF_PL_STN Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

97

Explicit Dynamics Workflow • TIMESTEP • INT_ENERGY The following variables are available as calculated directly from the solver in the element: • EFF_STN

98

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 3: Transforming an Implicit Model to run in Explicit Dynamics 3.1. When Implicit Models Can be Run in Explicit Implicit and Explicit finite element solvers use different methods to evaluate the underlying equations. A simple high level overview is given in the figure below. There is an overlap in the "Quasi-Static" application area, where both Implicit and Explicit methods can be used to solve a model. Implicit methods are typically bounded by the amount of deformation and contact nonlinearity that is taking place, where Explicit methods are typically bounded by the problem's time scale, which would lead to excessive run times. Figure 3.1: Different applications of the two solvers with respect to velocity

Problems that are in this "Quasi-Static" range have a good chance of being solved by either method until the limitations of a particular solver are reached. At that point, it can be beneficial to consider the use of the alternative solver. This chapter describes the steps necessary to transform a model that was initially set up for simulation in the Implicit solver to a model setup for simulation in the Explicit solver. Typically, you would want to consider doing this when the degree of nonlinearity in the model is starting to pose problems for Implicit methods. Because of the nature of the two methods, the explicit solver is more suitable for nonlinear problems, working with less computationally heavy but a much larger number of iterations that can follow the physical parameter changes at a much higher frequency. The implicit solver works with much more complex calculations for each iteration but has a lot fewer of them. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

99

Transforming an Implicit Model to run in Explicit Dynamics

3.2. When to Consider an Explicit Analysis There are numerous reasons why an implicit methods fails to solve properly. This section tries to give realistic guidelines for when to switch to an Explicit method. 3.2.1. Incorrect Model Setup 3.2.2. Large Deformations 3.2.3. Large Contact Models 3.2.4. Rigid Body Deformations

3.2.1. Incorrect Model Setup A model may fail when the Implicit method is used simply due to poor model setup, in which case Explicit methods will fail also. However, an incorrect model setup may be easier to detect with an Explicit analysis because the solution progresses with very small timesteps, and results can be visualized during the solution (by using result trackers (p. 119), or using the Autodyn component system). Once the problem is identified using the explicit dynamics analysis, it can be corrected and solved using implicit methods. The explicit dynamics solver is very useful when working with complex interacting mechanisms and geometries. The solver can be used to quickly check for fit and how the parts are positioned with respect to each other at the end of the simulation. The example model shown in Figure 3.2: Example Model Run with Explicit Dynamics Showing Problem Area (right) (p. 101) does not converge when run with the Static Structural (Implicit) solver. The output messages recommend checking for an 'insufficiently constrained model'. The geometry has multiple angles and edge lengths so the problematic area is not obvious. This is a good example of where explicit dynamics methods can be used to quickly identify model problems. The displacement of the interacting bodies is known and final body fit and alignment can be investigated. The Explicit analysis uses the same geometry and model setup as was used for the Static Structural analysis and the model is meshed using the Explicit meshing defaults. The endtime is chosen to obtain a fast solution in order to observe the relative movement of the parts and their final position at the end of the displacement. As a general guideline the endtime,Tend, should be chosen such that the average velocity of the parts, uavg, is in the order of 10 m/s during the displacement, d, of the parts:

For this example model, the endtime is set to 1 millisecond.

100

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

When to Consider an Explicit Analysis Figure 3.2: Example Model Run with Explicit Dynamics Showing Problem Area (right)

The Explicit analysis takes about a minute, and the model solves with all options being left to their defaults. The problematic area is obvious as can be seen above: the left notch of the upper part does not follow the bottom part geometry. This quickly points to where a change of the geometry is necessary.

3.2.2. Large Deformations Many models require the simulation of rubber-like highly deformable materials. This is associated with the use of hyperelastic material models in the setup. The implicit solver makes a strong effort to solve these models with options like Large Deflection and Nonlinear Adaptivity, which are recommended when such materials are used. Nevertheless these solutions may not converge. This would be a suitable situation in which to use explicit dynamics. You do need to specify all the input for the hyperelastic materials as opposed to the implicit solver, where the density and the incompressibility parameter can have zero values (see Materials (p. 105)), but the Explicit solver will provide a solution in most cases where the implicit solver cannot. Important things to look out for in the Explicit solver when using hyperelastic material models are the energy error/hourglassing and excessive mesh element distortion requiring the use of erosion (p. 115). Models with high nonlinear deformations are also a good candidate for mass scaling (p. 114). The following example demonstrates how the same setup works with the two different solvers. Figure 3.3: Comparison between the implicit (left) and the explicit (right) solvers for maximum deformation values (p. 102) shows the largest displacement achieved by the disc relative to a hyperelastic material complex part.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

101

Transforming an Implicit Model to run in Explicit Dynamics Figure 3.3: Comparison between the implicit (left) and the explicit (right) solvers for maximum deformation values

The implicit solver has trouble converging at around half of the total displacement but the explicit solver manages to complete the run, simulating the high deformations.

3.2.3. Large Contact Models Handling a large number of contacts can be problematic for the implicit solver. This is especially the case when the contact is not bonded but is sliding and moving. The explicit dynamics solver has standard out-of-the-box automatic contact options (trajectory contact) which work very well. Contact will be detected in the model automatically at any point without requiring the user to define specific contact regions. On top of that, the user can specify contacts manually (or generate them automatically) separate from the trajectory contact, which is done similarly to the Contacts feature in the implicit solver. Figure 3.4: Model Setup Showing Contact (left) and Boundary Conditions (right)

The model shown in Figure 3.4: Model Setup Showing Contact (left) and Boundary Conditions (right) (p. 102) demonstrates this contact issue. The implicit setup has a manually defined frictionless contact consisting of 40 contact and 38 target faces between the two parts. The explicit dynamics model simply has the default frictionless trajectory contact enabled. All other boundary conditions are the same for both analyses: a fixed support and a displacement boundary condition. Both models have the same mesh type and mesh density (the implicit setup does not make use of midside nodes in order to achieve maximum similarity in comparison, since the explicit solver cannot use midside nodes). The implicit model has problems converging while the explicit solve completes without issues. This model 102

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

When to Consider an Explicit Analysis exemplifies the possible problematic contact handling in the implicit solver. The model will converge when using a denser mesh; however the differences are clear for comparable mesh size (the implicit solver using midside nodes with the standard mesh size also does not converge). The final stress results can be seen in Figure 3.5: Final Stress Values Comparison Between the Explicit (left, 3.4E10 Pa) and Implicit (right, 3.7E10 Pa) Solvers (p. 103). Figure 3.5: Final Stress Values Comparison Between the Explicit (left, 3.4E10 Pa) and Implicit (right, 3.7E10 Pa) Solvers

3.2.4. Rigid Body Deformations A common analysis in the quasi-static range is the simulation of physical mechanisms. This means that rigid body movements are included in the analysis. A common simulation is a rigid or much stiffer body that snaps over a soft and flexible one. Some examples include: rubber seals for waterproofing, snapping of softer metal elements to ensure a tight fit or snapping through a notch to prevent backward movement. In these situations the implicit solver can encounter problems modeling the high deformations right before the snap, or the release of the high deformations after the snap. These problems are inherently unstable for the implicit solver and can be a challenge to solve successfully. Figure 3.6: The Clip Model Setup in the Implicit Solver with Final Deformation Values (right) (p. 103) shows an example of a clip snap through model where a metal clip has to pass over a rubber step. Figure 3.6: The Clip Model Setup in the Implicit Solver with Final Deformation Values (right)

The solution does not converge unless the mesh is much coarser - this means the initial clip to rubber step contact is missed (without any special settings). Also there is a problem of missed contact between the clip and the hinge, which you can solve in the implicit solver by applying a cylindrical support. This same model with the same setup for boundary conditions and less constraints (no cylindrical support or equivalent), can be successfully solved by the explicit solver, as seen in Figure 3.7: The Clip Model Setup in Explicit Dynamics with Final Deformation Values (right) (p. 104). The setup uses mostly default settings apart from a Static Damping value which is added because of the hyperelastic material (see Damping (p. 116)). The model will run successfully without damping, but due to the nature of the materials, strong oscillations will be introduced. This means the maximum stress on the clip will spike at a much larger value than in the damped solution and then gradually converge on a similar final value when the vibrations decrease.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

103

Transforming an Implicit Model to run in Explicit Dynamics Figure 3.7: The Clip Model Setup in Explicit Dynamics with Final Deformation Values (right)

3.3. Setting up the Explicit Dynamics Analysis This section will take you through the steps necessary to perform the implicit analysis using the explicit solver.

3.3.1. Attaching an Explicit Dynamics System to an Existing Static Structural System In general, you should use the Implicit analysis to set up the Explicit Dynamics analysis. When you identify the need to use the Explicit Dynamics solver, you must attach an Explicit Dynamics system to the existing Implicit one. You do this in the same way that you would attach systems in any other Workbench project schematic operation - by drag and drop. You have four choices of what to include in the component system information transfer (see the following figure). Figure 3.8: Choices for information sharing between cells of implicit and explicit systems

If you drop the Explicit Dynamics system on the Engineering Data cell, only the material data would be transferred. This is not what you want to do. Dragging and dropping on the cell Geometry or Model cell should be used when you want to transfer the model from Implicit to Explicit. Dropping the system on the Solution cell transfers all of the end results, deformation, and stress from the Implicit solution, so that should only be done in prestressing cases. If you drop the system on the Geometry cell, all of the Implicit setup has to be recreated manually for the Explicit solver. This is the better choice when dealing with very simple models with very few options

104

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting up the Explicit Dynamics Analysis for the mesh, virtual topology, contacts, and boundary conditions. This connects the two systems, but the model is launched in two separate Mechanical instances, only sharing the material and geometry data. If you drop the system on the Model cell, the models are much more connected. They share a single Mechanical instance and the same meshing and contact options. Due to the large variation in boundary conditions, they are not transferred automatically.

Note Changing some options for meshing, materials, or others to make the Explicit analysis work might interfere with the Implicit solver and make the model not solve properly. These options are discussed in the next sections. If you want to create an Explicit simulation using the Model cell transfer, it is recommended that you do this in a duplicate project file.

3.3.2. Materials There are some material models that are not available for both solvers. Whenever a question mark symbol is observed next to the Engineering Data cell, it must be properly addressed. By inspecting the materials, it should be clear where the problem is. For example, it might be a missing density value or a parameter which has not been set; something which might be required for the Explicit solver but not for the Implicit one. This is the case with hyperelastic materials using the Mooney-Rivlin material model. To get a value for the incompressibility parameter, the user must either have the experimental data and use curve fitting, use a value from another material specification, or just use the rubber model in the Explicit material database. Another issue you might encounter is where a parameter that is required for the Explicit simulation can interfere with the Implicit solution and make it unable to solve. This often occurs since both systems share the same material data, and can be fixed by using different material assignments (if you are using the Geometry cell data transfer and have separate Mechanical instances). A problem with unsupported material model types is usually seen as an error message in the solver.log file or the Solution Information when a solve is attempted. Another common example of a problem is having tabular data input for a material property in Implicit with, for example, 12 stress strain pairs. This would trigger an error in the explicit solver, which only supports 10 or less stress strain pairs. An easy workaround for this would be to take the curve formed by the 12 points and delete two points, relocating the others so that the curve shape remains the same.

3.3.3. Meshing Before running the simulation, the meshing has to be thoroughly checked to ensure all requirements are met. The Explicit and Implicit solvers require different types of meshes. The simplest way to differentiate is to switch the Physics Preference option between Explicit and Mechanical. However, if the Model cell connection is used, the models are going to make use of the same mesh; this might mean that when the mesh is made to work with the Explicit solver it might not solve anymore with the Implicit solver. Generally, with a complex geometry we do not want to use the same mesh for both solvers.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

105

Transforming an Implicit Model to run in Explicit Dynamics Figure 3.9: Meshing options menu - physics preference

3.3.3.1. Uniform Mesh Works Best The Implicit solver works well when the areas of interest have much denser meshes. This is not the case for the Explicit solver. First, the time step (the time increment at which the Explicit solver advances) is controlled by the smallest mesh element - thus the size of the smallest elements in the interest area will control the solve for the whole model, increasing the run times. Second, the nature of the Explicit Dynamics solver is such that it works best with cuboid, evenly distributed mesh elements throughout the model. Lastly, this element size difference will skew the results much more than with the Implicit solver, because of the use of each individual element mass, deformation, and velocity for the calculations. To ensure a good Explicit solve, you need to look at the mesh maximum and minimum element size in the mesh statistics. The smaller the spread of element sizes, the better.

3.3.3.2. Midside Nodes not Used The implicit solver can create midside nodes in the elements to aid the accuracy of the solution. This is not possible with the Explicit solver. If you want to use the same mesh for both solvers, set Element Order to Linear in the Defaults section of the Mesh settings. If this is not set, the error Higher order elements detected. Element Order must be Linear for Explicit Dynamics analyses. will be generated.

106

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting up the Explicit Dynamics Analysis Figure 3.10: Meshing options menu - Defaults

Note It is important when there are regions of the geometry which are relatively thin and will encounter bending, that they are meshed with at least two mesh elements across their thickness to ensure the Explicit solver models the bending correctly. Because of this, you may want to use shell bodies where more appropriate; the two elements across recommendation can lead to a very small time step overall.

3.3.3.3. Hex/Rectangular Mesh Elements most Effective Even though more complex geometry is quite difficult to mesh with hex elements, they are the most suitable type for the simulation. If you are familiar with the Implicit solver, you should understand the various ways to control how the mesher approaches the geometry. The geometry should be swept meshed wherever possible. Shell bodies should be face meshed to ensure only rectangular elements are used.

3.3.4. Contact/Connections The contact options in Explicit Dynamics are very similar to the ones in the Implicit solver. When the two are connected via the Model cell, all of the options for the contacts are the same as for Implicit (apart from the addition of the Body Interactions option). Differences in the Contacts tab are only visible when looking at a standalone explicit dynamics system or a system only sharing material and geometry data. Unlike with meshing, the Explicit solver can use contacts defined for the Implicit solver without any problems, although some of the options do not directly affect the Explicit solution.

3.3.4.1. Contacts Tab In the Explicit Dynamics system, the contact region options lack the Advanced and Geometric Modification expandable tabs. These tabs offer features which help the Implicit solver deal with actions like impact and sliding which are easily simulated with the Explicit solver, making the tabs unnecessary. The scoping mechanism and the contact types are the same for both solvers. When using Bonded contact with the Explicit solver, one of the most important settings is the Maximum Offset. This should be set to a value greater than the maximum estimated distance between the scoped geometries expected during the simulation to allow the contact to function as it should. Setting a very large value will increase the computational load so a good estimate is preferable.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

107

Transforming an Implicit Model to run in Explicit Dynamics The Shell Thickness Effect option in Implicit does not affect the Explicit solve and the desired value should be set to the Shell Thickness Factor in the Body Interactions options. Rather than on or off, the thickness can be set to a specific portion of the shell - from 0 to 1.

3.3.4.2. Body Interactions Tab By default, the Body Interactions object is always present for the Explicit Dynamics system. This is an automated contact detection feature which perfectly suits the nature of the solver. It can be very useful since Explicit Dynamics mostly models impacts and crashes, where which bodies will be in contact is usually unknown. There are general options in the main Body Interactions object and different specified contacts can be added. Contact types include primary types such as Frictionless, Frictional, and Bonded, but also a specific Explicit Dynamics type, Reinforcement. It is used to model reinforced structures like steel reinforced concrete columns, for example. The default trajectory contact settings allow you to understand where the contact points are in the simulation after an initial coarse mesh run and then refine the contact options and scoping. Figure 3.11: Body Interactions Object under Connections

3.3.5. Boundary Conditions Even though both solvers model structural problems, the boundary conditions have a number of differences. Unlike the Explicit dynamic structural solver, the Implicit static structural solver has no real dependency on inertia. That is why the load cases in Implicit are usually 1 second per step, which is an arbitrary amount. Altering this value does not really have any effect on the solution. The Explicit Dynamics solver, on the other hand, uses time as its main reference for the calculations since the duration of the events in an Explicit problem are extremely short, and it is one of the most important aspects of the solve. When the two systems are connected and use the same Mechanical instance, boundary conditions can be copied by dragging and dropping from the Implicit to the Explicit system. This is the initial step in transferring the boundary conditions, but before the Explicit solve, adjustments to the boundary condition definitions must be made.

3.3.5.1. Adjusting Load Cases for Reasonable Run Times Unlike the Explicit solver, the Implicit solver has no real dependency on inertia (in the static structural solver). That is why the load cases in Implicit are usually 1 second per step, which is an arbitrary amount. Altering this value does not really have any effect on the solution. The Explicit Dynamics solver, on the other hand, uses time as its main reference for the calculations since the duration of the events in an Explicit problem are extremely short, and it is one of the most important aspects of the solve (see Timestep Controls (p. 112)). As a starting point, a time scale factor of 100 or 1000 should be used; that is, 1 second in the implicit solver becomes 1E-2 or 1E-3 seconds in the explicit solver. The main thing to monitor are the velocities in the model. A good velocity to aim for is 5 m/s; it is not too low going into the static setup realm and it is not too high which would introduce significant inertial effects.

108

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting up the Explicit Dynamics Analysis

3.3.5.2. Missing Boundary Conditions from Explicit Dynamics There are a few Mechanical boundary conditions that do not exist in Explicit Dynamics. Some of them can be simulated by using other boundary conditions. These include cylindrical support, frictionless support, bolt pretension and others. Refer to the table below for ways to simulate some of the missing boundary conditions. Boundary condition

Implicit solver

Explicit solver

Frictionless support

Available

Available/ Simulated by using an equivalent symmetry plane (rigid behavior) or by creating displacement with fixed components to provide the desired constraint.

Bolt pretension

Available

Pre-stress the bolt by using load steps: • Cut the bolt geometry in half with a small gap. • Scope a translational joint to both cut planes. • Load step 1: Apply a (ramped) force on the cut planes. • Load step 2: Lock the joint with a velocity joint load.

Cylindrical support

Available

Simulated using remote displacement to restrict rotation.

Displacement (step applied)

Available

Simulated using different boundary conditions to give the same movement - force, velocity etc.

Pressure (tabular variable value)

Available

Simulated using the Magnitude - Function setting to create a function giving the same values across the scoped geometry.

3.3.5.3. Avoiding Conflicting Boundary Conditions When the scoping of two (or more) boundary conditions is done on two (or more) intersecting planes, the constraints on the shared edge (node) may trigger an error. The Explicit solver will only allow more than one boundary condition to be applied to the same edge in the following scenarios. Note that each of the following scenarios is evaluated for each of the load steps defined under analysis settings. • Both boundary conditions are defined on the same coordinate system and the combination of constraints do not conflict. • Both boundary conditions are defined on mutually orthogonal cartesian coordinate systems and the combination of constraints do not conflict. • Both boundary conditions are defined on cylindrical coordinate systems whose z-axes are aligned with one another and the combination of constraints do not conflict. • Both boundary conditions are defined on cartesian coordinate systems that have one axis aligned (and the constraints in the two boundary conditions in that direction do not conflict) but the other two do not. This scenario is depicted in Figure 1 where the y axis in CS1 is parallel to the y axis in CS2. Then the allowed constraints in the remaining axes x and z in both CS1 and CS2 are:

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

109

Transforming an Implicit Model to run in Explicit Dynamics – If the x and z constraints in one boundary condition are both free (then there are no restrictions on the constraints in x and z on the other boundary condition). – Where all of the constraints in x and z in both boundary conditions are either fixed or free

Figure depicting two boundary conditions whose scoping shares a common edge and that are defined on coordinate systems that are not orthogonal. BoundaryCondition1 is defined on the coordinate system (CS1) shown on the left. BoundaryCondition2 is defined on the coordinate system (CS2) shown on the right. CS1 and CS2 both have their y axes aligned, but the x in CS1 is not orthogonal to x in CS2, and z in CS1 is not orthogonal to z in CS2. When the two coordinate systems share one axis in the same direction and the other two sets of two axes are not aligned, the constraints allowed on these remaining four axes are those shown in the table below marked with green checkmark.

Note • Two functions that are the same function but are expressed using a different string (including differences in white space) may cause conflicts which cannot be resolved by the Explicit Dynamics solver (although they are not technically conflicting constraints).

110

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Analysis Settings • The check for conflicting boundary conditions becomes more stringent if multiple load steps are defined under analysis settings and one (or more) of these boundary conditions is deactivated during the analysis. An additional conflict may exist if the solver is not able to combine the active and deactivated boundary condition into a single new boundary condition and apply it to the common nodes. An error along the following lines will be given, followed by a suggestion to circumvent the conflict: The coordinate systems of two boundary conditions are compatible (or incompatible) but a deactivated load step causes the values of the boundary conditions to conflict.

3.3.5.4. Initial Conditions The Initial Conditions object in the Explicit Dynamics system can be helpful when certain aspects of the Implicit model cannot be directly recreated. It is a simple initial velocity, angular or directional, that is scoped to a body and is assigned at the initial cycle. This can be altered freely by different boundary conditions and events during the solve; its value is not constrained or limited. Another use for Initial Conditions is adding a pre-stress, usually from an Implicit solve. This is useful when an extensive complex combined simulation is required, and is not intended for situations where you need to run the same model setup with the two different solvers. Figure 3.12: Initial Conditions Object

3.4. Analysis Settings The final step before running the Explicit simulation is checking the options in the Analysis Settings. They are very different compared those used for the Implicit solver, and there are many more options. Most of them have defaults that work fine for quasi-static models but there are a few important options to focus on.

3.4.1. Analysis Setting Preference This setting has various options, but for quasi static simulations the two to use are Quasi Static and Low Velocity. The default Program Controlled option should be used initially; it automatically detects the best default options for the simulation settings. Both preference options require an input for the mass scaling (discussed later) and apply changes to various parts of the setup to suit the velocity mode.

3.4.2. Step Controls When using the Explicit solver to investigate a problem that was originally solved using the Implicit solver, you should set up the analysis to take advantage of the features unique to the Explicit solver. As discussed earlier, the Explicit simulation takes into account the inertial forces and one of its most important parameters is the solve time (not to be mistaken with the actual run time it takes for the Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

111

Transforming an Implicit Model to run in Explicit Dynamics model to solve). The Explicit simulation can be seen as a chunk of the real time of an event that is slowed down as if using a high speed camera. The time values that the Explicit solver usually works with are much smaller than 1 second. For these quasi-static Implicit to Explicit simulations, we are working with a total time of around one millisecond to 1 second.

3.4.2.1. End Time As stated earlier, one of the main parameters governing the solution is the time. The End Time defines the time frame which the solver simulates, starting from zero going up to the End Time value. The End Time should match the last entry in any of the boundary conditions tabular data time setting. This is a good place to estimate the maximum velocity in the model—if there are any displacements or deformations, dividing the distance covered by the end time gives a good estimate for the initial run. An end time target would be between 0.001 seconds and 1 second for the quasi-static simulations. Typically the explicit models are constrained by the end time so the Maximum Number of Cycles should be left at the default value or set to a very large number (for example, 1E7). Each cycle is a piece of the solution time with the length of the current timestep and it is the constraint for a single iteration. It has a variable time value depending on the settings and the events during the solve so it is by no means guaranteed to be consistent. The maximum cycle number is rarely used to control the solution in explicit dynamics. Its most common use is when you need to do a short solution to check something in the setup and the Maximum Number of Cycles is set to a very small value (10,100,1000 etc). Even if we calculate the exact number of cycles we need and we have set a time step value, it is always better to use the end time to determine when the solve will terminate.

3.4.2.2. Timestep Controls The timestep is the time increment at which the solve advances, and the solve time between two calculation cycles. The smaller the timestep is and the more complex the calculations per cycle are (dense mesh, material models etc.) the longer run time the solution will take. Having control over the timestep is crucial for achieving an effective simulation. There are numerous ways to keep track of and control the timestep. The governing factor for the timestep value is the smallest mesh element size and its mass. The timestep is calculated based on sound speed (which depends on density and material properties) and it needs to have a small enough value to accurately simulate the stress waves traveling through the body. The following equation is used to determine the minimum timestep:

where is the timestep safety factor (usually not changed from default value), is the element characteristic dimension (determined by smallest element size) and is the sound speed in the material (depending on density and elasticity).

112

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Analysis Settings Figure 3.13: Analysis Settings - Step Controls

The initial, minimum, and maximum time step values usually should be left as default (Program Controlled), except in a few cases. The Minimum Time Step value is sometimes set to a very small number to allow the solve to continue to run and not abort with the message: Time step too small. You would set the Minimum Time Step like this when the time step is expected to become much smaller than its initial value during the solve due to large deformations or complex contact. When you set the value, this overrides the minimum time step conditions determined by the solver, based on the initial setup. This user-defined minimum time step value might lead to a much longer analysis run time. Another case where user input might be required is when the analysis time step is determined by an element of a rigid body. A reasonably smaller time step should be used to prevent the simulation going forward using too large steps and becoming unstable. This can be achieved by a user defined Maximum Time Step value. Figure 3.14: Default Solution Information display during solve with the estimated time remaining highlighted in yellow

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

113

Transforming an Implicit Model to run in Explicit Dynamics When you view the Solution Information while the solve is running, the Est. Clock Time Remaining can be observed. This is an new concept if you've only previously used the Implicit solver. This value gives an estimate of the remaining time needed to finish the solution. After the initial few cycles, and providing there are no abnormal deformations and unexpected events in the model during the solve, this value is quite accurate. It is based upon the time needed to calculate each cycle and the expected remaining number of cycles. Usually when dealing with hyperelastic materials with a lot of deformation or other special cases, this remaining time will get a lot higher once the part of the simulation dealing with the large deformations is reached. This estimated time is also a good way to judge how changes to the mesh and setup will affect the solution time. After each change the model can be solved until a certain cycle number then interrupted, and the estimated time can be compared. This gives a rough estimate since it does not take into account any possible difficulties which might arise, but it is a useful tool for comparison.

3.4.2.3. Restarting an Analysis As discussed earlier, the simulation will create a number of restart files that can be used to resume the solve following an interruption. There are a few things to consider when restarting a simulation. First, you have to make sure that the run will restart from the correct point. Set the Resume From Cycle value, which is based on the cycle number rather than simulation time. Another thing to note is that the boundary conditions cannot be altered before restarting and if, for example, the end time is extended and the user wants to continue the run, all of boundary conditions will assume they are kept constant at the last value of the normal solve time (before the time extension). Any change made to the setup while the solve is interrupted will mean that the restart is no longer possible. You must be careful when examining the interrupted solve results.

3.4.3. Solution Stability Although, there are no convergence criteria and stability requirements in the Explicit solver, there are tools to ensure the user gets a good solution. These mainly control the time step, excessive deformations, and unwanted oscillations. These tools are discussed in this section.

3.4.3.1. Mass Scaling The use of mass scaling can be very helpful, especially in these quasi static simulations. It is useful in cases where we need an area of interest to be more densely meshed, as is commonly seen in the Implicit solver's mesh. Automatic Mass Scaling increases the mass of the smallest elements which in turn increases the required time step. Mass scaling is automatically switched on when the Quasi Static or Low Velocity analysis types are chosen. When using Mass Scaling, there are several parameters to consider, but the primary one is the Minimum CFL Time Step. This should be set to the minimum desired value of the time step, but this has to be based on the standard time step that the model would use without scaling. Usually the mass scaling is set up after the initial run. This minimum time step is usually within the region of 5-10 times larger than the normal time step. The larger the increase that's required, the more scaling must be put in. Sometimes the default maximum scaling values have to be increased to achieve the minimum time step, but when this is done, emphasis has to be put on ensuring that the mass values are still realistic and do not interfere with the results. It is recommended that the default maximum scaling values are not changed.

114

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Analysis Settings

3.4.3.2. Erosion Another important tool is erosion. This allows for elements from the mesh to be removed and separated from the rest of the mesh in certain cases. There are three criteria that can be enabled to cause element erosion—maximum strain, minimum time step, and material failure. The most commonly used is the On Geometric Strain Limit erosion. It is used when excessive deformations are expected, and prevents the solution from stopping because of nodes displaced an abnormal distance away from the rest of the element or heavy deformation. Once the solve with erosion is completed, you can see where the eroded elements are and decide how the solution can be improved. The erosion criteria On Material Failure is commonly used to realistically simulate the failure of materials based on their definitions. This can be due to stress, strain, shear or any other mode of failure that is defined in the material data. The last criterion is the On Minimum Element Time Step erosion. This is a very crude way of controlling the minimum time step by simply removing the elements which would otherwise yield a smaller computational time step than desired. By default, the Retain Inertia of Eroded Material is set to Yes. This allows you to examine the erosion process and follow the debris distribution (the defaults are different for Low Velocity and Quasi Static simulation types). An example of eroded material can be seen in the following figure. Figure 3.15: Example of Eroded Material in a Model Simulating a Bullet going Through a Vase (eroded elements colored red)

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

115

Transforming an Implicit Model to run in Explicit Dynamics

3.4.3.3. Damping Sometimes, especially when highly flexible materials are present, constant frequency oscillations can arise in the Explicit simulation. This can be avoided by the use of Static Damping. A damping value is calculated by dividing double the time step by the longest period of oscillation in the system. In other words, this value should be aimed at damping the slowest vibration in the analysis. When you are not sure of the value that should be used, it is best to start from the smallest damping valude to prevent overdamping. If the simulation is underdamped there will still be vibration visible, but when the simulation is overdamped it can lead to longer end time requirement and skewing of results. The other damping controls should be left at their defaults.

3.4.4. Output Controls The Output Controls section in an Explicit Dynamics system is important for the results visualization and post processing. There are three types of output controls for saving results, restart points, and results tracker data. The Result Number of Points controls how the visualization of the chosen solution tools will look. This determines how many and how frequent the evaluation points will be; these will later become frames in the post-processing animation. Having a lot of points that are tightly packed will increase the total solution run time. The Restart Number of Points are useful when the simulated model goes through complex actions and it is important for you to be able to rerun the simulation from a certain point. The evaluation points are usually much less dense than the results points and one restart file is created at the end of the solve, or at a solve interruption. The results trackers save very specific information from small, localized areas and are important for monitoring places of interest. Depending on the setup, they can be computationally heavy, so they are usually only used in the initial runs to aid in setting up the model as desired. Figure 3.16: Analysis Settings - Output Controls

The defaults are Equally Spaced Points for the results and the restart files, and saving is based on Cycles for the result trackers. In general, these defaults are fine for the initial Explicit run. Since the number of cycles is initially unknown, if any changes are made to the defaults they should generally use the Equally Spaced Points options which will automatically distribute the points.

116

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Solution Information

3.5. Solution Information Once the solve has been initiated, there are a number of ways to monitor how well it is performing. Different data and values can give clues as to which parts of the simulation are going well and which aren't. You can also see what might be the reason for a slowdown in the simulation. The main monitoring tool is the Solver Output viewed from the Solution Information object. Solution output is constantly updated, providing information for each cycle - the cycle number, the simulation time, the time step (time increment), the progress (in percent) and the estimated run time remaining. An indication of an issue here would be inconsistency in the estimated time remaining or a decrease of the time increment. This can be more precisely monitored by viewing the Time Increment graph of the time step value with respect to simulation time. There are also a number of graphs available under the Solver Output to help you determine the health of your solve. Energy error can also indicate problems in the simulation. You can keep track of it with the Energy Conservation graph (seen in Figure 3.17: Graph of Energy Conservation for an Explicit Simulation (p. 118)) which also shows the total energy and work done in the solve. The default threshold is 10%; any error above this will terminate the solve. The reference value for the energy is usually the zero cycle. These values can be altered in the Analysis Settings. Sometimes it is useful to see what is happening in the simulation even though there is a large energy error. There are two ways this can be achieved - either increasing the reference cycle so that its value is higher than or equal to the maximum number of cycles, or increasing the Maximum Energy Error value. This should only be done to observe what is happening during the solve that gives rise to the error. The results of a simulation completed with high energy errors should not be considered accurate. The Momentum Summary graph is also useful for monitoring the dynamics of the simulation, and it can give some indication of a stability problem. The last monitoring tool is the Energy Summary graph. High values of hourglass energy here usually indicate problems with the mesh. This graph also shows the kinetic energy during the solve. The value should be insignificant with respect to the model in the quasi static simulations to ensure that inertial effects are not altering the results.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

117

Transforming an Implicit Model to run in Explicit Dynamics Figure 3.17: Graph of Energy Conservation for an Explicit Simulation

Another way to monitor the solve is through Results Trackers. These update in real time, giving information about their values for each cycle, or at whatever frequency is set in the Output Controls (p. 116) in the Analysis Settings. These trackers have to be defined before the start of a solve, and in order to suppress or remove them they have to be cleared from the data. They cannot be added at a restart point or at the end of a solve. The other results tools can only be examined after the solve stops (see Result Sets (p. 119)). If a live picture of what is happening during the solve is required, the Autodyn component system can be used. It can refresh the visualization of the solution as often as each cycle and can show various details about whole bodies like velocity vectors, stresses, other data values, and more. When the solve is initiated, the checks done before the first cycle can find problems and produce warning or error messages. These are usually related to the material models, the boundary conditions setup, or the restart options. When a General failure error is seen, this usually means there are possible problems with the licensing or the remote solve manager, but it can also signify other problems. Errors or warnings can also be seen during or after the solve. The two primary reasons for a terminated solve are the Energy error exceeded and Time step too small errors. Both of them can mean a variety of problems - meshing, high deformation, incorrectly applied forces, etc. Usually observing the results up to that point or using the erosion or error options to bypass the termination should give an indication of what the problem might be.

3.6. Postprocessing Evaluating the results is the most crucial point of any simulation. The explicit dynamics solver offers many tools for efficient post processing. This gives not only quantifiable results but also, through observing animations and graphs, indication of what went on during the simulation and how well it represents the real experimental situation.

118

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing

3.6.1. Result Trackers As stated in the previous section, the result trackers can be a useful tool for initial evaluation of the setup. They are usually scoped to strategic locations to give detailed information on the physical parameters. The trackers are the most suitable tool to use to evaluate the oscillations and vibrations in a simulation, and are used for calculating the required damping coefficient. Because of their dense data points, the graphs created are very smooth and accurate, suitable for even very small amplitude oscillations. Depending on the type, they can be scoped to different geometry entities and evaluate a variety of parameters. The trackers are also useful for evaluating contact forces and local energy values.

3.6.2. Result Sets One of the main tools used for post processing are the result sets. They can help you evaluate stress, strain, deformation, etc. They work in a similar way as in the Implicit simulation, with all of the controls and settings being the same. All of the scoping, scaling, and contouring options should also be familiar. Generally, there are a fewer number of result sets and tools than available for the Implicit solver, similarly to the boundary conditions. The sets can be added before or after the simulation and then evaluated. Apart from the standard sets of results, you can also include User Defined Result (p. 93) objects. As the name suggests, this result can be customized to suit your needs, and can use a variety of variables (seen by clicking Worksheet from the View drop-down of the Solution Context tab). It can also evaluate expressions using any of the variables. These results are useful in situations where you want to evaluate something in a similar way as the results trackers but scoped to whole parts or the whole model. It can also be used to compare manually calculated values from an equation expression (using the simple variables), which does not have an equivalent in the standard results. Animating the results is done using the same tools as the Implicit solver, but because of the nature of the Explicit solver, this gives much more detailed and valuable information about the solution. It is important to keep track of the results point density and restart points in order to have an animation which best represents the solution behavior. The animations are very useful because they are based on the simulation time, unlike the implicit simulations. This can be helpful to adjust the setup and the boundary conditions following the initial run. Furthermore, the animation can give an indication of which parts are oscillating and need damping; you can scope trackers to them to determine the frequency. The graph of a deformation result set can be seen in the following figure.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

119

Transforming an Implicit Model to run in Explicit Dynamics Figure 3.18: Deformation Graph (with respect to simulation time) and Results Table

Note If the Implicit solver has the result scaling setting at anything other than True Scale (default) this will not be transferred to the Explicit solver results. This may be the reason if you observe very different deformations at first glance.

3.6.3. Improving your Simulation There are many parameters you can check to ensure the simulation has achieved the desired output. Most of them are indicators that something went wrong rather than that something is working as it should. Start with the stability of the time step, the energy errors, and unexpected erosion. These should be examined and the reasons behind any unexpected results should be investigated. Using the animations to determine the eroding areas can show a number of issues either with the mesh, the setup, or the geometry. Missed contact is also something to watch out for in the animations, especially because the Explicit solver does not have a specific contact tool like the Implicit simulation. Such problems can be addressed by increasing the mesh density or examining the overlap of the parts. It is also useful to examine parts of the model using a section plane. This might give insight to some problems which are not obvious at first glance. It is important for these quasi-static simulations that the velocity values in the model are in the range of 1 to 10 m/s. If they are too low, it means that the Explicit solver might not be modeling the activity correctly because it is out of range of its normal velocity modes. If they are too high, this means that higher stresses and strains may have been introduced due to inertial and shock effects. Evaluating the velocity also gives indication of how close the simulation is to the real, experimental expectations. Ideally, the solver should simulate the velocities that are desired for the actual mechanism at work. This is not always possible but it is the target to aim for. Increasing the end time while keeping the same displacement values, for example, will decrease the velocities in the simulation but will also increase the run time required. The solution output includes files that also hold information, though more technical and not as easy to understand as the details in the graphical interface. One example is the .prt file which gives extensive information about the setup and the solve, including which operations took more CPU time, the energy and momentum balance, and errors. After careful examination of the results, you can start working on model improvements. Optimization may include: stabilization (damping), modifying the mesh to give more consistent results, modifying displacement boundary conditions, adding or removing constraints, and so on. The Explicit solver has extensive capabilities for postprocessing, allowing you to get the information you need for making necessary adjustments.

120

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 4: Applying Pre-Stress Effects for Explicit Analysis Because an Explicit Dynamics analysis is better suited for short duration events, preceding it with an Implicit analysis may produce a more efficient simulation, especially for cases in which a generally slower (or rate-independent) phenomenon is followed by a much faster event, such as the collision of a pressurized container. To produce this combination, you can define pre-stress as an initial condition in an Explicit Dynamics system, specifying the transfer of either displacements only or the more complete Material State (displacements, velocities, stresses, and strains), from a static or transient structural analysis to an Explicit Dynamics analysis. Characteristics of the Implicit to Explicit pre-stress feature: • Applicable to 3-D analyses only. • The Material State mode, for mapping stresses, plastic strains, displacements, and velocities is valid for solid models only. • The displacements only mode is valid for solid, shell, and beam models. • The same mesh is required for both Implicit and Explicit analyses and only low order elements are allowed. If high order elements are used, the solve will be blocked and an error message will be issued. • For a nonlinear Implicit analysis, the Strain Details view property in the Output Controls category under the Analysis Settings object must be set to Yes because plastic strains are needed for the correct results.

4.1. Recommended Guidelines for Pre-Stress Explicit Dynamics The following guidelines are recommended when using pre-stress with an Explicit Dynamics analysis: • Lower order elements must be used in the static or transient structural analysis used to pre-stress the Explicit Dynamics analysis. To do so, set the Mesh object property, Element Order (Defaults category), to Linear. • On the Brick Integration Scheme of all relevant bodies, use the Reduced option, to provide the most consistent results between the Static Structural or Transient Structural system and the Explicit Dynamics system. Such a selection amounts to a single integration point per lower order solid element. • For models containing Line or Surface bodies, the data transfer is limited to displacements only. In this mode, under Analysis Settings, the Static Damping option (under Damping) should be used to remove any dynamic oscillations in the stress state due to the imposed static displacements. • The temperature state is also transferred to the Explicit Dynamics analysis. The Unit System is taken care of automatically, and Internal Energy due to difference in temperature will be added to each element based on: Einternal = Einternal + Cp(T-Tref) Where:

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

121

Applying Pre-Stress Effects for Explicit Analysis Cp = specific heat coefficient Tref = room temperature Note that stresses may still dissipate because the thermal expansion coefficient is not taken into account in the Explicit Dynamics analysis. Example - Drop Test on Pressurized Container:

Pre-stress condition:

Transient stress distribution during drop test:

122

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Pre-Stress Object Properties

4.2. Pre-Stress Object Properties Mode Displacement Node-based displacements from a static analysis are used to initialize the Explicit node positions. These displacements are converted to constant node-based velocities and applied for a pre-defined time in order to obtain the required displaced coordinates. During this times, element stresses and strains are calculated as normal by the Explicit solver. Once the displaced node positions are achieved, all nodebased velocities are set to 0 and the solution is completely initialized. This option is applicable to unstructured solids (hexahedral and tetrahedral), shells, and beams. Time Step Factor The initial time step from the explicit solution is multiplied by the time step factor. The resulting time is used with the nodal displacements from the ANSYS Mechanical analysis to calculate constant nodal velocities. These nodal velocities are applied to theExplicit model over the resulting time in order to initialize the Explicit nodes to the correct positions. Material State Node-based displacements, element stresses and strains, and plastic strains and velocities from an Implicit solution are used to initialize an Explicit analysis at cycle 0. This option is applicable to results from a linear static structural, nonlinear static structural, or transient dynamic Mechanical system. The ANSYS solution may be preceded with a steady-state thermal solution in order to introduce temperature differences into the solution. In this case, the accompanying thermal stresses due to the thermal expansion coefficient will be transferred but may dissipate since the thermal expansion coefficient is not considered in an Explicit analysis. This option is only applicable to unstructured solid elements (hexahedral and tetrahedral). Pressure Initialization From Deformed State The pressure for an element is calculated from its compression, which is determined by the initial displacement of the element's nodes. This is the default option and should be used for almost all Implicit-Explicit analyses. From Stress State The pressure for an element is calculated from the direct stresses imported from the implicit solution. This option is only available for materials with a linear equation of state. If the pressure Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

123

Applying Pre-Stress Effects for Explicit Analysis for an element is already initialized, this calculation will be ignored. This is for a pre-stress analysis from an Implicit solution that has been initialized from an INISTATE command and has an .rst file with all degrees of freedom fixed. Time The time at which results are extracted from the Implicit analysis.

124

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 5: Using Explicit Dynamics to Define Initial Conditions for Implicit Analyses 5.1. Transfering Explicit Results to MAPDL It is possible to initialize a Mechanical APDL implicit analysis from the results of an Explicit Dynamics analysis by using features of the Mechanical APDL command language. You can obtain results from the Explicit analysis by using an Explicit Dynamics Workbench system followed by a Design Assessment system that uses a python script to extract the results and write the additional Mechanical APDL commands to a file. A Commands object can be added to the Transient or Static Structural system to include the execution of the Mechanical APDL commands from the file. A full description of the process follows, and an example has been detailed in the Design Assessment documentation.

Note This method is currently limited to cases where there is no change in mesh topology between the start of both the Explicit and Implicit analyses.

Follows these steps to perform the Explicit-to-Implicit analysis: 1. Add an Explicit Dynamics analysis to the Workbench Project Schematic. 2. Add a Design Assessment system to the Explicit Dynamics system in the Project Schematic. You will create an XML Definition File for the Design Assessment system that specifies a python script to be run on “solve”. Set your Design Assessment type to be User Defined, and choose the XML Definition File that you created. 3. Create the python script to write to a file the necessary Mechanical APDL commands to initialize the implicit model. The script should: a. Get nodal deformations, stresses, and plastic strains from the end of the Explicit Dynamics analysis using the Design Assessment API. b. Write the Mechanical APDL commands:

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

125

Using Explicit Dynamics to Define Initial Conditions for Implicit Analyses i.

Enter the preprocessor. Command(s): /PREP7

ii. Get initial nodal locations from the Implicit analysis. Command(s): *GET, and so on iii. Redefine Implicit elements to the deformed configuration by adding values from steps 3(a) and 3(b)(ii). Command(s): N, and so on iv. Specify reduced element integration if using solid elements. Workbench automatically converts explicit elements to Implicit elements. However, due to Explicit elements having only one integration point per element, it is necessary to specify this manually for the Implicit elements in order that results can be transferred between the two analyses.

Note Explicit uses SHELL163 for shells and SOLID164 for solids. These get automatically converted to SHELL181 and SOLID185 respectively. Command(s): ET, 1, 185, , 1 and so on v. Reenter the solution processor. Command(s): /SOLU vi. Set any necessary constraints on the model by modifying or adding to the boundary conditions defined during the Explicit analysis (for example, in a metal forming analysis, you need to constrain the blank). Command(s): D, and so on vii. Import stresses from the Explicit Dynamics analysis. For solids, this will be one set of values per element. For shells, this will be one set of values for every layer within each element. Command(s): INISTATE, SET, DTYPE, STRESS Command(s): INISTATE, DEFINE, and so on viii.Import plastic strains and accumulated equivalent plastic strain from Explicit Dynamics analysis Command(s): INISTATE, SET, DTYPE, EPPL Command(s): INISTATE, DEFINE, and so on Command(s): INISTATE, SET, DTYPE, PLEQ Command(s): INISTATE, DEFINE, and so on ix. Solve analysis. Command(s): SOLVE

126

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Transfering Explicit Results to MAPDL 4. Add an Implicit system, either Static Structural or Transient Structural. In this system include the file that was created with the Design Assessment script by adding a Commands object that reads in the file that was created by the python script. Command(s): /INPUT, and so on 5. When post processing, view results by issuing Mechanical APDL commands in order to view results with the initial deformed mesh. When post processing in the standard Workbench view, results will appear to deform in the opposite direction to the Explicit Dynamics analysis because it has not taken into account the redefined deformed mesh. To create graphic files showing the correctly deformed mesh, add a new Commands object under the Solution branch of the Implicit analysis. Command(s): /SHOW, PNG Command(s): PLNSOL, and so on 6. When using shell elements, another step must be included in order to view the results. Shells only accept INISTATE in the element coordinate system, and so when the stresses are initialized they are not in the global coordinate system. Therefore, in order to view the results correctly, you must first change the solution to plot the results in the solution coordinate system. Command(s): /VIEW, , , -1 Command(s): /SHOW, PNG Command(s): PLNSOL, and so on

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

127

128

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 6: Explicit Dynamics Theory Guide This chapter describes the theoretical basis of the Explicit Dynamics system available in Workbench. The following topics are covered in this chapter: 6.1. Why use Explicit Dynamics? 6.2. What is Explicit Dynamics? 6.3. Analysis Settings 6.4. Model Size Limitations in Explicit Dynamics 6.5. References

6.1. Why use Explicit Dynamics? The Explicit Dynamics system is designed to enable you to simulate nonlinear structural mechanics applications involving one or more of the following: • Impact from low [1m/s] to very high velocity [5000m/s] • Stress wave propagation • High frequency dynamic response • Large deformations and geometric nonlinearities • Complex contact conditions • Complex material behavior including material damage and failure • Nonlinear structural response including buckling and snapthrough • Failure of bonds/welds/fasteners • Shock wave propagation through solids and liquids • Rigid and flexible bodies Explicit Dynamics is most suited to events which take place over short periods of time, a few milliseconds or less. Events which last more than 1 second can be modeled; however, long run times can be expected. Techniques such as mass scaling and dynamic relaxation are available to improve the efficiency of simulations with long durations.

6.2. What is Explicit Dynamics? An overview of the solution methodology used in an Explicit Dynamics simulation is provided in this section. 6.2.1.The Solution Strategy 6.2.2. Basic Formulations 6.2.3.Time Integration 6.2.4. Wave Propagation Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

129

Explicit Dynamics Theory Guide 6.2.5. Reference Frame 6.2.6. Explicit Fluid Structure Interaction (Euler-Lagrange Coupling)

6.2.1. The Solution Strategy In an Explicit Dynamics solution, we start with a discretized domain (mesh) with assigned material properties, loads, constraints and initial conditions. This initial state, when integrated in time, will produce motion at the node points in the mesh. • The motion of the node points produces deformation in the elements of the mesh • The deformation results in a change in volume (hence density) of the material in each element • The rate of deformation is used to derive material strain rates using various element formulations • Constitutive laws take the material strain rates and derive resultant material stresses • The material stresses are transformed back into nodal forces using various element formulations • External nodal forces are computed from boundary conditions, loads and contact (body interaction) • The nodal forces are divided by nodal mass to produce nodal accelerations • The accelerations are integrated Explicitly in time to produce new nodal velocities • The nodal velocities are integrated Explicitly in time to produce new nodal positions • The solution process (Cycle) is repeated until a user defined time is reached

6.2.2. Basic Formulations An introduction to the basic equations which are solved in Explicit Dynamics is provided in this section. 130

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

What is Explicit Dynamics? 6.2.2.1. Implicit Transient Dynamics 6.2.2.2. Explicit Transient Dynamics

6.2.2.1. Implicit Transient Dynamics The basic equation of motion solved by an implicit transient dynamic analysis is (6.1) Where: m = mass matrix c = damping matrix k = stiffness matrix F(t) = load vector At any given time, t, these equations can be thought of as a set of "static" equilibrium equations that also take into account inertia forces and damping forces. The Newmark time integration method (or an improved method called HHT) is used to solve these equations at discrete time points. The time increment between successive time points is called the integration time step.

6.2.2.2. Explicit Transient Dynamics The partial differential equations to be solved in an Explicit Dynamics analysis express the conservation of mass, momentum, and energy in Lagrangian coordinates. These, together with a material model and a set of initial and boundary conditions, define the complete solution of the problem. For the Lagrangian formulations currently available in the Explicit Dynamics system, the mesh moves and distorts with the material it models and conservation of mass is automatically satisfied. The density at any time can be determined from the current volume of the zone and its initial mass (6.2) The partial differential equations that express the conservation of momentum relate the acceleration to the stress tensor σij .

(6.3)

Conservation of energy is expressed via: (6.4) These equations are solved explicitly for each element in the model, based on input values at the end of the previous time step. Small time increments are used to ensure stability and accuracy of the solution. Note that in Explicit Dynamics we do not seek any form of equilibrium; we simply take results from the previous time point to predict results at the next time point. There is no requirement for iteration.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

131

Explicit Dynamics Theory Guide In a well-posed Explicit Dynamics simulation, mass, momentum, and energy should be conserved. Only mass and momentum conservation is enforced. Energy is accumulated over time and conservation is monitored during the solution. Feedback on the quality of the solution is provided via summaries of momentum and energy conservation (as opposed to convergent tolerances in implicit transient dynamics).

6.2.3. Time Integration In this section, the Explicit Dynamics time integration scheme is described and compared with an implicit formulation. 6.2.3.1. Implicit Time Integration 6.2.3.2. Explicit Time Integration 6.2.3.3. Mass Scaling

6.2.3.1. Implicit Time Integration For implicit time integration, ANSYS solves the transient dynamic equilibrium equation using the Newmark approximation (or an improved method known as HHT). For more information, see Transient Analysis. For linear problems, the implicit time integration is unconditionally stable for certain integration parameters. The time step size will vary to satisfy accuracy requirements. For nonlinear problems: • The solution is obtained using a series of linear approximations (Newton-Raphson method), so each time step may have many equilibrium iterations. • The solution requires inversion of the nonlinear dynamic equivalent stiffness matrix. • Small, iterative time steps may be required to achieve convergence. • Convergence tools are provided, but convergence is not guaranteed for highly nonlinear problems.

6.2.3.2. Explicit Time Integration The Explicit Dynamic solver uses a central difference time integration scheme (often referred to as the Leapfrog method). After forces have been computed at the nodes of the mesh (resulting from internal stress, contact, or boundary conditions), the nodal accelerations are derived by equating acceleration to force divided by mass. Therefore the accelerations are (6.5) Where: are the components of nodal acceleration (i=1,2,3) are the forces acting on the nodal points are the components of body acceleration m is the mass attributed to the node.

132

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

What is Explicit Dynamics? With the accelerations at time n determined, the velocities at time

are found from (6.6)

and finally the positions are updated to time n+1 by integrating the velocities (6.7) The advantages of using this method for time integration for nonlinear problems are: • The equations become uncoupled and can be solved directly (explicitly). There is no requirement for iteration during time integration. • No convergence checks are needed because the equations are uncoupled. • No inversion of the stiffness matrix is required. All nonlinearities (including contact) are included in the internal force vector. To ensure stability and accuracy of the solution, the size of the timestep used in Explicit time integration is limited by the CFL (Courant-Friedrichs-Lewy [1]) condition. This condition implies that the timestep be limited such that a disturbance (stress wave) cannot travel farther than the smallest characteristic element dimension in the mesh, in a single timestep. Thus the timestep criteria for solution stability is (6.8) Where Δt is the time increment f is the stability timestep factor (= 0.9 by default) h is the characteristic dimension of an element c is the local material soundspeed in an element The element characteristic dimension, h is calculated as follows: Table 6.1: Characteristic Element Dimensions Hexahedral/Pentahedral The volume of the element divided by the square of the longest diagonal of the zone and scaled by Tetrahedral

The minimum distance of any element node to it’s opposing element face

Quad Shell

The square root of the shell area

Tri Shell

The minimum distance of any element node to it’s opposing element edge

Beam

The length of the element

The time steps used in Explicit time integration will generally be smaller than those used in Implicit time integration.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

133

Explicit Dynamics Theory Guide For example, for a mesh with a characteristic dimension of 1mm and a material soundspeed of 5000m/s. The resulting stability time step would be 0.18µ seconds. To solve this simulation to a termination time of 0.1 seconds will require 555,556 time increments.

Note The minimum value of h/c for all elements in the model is used to calculate the time step that will be used for all elements in the model. This implies that the number of time increments required to solve the simulation is dictated by the smallest element in the model. Care should therefore be taken when generating meshes for Explicit Dynamics simulations to ensure that one or two very small elements do not control the timestep. The patch-independent meshing methods available in Workbench will generally produce a more uniform mesh with a higher timestep than patch-dependent meshing methods.

6.2.3.3. Mass Scaling The maximum timestep that can be used in Explicit time integration is inversely proportional to the soundspeed of the material, hence directionally proportional to the square root of the mass of material in an element (6.9) Where Cii is the material stiffness (i=1,2,3) ρ is the material density m is the material mass V is the element volume By artificially increasing the mass of an element, one can increase the maximum allowable stability timestep, and reduce the number of time increments required to complete a solution. When mass scaling is applied in an Explicit Dynamics system, it is applied only to those elements which have a stability timestep less than a specified value. If the model contains a relatively small number of small elements, this can be a useful mechanism for reducing the number of time steps required to complete an Explicit simulation.

Note Mass scaling changes the inertial properties of the portions of the mesh to which scaling is applied. The user is responsible for ensuring that the model remains representative for the physical problem being solved.

6.2.4. Wave Propagation The Explicit Dynamics systems are particularly well suited to capturing various types of wave propagation phenomena in solid and liquid materials. 6.2.4.1. Elastic Waves 6.2.4.2. Plastic Waves

134

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

What is Explicit Dynamics? 6.2.4.3. Shock Waves

6.2.4.1. Elastic Waves Different types of elastic waves can propagate in solids depending on how the motion of points in the solid material is related to the direction of propagation of the waves (Meyers [2]). The primary elastic wave is usually referred to as the longitudinal wave. Under uniaxial stress conditions (i.e. an elastic wave traveling down a long slender rod), the wave propagation speed is given by (6.10) For the more general three-dimensional case, the additional components of stress lead to the more general expression for the primary longitudinal elastic wave speed (6.11) The secondary elastic wave is usually referred to as the distortional/shear wave and it’s propagation speed can be calculated as (6.12) Other forms of elastic waves include surface (Rayleigh) waves, Interfacial waves and bending (or flexural) waves in bars/plates. Further details are provided by Meyers [2].

6.2.4.2. Plastic Waves Plastic (inelastic) deformation takes place in a ductile metal when the stress in the material exceeds the elastic limit. Under dynamic loading conditions the resulting wave propagation can be decomposed into elastic and plastic regions (Meyers [2]). Under uniaxial strain conditions, the elastic portion of the wave travels at the primary longitudinal wave speed whilst the plastic wave front travels at a local velocity (6.13) For an elastic perfectly plastic material, it can be shown [3] that the plastic wave travels at a slower velocity than the primary elastic wave (6.14)

6.2.4.3. Shock Waves Typical stress strain curves for a ductile metal under uniaxial stress and uniaxial strain conditions are given below. Table 6.2: Typical stress strain curves for a ductile metal

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

135

Explicit Dynamics Theory Guide a) Uniaxial stress

b) Uniaxial strain

Under uniaxial stress conditions, the tangent modulus of the stress strain curve decreases with strain. The plastic wave speed therefore decreases as the applied jump in stress associated with the stress wave increases – shock waves are unlikely to form under these conditions. Under uniaxial strain conditions the plastic modulus (AB) increases with the magnitude of the applied jump in stress. If the stress jump associated with the wave is greater than the gradient (OZ), the plastic wave will travel at a higher speed than the elastic wave. Since the plastic deformation must be preceded by the elastic deformation, the elastic and plastic waves coalesce and propagate as a single plastic shock wave. A shock wave can be considered to be a discontinuity in material state (density(ρ), energy(e), stress(σ), particle velocity(u)) which propagates through a medium at a velocity equal to the shock velocity (Us ). Figure 6.1: Conditions at a Moving Shock Front

Relationships between the material state across a shock discontinuity can be derived using the principals of conservation of mass, momentum and energy. The resulting Hugoniot equations are given by (6.15) (6.16) (6.17)

6.2.5. Reference Frame You can define the reference frame for bodies in an explicit dynamics analysis to be either Lagrangian or Eulerian. The following sections describe the two reference frames and how their use affects the analysis. 6.2.5.1. Lagrangian and Eulerian Reference Frames 6.2.5.2. Eulerian (Virtual) Reference Frame in Explicit Dynamics 6.2.5.3. Key Concepts of Euler (Virtual) Solutions

6.2.5.1. Lagrangian and Eulerian Reference Frames By default, all bodies in an Explicit Dynamics analysis system are discretized and solved in a Lagrangian reference frame: The material associated with each body is discretized in the form of a body-fitted mesh. Each element of the mesh is used to represent a volume of material. The same amount of material mass remains associated with each element throughout the simulation. The mesh deforms with the material deformation. Solving using a Lagrangian reference frame is the most efficient and accurate method to use for the majority of structural models. However, in simulations where the material undergoes extreme

136

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

What is Explicit Dynamics? deformations, such as in a fluid or gas flowing around an obstacle, the elements will become highly distorted as the deformation of the material increases. Eventually the elements may become so distorted that the elements become inverted (negative volumes) and the simulation cannot proceed without resorting to numerical erosion of highly distorted elements. In an Eulerian reference frame, the grid remains stationary throughout the simulation. Material flows through the mesh. The mesh does not therefore suffer from distortion problems and large deformations of the material can be represented. If the material you are going to model is likely to experience very large deformations, using an Eulerian reference frame is therefore preferable. Solving using an Eulerian reference frame is generally computationally more expensive than using a Lagrangian reference frame. The additional cost comes from the need to transport material from one cell to the next and also to track in which cells each material exists. Each cell in the grid can contain one or more materials (to a maximum of 5 in the Explicit Dynamics system). The location and interface of each material is tracked only approximately (to first order accuracy). The representative example below shows a block of material impacting a rigid wall. First the block is represented in the Lagrangian reference frame. During the impact process the nodes of the mesh follow the deformation of the material. The same problem can be modelled in an Eulerian reference frame; here the nodes of the mesh are fixed in space, they do not move. Instead the material is tracked as it moves through the mesh.

Solid, Liquid and Gaseous materials can be used with an Eulerian (Virtual) reference frame in the Explicit Dynamics system. Because of the computational cost and approximate tracking of material interfaces, the Eulerian reference frame should be used only when very large deformation or flow of the material is expected.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

137

Explicit Dynamics Theory Guide

6.2.5.2. Eulerian (Virtual) Reference Frame in Explicit Dynamics Switching the reference frame of a solid body in Explicit Dynamics systems from Lagrangian to Eulerian will result in that body being mapped into an Eulerian background grid at solve time and the material associated with the body will be solved in an Eulerian reference frame. If one or more solid bodies have a reference frame set to Eulerian (Virtual), the following process is used on initialization to map the Euler bodies to a background Eulerian domain: Virtual Euler Domain A background Eulerian (Virtual) domain is automatically generated to enclose all bodies in the model. By default, the domain size is set to 1.2 times the size of the bounding box of all bodies in the model. The domain is always aligned with the global Cartesian X, Y, and Z axes. Additional options to control the size of the domain are provided in the Analysis Settings.

The background Euler domain is discretized with a mesh of uniform cell size. The cell size is defined to give approximately 500,000 cells in total. Additional options to control the cell size are provided in the Analysis Settings. The entire Euler domain is initialized as void; the cells contain no material.

138

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

What is Explicit Dynamics?

Mapping of bodies with Euler reference frame to virtual Euler domain The standard mesh generated on bodies marked with Eulerian (Virtual) reference frame is only used to represent the geometry of the body during initialization of the model for the solver. The material and initial conditions defined on bodies marked as Eulerian reference frame are mapped to the Euler domain. The mesh associated with the original body is then deleted, prior to the solve. A unique material is created for each body that is mapped into the Euler domain for the purposes of post processing

If multiple bodies marked as Eulerian (Virtual) overlap, the body higher in the Outline view will take precedence. Therefore, the material assigned to the region of overlap will correspond to that assigned to the first Eulerian body. The exterior faces of the Euler domain can each have one of three types of boundary condition applied. The type of boundary condition for each face is controlled in the Analysis Settings (p. 45): Flow-out (Default) This condition will allow any material reaching the boundary of the Euler domain to flow out of the domain at constant velocity. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

139

Explicit Dynamics Theory Guide Rigid Wall This condition makes the external boundaries of the domain act as a rigid wall. Impedance This condition acts the same as a Flow-out condition and allows any material reaching the boundary of the Euler domain to flow out of the domain at constant velocity.

6.2.5.3. Key Concepts of Euler (Virtual) Solutions The conservation equations of mass, momentum and energy are solved on a block structured background mesh using a 2nd order accurate multi-material Godunov numerical scheme[17] with the second order upwind method by Van Leer [19, 20]. The computational cycle for bodies represented in an Eulerian reference frame is outlined below:

In comparison to a traditional Lagrangian numerical scheme, note the points in the following sections. 6.2.5.3.1. Multiple Material Stress States 6.2.5.3.2. Multiple Material Transport 6.2.5.3.3. Supported Material Properties 6.2.5.3.4. Known Limitations of Euler Solutions

6.2.5.3.1. Multiple Material Stress States During the simulation, material can flow from one cell to another. At some stage in the computation a given cell is likely to contain more than one material. Note that void (free space) is also considered as a material in this sense; a cell containing one material and void is typical at any free surface of the material. In the example below we can see two solid materials (green and yellow) and free surfaces (white, void material) represented in an Eulerian reference frame.

140

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

What is Explicit Dynamics?

A volume of fluid (VOF) method is used track the amount of material in each cell. Each material has a volume fraction and the sum of the volume fraction of each material, plus the volume fraction of void, will equate to unity. (6.18) Nearly all isotropic material properties can be used in an Eulerian reference frame to represent solids, liquids or gases. Special treatment is required to allow calculation of the strain rates, pressure and stresses in each material in a cell, and also to calculate a resultant stress tensor which is then used to calculate cell face impulses, momentum and mass transport. Two algorithms are used for this purpose: 1. A cell containing two different gases; here we use an iterative procedure to establish an Equilibrium state (a density and energy of each gas which results in a uniform pressure across both gases). 2. A cell containing two or more non-gaseous materials; here we use a stiffness weighted averaging technique to distribute strain rates and establish the resultant pressure and deviatoric stress in each cell. The choice of the above algorithms is automatic and local to each cell in the model.

Important At any point in time during the solution, only the volume fraction of each material in each cell is recorded and stored. The location of the material within the cell is not known. During post-processing of the model you will see an outline of the material displayed, this outline is an approximation derived from the volume fraction distribution in the cells. It is only accurate to within one cell dimension.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

141

Explicit Dynamics Theory Guide

6.2.5.3.2. Multiple Material Transport To move the solution through the mesh from one timestep to another, material must be transported across cell faces. If a cell contains only one material then we have a trivial solution and a volume fraction of that material will be transported across the face. If however we have multiple materials in a cell we need to employ an algorithm to decide which materials to transport and how much of each material to transport across each cell face. We are using the SLIC (Single Line Interface Construction) method [18] to calculate the order and quantity of material to transport across a cell face. This method takes information from both the upstream and downstream cells to make decisions on material transport.

6.2.5.3.3. Supported Material Properties The supported material properties are Density, Specific Heat, Isotropic Elasticity, Bilinear Isotropic Hardening, Multilinear Isotropic Hardening, Johnson Cook Strength, Cowper Symonds Strength, Steinberg Guinan Strength, Zerilli Armstrong Strength, Drucker-Prager Strength Linear, Drucker-Prager Strength Stassi, Drucker-Prager Strength Piecewise, Johnson-Holmquist Strength Continuous, Johnson-Holmquist Strength Segmented, RHT Concrete, MO Granular, Ideal Gas EOS, Bulk Modulus, Shear Modulus, Polynomial EOS, Shock EOS Linear, Shock EOS Bilinear, Explosive JWL, Explosive JWL Miller, Compaction EOS Linear, Compaction EOS Non-Linear, P-alpha EOS, Plastic Strain Failure, Tensile Pressure Failure, Johnson Cook Failure, Grady Spall Failure.

6.2.5.3.4. Known Limitations of Euler Solutions Sometimes the multimaterial Euler solver exhibits so called checkerboarding where the face values of Euler elements are correct, but the Euler element values (for example, pressure) are switching between positive and negative values from element to element. This can be seen when the smoothing of the contour values is switched off—the plot will show a checkerboard pattern. This introduces incorrect pressure (and other) values which will, for example, result in wrong coupling forces on a Lagrangian flexible or rigid body. The magnitude of the effect of this limitation on the solution may be large and easy to observe: for example, when the flow or distortion of the material in Euler shows overall incorrect behavior. Or it may be small and difficult to recognize: for example, in cases where the pressure switches locally, but the overall average pressure is still correct. Common solutions for this problem are: • A refinement of the mesh, with possibly some grading (smaller elements near the area of interest) to reduce runtimes • Reduction of the timestep safety factor to, for example, 0.333

6.2.6. Explicit Fluid Structure Interaction (Euler-Lagrange Coupling) In the Explicit Dynamics system, solid bodies can be assigned either a Lagrangian reference frame or an Eulerian (Virtual) reference frame. The reference frames can be combined in the simulation to allow the best solution technique to be applied to each type of material being modelled. During the simulation, bodies represented in the two reference frames will automatically interact with each other. For example, if one body is filled with steel using a Lagrangian reference frame, and another body filled with water using an Eulerian reference frame, the two bodies will automatically interact with each other if they come into contact. The interaction between Eulerian and Lagrangian bodies provides a capability for tightly coupled two way fluid structure interaction in the Explicit Dynamics system.

142

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

What is Explicit Dynamics? In the simple example below, a body with Lagrangian reference frame (grey) is moving from left to right over a body with Eulerian reference frame. As the body moves, it acts as a moving boundary in the Euler domain by progressively covering volumes and faces in the Euler cells. This induces flow of material in the Euler Domain. At the same time, a stress field will develop in the Euler domain which results in external forces being applied on the moving Lagrangian body. These forces will feedback into the motion and deformation (and stress) of the Lagrangian body.

In more detail, the Lagrangian body covers regions of the Euler domain. The intersection between the Lagrangian and Eulerian bodies results in an updated control volume on which the conservation equation of mass, momentum and energy are solved.

At the same time, the normal stress in the intersected Euler cell will act on the intersected area of the Lagrangian surface.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

143

Explicit Dynamics Theory Guide This provides a two-way closely coupled fluid-structure (or more generally Eulerian-Lagrangian) interaction. During a simulation, the Lagrangian structure can move and deform. Large deformations may also result in erosion of the elements from the Lagrangian body. The coupling interfaces are automatically updated in such cases. For accurate results when coupling Lagrangian and Eulerian bodies in Explicit Dynamics it is necessary to ensure that the size of the cells of the Euler domain are smaller than the minimum distance across the thickness of the Lagrangian bodies. If this is not the case, you may see leakage of material in the Euler domain through the Lagrange structure.

6.2.6.1. Shell Coupling In the case of coupling to thin bodies (typically modelled with shells), an equivalent solid body is generated to enable intersection calculations to be performed between a Lagrangian volume and the Euler domain. The thickness of the equivalent solid body is automatically calculated based on the Euler Domain cell size to ensure that at least one Euler element is fully covered over the thickness and no leakage occurs across the coupling surface. Note this 'artificial' thickness is only used for volume intersection calculations for the purposes of coupling and is independent of the physical thickness of the shell/surface body.

6.2.6.2. Sub-cycling The Lagrangian reference frame is most frequently used to model solid structures with materials which have soundspeeds in the order of several thousand meters/second. The Eulerian reference is most frequently used to represent fluids or gases which typically have soundspeeds in the order of hundreds of meters/second. In Explicit Dynamics simulations the maximum timestep that can be used is inversely proportional to the soundspeed of the material. The timestep required to model structures is therefore often significantly smaller than the timestep required to accurately model a gas. To enable the Lagrangian and Eulerian parts of a coupled simulation proceed at the optimum timestep (for efficiency and accuracy) a sub-cycling technique is used where possible. The Lagrangian domain uses its critical timestep. The Euler domain uses its critical timestep. Coupling information is exchanged at the end of each Euler domain timestep.

144

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Analysis Settings

6.3. Analysis Settings In the following sections you find theoretical background for specific controls available in the Explicit Dynamics system. 6.3.1. Step Controls 6.3.2. Damping Controls 6.3.3. Solver Controls 6.3.4. Erosion Controls

6.3.1. Step Controls Maximum Energy Error Energy conservation is a measure of the quality of an explicit dynamic simulation. Bad energy conservation usually implies a less than optimal model definition. This parameter allows you to automatically stop the solution if the energy conservation becomes poor. Enter a fraction of the total system energy at the reference cycle at which you want the simulation to stop. For example, the default value of 0.1 will cause the simulation to stop if the energy error exceeds 10% of the energy at the reference cycle. The global energy is accounted as follows: Reference Energy = [Internal Energy + Kinetic Energy + Hourglass Energy] at the reference cycle Current Energy = [Internal Energy + Kinetic Energy + Hourglass Energy] at the current cycle Work Done = Work done by constraints + Work done by loads + Work done by body forces + Energy removed from system by element erosion + Work done by contact penalty forces

Figure 6.2: Example energy conservation graph for model with symmetry plane and erosion

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

145

Explicit Dynamics Theory Guide

6.3.2. Damping Controls Treatment of Shock Discontinuities Strong impacts on solid bodies can give rise to the formation of shock waves in the material. Because of the nonlinearity of the equations being solved, shocks can form even though the initial conditions are smooth. In order to handle the discontinuities in the flow variables associated with such shocks, viscous terms are introduced into the solutions. These additional terms have the effect of spreading out the shock discontinuities over several elements and thus allow the simulation to continue to compute a smooth solution, even after shock formation and growth. Figure 6.3: Comparison of pressure solution at a shock wave discontinuity a) using no artificial viscosity b) using the default artificial viscosity

The viscous terms used in the Explicit Dynamics system is based on the work of von Neumann and Richtmeyer [4] and Wilkins [5]. (6.19)

Where CQ is the Quadratic Artificial Viscosity coefficient CL is the Linear Artificial Viscosity coefficient ρ is the local material density d is a typical element length scale c is the local sound speed

146

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Analysis Settings is the rate in change of volume The quadratic term smooths out shock discontinuities while the linear term acts to damp out oscillations which may occur in the solution behind the shock discontinuity. Figure 6.4: Effects of artificial viscosity on the solution

a) Quadratic term stabilizes

b) The linear term reduces noise

Note • The pseudo-viscous term is usually added only when the flow is compressing. The Linear Viscosity in Expansion option can be used to apply the pseudo-viscous term in both compression and expansion. This can lead to excessive dispersion in the solution. • The inclusion of the pseudo-viscous pressure imposes further restrictions on the time step in order to ensure stability: Due to the quadratic term,

Due to the linear term, The resulting critical time step is • The pseudo-viscous pressure is stored for each element and can be contoured using the custom variable VISC_PRESSURE

Hourglass Damping The reduced integration eight node hexahedral elements, or 4 node quadrilateral elements, used in Explicit Dynamics can exhibit “hourglass” modes of deformation. Since the expressions for strain rates and forces involve only differences in velocities and/or coordinates of diagonally opposite nodes of the cuboidal element, if the element distorts in such a way that these differences remain unchanged there will be no strain increase in the element and therefore no resistance Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

147

Explicit Dynamics Theory Guide to this distortion. Hourglass modes of deformation occur with no change in energy (also called zero energy modes) and are unphysical. An example of such a distortion in two dimensions is illustrated below where the two diagonals remain the same length even though the cell distorts.

Visualization in three dimensions is much more difficult but if such distortions occur in a region of many elements, patterns such as that shown below occur and the reason for the name of “hourglass instability” is more easily understood.

To avoid these zero energy modes of deformation from occurring, corrective forces (Hourglass forces) are added to the solution to resist the hourglass modes of deformation. Hexahedral Elements Two formulations for calculating the Hourglass forces are available for Hexahedral elements: The Standard formulation is based on the work of Kosloff and Frazier [6] and generates hourglass forces proportional to nodal velocity differences. This is often referred to as a viscous formulation. (6.20) Where FH is a vector of the hourglass forces at each node of the element CH is the Viscous Coefficient for hourglass damping ρ is the material density c is the material soundspeed V is the material volume is a vector function of the element nodal velocities aligned with the hourglass shape vector The standard formulation is the most efficient formulation in terms of CPU and is therefore the default option. It is not however invariant under rigid body rotation (i.e. under rigid body rotation the hourglass forces may not sum to zero)

148

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Analysis Settings The Flanagan Belytschko [7] formulation is invariant under rigid body rotation and is therefore recommended for simulations in which large rotations of hexahedral elements are expected. The Flanagan Belytschko formulation is similar to the standard form. (6.21) The difference lies in the construction of the vector function of element nodal velocities,

. These

are constructed to be orthogonal to both linear velocity field and the rigid body field.

Note • The Viscous Coefficient for hourglass forces usually varies between 0.05 and 0.15. The default value is 0.1. • The sum of the hourglass forces applied to an element is normally zero. The momentum of the system is therefore unaffected by hourglass forces. • The hourglass forces do however do work on the nodes of the elements. The energy associated with hourglass forces is a) stored locally in the specific internal energy of the element b) recorded globally over the entire model and available to review via the Solution Output, Energy Summary.

Static Damping The Explicit Dynamics system is primarily designed for solving transient dynamic events. Using the static damping option, a static equilibrium solution can also be obtained. The procedure is to introduce a damping force which is proportional to the nodal velocities and which is aimed to critically damp the lowest mode of oscillation of the static system. The solution is then computed in time in the normal manner until it converges to an equilibrium state. The user is required to judge when the equilibrium state is achieved. If the lowest mode of the system has period T then we may expect the solution to converge to the static equilibrium state in a time roughly 3T if the value of T is that for critical damping. When the dynamic relaxation option is used the velocity update is modified to (6.22) where the Static Damping Coefficient, Rd , is input by the user. The value of Rd for critical damping of the lowest mode is (6.23) where T is the period of the lowest mode of vibration of the system (or a close approximation to it). Usually (6.24) A reasonable estimate of T must be used to ensure convergence to an equilibrium state but if the value of T is not known accurately then is it recommended that the user overestimates it, rather than underestimating it. Approximate values of Δt and T can usually be obtained by first performing a dynamic analysis without static damping.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

149

Explicit Dynamics Theory Guide A static damping coefficient may be defined, or removed, at any point during an Explicit Dynamic simulation. Typical examples of its use would be: • To establish an initial stress distribution in a structure, prior to solving a transient dynamic event. For example applying gravity to a structure. • To establish the final static equilibrium position of a structure after it has experienced a transient dynamic event. For example finding the equilibrium position of structure after it has undergone large plastic deformation during a dynamic event.

6.3.3. Solver Controls Hexahedral Elements The preferred element for solid bodies in Explicit Dynamics systems is the eight node reduced integration hexahedral. These elements are well suited to transient dynamic applications including large deformations, large strains, large rotations and complex contact conditions. The basic element characteristics are Connectivity

8 Node

Nodal Quantities

Position, Velocity, Acceleration, Force Mass (lumped mass matrix)

Element Quantities

Volume, Density, Strain, Stress, Energy Other material state variables

Material Support

All available materials

Points to Note

Preferred element for Explicit Dynamics Reduced integration, constant strain element Requires hourglass damping to stabilize zero energy “hourglass” modes (see section Damping Controls, Hourglass Damping)

The default Integration Type for hexahedral elements is the Exact option. Here the element formulation based upon the work of Wilkins [8] results in an exact volume calculation even for distorted elements. This formulation is therefore the most accurate option, especially if the faces of the hex elements become warped. This is also computationally the most expensive formulation. It is possible to speed-up simulations by using the 1pt Gaussian quadrature integrated hexahedral element. This uses the element formulation described by Hallquist [9]. There will be some loss in accuracy

150

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Analysis Settings when using this formulation with warped element faces which are common place in large deformation analysis.

Tetrahedral Elements Linear 4 noded tetrahedron elements are available for use in Explicit Dynamic analysis. Connectivity

4 Node

Nodal Quantities

Position, Velocity, Acceleration, Force Mass (lumped mass matrix) Additionally ANP formulation: Volume, Pressure, Energy Additionally NBS: Volume, Density, Strain, Stress, Energy, Pressure and other material state variables

Element Quantities

Volume, Density, Strain, Stress, Energy Other material state variables Additionally NBS: If PUSO stability coefficient is set to a non-zero value, there is an additional variable set for all variables for the PUSO solver

Material Support

SCP: All available materials Only Isotropic materials can be used with the ANP formulation Only ductile materials can be used with the NBS formulation

Points to Note

Only the ANP and NBS are recommended for use in majority tetrahedral meshes For NBS models exhibiting zero energy modes, the Puso coefficient can be set to a non-zero value. A value of 0.1 is recommended. Reduced integration, constant strain element

The four noded linear tetrahedron is available with three forms of Pressure Integration • Standard Constant pressure integration (SCP), Zienkiewicz [10]. • Average Nodal Pressure (ANP) integration, based around the work of Burton [11]. • Nodal Based Strain (NBS) integration, based on work of (Bonet [21] and Puso [22]). The SCP tetrahedral element is a basic, constant strain element and can be used with all the material models. The element is intended as a “filler” element in meshes dominated by hexahedral elements. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

151

Explicit Dynamics Theory Guide The element is known to exhibit locking behavior under both bending and constant volumetric straining (that is, plastic flow). If possible the element should therefore not be used in such cases. The ANP tetrahedral formulation used here is an extension of the advanced tetrahedral element (Burton [11]) and can be used as a majority element in the mesh. The ANP tetrahedral overcomes problems of volumetric locking. The NBS tetrahedral formulation based on the work of (Bonet [21] and Puso [22]) is a further extension of the ANP tetrahedral element and can also be used as a majority element in the mesh. The NBS tetrahedral overcomes both problems of volumetric and shear locking, therefore is recommended over the other two tetrahedral formulations for models involving bending. Supported material types in the NBS tetrahedral element are currently limited to ductile materials. The following is a list of supported material properties for NBS tetrahedral elements: • Isotropic Elasticity • Bulk Modulus • Shear Modulus • Polynomial EOS • Shock EOS • Johnson Cook Strength • Zerilli Armstrong Strength • Cowper Symonds Strength • Steinberg Guinan Strength • Bilinear Isotropic Hardening • Multilinear Isotropic Hardening • Tensile Pressure Failure • Plastic Strain Failure • Principal Stress Failure • Principal Strain Failure • Principal Stress/Principal Strain Failure • Grady Spall Failure • Johnson Cook Failure

152

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Analysis Settings • Stochastic Failure

Note Both flexible and rigid bodies are supported for NBS tetrahedral elements. If a model containing NBS tetrahedral elements exhibits zero-energy modes (Puso, 2006 [22]), the PUSO stability coefficient can be set to a non-zero value. The recommended value is 0.1. Stabilization is achieved by taking a contribution to the nodal stresses from the SCP solution. Therefore, for models with a non-zero Puso stability coefficient, the solution is computed on both the nodes and the elements. NBS tetrahedral elements cannot share nodes with ANP tetrahedral elements, SCP tetrahedral elements, shell elements, or beam elements. Also note that the use of NBS tetrahedral elements with joins or spotwelds is not supported. Figure 6.5: Comparison of results of a Taylor test solved using SCP, ANP and NBS Tetrahedral elements. Results using NBS and ANP tetrahedral elements compare more favorably with experimental results than results using SCP (see table below). Tet-SCP

Tet-ANP

Tet-NBS

Table 6.3: Comparison of the performance of SCP, ANP, NBS and hex elements in a model involving bending. The displacement of the beam with NBS tetrahedral elements is the most similar to the beam meshed with hexahedral elements as it does not exhibit shear locking as is seen in the beams solved using SCP and ANP tetrahedral elements. Experiment

SCP Tet

ANP Tet

NBS Tet

Cylinder length (mm)

31.84

30.98

30.97

31.29

Impact diameter (mm)

12.0

10.66

11.32

11.28

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

153

Explicit Dynamics Theory Guide Figure 6.6: Example bending test using SCP (1), ANP (2), NBS tetrahedral (3), and hex (4) elements. The displacement of the beam with NBS tetrahedral elements is the most similar to the beam meshed with hexahedral elements as it does not exhibit shear locking.

Figure 6.7: Taylor test: Iron cylinder impacting rigid wall at 221m/s. Good correlation between ANP and Hex element results is obtained

154

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Analysis Settings Figure 6.8: Example pull out test simulated using both hexahedral elements and ANP tetrahedral elements. Similar plastic strains and material fracture are predicted for both element formulations used.

Pentahedral Elements Linear 6 noded pentahedral elements are available for use in Explicit Dynamics analysis. Connectivity

6 Node

Nodal Quantities

Position, Velocity, Acceleration, Force Mass (lumped mass matrix)

Element Quantities

All available materials Other material state variables

Material Support

All available materials

Points to Note

Reduced integration, constant strain element

The pentahedral element is a basic constant strain element and is intended as a filler element in meshes dominated by hexahedral elements.

Pyramid Elements Pyramid elements are not recommended for Explicit Dynamic simulations. Any pyramid elements present in the mesh will be converted to 2 tetrahedral elements in the solver initialization phase. Results are mapped back onto the Pyramid element for postprocessing purposes.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

155

Explicit Dynamics Theory Guide

Shell Quad Elements Bilinear 4 noded quadrilateral shell elements are available for use in Explicit Dynamics analysis. Connectivity

4 Node

Nodal Quantities

Position, Velocity, Angular Velocity, Acceleration, Force, Moment Mass (lumped mass matrix)

Element Quantities

Strain, Stress, Energy Other material state variables Data stored per layer

Material Support

Linear elasticity must be used Equations of state and porosity are not applicable to shell elements Pressure dependant material strength is not applicable to shell elements

Points to Note

Reduced integration, constant strain element Based on Mindlin plate theory, transverse shear deformable Shells have zero through thickness stress and are therefore not suitable for modelling wave propagation through the thickness of the surface body

The bilinear 4 noded quadrilateral shell element is based on the corotational formulation presented by Belytschko-Tsay [13]. The element has one quadrature point per layer and is stabilized using hourglass control. By default, additional curvature terms are added for warped elements in accordance with Belytschko [14]. This option can be deactivated using the Shell BWC Warp Correction setting in the Solver Controls. The number of through thickness integration points (sublayers) is controlled through the analysis settings option Solver Controls, Shell Sublayers. The default value is 3. The thickness of the shell element is updated during the simulation in accordance with the material response. The update is carried out at the shell nodes by default. The principal inertia of the shell nodes is recalculated every time increment (cycle) by default. This is the most robust method. It is more efficient to rotate the principal inertias rather than recalculate (although less robust for certain applications). The “Shell Thickness Update” option can be used to select this more efficient inertial update method.

156

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Analysis Settings

Shell Tri Elements Linear 3 noded triangular shell elements are available for use in Explicit Dynamics analysis. Connectivity

3 Node

Nodal Quantities

Position, Velocity, Angular Velocity, Acceleration, Force, Moment Mass (lumped mass matrix)

Element Quantities

Volume, Density, Stress, Energy Other material state variables Data stored per layer

Material Support

Linear elasticity must be used Equations of state and porosity are not applicable to shell elements Pressure dependant material strength is not applicable to shell elements

Points to Note

Reduced integration, constant strain element This element is only recommended for use as a “filler” element in quad dominant shell meshes Shells have zero through thickness stress and are therefore not suitable for modelling wave propagation through the thickness of the surface body

The bilinear 3 noded, C0, triangular shell element is based on the formulation presented by Belytschko et al. [15]. The number of through thickness integration points (sublayers) is controlled through the analysis settings option Solver Controls, Shell Sublayers. The default value is 3. The thickness of the shell element is updated during the simulation in accordance with the material response. The update is carried out at the element irrespective of the global settings for Shell Thickness update in Mechanical.

Beam Elements Linear 2 noded beam elements are available for use in Explicit Dynamics analysis. Connectivity

2 Node

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

157

Explicit Dynamics Theory Guide

Nodal Quantities

Position, Velocity, Angular Velocity, Acceleration, Force, Moment Mass (lumped mass matrix)

Element Quantities

Resultant Strain/Stress, Energy Other material state variables

Material Support

Linear elasticity must be used Equations of state and porosity are not applicable to beam elements Pressure dependant material strength is not applicable to beam elements

Points to Note

Supports symmetrical circular, square, rectangular, I-Beam and general cross sections Beams have zero transverse stress and are therefore not suitable for modelling wave propagation across the cross section

The 2 noded beam element is based on the resultant beam formulation of Belytschko [16] and allows for large displacements and resultant elasto-plastic response.

6.3.4. Erosion Controls Erosion is a numerical mechanism for the automatic removal (deletion) of elements during a simulation. The primary reason for using erosion is to remove very distorted elements from a simulation before the elements become inverted (degenerate). This ensures that the stability timestep remains at a reasonable level and solutions can continue to the desired termination time. Erosion can also be used to allow the simulation of material fracture, cutting and penetration. There are a number of mechanisms available to initiate erosion of elements. The erosion options can be used in any combination. Elements will erode if any of the criteria are met.

Geometric Strain Geometric strain is a measure of the distortion of an element and is calculated from the global strain components as

158

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Model Size Limitations in Explicit Dynamics (6.25) This erosion option allows removal of elements when the local element geometric strain exceeds the specified value. Typical values range from 0.5 to 2.0. The default value of 1.5 can be used in most cases. Custom result EFF_STN can be used to review the distribution of effective strain in the model.

Timestep This erosion option allows removal of elements when the local element timestep, multiplied by the time step safety factor falls below the specified value. Custom result TIMESTEP can be used to review the time step for each element.

Material Failure Using this option, elements will automatically erode if a material failure property is defined in the material used in the elements, and the failure criteria has been reached. Elements with materials including a damage model will also erode if damage reaches a value of 1.0.

Retained Inertia If all elements that are connected to a node in the mesh are eroded, the inertia of the resulting free node can be retained. The mass and momentum of the free node is retained and can be involved in subsequent impact events to transfer momentum in the system. If this option is set to No, all free nodes will be automatically removed from the simulation.

Note • Erosion is not a physical process and should be used with caution. • The internal energy of elements which are eroded is always removed from the system. This energy is accumulated in the work done term for global energy conservation purposes.

6.4. Model Size Limitations in Explicit Dynamics Exceedingly large (number of elements/nodes) models may not be able to complete an Explicit Dynamics solution in a reasonable amount of time for the following reasons: • As in any Mechanical application, you will start out with a coarse mesh and investigate convergence behavior while refining the mesh. This will typically lead to a satisfactory number of elements for a certain elapsed time. You may reduce the CPU time by distributing the model over multiple processors in parallel. With larger model sizes the initialization time (which is typically a small fraction of the total run time) may increase significantly because the initialization is not running in parallel. • When doing convergence studies you may run into hardware limitations. An Explicit Dynamics solution takes place in core memory, which means that RAM is the most limiting factor. Most modern workstations typically contain large amounts of RAM and will be able to cope with large models. Note that disk space is not generally a problem since result files are typically not exceedingly large.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

159

Explicit Dynamics Theory Guide • Although modern workstation hardware may allow large models to be meshed, the Explicit solver may not be able to handle some large models because most integer numbers are still allocated on a 32 bit based definition, and if a single internal array needs to be allocated with larger than 2e9 entries the solution will fail. The current limitations can be summarized as follows, although these numbers are only a guideline as to what to expect: • Although Workbench can mesh a single part up to a maximum of 100 million solid elements, or 10 million shell elements, the Explicit solver may not be able to calculate a solution in a reasonable amount of time with a mesh of this size. Each element and node has a number of associated variables. The number typically depends on the type of solver chosen along with material models used and the number of options activated; for example, Failure models or the type of Interaction. • The AUTODYN component system can be used to generate structured meshes, which in turn can be converted to unstructured. The limit for the number of elements that can be converted lies between 50 million and 60 million. • The number of objects that can be created in the AUTODYN component system is limited to 99 in 3D. • If the Explicit solver detects that more than 500,000 nodes are packed in an SPH object a warning will be given, since it will affect CPU and RAM resources. Please note that these limitations are approximate and serve as a guideline when modeling for Explicit Dynamics and AUTODYN component systems. To reduce the solution time, you should try using a coarser mesh or use Mass Scaling in your model.

6.5. References The following references are cited in this section: 1.

R. Courant, K. Friedrichs and H. Lewy, "On the partial difference equations of mathematical physics", IBM Journal, March 1967, pp. 215-234

2.

Meyers, M. A., (1994) “Dynamic behaviour of Materials”, John Wiley & Sons, ISBN 0-471-58262-X.

3.

Zukas, J. A., (1990) “High velocity impact dynamics”, John Wiley & Sons, ISBN 0-471-51444-6

4.

von Neumann, J., Richtmeyer, R. D. (1950).,“A Method for the Numerical Calculation of Hydrodynamic Shocks”, J. App. Phys., 21, pp 232-237, 1950

5. Wilkins, M. L., (1980). “Use of Artificial Viscosity in Multidimensional Fluid Dynamic Calculations”, J. Comp. Phys., 36, pp 281-303, 1980 6.

Kosloff D., Frazier G. A., (1978) “Treatment of hourglass patterns in low order finite element codes”, Int. J. Num. Anal. Meth. Geomech. 2, 57-72

7.

Flanagan D. P., Belytschko T., (1981) “A uniform strain hexahedron and Quadrilateral and Orthogonal Hourglass Control”, Int. J. Num. Meth. Eng. 17, 679-706.

8. Wilkins, M. L., Blum, R. E., Cronshagen, E. & Grantham, P. (1974). “A Method for Computer Simulation of Problems in Solid Mechanics and Gas Dynamics in Three Dimensions and Time.” Lawrence Livermore Laboratory Report UCRL-51574, 1974 9. Hallquist, J. O., (1982) "A theoretical manual for DYNA3D, LLNL Report UCID-19401. 160

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

References 10. Zienkiewicz, O. C., Taylor, R. L., "The finite element method, Volume 1", ISBN 0-07-084174-8 11. Burton, A..J.. (1996) 'Explicit, Large Strain, Dynamic Finite Element Analysis with Applications to Human Body Impact Problems', PhD Thesis, University of Wales. 12. Wilkins, M. L., Blum, R. E., Cronshagen, E., & Grantham, P. (1974). “A Method for Computer Simulation of Problems in Solid Mechanics and Gas Dynamics in Three Dimensions and Time.” Lawrence Livermore Laboratory Report UCRL-51574, 1974 13. Belytschko, T., et al. (1984),“Explicit algorithms for the nonlinear dynamics of shells”, Comp. Meth. Appl. Mech Eng., 42, 225-251. 14. Belytschko, T., et al. (1992),“Advances in one-point quadrature shell elements”, Comp. Meth. Appl. Mech Eng., 1992, 93-107. 15. Belytschko, T., et al. (1984),“A C0 Triangular Plate Element with One-point Quadrature”, Int. J. Num. Meth. Engng., 20, 787-802, 1984. 16. Belytschko, T. et al., 1977,“Large Displacement Analysis of Space Frames”, Int. J. Num. Meth. And Anal. Mech. Engng., 11, 65-84, 1977. 17. Godunov, S. K. (1959), "A Difference Scheme for Numerical Solution of Discontinuous Solution of Hydrodynamic Equations", Math. Sbornik, 47, 271-306, translated US Joint Publ. Res. Service, JPRS 7226, 1969. 18. Noh, W. F. and Woodward, P.,“SLIC (Simple line interface calculation),” in Lecture Notes in Physics (A. I. van der Vooren and P. J. Zandbergen, eds.), pp. 330–340, Springer-Verlag, 1976. 19. Van Leer, B (1977).“Towards the Ultimate Conservative Difference Scheme. IV. A new Approach to Numerical Convection”, J. Comp. Phys. 23, pp 276-299, 1977. 20. Van Leer, B (1979).“Towards the Ultimate Conservative Difference Scheme. V. A Second Order Sequel to Godunov’s Method”, J. Comp. Phys. 32, pp 101-136, 1979. 21. Bonet J., Marriott H., Hassan O.“An averaged nodal deformation gradient linear tetrahedral element for large strain explicit dynamics applications”. Communications in Numerical Methods in Engineering 2001; 17, 551-561. 22. Puso M. A.,Solberg J.“A stabilized nodally integrated tetrahedral”. International Journal for Numerical Methods in Engineering 2006; 67, 841-867.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

161

162

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 7: Material Models Used in Explicit Dynamics Analysis This chapter discusses the following: 7.1. Introduction 7.2. Explicit Material Library 7.3. Density 7.4. Linear Elastic 7.5.Test Data 7.6. Hyperelasticity 7.7. Plasticity 7.8. Brittle/Granular 7.9. Equations of State 7.10. Porosity 7.11. Failure 7.12. Strength 7.13.Thermal Specific Heat 7.14. Rigid Materials 7.15. References

7.1. Introduction In general, materials have a complex response to dynamic loading and the following phenomena may need to be modeled. • Non-linear pressure response • Strain hardening • Strain rate hardening • Pressure hardening • Thermal softening • Compaction (for example, porous materials) • Orthotropic response (for example, composites) • Crushing damage (for example, ceramics, glass, concrete) • Chemical energy deposition (for example, explosives) • Tensile failure • Phase changes (for example, solid-liquid-gas) The modeling of such phenomena can generally be broken down into three components:

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

163

Material Models Used in Explicit Dynamics Analysis

Equation of State An equation of state describes the hydrodynamic response of a material. This is the primary response for gases and liquids, which can sustain no shear. Their response to dynamic loading is assumed hydrodynamic, with pressure varying as a function of density and internal energy. This is also the primary response for solids at high deformation rates, when the hydrodynamic pressure is far greater than the yield stress of the material.

Material Strength Model Solid materials may initially respond elastically, but under highly dynamic loadings, they can reach stress states that exceed their yield stress and deform plastically. Material strength laws describe this nonlinear elastic-plastic response.

Material Failure Model Solids usually fail under extreme loading conditions, resulting in crushed or cracked material. Material failure models simulate the various ways in which materials fail. Liquids will also fail in tension, a phenomenon usually referred to as cavitation. Engineering Data properties for explicit analysis in the Mechanical application cover a wide range of materials and material behaviors. Some examples are provided below: Class of Material

Material Effects

Metals

Elasticity Shock Effects Plasticity Isotropic Strain Hardening Kinematic Strain Hardening Isotropic Strain Rate Hardening Isotropic Thermal Softening Ductile Fracture Brittle Fracture (Fracture Energy based) Dynamic Failure (Spall)

Concrete/Rock

Elasticity Shock Effects Porous Compaction Plasticity Strain Hardening

164

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Explicit Material Library Class of Material

Material Effects Strain Rate Hardening in Compression Strain Rate Hardening in Tension Pressure Dependent Plasticity Lode Angle Dependent Plasticity Shear Damage/Fracture Tensile Damage/Fracture

Solid/Sand

Elasticity Shock Effects Porous Compaction Plasticity Pressure Dependent Plasticity Shear Damage/Fracture Tensile Damage/Fracture

Rubbers/Polymers

Elasticity Viscoelasticity Hyperelasticity

Orthotropic

Orthotropic Elasticity

The Engineering Data properties supported by explicit analysis are described below. Additional material modeling options, particularly in the areas of composite materials and reactive materials, are available in the ANSYS Autodyn product.

7.2. Explicit Material Library An extensive set of material data is provided in the Engineering Data Explicit library. We strongly recommend that you review the material data before using it in production applications. In particular, some of the materials only contain a partial definition of the material. This data may need to be complemented with additional properties to give the full definition required for the simulation. Explicit Material Library PlasticsADIPRENE LUCITE NEOPRENE

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

165

Material Models Used in Explicit Dynamics Analysis POLYCARB POLYRUBBER POLYRUBBERH POLYSTYRENE RUBBER1 RUBBER2 RUBBER3 EPOXY RES EPOXY RES2 PHENOXY PLEXIGLAS POLYURETH NYLONS POLYETHYL TEFLON TEFLONH Sand/ConcreteCONC 140MPA CONC 35 MPA CONCRETEL INCENDPOWD PERICLASE SAND Mineral/ElementANTIMONY BARIUM BISMUTH CALCIUM GERMANIUM

166

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Explicit Material Library POTASSIUM QUARTZ SODIUM CHLORIDE SODIUM SULFUR VANADIUM VANADIUM2 Glass/CeramicsBORON CARBIDE FLOATGLASB FLOATGLASS LiquidParafin WATER WATER2 WATER3 Metals/AlloysAL 1100–O AL 2024 AL 2024–T4 AL 6061–T6 AL 7039 AL 7075–T6 AL 921–T AL 2024T351 AL 203–99.5 AL 203–99.7 AL203 CERA AL5083H116

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

167

Material Models Used in Explicit Dynamics Analysis ALUMINUM BERYLLIUM BERYLLIUM2 BRASS CADMIUM CART BRASS CHROMIUM COBALT COPPER COPPER2 CU OFHC CU OFHC CU OFHC2 CU-OFHC-F DU-.75TI GOLD GOLD 5%CU GOLD2 HAFNIUM HAFNIUM–2 INDIUM IRIDIUM IRON IRON-ARMCO IRON-ARMCO2 IRON-C.E. LEAD LEAD2 LEAD3

168

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Explicit Material Library LITHIUIM LITHIUM F LITH-MAGN MAG AZ-31B MAGNESIUM MAGNESIUM2 MERCURY MOLYBDENUM NICKEL NICKEL ALL NICKEL Z NICKEL-200 NICKEL 3 NIOBIUM NIOBIUM AL NIOBIUM 2 PALLADIUM PLATE 20% IR PLATINUM PLATINUM2 RHA RHENIUM RHODIUM RUBIDIUM SILVER SILVER2 SIS 2541–3 SS 21–6–9 SS 304 Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

169

Material Models Used in Explicit Dynamics Analysis SS-304 STEEL 1006 STEEL 4340 STEEL S-7 STEEL V250 STNL. STEEL STRONTIUM TANT 10%W TANTALUM TANTALLUM2 TANTALLUM3 THALLIUM THORIUM THORIUM2 TI 6% AL 4% V TIN TIN2 TITANIUM TITANIUM2 TITANIUM-2 TUNG.ALLOY TUNGSTEN TUNGSTEN2 TUNGSTEN3 U 0.75% TI U 5% MO U 8% NB3 %ZR U – 0.75% TI U3 WT %MD

170

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Linear Elastic URANIUM URANIUM2 URANIUM3 W 4% Ni 2%FE ZINC ZIRCONIUM ZIRCONIUM2

7.3. Density Density is the initial mass per unit volume of a material at time = 0.0.

Note The temperature dependence of the linear elastic properties is not available for explicit dynamics systems. Only a single value can be used. The first defined values in temperature dependent data will be used in the solver.

7.4. Linear Elastic • Young's Modulus • Poisson's Ratio

Note The temperature dependence of the linear elastic properties is not available for explicit dynamics systems. Only a single value can be used. The first defined values in temperature dependent data will be used in the solver.

7.4.1. Isotropic Elasticity Define isotropic linear elastic material behavior by specifying • Young's Modulus • Poisson's ratio

Note The temperature dependence of the linear elastic properties is not available for explicit dynamics systems. Only a single value can be used. The first defined values in temperature dependent data will be used in the solver.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

171

Material Models Used in Explicit Dynamics Analysis

7.4.2. Orthotropic Elasticity Define orthotropic linear elastic material behavior by specifying: • Young's Modulus in direction X • Young's Modulus in direction Y • Young's Modulus in direction Z • Poisson's ratio XY • Poisson's ratio YZ • Poisson's ratio XZ • Shear Modulus XY • Shear Modulus YZ • Shear Modulus XZ

Note The coordinate system X, Y, Z relates to the local coordinate system assigned to the body.

7.4.3. Viscoelastic To represent strain rate dependent elastic behavior, a linear viscoelastic model can be used. The long term behavior of the model is described by the long term or elastic shear modulus G∞. Viscoelastic behavior is introduced via an instantaneous shear modulus and a viscoelastic decay constant . The viscoelastic deviatoric stress at time increment n+1 is calculated from the viscoelastic stress at time increment n and the deviatoric strain increments at time increment n via

where is the long term shear modulus of the material is the instantaneous shear modulus of the material. This value is derived from linear elastic properties or defined directly using the equation of state, shear modulus property is the viscoelastic decay constant The deviatoric viscoelastic stress is added to the elastic stress to give the total stress at the end of each cycle.

Note The model must be combined with either the linear elastic property or an equation of state property (including shear modulus).

172

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Hyperelasticity The model can only be applied to solid bodies. Table 7.1: Input Data Name

Symbol

Units

Instantaneous Shear Modulus (High rate)

Stress

Viscoelastic Decay Constant

1/ time

Notes

Custom results variables available for this model. Name

Description

Solids

Shells

Beams

VTXX

Viscoelastic stress XX

Yes

No

No

VTYY

Viscoelastic stress YY

Yes

No

No

VTZZ

Viscoelastic stress ZZ

Yes

No

No

VTXY

Viscoelastic stress XY

Yes

No

No

VTYZ

Viscoelastic stress YZ

Yes

No

No

VTZX

Viscoelastic stress ZX

Yes

No

No

7.5. Test Data Uniaxial Test Data Biaxial Test Data Shear Test Data Volumetric Test Data

7.6. Hyperelasticity Following are several forms of strain energy potential (Ψ) provided for the simulation of nearly incompressible hyperelastic materials. The different models are generally applicable over different ranges of strain as illustrated in the table below, however these numbers are not definitive and users should verify the applicability of the model chosen prior to use. Currently hyperelastic materials may only be used in solid elements for explicit dynamics simulations. Model

Applied Strain Range

Neo-Hookean

30%

Mooney-Rivlin

30%-200% depending on order

Polynomial Ogden

Up to 700%

Neo-Hookean The strain energy function for the Neo-Hookean hyperelastic model is, Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

173

Material Models Used in Explicit Dynamics Analysis

where is the deviatoric first principal invariant, J is the Jacobian and the required input parameters are defined as: µ = initial shear modulus of the material d= incompressibility parameter. and the initial bulk modulus is defined as: K = 2/d

Mooney-Rivlin The strain energy function of a hyperelastic material can be expanded as an infinite series in terms of the first and second deviatoric principal invariants and , as follows,

The 2, 3, 5 and 9 parameter Mooney-Rivlin hyperelastic material models have been implemented and are described in turn below.

2–Parameter Mooney-Rivlin Model The strain energy function for the 2–parameter model is,

where: C10, C01 = material constants d = material incompressibility parameter. The initial shear modulus is defined as:

and the initial bulk modulus is defined as: K = 2/d

3–Parameter Mooney-Rivlin Model The strain energy function for the 3–parameter model is,

where the required input parameters are defined as: C

174

10

,C

01

,C

11

= material constants

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Hyperelasticity d = material incompressibility parameter The bulk and shear modulus are as defined for the 2–parameter Mooney-Rivlin model.

5–Parameter Mooney-Rivlin Model The strain energy function for the 5–parameter model is, (7.1) where the required input parameters are defined as: C 10 ,C 01 ,C 20 ,C 11 ,C 02 = material constants d = material incompressibility parameter. The bulk and shear modulus are as defined for the 2–parameter Mooney-Rivlin model.

9–Parameter Mooney-Rivlin Model The strain energy function for the 9–parameter hyperelastic model is, (7.2)

where the required input parameters are defined as: C 10 ,C 01 ,C 20 ,C 11 , C 02 , C 30 , C 21 , C d = material incompressibility parameter.

12

,C

03

= material constants

The bulk and shear modulus are as defined for the 2–parameter Mooney-Rivlin model.

Polynomial The strain energy function of a hyperelastic material can be expanded as an infinite series of the first and second deviatoric principal invariants l 1 and l 2. The polynomial form of strain energy function is given below:

1st, 2nd, and 3rd order polynomial hyperelastic material models have been implemented in the solver where N is 1, 2 or 3 respectively. Cmn = material constants dk = material incompressibility parameters. The initial shear modulus is defined as:

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

175

Material Models Used in Explicit Dynamics Analysis and the initial bulk modulus is defined as: K = 2/d1

Yeoh The Yeoh hyperelastic strain energy function is similar to the Mooney-Rivlin models described above except that it is only based on the first deviatoric strain invariant. It has the general form,

Yeoh 1st order The strain energy function for the first order Yeoh model is,

where: N=1 C10 = material constant d1 = incompressibility parameter The initial shear modulus is defined as: µ = 2c10 and the initial bulk modulus is defined as: K = 2/d1

Yeoh 2nd order The strain energy function for the second order Yeoh hyperelastic model is

where the required input parameters are defined as: N = 2. C10, C20 = material constants d1, d2 = incompressibility parameters See 1st order Yeoh model for definitions of the initial shear and bulk modulus.

Yeoh 3rd order The strain energy function for the third order Yeoh hyperelastic model is,

176

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Hyperelasticity

where the required input parameters are defined as: N = 3. C10, C20, C30 = material constants d1, d2, d3 = incompressibility parameters See 1st order Yeoh model for definitions of the initial shear and bulk modulus.

Ogden The Ogden form of the strain energy function is based on the deviatoric principal stretches of the leftCauchy-Green tensor and has the form,

Ogden 1st Order The strain energy function for the first order Ogden hyperelastic model is, where: λ p = deviatoric principal stretches of the left-Cauchy-Green tensor J = determinant of the elastic deformation gradient µp, αp and dp = material constants The initial shear modulus is given as:

and the initial bulk modulus is:

Ogden 2nd order The strain energy function for the first order Ogden hyperelastic model is,

where: λ p= deviatoric principal stretches of the left-Cauchy-Green tensor J = determinant of the elastic deformation gradient

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

177

Material Models Used in Explicit Dynamics Analysis µp, α

p

and dp = material constants

The initial shear modulus is given as:

and the initial bulk modulus is:

Ogden 3rd order The strain energy function for the first order Ogden hyperelastic model is,

where: λ p= deviatoric principal stretches of the left-Cauchy-Green tensor J = determinant of the elastic deformation gradient µp, α p and dp = material constants The initial shear modulus is given as:

and the initial bulk modulus is:

7.7. Plasticity All stress-strain input should be in terms of true stress and true (or logarithmic) strain and result in all output as also true stress and true strain. For small-strain regions of response, true stress-strain and engineering stress-strain are approximately equal. If your stress-strain data is in the form of engineering stress and engineering strain you can convert: • strain from engineering strain to logarithmic strain using: • engineering stress to true stress using:

Note This stress conversion is only valid for incompressible materials.

178

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Plasticity The following Plasticity models are discussed in this section: 7.7.1. Bilinear Isotropic Hardening 7.7.2. Multilinear Isotropic Hardening 7.7.3. Bilinear Kinematic Hardening 7.7.4. Multilinear Kinematic Hardening 7.7.5. Johnson-Cook Strength 7.7.6. Cowper-Symonds Strength 7.7.7. Steinberg-Guinan Strength 7.7.8. Zerilli-Armstrong Strength

7.7.1. Bilinear Isotropic Hardening This plasticity material model is often used in large strain analyses. A bilinear stress-strain curve requires that you input the Yield Strength and Tangent Modulus. The slope of the first segment in the curve is equivalent to the Young's modulus of the material while the slope of the second segment is the tangent modulus. Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

Yes*

Yes*

SUBL_EPS

Effective sublayer plastic strain

No

Yes

No

*Resultant value over shell/beam section.

7.7.2. Multilinear Isotropic Hardening This plasticity material model is often used in large strain analyses. Do not use this model for cyclic or highly nonproportional load histories in small-strain analyses. You must supply the data in the form of plastic strain vs. stress. The first point of the curve must be the yield point, that is, zero plastic strain and yield stress. The slope of the stress-strain curve is assumed to be zero beyond the last user-defined stress-strain data point. No segment of the curve can have a slope of less than zero.

Note You can define up to 10 stress strain pairs using this model in explicit dynamics systems. Temperature dependence of the curves is not directly supported. Temperature dependent plasticity can be represented using the Johnson-Cook plasticity model. Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

Yes*

Yes*

SUBL_EPS

Effective sublayer plastic strain

No

Yes

No

*Resultant value over shell/beam section.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

179

Material Models Used in Explicit Dynamics Analysis

7.7.3. Bilinear Kinematic Hardening This plasticity material model assumes that the total stress range is equal to twice the yield stress, to include the Bauschinger effect. This model may be used for materials that obey Von Mises yield criteria (includes most metals). The tangent modulus cannot be less than zero or greater than the elastic modulus. Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

Yes*

Yes*

SUBL_EPS

Effective sublayer plastic strain

No

Yes

No

*Resultant value over shell/beam section.

7.7.4. Multilinear Kinematic Hardening This plasticity model simulates metal plasticity behavior under cyclic loading. You must supply the data in the form of plastic strain vs. stress. The first point of the curve must be the yield point, that is, zero plastic strain and yield stress. No segment can have a slope of less than zero. The slope of the stressstrain curve is assumed to be zero beyond the last user-defined stress-strain data point. No segment of the curve can have a slope of less than zero.

Note You can define up to 10 stress strain pairs using this model in explicit dynamics systems. Temperature dependence of the curves is not directly supported. Temperature dependent plasticity can be represented using the Johnson-Cook plasticity model. This model is available for solid elements in explicit dynamics systems. Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

No

No

SUBL_EPS

Effective sub layer plastic strain

No

No

No

Note This material property can only be applied to solid bodies.

7.7.5. Johnson-Cook Strength Use this model to represent the strength behavior of materials, typically metals, subjected to large strains, high strain rates and high temperatures. Such behavior might arise in problems of intense impulsive loading due to high velocity impact. With this model, the yield stress varies depending on strain, strain rate and temperature. The model defines the yield stress Y as

180

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Plasticity

where = effective plastic strain = normalized effective plastic strain rate TH = homologous temperature = (T-Troom)/(Tmelt -Troom) The five material constants are A, B, C, n and m. The expression in the first set of brackets gives the stress as a function of strain when = 1.0 sec-1 and TH = 0 (for laboratory experiments at room temperature). The constant A is the basic yield stress at low strains while B and n represent the effect of strain hardening. The expressions in the second set of brackets represent the effects of strain rate on the yield strength of the material. The reference strain rate against which the material data was measured is used to normalize the plastic strain rate enhancement. 1.0/second is used by default. The expression in the third set of brackets represents thermal softening such that the yield stress drops to zero at the melting temperature Tmelt. The plastic flow algorithm used in this model has an option to reduce high frequency oscillations that are sometimes observed in the yield surface under high strain rates. A first order strain rate correction is applied by default. An additional implicit strain rate correction is available that can be used in cases where the first order strain rate correction doesn’t suffice, although at the cost of extra CPU time usage. The Johnson-Cook strength model can be used in all element types and in combination with all equations of state and failure properties.

Note A specific heat capacity property should be defined to enable the calculation of temperature hence thermal softening effects. Name

Symbol

Units

Initial Yield Stress

A

Stress

Hardening Constant

B

Stress

Hardening Exponent

n

None

Strain Rate Constant

C

None

Thermal Softening Exponent

m

None

Melting Temperature

Tmelt

Temperature

Reference Strain Rate

None

Notes

Units fixed at 1/sec Default = 1.0

Strain Rate Correction

None

Option List: None

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

181

Material Models Used in Explicit Dynamics Analysis Name

Symbol

Units

Notes 1st Order (Default) Implicit

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

Yes*

Yes*

EFF_PL_STN_RATE

Effective Plastic Strain Rate

Yes

Yes*

Yes*

TEMP

Temperature**

Yes

Yes*

Yes*

SUBL_EPS

Effective sublayer plastic strain

No

Yes

No

*Resultant value over shell/beam section. **Temperature will be non-zero only if a specific heat capacity is defined.

7.7.6. Cowper-Symonds Strength The Cowper-Symonds strength model lets you define the yield strength of isotropic strain hardening, strain rate dependent materials. The yield surface is defined as

where A is yield stress at zero plastic strain B is the strain hardening coefficient n is the strain hardening exponent D and q are the strain rate hardening coefficients It should be noted that, in the implementation within the Explicit Dynamics solver, the plastic strain rate ( ) used in the Cowper Symonds model has a minimum value of unity to allow for compatibility with the linear strain rate correction method. The consequence of this is that for plastic strain rates less than unity, the material will exhibit a strain rate hardening effect equal to that for a strain rate of unity. The plastic flow algorithm used in this model has an option to reduce high frequency oscillations that are sometimes observed in the yield surface under high strain rates. A first order strain rate correction is applied by default. An additional implicit strain rate correction is available that can be used in cases where the first order strain rate correction doesn’t suffice, although at the cost of extra CPU time usage. Note that the strain rate constants should be input assuming that the units of strain rate are 1/second. The Cowper-Symonds strength model can be used in all element types and in combination with all equations of state and failure properties. Name

Symbol

Units

Initial Yield Stress

A

Stress

Hardening Constant

B

Stress

182

Notes

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Plasticity Name

Symbol

Units

Hardening Exponent

n

None

Strain Rate Constant

D

None

Strain Rate Constant

q

None

Strain Rate Correction

-

None

Notes Assumed 1/second in all cases Option List: None 1st Order (Default) Implicit

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

Yes*

Yes*

EFF_PL_STN_RATE

Effective Plastic Strain Rate

Yes

Yes*

Yes*

SUBL_EPS

Effective sublayer plastic strain

No

Yes

No

*Resultant value over shell/beam section.

7.7.7. Steinberg-Guinan Strength In this formulation the authors have assumed that while yield stress initially increases with strain rate, experimental data on shock-induced free surface velocity versus time records indicate that at high strain rates (greater than 105sec-1) strain rate effects become insignificant compared to other effects and that the yield stress reaches a maximum value which is subsequently strain rate independent. They have also postulated that the shear modulus increases with increasing pressure and decreases with increasing temperature and in doing this they have attempted to include modeling of the Bauschinger effect into their calculations. They have therefore produced expressions for the shear modulus and yield strength as functions of effective plastic strain, pressure and internal energy (temperature). The constitutive relations for shear modulus G and yield stress Y for high strain rates are :

subject to where ε = effective plastic strain T = temperature (degrees K) η = compression = ν0/ ν

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

183

Material Models Used in Explicit Dynamics Analysis and the primed parameters with the subscripts p and T are derivatives of that parameter with respect to pressure and temperature at the reference state (T = 300 K, p= 0, ε = 0). The subscript zero also refers to values of G and Y at the reference state. If the temperature of the material exceeds the specified melting temperature the shear modulus and yield strength are set to zero.

Note A specific heat capacity property should be defined to enable the calculation of temperature hence the melting effect. Table 7.2: Input Data Name

Symbol

Units

Initial Yield Stress

Y

Stress

Maximum Yield Stress

Ymax

Stress

Hardening Constant

Notes

None

Hardening Exponent

n

None

Derivative dG/dP

G'P

None

Derivative dG/dT

G'T

Stress/Temperature

Derivative dY/dP

Y'P

None

Melting Temperature

Tmelt

Temperature

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

Yes*

Yes*

EFF_PL_STN_RATE

Effective Plastic Strain Rate

Yes

Yes*

Yes*

TEMP

Temperature**

Yes

Yes*

Yes*

SUBL_EPS

Effective sublayer plastic strain

No

Yes

No

*Resultant value over shell/beam section. **Temperature will be non-zero only if a specific heat capacity is defined.

7.7.8. Zerilli-Armstrong Strength While the Johnson-Cook model predicted the behavior of most materials in the Taylor tests, the model's prediction and test results for OFHC (oxygen free high conductivity) copper did not agree well. In an approach seeking to improve on Johnson-Cook, Zerilli and Armstrong proposed a more sophisticated constitutive relation obtained through the use of dislocation dynamics. The effects of strain hardening, strain-rate hardening and thermal softening (based on thermal activation analysis) have been incorporated into the formulation. The effect of grain size has also been included.

184

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Plasticity The relation has a relatively simple expression and should be applicable to a wide range of fcc (face centered cubic) materials. A relation for iron has also been developed and is also applicable to other bcc (body centered cubic) materials. An important point made by Zerilli and Armstrong is that each material structure type (fcc, bcc, hcp) will have its own constitutive behavior, dependent on the dislocation characteristics for that particular structure. For example, a stronger dependence of the plastic yield stress on temperature and strain rate is known to result for bcc metals as compared with fcc metals. With this model, the yield stress varies depending on strain, strain rate and temperature. The yield stress is given by: For fcc metals

For bcc metals:

where ε = effective plastic strain = normalized effective plastic strain rate T = temperature (degrees K) The parameters Y0, C1, C2, C3, C4, C5 and n are material constants. The plastic flow algorithm used in this model has an implicit strain rate correction option to reduce high frequency oscillations that are sometimes observed in the yield surface under high strain rates. The strain rate correction algorithm will be at the expense of increased CPU usage.

Note A specific heat capacity property should be defined to enable the calculation of temperature hence the melting effect. Table 7.3: Input Data Name

Symbol

Units

Initial Yield Stress

Y0

Stress

Hardening Constant #1

C1

Stress

Hardening Constant #2

C2

Stress

Hardening Constant #3

C3

None

Hardening Constant #4

C4

None

Hardening Constant #5

C5

Stress

Hardening Constant n

n

None

Notes

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

185

Material Models Used in Explicit Dynamics Analysis Name

Symbol

Reference Strain Rate

Units

Notes

None

Units fixed at 1/sec Default = 1.0

Strain Rate Correction

None

Option List: None (Default) Implicit

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

Yes*

Yes*

EFF_PL_STN_RATE

Effective Plastic Strain Rate

Yes

Yes*

Yes*

TEMP

Temperature**

Yes

Yes*

Yes*

SUBL_EPS

Effective sublayer plastic strain

No

Yes

No

*Resultant value over shell/beam section. **Temperature will be non-zero only if a specific heat capacity is defined.

7.8. Brittle/Granular A number of properties are available to allow modeling of brittle/granular materials such as concrete, rock, soil, glass and ceramics. 7.8.1. Drucker-Prager Strength Linear 7.8.2. Drucker-Prager Strength Stassi 7.8.3. Drucker-Prager Strength Piecewise 7.8.4. Johnson-Holmquist Strength Continuous 7.8.5. Johnson-Holmquist Strength Segmented 7.8.6. RHT Concrete Strength 7.8.7. MO Granular

7.8.1. Drucker-Prager Strength Linear This model is used to represent the behavior of dry soils, rocks, concrete and ceramics where the cohesion and compaction behavior of the materials result in an increasing resistance to shear up to a limiting value of yield strength as the loading increases. The yield strength of these materials is highly dependent on pressure. There are three forms available for this model; linear, stassi and piecewise. Although the yield stress is pressure dependent in each case, the flow rule is volume independent; in other words, a Prandtl-Reuss type.

186

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Brittle/Granular Figure 7.1: Drucker-Prager Strength Linear Y

P

The yield stress is a linear function of pressure (the original Drucker-Prager model)

Note This property can only be applied to solid bodies. Table 7.4: Input Data Name

Symbol

Yield Stress (at zero pressure)

Units

Notes

Stress Θ

Slope (degrees)

None

Slope in degrees

Custom results variables available for this model: Name

Description

Solids Shells Beams

EFF_PL_STN Effective Plastic Strain

Yes

No

No

Pressure

Yes

No

No

Material Pressure

Note This material property can only be applied to solid bodies.

7.8.2. Drucker-Prager Strength Stassi Figure 7.2: Drucker-Prager Strength Stassi Y

P

The Stassi yield condition takes the form:

where J2Y is the second invariant of the deviatoric stress yield Y0 is the yield strength in simple tension Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

187

Material Models Used in Explicit Dynamics Analysis k is the ratio between the yield strengths in compression and tension p is the pressure

Note This property can only be applied to solid bodies. Table 7.5: Input Data Name

Symbol Units Notes

Yield Stress Uniaxial Tension

Y0

Stress Measure under uniaxial stress conditions

Yield Stress Uniaxial Compression

Stress Measure under uniaxial stress conditions

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

No

No

Pressure

Pressure

Yes

No

No

7.8.3. Drucker-Prager Strength Piecewise Figure 7.3: Drucker-Prager Strength Piecewise Yield stress Y varies with pressure as a piecewise linear function. Constant shear modulus G Yield Stress Y Ymax

Piecewise Linear

Pressure P

The yield stress is a piecewise linear function of pressure. In tension (negative values of pressure), such materials have little tensile strength and this is modeled by dropping the yield stress rapidly to zero as pressure goes negative to give a realistic value for the limited tensile strength.

Note You can use up to 10 pressure-yield points to define the material strength curve. This property can only be applied to solid bodies. Table 7.6: Input Data Name

Symbol

Units

Yield Stress vs Pressure

Y vs P

Stress

188

Notes

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Brittle/Granular Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

No

No

Pressure

Material Pressure

Yes

No

No

7.8.4. Johnson-Holmquist Strength Continuous This model is used for modeling brittle materials such as glass and ceramics (Johnson & Holmquist 1993) [1] subjected to large pressures, shear strain and high strain rates. Two forms of this model are found in the literature and are available in explicit dynamics systems; continuous (JH2), segmented (JH1). Both these forms can be used with a linear or energy dependent polynomial equation of state. The strength of the brittle material is described as a smoothly varying function of intact strength, fractured strength, strain rate and damage via a dimensionless analytic function as described below. P* is the pressure normalized by the pressure at the Hugoniot Elastic Limit (PHELL) and T* is the maximum tensile hydrostatic pressure normalized by PHELL. The effective plastic strain rate, , is normalized by a reference strain rate of 1.0/second. Figure 7.4: Johnson-Holmquist Strength Model

Intact Surface, Damage, Fractured, As the material undergoes inelastic deformation, damage is assumed to accumulate which degrades the overall load carrying capacity of the materials. The Johnson-Holmquist Damage model was developed for the simulation of the compressive and shear induced strength and failure of brittle materials. Damage is accumulated as the ratio of incremental plastic strain over the current estimated fracture strain. The effective fracture strain is pressure dependent as described below.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

189

Material Models Used in Explicit Dynamics Analysis Figure 7.5: Johnson-Holmquist Damage Model

There are two methods for the application of damage to the material strength. The default Gradual failure type results in damage being incrementally applied to the material strength as it accumulates. If the Instantaneous failure type is selected, damage accumulates over time, however it is only applied to the failure surface when its value reaches unity. The material strength instantaneously transitions from intact to fully failed in this case. The model includes an option to represent volumetric dilation of the material due to shear deformation (Bulking). The work done in deforming the material inelastically in shear can be converted into a pressure increase, hence volumetric dilation (if unconstrained). The amount of work which is converted into dilation pressure is controlled through the Bulking constant, B. This can have values ranging from 0.0 (representing no shear induced dilatancy) to 1.0 (producing maximum dilatancy effects).

Note If the Bulking constant, B is greater than zero then the Johnson-Holmquist model should be used in conjunction with a polynomial equation of state or linear elasticity. This property can only be applied to solid bodies. Table 7.7: Input Data Name

Symbol

Units

Notes

Hugoniot Elastic Limit

σHEL

Stress

Elastic limit under dynamic compressive uniaxial strain conditions

Intact Strength Constant A

A

None

Intact Strength Exponent n

n

None

Strain Rate Constant C

C

None

Fracture Strength Constant B

B

None

190

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Brittle/Granular Name

Symbol

Units

Fracture Strength Exponent m

m

None

Maximum Fracture Strength Ratio

σF Max

None

Damage Constant D1

D1

None

Damage Constant D2

D2

None

Bulking Constant

B

None

Hydrodynamic Tensile Limit

T

Stress

Notes

Maximum fracture strength as fraction of intact strength

Failure Type

Option list: Gradual (Default) Instantaneous

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_Pl_STN

Effective Plastic Strain

Yes

No

No

EFF_Pl_STN_RATE

Effective Plastic Strain Rate

Yes

No

No

PRESSURE

Pressure

Yes

No

No

DAMAGE

Damage

Yes

No

No

STATUS

Material Status**

Yes

No

No

PRES_BULK

Dilation pressure

Yes

No

No

ENERGY_DAM

Damage energy contributing to bulking

Yes

No

No

**Material status indicators (1= elastic, 2= plastic, 3 = bulk failure, 4 = bulk failure, 5 = failed principal direction 1, 6 = failed principal direction 2, 7 = failed direction 3)

7.8.5. Johnson-Holmquist Strength Segmented Recent studies (Holmquist and Johnson 2002) have showed that gradual softening in the JH2 model has not been supported by available experimental data yet while there are some indications that an early variant of the model, known as JH1, may be more accurate. In the JH1 material model, material strength is described by linear segments and the damage is always applied instantaneously.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

191

Material Models Used in Explicit Dynamics Analysis Figure 7.6: Johnson-Holmquist Strength Segmented

Note If the Bulking constant, B is greater than zero then the Johnson-Holmquist model should be used in conjunction with a polynomial equation of state or linear elasticity. This property can only be applied to solid bodies. Holmquist, T.J. & Johnson, G.R. (2002). Response of silicon carbide to high velocity impact. Journal of Applied Physics, pp 5858-5866, Vol 91, No. 9, May 1, 2002. Table 7.8: Input Data Name

Symbol

Units

Notes

Hugoniot Elastic Limit

σHEL

Stress

Elastic limit under dynamic compressive uniaxial strain conditions

Intact Strength Constant S1

S1

Stress

Intact Strength Constant P1

P

1

Stress

Intact Strength Constant S2

S2

Stress

Intact Strength Constant P2

P

2

Stress

Strain Rate Constant C

C FMax

None

Maximum Fracture Strength

S

Stress

Failed Strength Constant

α

None

Damage Constant

D1

None

Damage Constant

D2

Stress

Bulking Constant

B

None

Hydrodynamic Tensile Limit

T

Stress

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

No

No

192

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Brittle/Granular Name

Description

Solids

Shells

Beams

EFF_PL_STN_RATE

Effective Plastic Strain Rate

Yes

No

No

PRESSURE

Pressure

Yes

No

No

DAMAGE

Damage

Yes

No

No

STATUS

Material Status**

Yes

No

No

PRES_BULK

Dilation pressure

Yes

No

No

ENERGY_DAM

Damage energy contributing to bulking

Yes

No

No

**Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4 = bulk failure, 5 = failed principal direction 1, 6 = failed principal direction 2, 7 = failed principal direction 3)

7.8.6. RHT Concrete Strength The RHT concrete model is an advanced plasticity model for brittle materials developed by Riedal et al [2], [3], [4]. It is particularly useful for modeling the dynamic loading of concrete. It can also be used for other brittle materials such as rock and ceramic. The RHT constitutive model is a combined plasticity and shear damage model in which the deviatoric stress in the material is limited by a generalized failure surface of the form: (7.3) This failure surface can be used to represent the following aspects of the response of geological materials • Pressure hardening • Strain hardening • Strain rate hardening in tension and compression • Third invariant dependence for compressive and tensile meridians • Strain softening (shear induced damage) • Coupling of damage due to porous collapse The model is modular in nature and is designed such that individual aspects of the material behavior can be turned on and off. This gives the model significant practical usefulness. Further details of how the model represents the various aspects of the material behavior are now presented.

Fracture surface The fracture surface is represented through the expression (7.4) where fc' is the cylinder strength AFAIL, NFAIL are user defined parameters Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

193

Material Models Used in Explicit Dynamics Analysis P* is pressure normalized with respect to fc' Pspall* is the normalized hydrodynamic tensile limit FRATE is a rate dependent enhancement factor Additionally, there is an option to truncate the fracture surface to fit through the characteristic points that can be observed experimentally at low pressures, while retaining the flexibility to match data at high pressures. This feature is described in the figure below. Figure 7.7: RHT Representation of Compressive Meridian

Tensile and Compressive Meridians The RHT model can represent the difference between the compressive and tensile meridian in terms of material strength using the third invariant dependence term (R3). This can be utilized to represent the observed reduction in strength of concrete under triaxial extension, compared with triaxial compression. The third invariant dependence term is formulated using the expression

(7.5)

The input parameter Q2.0 defines the ratio of strength at zero pressure and the coefficient BQ defines the rate at which the fracture surface transitions from approximately triangular in form to a circular form with increasing pressure (Figure 7.8: Third invariant dependence (p. 195)).

194

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Brittle/Granular Figure 7.8: Third invariant dependence Te nsile meridian Q 2 = 1.0

Compressive meridian

Q 2 = 0.5

Strain Hardening Strain hardening is represented in the model through the definition of an elastic limit surface and a “hardening” slope. The elastic limit surface is scaled down from the fracture surface by user defined ratios; (elastic strength/fc) and (elastic strength/ft). The pre-peak fracture surface is subsequently defined through interpolation between the elastic and fracture surfaces using the “hardening” slope,

.

This is shown in Figure 7.9: Bi-linear strain hardening function (p. 195) for the case of uniaxial compression.

where

Figure 7.9: Bi-linear strain hardening function

Shear Damage Damage is assumed to accumulate due to inelastic deviatoric straining (shear induced cracking) using the relationships

(7.6)

where D1 and D2 are material constants used to describe the effective strain to fracture as a function of pressure. Damage accumulation can have two effects in the model • Strain softening (reduction in strength) Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

195

Material Models Used in Explicit Dynamics Analysis The current fracture surface (for a given level of damage) is scaled down from the intact surface using the expression (7.7) where (7.8) The term Y XTC*SFMAX is used to limit the maximum residual shear strength (for completely damaged material) to be a fraction (SFMAX) of the current fracture strength. • Reduction in shear stiffness The current shear modulus is defined through the expression (7.9)

Porous Collapse Damage The model includes the option to include a cap to limit the elastic deviatoric stress under large compressions. This effectively leads to the assumption that porous compaction results in a reduction in deviatoric strength. The final combination of elastic, fracture and residual failure surfaces is shown schematically below in Figure 7.10: RHT Elastic, Fracture and Residual Failure Surfaces (p. 196). Figure 7.10: RHT Elastic, Fracture and Residual Failure Surfaces

Strain Rate Effects Strain rate effects are represented through increases in fracture strength with plastic strain rate. Two different terms can be used for compression and tension with linear interpolation being used in the intermediate pressure regime.

where = 3e-6 in tension and 30e-6 in compression.

196

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Brittle/Granular

Tensile Failure By default, tensile failure is achieved using a hydrodynamic tensile limit. The maximum tensile pressure in the material is limited to (7.10) Using this option, no additional user input is required since the value of Pmin is derived from ft, which forms part of the input for the strength model. Note that the principal tensile stress and crack softening failure properties may also be used in conjunction with this model. Data for concrete with cube strengths of 35MPa and 140MPa are included in the distributed material library. The model is formulated such that input can be scaled with the cube strength; fc for example. you can retrieve one of the two concretes in the library, change its cube strength to match the concrete you want to model and the remaining terms will automatically scale proportionately. The resulting data set will be approximate and we recommend validation of the material data against experimental characterization tests in all cases.

Note This property can only be applied to solid bodies. Table 7.9: Input Data Name

Symbol

Units

Compressive Strength

fc

Stress

Tensile Strength

ft/fc

None

Shear Strength

fs/fc

None

Intact failure surface constant A

AFAIL

None

Intact failure surface exponent N

NFAIL

None

Tens./Comp. Meridian ratio

Q2.0

None

Brittle to Ductile Transition

BQ

None

Hardening Slope

None

Elastic Strength/ft

None

Elastic Strength/fc

None

Fracture Strength Constant

B

None

Fracture Strength Exponent

m

None

Compressive strain rate exponent

α

None

Notes

Gel/(Gel-Gpl)

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

197

Material Models Used in Explicit Dynamics Analysis Name

Symbol

Units

Tensile strain rate exponent

δ

None

Maximum fracture strength ratio

SFMAX

None

Use cap on elastic surface

Notes

None

Option: Yes (default) No

Damage constant D1

D1

None

Damage constant D2

D2

None

Minimum strain to failure

None

Residual Shear modulus fraction

None

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

No

No

EFF_PL_STN_RATE

Effective Plastic Strain Rate

Yes

No

No

PRESSURE

Pressure

Yes

No

No

DAMAGE

Damage

Yes

No

No

STATUS

Material Status**

Yes

No

No

**Material status indicators (1=elastic, 2= plastic, 3 = bulk failure, 4 = bulk failure, 5= failed principal direction 1, 6= failed principal direction 2, 7 = failed principal direction 3)

7.8.7. MO Granular This model is an extension of the Drucker-Prager model that takes into account effects associated with granular materials such as powders, soil and sand. In addition to pressure hardening, the model also represents density hardening and variations in the shear modulus with density. The yield stress is made up of two components, one dependent on the density and one dependent on the pressure,

where σy, σp and σρ denote the total yield stress, the pressure yield stress and the density yield stress respectively.

198

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Equations of State The unload/reload slope is defined by the shear modulus which is defined as a function of the zero pressure density of the material.

Note The yield stress is defined by a yield stress - pressure and a yield stress - density curve with up to 10 points in each curve. The shear modulus is defined by a shear modulus - density curve with up to 10 points. All three curves must be defined. This model can only be applied to solid bodies. Table 7.10: Input Data Name

Symbol

Units

Notes

Yield Stress vs Pressure

Stress

Tabular data

Yield Stress vs Density

Stress and Density

Tabular data

Shear Modulus vs Density

Stress and Density

Tabular data

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

No

No

PRESSURE

Pressure

Yes

No

No

DENSITY

Density

Yes

No

No

7.9. Equations of State Background information is discussed in this section along with available EOS models: 7.9.1. Background 7.9.2. Bulk Modulus 7.9.3. Shear Modulus 7.9.4. Ideal Gas EOS 7.9.5. Polynomial EOS 7.9.6. Shock EOS Linear 7.9.7. Shock EOS Bilinear 7.9.8. JWL EOS

7.9.1. Background A general material model requires equations that relate stress to deformation and internal energy (or temperature). In most cases, the stress tensor may be separated into a uniform hydrostatic pressure (all three normal stresses equal) and a stress deviatoric tensor associated with the resistance of the material to shear distortion. Then the relation between the hydrostatic pressure, the local density (or specific volume) and local specific energy (or temperature) is known as an equation of state.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

199

Material Models Used in Explicit Dynamics Analysis Hooke's law is the simplest form of an equation of state and is implicitly assumed when you use linear elastic material properties. Hooke's law is energy independent and is only valid if the material being modeled undergoes relatively small changes in volume (less than approximately 2%). One of the alternative equation of state properties should be used if the material is expected to experience high volume changes during an analysis. Before looking at the various equations of state available, it is good to understand some of the fundamental physics behind their formulations. Details are provided in Explicit Dynamics Analysis Guide (to be published).

7.9.2. Bulk Modulus Bulk Modulus — A bulk modulus can be used to define a linear, energy independent equation of state. Combined with a shear modulus property, this material definition is equivalent to using linear elasticity; in other words, Young's Modulus and Poisson's ratio.

7.9.3. Shear Modulus Shear Modulus — A shear modulus must be used when a solid or porous equation of state is selected to fully define the elastic stiffness of a material. To represent fluids, specify a small value.

7.9.4. Ideal Gas EOS One of the simplest forms of equation of state is that for an ideal polytropic gas which may be used in many applications involving the motion of gases. This may be derived from the laws of Boyle and GayLussac and expressed in the form

This form of equation is known as the Ideal Gas equation of state, and only the value of the adiabatic exponent γ must be supplied. In order to avoid complications with problems with multiple materials where initial small pressures in the gas would generate small unwanted velocities the equation is modified for use in these cases

where pshift is a small initial pressure defined to give a zero starting pressure. The definition of a non-zero adiabatic constant, c, will turn the energy dependent ideal gas equation of state into the following energy independent adiabatic equation of state

200

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Equations of State

Note This equation of state can only be applied to solid bodies. A specific heat capacity should be defined with this property to allow the calculation of temperature. Table 7.11: Input Data Name

Symbol Units

Adiabatic exponent

γ

None

Adiabatic constant

c

None

Pressure shift

Pshift

Pressure

Notes

This equation of state can only be used with solid elements. Custom results variables available for this model: Name

Description

Solids

Shells

Beams

PRESSURE

Pressure

Yes

No

No

DENSITY

Density

Yes

No

No

COMPRESSION

Compression

Yes

No

No

INT_ENERGY

Internal Energy

Yes

No

No

TEMPERATURE

Temperature

Yes

No

No

7.9.5. Polynomial EOS This is a general form of the Mie-Gruneisen form of the equation of state and it has different analytic forms for states of compression and tension. This equation of state defines the pressure as µ> 0 (compression):

µ< 0 (tension)

where µ = compression = ρ/ρ0-1 ρ0 = solid, zero pressure density e = internal energy per unit mass A1, A2, A3, B0,, B1, T1 and T2 are material constants

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

201

Material Models Used in Explicit Dynamics Analysis If T1 is input as 0.0 it is reset to T1 = A1 in the solver. The validity of this equation depends upon the ability to represent the variation of pressure at e = 0 (or some other reference curve) as a simple polynomial in µ of no more than three terms. This is probably true as long as the range in density variation (and hence range in µ) is not too large. The Polynomial equation of state defines the Gruneisen parameter as

This allows a number of useful variants of the Gruneisen parameter to be described:

Note This equation of state can only be used with solid elements. The Poisson's ratio is assumed to be zero when calculating effective strain. A specific heat capacity should be defined with this property to allow the calculation of temperature. Table 7.12: Input Data Name

Symbol

Units

Notes

Parameter A1

A1

Stress

Often equivalent to the material bulk modulus

Parameter A2

A2

Stress

Parameter A3

A3

Stress

Parameter B0

B0

None

Parameter B1

B1

None

Parameter T1

T1

Stress

Parameter T2

T2

Stress

This value will be automatically set to the material bulk modulus if entered as zero.

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

PRESSURE

Pressure

Yes

No

No

202

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Equations of State Name

Description

Solids

Shells

Beams

DENSITY

Density

Yes

No

No

COMPRESSION

Compression

Yes

No

No

VISC_PRESSURE

Viscous Pressure

Yes

No

No

INT_ENERGY

Internal Energy

Yes

No

No

TEMPERATURE

Temperature

Yes

No

No

7.9.6. Shock EOS Linear The Rankine-Hugoniot equations for the shock jump conditions can be regarded as defining a relation between any pair of the variables ρ(density), P (pressure), e (energy), up (particle velocity) and U (shock velocity). In many dynamic experiments making measurements of up and U it has been found that for most solids and many liquids over a wide range of pressure there is an empirical linear relationship between these two variables:

It is then convenient to establish a Mie-Gruneisen form of the equation of state based on the shock Hugoniot:

where it is assumed that Γ ρ = Γ0 ρ0 = constant and

Note that for s>1 this formulation gives a limiting value of the compression as the pressure tends to infinity. The denominator of the first equation above becomes zero and the pressure therefore becomes infinite for 1– (s-1)µ= 0 giving a maximum density of ρ = s ρ0 (s-1). However, long before this regime is approached, the assumption of constant Γ ρ is probably not valid. Furthermore, the assumption of linear variation between the shock velocity U and the particle velocity up does not hold for too large a compression. Γ is known as the Gruneisen coefficient and is often approximated to Γ ~2s-1 in the literature. The Shock EOS linear model lets you optionally include a quadratic shock velocity, particle velocity relation of the form:

The input parameter, S2, can be set to a non-zero value to better fit highly non-linear Us - up material data. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

203

Material Models Used in Explicit Dynamics Analysis Data for this equation of state can be found in various references and many of the materials in the explicit material library.

Note This equation of state can only be applied to solid bodies. The Poisson's ratio is assumed to be zero when calculating effective strain. A specific heat capacity should be defined with this property to allow the calculation of temperature. Table 7.13: Input Data Name

Symbol

Units

Notes

Gruneisen coefficient

Γ

None

Parameter C1

C1

Velocity

Parameter S1

S1

None

Parameter Quadratic S2

S2

1/Velocity

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

PRESSURE

Pressure

Yes

No

No

DENSITY

Density

Yes

No

No

COMPRESSION

Compression

Yes

No

No

VISC_PRESSURE

Viscous Pressure

Yes

No

No

INT_ENERGY

Internal Energy

Yes

No

No

TEMPERATURE

Temperature

Yes

No

No

7.9.7. Shock EOS Bilinear This is an extension of the Shock EOS Linear property. At high shock strengths nonlinearity in the shock velocity - particle velocity relationship is apparent, particularly for non-metallic materials. To account for this nonlinearity, the input calls for the definition of two linear fits to the shock velocity - particle velocity relationship; one at low shock compressions defined by Up > VB and one at high shock compressions defined by Up < VE. The region between VE and VB is covered by a smooth interpolation between the two linear relationships as shown below.

204

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Equations of State Figure 7.11: Fit to Shock Velocity-Particle Velocity Relationship

In the input you are prompted for values of the parameters c1, c2, s1, s2, VE/Vo, VB/Vo, Γo and ρo. Then

Note This equation of state can only be applied to solid bodies. The Poisson's ratio is assumed to be zero when calculating effective strain. A specific heat capacity should be defined with this property to allow the calculation of temperature. Table 7.14: Input Data Name

Symbol

Units

Gruneisen coefficient

Γ

None

Parameter C1

C1

Velocity

Parameter S1

S1

None

Parameter C2

C2

Velocity

Parameter S2

S2

None

Relative Volume VB/V0

VB/V0

None

Relative Volume VE/V0

VE/V0

None

Notes

This equation of state can only be used with solid elements. Custom results variables available for this model: Name

Description

Solids

Shells

Beams

PRESSURE

Pressure

Yes

No

No

DENSITY

Density

Yes

No

No

COMPRESSION

Compression

Yes

No

No

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

205

Material Models Used in Explicit Dynamics Analysis Name

Description

Solids

Shells

Beams

VISC_PRESSURE

Viscous Pressure

Yes

No

No

INT_ENERGY

Internal Energy

Yes

No

No

TEMPERATURE

Temperature

Yes

No

No

7.9.8. JWL EOS The JWL equation of state describes the detonation product expansion down to a pressure of 1 kbar for high energy explosive materials and has been proposed by Jones, Wilkins and Lee according to the following equation

, where ρ0 is the reference density, ρ the density and η = ρ/ρ0. The values of the constants A, B, R1, R2 and ω for many common explosives have been determined from dynamic experiments. Figure 7.12: Pressure as function of density for the JWL equation of state

The standard JWL equation of state can be used in combination with an energy release extension whereby additional energy is deposited over a user-defined time interval. Thermobaric explosives show this behavior and produce more explosive energy than conventional high energy explosives through combustion of inclusions, like aluminum, with atmospheric oxygen after detonation. This option is activated when the additional specific energy is specified different from zero.

206

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Equations of State

Burn on Compression In this process the detonation wave is not predefined but the unburned explosive is initially treated similarly to any other inert material. However, as an initiating shock travels through the unburned explosive and traverses elements within the explosive the compression of all explosive elements is monitored. If and when the compression in a cell reaches a predefined value the chemical energy is allowed to be released at a controlled rate. Burn on compression may be defined in one of two ways: • Pre-burn bulk modulus KBK is zero. The elements start to release their energy when the element compression μ exceeds a specified fraction of the Chapman-Jouguet compression: μ > BCJμCJ, where μCJ = PCJ/(ρDCJ 2) • Pre-burn bulk modulus KBK is non zero. The elements start to release their energy when the element pressure exceeds a specified fraction of the Chapman-Jouguet pressure: P = KBK(ρ/ρ0–1) > BCJPCJ The critical threshold compression and the release rate are parameters that must be chosen with care in order to obtain realistic results. The burn on compression option may give unrealistic results for unconfined regions of explosive since the material is free to expand at the time of initial shock arrival and may not achieve sufficient compression to initiate energy release in a realistic time scale. Typically, a burn logic based upon compression is more successful in Lagrangian computations rather than Eulerian.

Note The constants A, B, R1, R2 and ω should be considered as a set of interdependent parameters and one constant cannot be changed unilaterally without considering the effect of this change on the other parameters. This equation of state can only be applied to solid bodies. The Poisson's ratio is assumed to be zero when calculating effective strain. A specific heat capacity should be defined with this property to allow the calculation of temperature. Table 7.15: Input Data Name

Symbol

Units

Parameter A

A

Stress

Parameter B

B

Stress

Parameter R1

R1

None

Parameter R2

R2

None

Parameter ω

ω

None

C-J Detonation Velocity

DCJ

Velocity

Notes

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

207

Material Models Used in Explicit Dynamics Analysis Name

Symbol

Units

C-J Energy/unit mass

Notes

Energy/mass

C-J Pressure

PCJ

Stress

Burn on compression logic

Burn on compression fraction

BCJ

None

Burn on compression logic

Pre-burn bulk modulus

KBK

Stress

Burn on compression logic

Adiabatic constant

None

Additional specific internal energy/unit mass

Energy/mass

Additional energy release

Begin Time

Time

Start time of additional energy release

End Time

Time

End time of additional energy release

This equation of state can only be used with solid elements. Custom results variables available for this model: Name

Description

Solids

Shells

Beams

PRESSURE

Pressure

Yes

No

No

DENSITY

Density

Yes

No

No

COMPRESSION

Compression

Yes

No

No

INT_ENERGY

Internal Energy

Yes

No

No

TEMPERATURE

Temperature

Yes

No

No

BURN_FRAC

Burn Fraction

Yes

No

No

7.10. Porosity The following Porosity models are discussed in this section: 7.10.1. Porosity-Crushable Foam 7.10.2. Compaction EOS Linear 7.10.3. Compaction EOS Non-Linear 7.10.4. P-alpha EOS

7.10.1. Porosity-Crushable Foam This is a relatively simple strength model designed to represent the crush characteristics of foam materials under impact loading conditions (non-cyclic loading). The model principal stress vs volumetric strain behavior is shown below.

208

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Porosity

The strength model must be used with isotropic elasticity and the following incremental elastic update of pressure and stress deviators is used.

In tension, the model additionally includes the possibility to apply a tension cut-off to the maximum allowable principal tensile stress. If the tensile stress exceeds this value, it is maintained at this value. The model cannot currently be used with other failure properties.

Note This property must be used in combination with isotropic elasticity. The property can only be applied to solid bodies. Note that the plastic strain variable is used to store the inelastic volumetric strain for this porosity model. Table 7.16: Input Data Name

Symbol

Units

Notes

Maximum Principal Stress vs Volumetric Strain

Stress and strain

Tabular data

Maximum Tensile Stress

Stress

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

No

No

PRESSURE

Pressure

Yes

No

No

DENSITY

Density

Yes

No

No

Porous Materials Porous materials are extremely effective in attenuating shocks and mitigating impact pressures. The material compacts to its solid density at relatively low stress levels but, because the volume change is Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

209

Material Models Used in Explicit Dynamics Analysis relatively large, a large amount of energy is irreversibly absorbed thereby attenuating shocks by lengthening the wave in time and reducing it in amplitude as more material is compacted. Cellular porous materials contain a population of microscopic cells separated by cell walls. When stressed the initial elastic compression is assumed to be due to elastic buckling of the cell walls and the plastic flow to be due to plastic deformation of these cell walls. Materials with low initial porosity has fewer cells and thicker cell walls so that the stress required to cause buckling and subsequent deformation of the cell walls will be greater. Once some plastic flow has taken place, even if the fully compacted density hasn't been reached, unloading to zero stress and reloading to the elastic limit will be elastic. This phenomenological behavior is illustrated in the following figure.

pressure

Figure 7.13: Loading-Unloading Behavior for a Porous Solid

Plastic compaction

Fully compacted

Elastic loading Elastic unloading (variable slope)

density

7.10.2. Compaction EOS Linear The response of porous materials is represented via • A plastic compaction path defined as a piecewise linear function of pressure versus density • The elastic unloading/reloading path defined via a piecewise linear function of sound speed versus density. The use of a fixed compaction path (which may be derived from static compression data, either in its original state or arbitrarily enhanced to model dynamic data) is equivalent to using a Mie-Gruneisen equation of state with an assumed value of zero for the Gruneisen Gamma. This ignores the pressure enhancement due to the energy absorption. The elastic bulk stiffness of the material is defined as a piecewise linear curve of sound speed (c) versus density (ρo). The bulk stiffness of the material is given by

The level of compaction in the material is given by

Initially, ρo will be equal to the value defined in the density property of the material. Material property ρs is the solid zero pressure density of the material and corresponds to the fully compacted material density. For a porous material the initial density will be less than the solid density hence the value of

210

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Porosity α will be greater than 1.0. As compaction takes place, α will reduce to a value of 1.0 for the fully compacted state.

Note It is important when using the model to ensure that the input data is such that the elastic loading line from the initial porous density intersects the plastic compaction curve at the intended position. This property must be used in combination with a shear modulus to define the total elastic stiffness of the material. The property can only be applied to solid bodies. The Poisson's ratio is assumed to be zero when calculating effective strain. The input data for the porous model is as follows: Name

Symbol

Solid Density

ρs

Units

Notes Density at zero pressure for fully compacted material

Compaction Curve

Tabular data of compaction pressure against density

Linear Unloading Curve

Tabular data of sound speed against density

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

PRESSURE

Pressure

Yes

No

No

DENSITY

Density

Yes

No

No

COMPRESSION

Compression

Yes

No

No

VISC_PRESSURE

Viscous Pressure

Yes

No

No

INT_ENERGY

Internal Energy

Yes

No

No

ALPHA

Porosity (Alpha)

Yes

No

No

7.10.3. Compaction EOS Non-Linear This property is an extension of the Compaction EOS linear property and can provide a more accurate representation of non-linearity when unloading a porous material. The response of porous materials is represented via • A plastic compaction path defined as a piecewise linear function of pressure versus density • The non-linear unloading defined by means of a piecewise curve of bulk modulus versus density For the non-linear unloading, if the current pressure is less than the current compaction pressure, the pressure is defined by

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

211

Material Models Used in Explicit Dynamics Analysis

This produces a nonlinear unloading pattern, an example of which is shown below:

Note It is important when using the model to ensure that the input data is such that the elastic loading line from the initial porous density intersects the plastic compaction curve at the intended position. This property must be used in combination with a shear modulus to define the total elastic stiffness of the material. The property can only be applied to solid bodies. The Poisson's ratio is assumed to be zero when calculating effective strain. The input data for the porous model is as follows: Name

Symbol

Solid Density

ρs

Units

Notes Density at zero pressure for fully compacted material

Compaction Curve

Tabular data of compaction pressure against density

Nonlinear Unloading Curve

Tabular data of bulk modulus against density

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

PRESSURE

Pressure

Yes

No

No

DENSITY

Density

Yes

No

No

212

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Porosity Name

Description

Solids

Shells

Beams

COMPRESSION

Compression

Yes

No

No

VISC_PRESSURE

Viscous Pressure

Yes

No

No

INT_ENERGY

Internal Energy

Yes

No

No

ALPHA

Porosity (Alpha)

Yes

No

No

7.10.4. P-alpha EOS Although the compaction models give good results for low stress levels and low α materials, it is very desirable to obtain a single formulation for the modeling of a porous material which gives a good representation over a wide stress range and variety of materials. Such a model has been derived by Hermann (1969) [5] and this is available in explicit dynamics. Hermann's P-alpha model uses a phenomenological approach to devising a representation which gives the correct behavior at high stresses but at the same time provides a reasonably detailed description of the compaction process at low stress levels. The principal assumption is that the specific internal energy is the same for a porous material as for the same material at solid density at identical conditions of pressure and temperature. Then the porosity, α, is given by (7.11) where v is the specific volume of the porous material and vs is the specific volume of the material in the solid state and at the same pressure and temperature (note that vs is only equal to 1/ρsolid at zero pressure). α becomes unity when the material compacts to a solid. If the equation of state of the solid material, neglecting shear strength effects, is given by (7.12) then the equation of state of the porous material is simply (7.13) This function can be any of the equations of state which describe the compressed state of material; in other words Linear, Polynomial and Shock, but not those describing the expanded state. In order to complete the material description the porosity α must be specified as a function of the thermodynamic state of the material, say, (7.14) There is not enough data usually available to determine the function g(p,e) completely but fortunately most problems of interest involve shock compaction of the porous material, i.e. the region of interest lies on or near the Hugoniot. On the Hugoniot, pressure and internal energy are related by the RankineHugoniot conditions so therefore along the Hugoniot equation Equation 7.14 (p. 213) can be expressed as (7.15) with the variation with energy implicitly assumed. It is assumed this equation Equation 7.15 (p. 213) remains valid in the neighborhood of the Hugoniot (tacitly assuming that the compaction strength is insensitive to the small changes in temperature in extrapolating small distances from the Hugoniot). Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

213

Material Models Used in Explicit Dynamics Analysis The general behavior of the compacting porous material has been described earlier and the P-α model is constructed to reproduce this behavior. The P-α variation to provide this performance is shown schematically in the figure below. The material deforms elastically up to onset of plastic compaction, α p, and subsequent deformation is plastic until the material is fully compacted at a pressure ps.

Intermediate unloading and reloading is elastic up to the plastic loading curve. The choice of a suitable function g(p) is somewhat arbitrary as long as it satisfies certain simple analytic properties enumerated by Herrmann in his original paper, and several forms have been used by different researchers. A simple form (Butcher & Karnes 1968) [6] found adequate for porous iron is a quadratic form, but cubic and exponential forms have also been proposed and the parameters adjusted to fit experimental data. The following choices for the plastic compaction curve are available:

Standard This is the default option, whereby the plastic compaction curve is defined by the solid compaction pressure, ps, at full compaction, the initial compaction pressure, pe, at porous compaction, α i, and the compaction exponent n.

214

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Porosity

Alpha Plastic (AUTODYN component system only) The plastic compaction curve is defined by the solid compaction pressure, ps, at full compaction, the initial compaction pressure, pe, at the onset of plastic compaction, α p, and the compaction exponent n.

Carroll & Holt (1972) [7] modified the equation of state of the porous material to give (7.16)

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

215

Material Models Used in Explicit Dynamics Analysis where the factor 1/α was included to allow for their argument that the pressure in the porous material is more nearly 1/α times the average pressure in the matrix material. It is this form of the model that is available in explicit dynamics.

Note The solid equation of state must be defined using one of the following properties Bulk modulus Polynomial EOS Shock EOS Linear Shock EOS Bilinear This property must be used in combination with a shear modulus to define the total elastic stiffness of the material. The property can only be applied to solid bodies. The Poisson's ratio is assumed to be zero when calculating effective strain. Table 7.17: Input Data Name

Symbol

Units

Solid Density

ρsolid

Density

Porous Soundspeed

Notes

Velocity

Initial Compaction Pressure

Pe

Stress

Solid Compaction Pressure

Ps

Stress

Compaction Exponent

n

None

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

PRESSURE

Pressure

Yes

No

No

DENSITY

Density

Yes

No

No

COMPRESSION

Compression

Yes

No

No

VISC_PRESSURE

Viscous Pressure

Yes

No

No

INT_ENERGY

Internal Energy

Yes

No

No

ALPHA

Porosity (Alpha)

Yes

No

No

7.11. Failure Background Materials are not able to withstand tensile stresses which exceed the material's local tensile strength. The computation of the dynamic motion of materials assuming that they always remain continuous, even if the predicted local stresses reach very large values, will lead to unphysical solutions. A model has to be constructed to recognize when tensile limits are reached to modify the computation to deal with this and to describe the properties of the material after this formulation has been applied.

216

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Failure Several different modes of failure initiation can be represented in the explicit dynamics system. Element failure in the explicit dynamics system has two components:

Failure initiation A number of mechanisms are available to initiate failure in a material (see properties Plastic Strain Failure, Principal Stress Failure, Principal Strain Failure, Tensile Pressure Failure, Johnson-Cook Failure, Grady Spall Failure). When specified criteria are met within an element, a post failure response is activated. Failure initiation can be identified in the model via the custom result MAT_STATUS. The following key is used. MAT_STATUS

Meaning

1

Material is currently undergoing elastic deformation, or no deformation

2

The plastic strain in the material increased during the last time increment

3

The material has failed due to isotropic (bulk) criteria

4

The material has failed due to isotropic (bulk) criteria

5

The material has failed in tension due to principal value 1

6

The material has failed in tension due to principal value 2

7

The material has failed in tension due to principal value 3

Post failure response After failure initiation in an element, the subsequent strength characteristics of the element will change depending on the type of failure model • Instantaneous Failure Upon failure initiation, the element deviatoric stress will be immediately set to zero and retained at this level. Subsequently, the element will only be able to support compressive pressures. • Gradual Failure (Damage) After failure initiation, the element stress is limited by a damage evolution law. Usually this results in a gradual reduction in an elements capability to carry deviatoric and/or pressure stresses. By default, tensile failure models will produce an instantaneous post failure response. Inserting the crack softening failure property, in addition to other failure initiation properties results in a gradual failure response. The following Failure models are discussed in this section: 7.11.1. Plastic Strain Failure 7.11.2. Principal Stress Failure 7.11.3. Principal Strain Failure 7.11.4. Stochastic Failure 7.11.5.Tensile Pressure Failure 7.11.6. Crack Softening Failure 7.11.7. Johnson-Cook Failure 7.11.8. Grady Spall Failure

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

217

Material Models Used in Explicit Dynamics Analysis

7.11.1. Plastic Strain Failure Plastic strain failure can be used to model ductile failure in materials. Failure initiation is based on the effective plastic strain in the material. The user inputs a maximum plastic strain value. If the material effective plastic strain is greater than the user defined maximum, failure initiation occurs. The material instantaneously fails.

Note This failure model must be used in conjunction with a plasticity or brittle strength model. Name

Symbol

Maximum Equivalent Plastic Strain

Epl

max

Units

Notes

None

Input data > zero

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

EFF_PL_STN

Effective Plastic Strain

Yes

Yes

Yes

STATUS

Material Status**

Yes

No

No

**Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3)

7.11.2. Principal Stress Failure Principal stress failure can be used to represent brittle failure in materials. Failure initiation is based on one of two criteria • Maximum principal tensile stress • Maximum shear stress (derived from the maximum difference in the principal stresses) Failure is initiated when either of the above criteria is met. The material instantaneously fails. If this model is used in conjunction with a plasticity model, it is often recommended to deactivate the Maximum Shear stress criteria by specifying a large value. In this case the shear response will be handled by the plasticity model.

Note The crack softening failure property can be combined with this property to invoke fracture energy based softening. Name

Symbol

Maximum Tensile Stress

218

Units

Notes

Stress

User must input a positive value. Default = +1e+20

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Failure Name

Symbol

Maximum Shear Stress

Units

Notes

Stress

User must input a positive value. Default = +1e+20

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

STATUS

Material Status**

Yes

No

No

**Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3)

7.11.3. Principal Strain Failure Principal strain failure can be used to represent brittle or ductile failure in materials. Failure initiation is based on one of two criteria • Maximum principal tensile strain • Maximum shear strain (derived from the maximum difference in the principal strains) Failure is initiated when either of the above criteria is met. The material instantaneously fails. If this model is used in conjunction with a plasticity model, it is often recommended to deactivate the maximum shear strain criteria by specifying a large value. In this case the shear response will be treated by the plasticity model.

Note The crack softening failure property can be combined with this property to invoke fracture energy based softening. Table 7.18: Input Data Name

Symbol

Units

Notes

Maximum Principal Strain

None

User must input a positive value. Default = +1e+20

Maximum Shear Strain

None

User must input a positive value. Default = +1e+20

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

STATUS

Material Status**

Yes

No

No

**Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3) Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

219

Material Models Used in Explicit Dynamics Analysis

7.11.4. Stochastic Failure To model fragmentation for symmetric loading and geometry it is necessary to impose some material heterogeneity. Real materials have inherent microscopic flaws, which cause failures and cracking to initiate. An approach to reproducing this numerically is to randomize the failure stress or strain for the material. Using this property, a Mott distribution is used to define the variance in failure stress or strain. Each element is allocated a value, determined by the Mott distribution, where a value of one is equivalent to the failure stress or strain of the material. The Mott distribution takes the form

where P is the probability of fracture ε is the strain C and γ are material constants For the implementation in explicit dynamics, the fracture value of 1 is forced to be at a probability of 50%; therefore, you need only specify a gamma value and the constant C is derived from this. Figure 7.14: Mott Distribution for Varying Values of Gamma

The stochastic failure option may be used in conjunction with many of the failure properties, including hydro (Pmin), plastic strain, principal stress and/or strain. It can also be used in conjunction with the RHT concrete model. You must specify a value of the stochastic variance, γ, and also the distribution seed type. If the “random” option is selected every time a simulation is performed a new distribution will be calculated. If the

220

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Failure “fixed” option is selected the same distribution will be used for each solve. However, this fixed distribution may also change when the model is run in one release compared to when it is run in a later release Table 7.19: Input Data Name

Symbol

Units

Notes

Distribution Type

Option List: Random Fixed (default) γ

Stochastic Variance Minimum Fail Fraction

None None

Default = 0.1

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

STATUS

Material Status**

Yes

No

No

STOCH_FACT

Stochastic Factor

Yes

No

No

**Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3)

7.11.5. Tensile Pressure Failure The tensile pressure failure model allows a maximum hydrodynamic tensile limit to be specified. This is used to represent a dynamic spall (or cavitation) strength of the material. The algorithm simply limits the maximum tensile pressure in the material as

If the material pressure P becomes less than the defined maximum tensile pressure, failure initiation occurs. The material instantaneously fails. If the material definition contains a damage evolution law, the user defined maximum tensile pressure is scaled down as the damage increases from 0.0 to 1.0.

Note The property can only be applied to solid bodies. The crack softening failure property can be combined with this property to invoke fracture energy based softening. Table 7.20: Input Data Name

Symbol

Maximum Tensile Pressure

Units

Notes

Stress

User must input a negative value. Default = –1e+20

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

221

Material Models Used in Explicit Dynamics Analysis Custom results variables available for this model: Name

Description

Solids

Shells

Beams

PRESSURE

Pressure

Yes

No

No

STATUS

Material Status**

Yes

No

No

**Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3)

7.11.6. Crack Softening Failure The tensile crack softening model is fracture energy based damage model which can be used with many different types of failure initiation models to provide a gradual reduction in the ability of an element to carry tensile stress. The model is primarily used for investigating failure of brittle materials, but has been applied to other materials to reduce mesh dependency effects. • Failure initiation is based on any of the standard tensile failure models; for example, Hydro, Principal Stress/Strain • On failure initiation, the current maximum principal tensile stress in the element is stored (custom result FAIL.STRES) • A linear softening slope (custom result SOFT.SLOPE) is then defined to reduce the maximum possible principal tensile stress in the material as a function of crack strain. This softening slope is defined as a function of the local element size and a material parameter, the fracture energy Gf. Slope =

Lf t2 2G f

Area = G f /L Total Frac ture

The extent of damage in a material can be inspected by using the custom result DAMAGE. The damage is defined to be 0.0 for an intact element and 1.0 for a fully failed element. • After failure initiation, a maximum principal tensile stress failure surface is defined to limit the maximum principal tensile stress in the element and a flow rule is used to return to this surface and accumulate the crack strain There are currently three options in relation to the crack softening plastic return algorithm: – Radial Return — Non-associative in π– and meridian planes – No-Bulking — Associative in π– plane only (Default) – Bulking — Associative in π– and meridian planes The default setting has been selected based on practical experiences of using the model to simulate impacts onto brittle materials such as glass, ceramics, and concrete. • The recompression behavior after crack softening and failure can be modified. When one of the failure criteria (for instance principal stress, hydro (Pmin), or RHT concrete) has been set and Crack Softening is set

222

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Failure to Yes, the Onset Compression after failure option can be used to change the compression criterion at which pressure can build up again in failed elements.

The effects of different values in this field are as follows: – Onset compression = 0.0 (default) — Pressure can only build up if the material is in compression. – Onset compression < 0 — For large negative values, the material will be able to immediately build up pressure after tensional failure when fractured material resists compression. For real-world applications, you should determine a value for this field which is less than or equal to zero and appropriate for the material in the analysis. The crack softening algorithm can only be used with solid elements. It can be used in combination with any solid equation of state, plasticity model or brittle strength model. When used in conjunction with a plasticity/brittle strength model, the return algorithm will return to the surface giving the minimum resulting effective stress, J2.

Meridian Plane Trial Elastic Stresses

Rankine Failure Surface

J2 Associate flow in Meridional Plane(Option)

Yield Surface (Strength Model)

Non-associative flow-in Meridional Plane (Default) Pressure Yielding

Rankine Plasticity (Te nsile Cracking)

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

223

Material Models Used in Explicit Dynamics Analysis

π- space

Note The property can only be applied to solid bodies. Table 7.21: Input Data Name

Symbol

Units

Fracture Energy

Gf

Energy/Area

Flow rule

Notes Option List: Radial Return No Bulking (Default) Bulking (Associative)

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

DAMAGE

Current damage level

Yes

No

No

FAIL.STRES

Principal tensile failure stress

Yes

No

No

SOFT.SLOPE

Softening slope

Yes

No

No

7.11.7. Johnson-Cook Failure The Johnson-Cook failure model can be used to model ductile failure of materials experiencing large pressures, strain rates and temperatures. This model is constructed in a similar way to the Johnson-Cook plasticity model in that it consists of three independent terms that define the dynamic fracture strain as a function of pressure, strain rate and temperature:

224

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Failure

The ratio of the incremental effective plastic strain and effective fracture strain for the element conditions is incremented and stored in custom results variable, DAMAGE. The material is assumed to be intact until DAMAGE = 1.0. At this point failure is initiated in the element. An instantaneous post failure response is used.

Note The property can only be applied to solid bodies. Table 7.22: Input Data Name

Symbol

Units

Damage Constant D1

D1

None

Damage Constant D2

D2

None

Damage Constant D3

D3

None

Damage Constant D4

D4

None

Damage Constant D5

D5

None

Melting Temperature

Notes

Temperature

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

DAMAGE

Damage

Yes

No

No

**Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3)

7.11.8. Grady Spall Failure The Grady Spall model can be used to model dynamic spallation of metals under shock loading. The critical spall stress for a ductile material can be calculated according to:

where: ρ is the density c is the bulk sound speed Y is the yield stress at EPS = 0 Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

225

Material Models Used in Explicit Dynamics Analysis ε cis a critical strain value, usually set to 0.15 This critical spall stress is calculated for each element in the model at each time step and compared with local maximum principal tensile stress. If the maximum element principal tensile stress exceeds the critical spall stress, instantaneous failure of the element is initiated. A typical value for the critical strain is 0.15 for aluminum.

Note The property can only be applied to Lagrangian solid bodies. The property must be used in conjunction with a plasticity model. Table 7.23: Input Data Name

Symbol Units Notes

Critical Strain Value

εc

None

Custom results variables available for this model: Name

Description

Solids

Shells

Beams

STATUS

Material Status

Yes

No

No

**Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3)

7.12. Strength The following table summarizes the applicable strength-limit constants for each failure criterion: Strength Limit Constant

Orthotropic Stress Limit

Orthotropic Strain Limit

Tsai-Wu Constants

Tensile X-Direction

Y

Y

Y

Tensile Y-Direction

Y

Y

Y

Tensile Z-Direction

Y

Y

Compressive X

Y

Compressive Y

Y

Compressive Z Shear XY

Y

Y

Shear YZ

Y

Y

Shear XZ

Y

Y

Y

Coupling Coefficient XY

226

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

References Coupling Coefficient YZ Coupling Coefficient XZ Tsai-Wu Constants must be used in conjunction with Orthotropic Stress Limit. Tsai-Wu Constants used in conjunction with Orthotropic Strain Limit are not supported. The TSai-Wu coefficients are always reset to -1 in an Explicit solve. The Tsai-Wu Constants property changes how the Explicit Dynamics solver uses the data from the Orthotropic Stress Limit property. Without the Tsai-Wu Constants property, the Explicit Dynamics solver uses all three tensile stress and all three shear stress constants from the Orthotropic Stress Limit. With the Tsai-Wu Constants property, the Explicit Dynamics solver uses the tensile and compressive stress constants in the X and Y direction only (not Z) and the XY shear stress constant (not YZ and XZ shears).

7.13. Thermal Specific Heat Specific heat is the amount of heat per mass required to raise the temperature of a material. Custom results variables available for this model: Name

Description

Solids

Shells

Beams

TEMPERATURE

Temperature

Yes

Yes

Yes

**Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3)

7.14. Rigid Materials Rigid materials can be modeled in an explicit dynamics system by selecting geometry, “Stiffness behavior = rigid” on a body. In such cases only the density property of the material associated with the body will be used. For explicit dynamics systems all rigid bodies must be discretized with a full mesh. This will be specified by default for the explicit meshing physics preference. The mass and inertia of the rigid body will be derived from the elements and material density for each body. By default, a kinematic rigid body is defined in explicit dynamics and its motion will depend on the resultant forces and moments applied to it through interaction with other parts of the model. Elements filled with rigid materials can interact with other regions via contact. Constraints can only be applied to an entire rigid body. For example, a fixed displacement cannot be applied to one edge of a rigid body; it must be applied to the whole body.

7.15. References The following references are cited in this section: 1. Johnson G. R. & Holmquist T. J. (1993). An Improved Computational Constitutive Model for Brittle Materials, Joint AIRA/APS Conference, Colorado Springs, Colorado, June 1993. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

227

Material Models Used in Explicit Dynamics Analysis 2. Riedel W., Thoma K., Hiermaier S., Schmolinske E.: Penetration of Reinforced Concrete by BETA-B-500, Numerical Analysis using a New Macroscopic Concrete Model for Hydrocodes. Proc. (CD-ROM) 9. Internationales Symposium, Interaction of the Effects of Munitions with Structures, Berlin Strausberg, 03.-07. Mai 1999, pp 315 - 322 3. W. Riedel, Beton unter dynamischen Lasten: Meso- und makromechanische Modelle und ihre Parameter, Ed.: Fraunhofer-Institut für Kurzzeitdynamik, Ernst-Mach-Institut EMI, Freiburg/Brsg., Fraunhofer IRB Verlag 2004, ISBN 3-8167-6340-5, http://www.irbdirekt.de/irbbuch/ 4. Werner Riedel, Nobuaki Kawai and Ken-ichi Kondo, Numerical Assessment for Impact Strength Measurements in Concrete Materials, International Journal of Impact Engineering 36 (2009), pp. 283-293 DOI information: 10.1016/j.ijimpeng.2007.12.012 5. Herrmann, W (1969).“Constitutive Equation for the Dynamic Compaction of Ductile Porous Materials”, J. Appl. Phys., 40, 6, pp 2490-2499, May 1969 6. Butcher, B M, & Karnes, C H (1968). Sandia Labs. Res Rep. SC-RR-67-3040, Sandia Laboratory, Albuquerque, NM, April 1968 7. Carroll, M M, & Holt, A C (1972).“Static and Dynamic Pore Collapse Relations for Ductile Porous Materials.” J. Appl.Phys., 43, 4, pp1626 et seq., 1972

228

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 8: Using Workbench LS-DYNA for an Explicit Dynamics Analysis The Workbench LS-DYNA ACT extension allows you to run an explicit dynamics analysis for your model using the LS-DYNA solver. This chapter describes the following: 8.1. How to Load Workbench LS-DYNA 8.2. How to use Workbench LS-DYNA 8.3. Using the Workbench LS-DYNA Extension 8.4. LS-DYNA Keywords used by Workbench LS-DYNA 8.5. Material Models Available in Workbench LS-DYNA 8.6. Customizing Workbench LS-DYNA using ACT 8.7. References

8.1. How to Load Workbench LS-DYNA The Workbench LS-DYNA ACT extension is included in the ANSYS product but must be loaded into Workbench. To do so: 1. Start Workbench. 2. Select Extensions → Manage Extensions... 3. In the Extensions Manager window, select the check box next to LSDYNA, then click Close.

8.2. How to use Workbench LS-DYNA Once you load the extension, a Workbench LS-DYNA section appears in the project Toolbox. To run an LS-DYNA analysis, expand the Workbench LS-DYNA section in the toolbox. You will see the Workbench LS-DYNA template. You can now drag the template into a project and set up and run your model as usual. The Workbench LS-DYNA extension will create an LS-DYNA keyword (.k) file that contains all the necessary information to carry out the analysis, and will run the LS-DYNA solver using that file. For general information about setting up an Explicit Dynamics analysis, see Explicit Dynamics Workflow (p. 3) All the LS-DYNA keywords are implemented according to the LS-DYNA Keyword User's Manual R10.0. All the LS-DYNA keywords that can currently be exported are described in detail in LS-DYNA Keywords used by Workbench LS-DYNA (p. 252). Any parameters that are not shown for a card are not used, and their default values will be assigned for them by the LS-DYNA solver. When using Commands objects with Workbench LS-DYNA, be aware of the following: • Keyword cards read from Commands object content (renamed to Keyword Snippets for Workbench LSDYNA) should not have any trailing empty lines if they are not intentional. This is because some keywords Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

229

Using Workbench LS-DYNA for an Explicit Dynamics Analysis have more than one mandatory card that can be entered as blank lines, in which case the default values for the card will be used. Therefore, trailing blank lines should be used only if intended; otherwise they may cause solver execution errors. • The first entry in the Commands object content must be a command name which is preceded by the * symbol.

Using a Different Version of LS-DYNA Workbench LS-DYNA enables the use of LS-DYNA executables other than the one available in the ANSYS installation. In order to use other versions in conjunction with Workbench LS-DYNA, these executables need to be properly licensed by ANSYS or LSTC. If the licensing is using the ANSYS license manager, the environment variable LSTC_LICENSE should be set to ANSYS. This variable is normally set during the ANSYS Workbench installation. If the licensing is using the LSTC license manager, this environment variable needs to be set to network ( LSTC_LICENSE = network). Please contact your LSTC distributor if you need additional information in order to setup the LSTC license manager. Workbench LS-DYNA assumes that the executables are in the directory defined by the environment variable CUSTOM_WB_LSDYNA_DIR. All the executables should be placed in this directory with the following naming conventions: • lsdyna_sp.exe for the SMP Single Precision executable • lsdyna_dp.exe for the SMP Double Precision executable • lsdyna_mpp_sp_impi.exe for the MPP Single Precision executable • lsdyna_mpp_dp_impi.exe for the MPP Double Precision executable

8.3. Using the Workbench LS-DYNA Extension The the version of LS-DYNA in the ANSYS installation is able to run the complete keyword set published in the LS-DYNA® KEYWORD USER'S MANUAL (R10.0). In the current implementation, a limited subset of the extensive list of keyword inputs can be generated by Workbench LS-DYNA. The keywords generated through the standard user interface are supported by ANSYS technical support. The following areas of use are not supported with Workbench LS-DYNA: • User-defined material definition • LS-DYNA user subroutines • Mesh-free methods: SPH & EFG • Some special elements such as Seat Belt and others • Fluid Structure Interaction (FSI) Advanced, knowledgeable users may modify the input file generated and take advantage of the full keyword set, however ANSYS, Inc. does not provide technical support for modified input files. Note that post-processing may not work correctly with modified .k files. For those cases use LS-Prepost, available in the standard installation. This section describes all of the steps needed to run an analysis using the Workbench LS-DYNA extension. 8.3.1. Licensing Requirements

230

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Using the Workbench LS-DYNA Extension 8.3.2. Running a Distributed Solution 8.3.3. Setting up a Project 8.3.4. Defining Initial Conditions 8.3.5. Defining Boundary Conditions 8.3.6. Accessing Results 8.3.7. Special Analysis Topics 8.3.8. Restarting a Workbench LS-DYNA Analysis 8.3.9. Additional LS-DYNA Analysis Tools

8.3.1. Licensing Requirements The Workbench LS-DYNA environment is available to all customers with an ANSYS LS-DYNA license and requires that license to run analyses. The Workbench LS-DYNA environment is available for pre- and post-processing (only) with the Enterprise Prepost license. SMP and MPP Parallel processing are both available. They do, however, require the use of ANSYS LSDYNA HPC licenses. The standard ANSYS HPC packs and HPC Workgroup licenses do not work with Workbench LS-DYNA. Use ANSYS LS-DYNA HPC licenses for running in parallel.

8.3.2. Running a Distributed Solution If you are planning to use the LS-DYNA distributed solution, LS-DYNA is using Intel MPI, which needs additional configuration and password caching. To cache your Windows password, open a Command Prompt window and run: %AWP_ROOT194%\commonfiles\MPI\Intel\2017.3.210\Windows\setimpipassword.bat

8.3.3. Setting up a Project The general guidelines for setting up an explicit dynamics analysis can be found in Explicit Dynamics Workflow (p. 3). LS-DYNA related information is included in that chapter; the use of the Workbench LS-DYNA extension is described in this section. 8.3.3.1. Defining Materials 8.3.3.2. Attaching Geometry 8.3.3.3. Defining Part Behavior 8.3.3.4. Defining Connections 8.3.3.5. Defining Mesh Settings 8.3.3.6. Defining Analysis Settings

8.3.3.1. Defining Materials You can find information about Materials in Define Engineering Data (p. 4).

Note The Material Assignment folder is not supported by Workbench LS-DYNA.

8.3.3.2. Attaching Geometry You can find information about Geometry in Attach Geometry (p. 4).

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

231

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

8.3.3.3. Defining Part Behavior You can find information about Part Behavior in Define Part Behavior (p. 6). Add the objects under Part from the LSDYNA Pre tab to specify Section properties such as element formulations, and specify different Hourglass Control objects for each part.

You can also add an adaptive region to your model.

8.3.3.3.1. Adaptive Region

In metal forming and high-speed impact analyses, a body may experience very large amounts of plastic deformation. Single point integration explicit elements, which are usually robust for large deformations, may give inaccurate results in these situations due to inadequate element aspect ratios. To counteract this problem, Workbench LS-DYNA has the ability to automatically remesh a surface during an analysis to improve its integrity. This capability, known as adaptive meshing, is controlled with the adaptive region: •  -adaptive for 3-D shells. • Passive  -adaptive for 3-D shells. The elements in this part will not be split unless their neighboring elements in other parts need to be split more than one level. At 18.1 when this feature is used, the postprocessing has to be done within LS-Prepost

8.3.3.4. Defining Connections You can find information about Connections in Define Connections (p. 7). In Workbench LS-DYNA Springs can be added in Connections. Both Longitudinal Stiffness and Damping are supported. Preloads are supported. Supported spring behavior is linear only.

232

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Using the Workbench LS-DYNA Extension

8.3.3.5. Defining Mesh Settings You can find information about Mesh Settings in Apply Mesh Controls/Preview Mesh (p. 40). Dimensionally Reduced Rigid Body Behavior is not available for Workbench LS-DYNA.

8.3.3.6. Defining Analysis Settings You can find information about Analysis Settings in Establish Analysis Settings (p. 41). You can set Solver Precision to Single or Double under Solver Controls, or leave it as Program Controlled. In Workbench LS-DYNA, the End Time is the only required input. SMP or MPP parallel processing can be activated by changing the Number of CPU's. Note that ANSYS LS-DYNA HPC licenses are required for using more than 1 core.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

233

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

8.3.4. Defining Initial Conditions You can find information about Initial Conditions in Define Initial Conditions (p. 67).

8.3.5. Defining Boundary Conditions You can find information about Boundary Conditions in Apply Loads and Supports (p. 67). For a Workbench LS-DYNA system, Remote Displacement is available in addition to the boundary conditions discussed there.

The Conditions , Contact Property , and Rigid Wall constraints are available on the LSDYNA Pre tab. The following boundary conditions are also available: 8.3.5.1. Rigid Body Tools 8.3.5.2. Airbag or Simple Pressure Volume 8.3.5.3. Input File Include Constraint 8.3.5.4. Keyword Snippet (LS-DYNA) Constraint 8.3.5.5. Bolt Pretension 8.3.5.6. Dynamic Relaxation

234

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Using the Workbench LS-DYNA Extension

8.3.5.1. Rigid Body Tools

A number of rigid body conditions are available to allow you to specify your rigid body behavior. These include:

• Explicit Rigid Bodies scoping to the geometry.

• Merge Rigid Bodies body.

• Rigid Body Additional Nodes existing rigid body.

- use this tool to specify rigid body(ies) for the Explicit analysis by directly

- use this tool to merge multiple rigid bodies together into a single rigid

- use this tool to add additional nodes from flexible body to the

8.3.5.2. Airbag or Simple Pressure Volume The Airbag object provides a way of defining thermodynamic behavior of the gas flow into the airbag as well as a reference configuration for the fully inflated bag.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

235

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

Simple Pressure Volume

When Formulation is set to Simple Pressure Volume: • The pressure is a function of the ratio of current volume to the initial volume. • This simple model can be used when an initial pressure is given. • No leakage, no temperature change, and no input mass flow are assumed. • A typical application is the modeling of air in automobile tires. • Pressure Volume Airbag controls: Coefficient versus Time (CN) can be defined in a table. β is a scale factor for the curve defining the coefficient versus time (CN), with a default value of 1.

236

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Using the Workbench LS-DYNA Extension

Simple Airbag Model

The volume pressure relationships is defined by the Simple Airbag Model for control volumes. • The gamma law equation of state used to determine the pressure in the airbag: p = (γ-1)ρe where p is the pressure, ρ is the density, e is the specific internal energy of the gas, and γ is the ratio of the specific heats: γ = cp/cv • Input Mass Flow Rate can be defined in a table.

8.3.5.3. Input File Include Constraint Advanced users can insert additional LS-DYNA keywords by using the Input File Include constraint to specify the name of a file that contains LS-DYNA keywords. An include file *INCLUDE Filename1 keyword card will be generated pointing to the file you specify. Included files can contain any valid LS-DYNA keyword cards. Using include files eliminates the need for you to edit the .k input file each time the file is created by Workbench LS-DYNA if you have other keywords you want to use. Note that the included file can contain other include file statements, providing a fairly general capability for easily adding predefined inputs.

Note ANSYS Support does not provide technical assistance for keywords not generated by Workbench LS-DYNA.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

237

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

8.3.5.4. Keyword Snippet (LS-DYNA) Constraint You can also insert additional LS-DYNA keywords by using the Keyword Snippet (LS-DYNA) constraint to insert individual LS-DYNA keywords. Note that this can only be inserted under Connections to use contact types not supported by Workbench LS-DYNA.

Note ANSYS Support does not provide technical assistance for keywords not generated by Workbench LS-DYNA.

8.3.5.5. Bolt Pretension This boundary condition applies a pretension load to a beam connection, typically to model a bolt under pretension.

Analysis Types Bolt Pretension is specific to Workbench LS-DYNA and is not compatible with the Bolt Pretension feature of the Mechanical Application. The Bolt Pretension can be either used during dynamic relaxation or during the explicit phase of the calculation.

Boundary Condition Application To apply a Bolt Pretension: 1. Right-click the Environment tree object or an active Dynamic Relaxation Object and select Insert → Bolt Pretension. 2. Define the Beam Connection. 3. Specify the Magnitude of the loading.

4. If the bolt pretension is used during the explicit phase, you need additionally an Initialization End Time to specify the termination of the loading.

238

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Using the Workbench LS-DYNA Extension

Note • The Bolt Pretension Load is not supported for a Full Restart. • When a Bolt Pretension within the Dynamic Relaxation Folder and a Bolt Pretension under the Workbench LS-DYNA Transient Analysis are defined for the same Beam connection, only the last one defined is used in the analysis.

8.3.5.6. Dynamic Relaxation

The dynamic relaxation feature (available by clicking on the LSDYNA Pre tab) provides preloading for explicit dynamics solutions in Workbench LS-DYNA. True dynamic relaxation (Relaxation Type: Explicit) allows an explicit solver to conduct a static analysis by increasing the damping until the kinetic energy drops to zero.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

239

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

The damping works by scaling nodal velocities by the Dynamic Relaxation Factor each time step until the ratio of current distortional kinetic energy to peak distortional kinetic energy (the convergence factor) falls below the convergence tolerance (Tolerance). By default, the convergence is checked on the whole model. It can be restricted to a set of bodies by setting the Convergence Scope to Geometry Selection. When the ANSYS Implicit solver is used to provide the preload (Relaxation Type: Explicit After Ansys Solution), a slightly different approach is taken in that the stress initialization is based on a prescribed geometry (in other words, the nodal displacement results from the Implicit solution). In this case, the explicit solver only uses 101 time steps to apply the preload. In the former case, the solver will check the kinetic energy every 250 cycles (by default) until the kinetic energy from the applied preload is dissipated.

240

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Using the Workbench LS-DYNA Extension

If the convergence type is set to Termination occurs at Pseudo End Time instead of Program Controlled, the termination of the dynamic relaxation occurs at the pseudo end time. The Time Step Scale factor enables you to scale the computed time step during dynamic relaxation. Alternatively, the LS-DYNA Implicit solver can be used to conduct a dynamic analysis to calculate the preloading. An initial time step needs to be provided to start the nonlinear implicit transient analysis. The convergence of this Newton-Raphson analysis is controlled by the Line Search convergence tolerance and a Displacement Convergence tolerance. Workbench LS-DYNA supports all these methods, which occur in pseudo time before the transient portion of the analysis begins at time zero.

Preloading Preloading works by specifying that a given load will be active during the dynamic relaxation, when the relaxation type is set to Explicit or Implicit.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

241

Using Workbench LS-DYNA for an Explicit Dynamics Analysis Currently only Acceleration and Standard Earth Gravity can be used as General Preload (preloads) for dynamic relaxation.

Workbench LS-DYNA also enables preloading of Beam Connections through the Bolt Pretension.

8.3.6. Accessing Results You can find information about Results Processing in Review Results (p. 88). To collect Nodal Data, insert one or more Result Trackers under Solution prior to running the simulation. Result trackers must be scoped to a node. Stress and Plastic Strain are written by default (can be suppressed) but Strain is not written by default and you must select it if desired. LS-DYNA keeps track of Total Strain and Plastic Strain. Elastic Strain will always show as 0. To plot elastic plastic strain or elastic strain, click Solution, then click Worksheet from the Home tab and select Available Solution Quantities within the Worksheet. Right click the expression and select Create User Defined Result.

242

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Using the Workbench LS-DYNA Extension

Time History Outputs (ASCII files) can be generated. All the files shown below can be created using the Workbench LS-DYNA GUI. Note however that some data in the ASCII files currently cannot be viewed.

To view Time History Outputs select the ones desired from the ASCII drop-down menu. Using LS-DYNA terminology, the following results can be viewed within Workbench LS-DYNA: • GLSTAT (Global Data : Kinetic Energy, Hourglass, ....). • BNDOUT (Boundary Conditions Data).

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

243

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • RCFORC (Contact Forces Data). • SPCFORC (Reaction Forces on Boundary Conditions) using *BOUNDARY_SPC (Fixed Support) to view Reaction Force. • MATSUM (Body Data). • NODOUT (Nodal Data) Trackers must be defined during pre-processing for the nodal data to be available during Results processing.

8.3.7. Special Analysis Topics The Workbench LS-DYNA system can interact with other Workbench systems.

8.3.7.1. Importing the Results of a Thermal Analysis A Steady-State or Transient Thermal analysis system can be directly linked to a Workbench LS-DYNA system to import the calculated temperatures and provide thermal stress. For information on setting up this transfer, follow the description of how it is done for a structural system in Thermal-Stress Analysis in the Mechanical User's Guide

Note • Imported temperatures cannot be scoped to beams. • Workbench LS-DYNA requires the definition of the Instantaneous Thermal Expansion Coefficient on materials to calculate thermal deformations.

8.3.8. Restarting a Workbench LS-DYNA Analysis Restarting means performing an analysis which continues from a previous analysis. A restart can begin from either the conclusion of or the middle of a prior analysis. Possible Reasons for Performing A Restart • The previous analysis was killed by the operating system or the user (sw1). • The previous analysis exceeded the user defined CPU limit. • There was an error in the previous analysis and a restart is used to diagnose and/or correct the error. • The previous analysis was not run to a long enough termination time. There are three types of restarts: simple restarts, small restarts, and full restarts. A simple restart is one for which the original model has not been altered in the new analysis. A simple restart is performed when the LS-DYNA solution was prematurely interrupted by the exceeding of a user defined CPU limit or by the issuing of the sense switch control sw1. A small restart is used to run an analysis to a longer termination time than initially specified and/or to make minor modifications to the model. The following actions are permitted in a small restart. • Specifying rigid/deformable switch controls.

244

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Using the Workbench LS-DYNA Extension • Switching parts from deformable to rigid & back. A full restart supports most new analysis actions, including: • Portions of the model may be added or removed. • Additional materials and loading changes are permitted. There are some restrictions for full restarts, including: • Contact specifications and initial velocities cannot be changed. • Adaptive meshing is not supported, even if present in the initial run. Stress initialization is available for full restarts. Deformed nodal positions and stresses/strains from a previous analysis are carried forward into a full restart analysis.

Note In order to switch the stiffness in either a small restart or full restart, you must add a Deformable To Rigid object under the original Workbench LS-DYNA system as shown here:

To add the object, select the Workbench LS-DYNA object, right-click and select Insert Deformable To Rigid. After you add the object, select it and in the Details view, scope the object to the body whose stiffness you want to change. Be sure that the Stiffness Behavior attribute of the scoped body is set to Flexible.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

245

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

8.3.8.1. Performing a Simple Restart In order to perform a simple restart: 1. On the Project Schematic page, select Restart Workbench LS-DYNA from the Toolbox and drag and drop it onto the Solution cell of an existing Workbench LS-DYNA system.

2. Under the Restart Workbench LS-DYNA object, select Initial Conditions and set Mode to Displacements in the Details panel.

3. In the Details panel of the Analysis Settings object, choose Simple Restart for Restart Type and then Solve.

246

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Using the Workbench LS-DYNA Extension

8.3.8.2. Performing a Small Restart In order to perform a Small Restart: 1. On the Project Schematic page, select Restart Workbench LS-DYNA from the Toolbox and drag and drop it onto the Solution cell of an existing Workbench LS-DYNA system.

2. Under the Restart Workbench LS-DYNA object, select Initial Conditions and set Mode to Displacements in the Details panel.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

247

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

3. In the Details panel of the Analysis Settings object, choose Small Restart for Restart Type and define a new termination time.

4. Make any additional changes to the project. The allowed changes are:

248

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Using the Workbench LS-DYNA Extension Actions

Tab Selection

• Reset termination time.

None

Details Panel

• Reset output printing interval. • Reset output plotting interval. • Change damping options.

• Change velocity options.

• Delete contact surfaces. • Delete elements and parts.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

249

Using Workbench LS-DYNA for an Explicit Dynamics Analysis Actions

Tab Selection

Details Panel

• Switch deformable bodies to rigid. • Switch rigid bodies to deformable.

Note A small restart cannot be done if you are running a serial solution in single precision. To do a small restart you must be running a parallel solution or using double precision.

8.3.8.3. Performing a Full Restart A full restart is a new analysis starting from an initialized state. New data may be entered into the model, including nodes, elements, material data, and loading. 1. On the Project Schematic page, select Restart Workbench LS-DYNA from the Toolbox and drag and drop it onto the Solution cell of an existing Workbench LS-DYNA system.

2. In the Details panel of the Analysis Settings object, choose Full Restart for Restart Type.

250

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Using the Workbench LS-DYNA Extension

3. Make any other changes to the project that you require and then Solve.

Note A full restart begins at the point in time where the previous calculation ended. Any new time-dependent loading applied during a full restart must start after the physical time that elapsed in the previous calculation. For example, if you want to ramp a velocity from 10 m/s to 20 m/s in the full restart for a total duration of 2ms and the previous calculation ended at 1ms, the loading should have a point in time at 1ms with a value of 10 m/s, and a point in time at 3ms with a value of 20m/s.

8.3.9. Additional LS-DYNA Analysis Tools When the Workbench LS-DYNA system is selected in the Outline view, you will see these additional analysis tools on the LSDYNA Pre tab:

•

- use this tool to define the time step for the analysis of rigid body dynamics.

•

- use this tool to calculate CFL time step before the calculation starts.

•

- use this tool to write the .k file of the Workbench LS-DYNA model to the specified directory, including all keywords from Keyword Snippets and Include Files.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

251

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

8.4. LS-DYNA Keywords used by Workbench LS-DYNA The Workbench LS-DYNA ACT extension allows you to run an explicit dynamics analysis for your model using the LS-DYNA solver. This section shows all LS-DYNA supported keywords and their syntax. Keywords conform to the LS-DYNA Keyword User's Manual R10.0. Each keyword consists of one or more cards, each with one of more parameters. If a parameter is not shown, it will be assigned default values by the LS-DYNA solver. This chapter describes the following: 8.4.1. Input File Header 8.4.2. Database Format 8.4.3. Control Cards 8.4.4. Part Setup 8.4.5. Engineering Data Materials and Equations of State 8.4.6. Mesh Definition 8.4.7. Coordinate Systems 8.4.8. Components and Named Selections 8.4.9. Remote Points and Point Masses 8.4.10. Contacts and Body Interactions 8.4.11. Magnitude and Tabular Data 8.4.12. Acceleration and Gravity 8.4.13. Supports 8.4.14. Loads 8.4.15. Discrete Connections 8.4.16. Other Supports 8.4.17. Environment Temperature 8.4.18. ASCII Files 8.4.19. Database Output Settings 8.4.20. End of Input File

8.4.1. Input File Header *KEYWORD Marks the beginning of a keyword file.

8.4.2. Database Format *DATABASE_FORMAT Specifies the format in which to write binary results files like D3PLOT and D3THDT. Card • IFORM = 0. Binary results will be written only in the LS-DYNA format. • IFORM = 2. Both LS-DYNA and ANSYS database formats will be written. • IBINARY = 0. Word size of the binary output files (D3PLOT, D3THDT, ...) defaults to 64 bit format.

252

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA

8.4.3. Control Cards *CONTROL_ACCURACY Specifies control parameters that can improve the accuracy of the calculation. Card • OSU = 1. Global flag for objective stress updates. Required for parts that undergo large rotations. When set to 1 the flag is on. • INN = 4. Invariant node numbering for shell and solid elements. When set to 4 the flag is on for both shell and solid elements.

*CONTROL_ALE Set global control parameters for the Arbitrary Lagrange-Eulerian (ALE) and Eulerian calculations.

Card • DCT = Continuum Treatment from the ALE Controls section of the Analysis Settings (Defaults to 1): – = 1 if the Continuum Treatment is set to Lagrangian. – = 2 if the Continuum Treatment is set to Eulerian. – = 3 if the Continuum Treatment is set to Arbitrary Lagrangian Eulerian. – = 4 if the Continuum Treatment is set to Eulerian Ambiant. • NDV = Cycles Between Advection from the ALE Controls section of the Analysis Settings (Default to 1). • METH = Advection Method from the ALE Controls section of the Analysis Settings (Default to 1): – = 1 if the Advection Method is set to Donor cell + Half-Index-Shift METH. – = 2 if the Advection Method is set to Van Leer + Half-Index-Shift.

*CONTROL_BULK_VISCOSITY Sets the bulk viscosity coefficients globally. Card • Q1 = 1.5. Quadratic Artificial Viscosity. • Q2 = 0.06. Linear Artificial Viscosity.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

253

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • TYPE = -2. Internal energy dissipated by the viscosity in the shell elements is computed and included in the overall energy balance.

*CONTROL_CONTACT Specifies the defaults for computations of contact surfaces. Card 1 • SLSFAC = 0 (uses the default = 0.1). Scale factor for sliding interface penalties. • RWPNAL = 0. Scale factor for rigid wall penalties. When equal to 0 the constrain method is used and nodal points which belong to rigid bodies are not considered. • ISLCHK = 1. Initial penetration check in contact surfaces. When set to 1 there is no checking. • SHLTHK = 1 (default). Shell thickness considered in surface to surface and node to surface contact types. When set to 1, thickness is considered but rigid bodies are excluded. • PENOPT = 1 (default). Penalty stiffness value option. • THKCHG = 0 (default). • ORIEN = 2. Automatic reorientation for contact segments during initialization. When set to 2 it is active for manual (segment) and automated (part) input. • ENMASS = 0. This parameter regulates the treatment of the mass for eroded nodes in contact. When set to 0 eroding nodes are removed from the calculation. Card 2 • USRSTR = 0. Storage per contact interface for user supplied interface control subroutine. When set to 0 no input data is read and no interface storage is permitted in the user subroutine. • Default values are used for all other parameters. Card3 • SFRIC = 0. Default static coefficient of friction. • Default values are used for all other parameters. Card4 • IGNORE = 2. Specifies whether to ignore initial penetrations in the *CONTACT_AUTOMATIC options. When set to 2 initial penetrations are allowed to exist by tracking them. Also, warning messages are printed with the original and the recommended coordinates of each slave node. • FRCENG = 1. Calculate frictional energy in contact. Convert mechanical frictional energy to heat when doing a coupled thermal-mechanical problem. • SKIPRWG = 0 (default). • OUTSEG = 1. Yes, output each beam spot weld slave node and its master segment for *CONTACT_SPOTWELD into D3HSP file.

254

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • SPOTSTP = 0 (default). • SPOTDEL = 1.Yes, delete the attached spot weld element if the nodes of a spot weld beam or solid element are attached to a shell element that fails and the nodes are deleted. • SPOTHIN = 0.5. This factor can be used to scale the thickness of parts within the vicinity of the spot weld. This factor helps avert premature weld failures due to contact of the welded parts with the weld itself. Should be greater than zero and less than one.

*CONTROL_ENERGY Specifies the controls for energy dissipation options. Card • HGEN = 2. Hourglass energy is computed and included in the energy balance. Results are reported in ASCII files GLSTAT and MATSUM. • RWEN = 2 (default). • SLNTEN = 2. Sliding interface energy dissipation is computed and included in the energy balance. Results are reported in ASCII files GLSTAT and SLEOUT. • RYLEN = 2. Rayleigh energy dissipation is computed and included in the energy balance. Results are reported in ASCII file GLSTAT.

*CONTROL_HOURGLASS Defines the default values of hourglass control type and coefficient.

Card • IHQ = Default Hourglass from the Hourglass Controls section of the Analysis Settings ( Default to 1 and Standard LS-DYNA Hourglass ): – = 1 if the Default Hourglass is set to Standard LS-DYNA. – = 2 if the Default Hourglass is set to Flanagan-Belytschko Viscous Form. – = 3 if the Default Hourglass is set to Exact Volume Flanagan-Belytschko. – = 4 if the Default Hourglass is set to Flanagan-Belytschko Stiffness Form. – = 5 if the Default Hourglass is set to Exact Volume Flanagan-Belytschko Stiffness Form. – = 6 if the Default Hourglass is set to Belytschko-Bindeman IHQ. – = 7 if the Default Hourglass is set to Belytschko-Bindeman Linear Total Strain.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

255

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • QH = Default Hourglass Coefficient from the Hourglass Controls section of the Analysis Settings ( Default to 0.1 ).

*CONTROL_OUTPUT This keyword controls the printing of various LS-DYNA output text files. Card • NPOPT is the only parameter that is set. The value is set to 1. With that parameter set, nodal coordinates, element connectivities, rigid wall definitions, nodal SPCs, initial velocities, initial strains,adaptive constraints, and SPR2/SPR3 constraints are not printed.

*CONTROL_PARALLEL Controls parallel processing usage for shared memory computers by defining the number of processors and invoking the optional consistency of the global vector assembly. Card • CONST = 1. Consistency flag disabled for a faster solution

*CONTROL_SOLUTION Specify the analysis solution procedure if thermal, coupled thermal analysis, or structural-only is performed. Card • SOLN – = 0. Structural analysis only, if the Solver Type is set to Program Controlled or Structural Analysis Only. – = 2. Coupled structural thermal analysis, if the Solver Type is set to Coupled Structural Thermal Analysis.

*CONTROL_SHELL Specifies global parameters for shell element types. Card • WRPANG = 20 (default). Shell element warpage angle in degrees. If a warpage greater than this angle is found, a warning message is printed. • ESORT = 1, full automatic sorting of triangular shell elements to treat degenerate quadrilateral shell elements as C0 triangular shells. • IRNXX = -1, shell normal update option. When set to -1, fiber directions are recomputed at each cycle. • ISTUPD = 4, shell thickness update option for deformable shells. Membrane strains cause changes in thickness in 3 and 4 node shell elements, however elastic strains are neglected. This option is very important in sheet metal forming or whenever membrane stretching is important. For crash analysis, setting 4 may improve energy conservation and stability. • THEORY = 2 (default). Belytschko-Tsay formulation. 256

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • BWC = 1. For this setting, Belytschko-Wong-Chiang warping stiffness is added. • MITER = 1 (default). Plane stress plasticity: iterative with 3 secant iterations. • PROJ = 1, the full projection method is used for the warping stiffness in the Belytschko-Tsay and BelytschkoWong-Chiang shell elements. This option is required for explicit calculations. • NFAIL1 = 1. Flag to check for highly distorted under-integrated shell elements, print a message, and delete the element. • NFAIL4 = 1. Flag to check for highly distorted fully-integrated shell elements, print a message, and delete the element. • CNTO = 2. Flag to account for shell reference surface offsets in the contact treatment. Offsets are treated using the user defined contact thickness which may be different than the shell thickness used in the element.

*CONTROL_SOLID Specifies global parameters for solid element types. Card • ESORT = 1, full automatic sorting of tetrahedron and pentahedron elements to treat degeneracies. Degenerate tetrahedrons will be treated as ELFORM = 10 and pentahedron as ELFORM = 15 solids respectively (see *SECTION_SOLID).

*CONTROL_TERMINATION Specifies the termination criteria for the solver. Card • ENDTIM = End Time in the Step Controls section of the Analysis Settings. • ENDCYC = 10000000(constant) Maximum Time Steps. • DTMIN = 0.001 (constant). • ENDENG = 1000 (constant) Maximum Energy Error. • ENDMAS = 100000 (constant) Maximum Part Scaling.

*CONTROL_THERMAL_TIMESTEP This keyword is written if the simulation is determined to be a thermal one (for example, Coupled Structural Thermal Analysis). See Solver Type from the Solver Controls section of the Analysis Settings.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

257

Using Workbench LS-DYNA for an Explicit Dynamics Analysis Card • TS = Auto Time Stepping from Thermal Step Controls (default to 1): – 0 if Auto Time Stepping from Thermal Step Controls is set to No. The time step is fixed. – 1 if Auto Time Stepping from Thermal Step Controls is set to Yes. The time step is variable (may increase or decrease). • TIP = Time integration parameter from Thermal Step Controls (default to Crank Nicholson Scheme TIP = 0): – 0 if Time integration parameter from Thermal Step Controls is set to Crank-Nicholson scheme. – 1 if Time integration parameter from Thermal Step Controls is set to Fully Implicit. • ITS = Initial Time Step from Thermal Step Controls. • TMIN = Minimum Time Step from Thermal Step Controls. If TMIN = 0.0, it is set to the structural explicit time step. • TMAX = Maximum Time Step from Thermal Step Controls. If TMAX = 0.0, it is set to 100 * the structural explicit time step.

*CONTROL_THERMAL_SOLVER This keyword is written if the simulation is determined to be a thermal one (for example, Coupled Structural Thermal Analysis). See Solver Type from the Solver Controls section of the Analysis Settings.

Card • ATYPE = Thermal Analysis Type from Thermal Solver Controls (default to 1) – 0 if Thermal Analysis Type from Thermal Solver Controls is set to Steady State Analysis. – 1 if Thermal Analysis Type from Thermal Solver Controls is set to Transient Analysis. • SOLVER = Solver Type from Thermal Solver Controls (defaults to 1): – 1 if Solver Type is set to Symmetric Direct Solver. – 2 if Solver Type is set to Nonsymmetric Direct Solver. – 3 if Solver Type is set to Diagonal Scaled Conjugate Gradient Iterative. – 4 if Solver Type is set to Incomplete Choleski Conjugate Gradient Iterative. – 5 if Solver Type is set to Nonsymmetric Diagonal Scaled bi-Conjugate Gradient. – 12 if Solver Type is set to Diagonal Scaling Conjugate Gradient Iterative.

258

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA – 13 if Solver Type is set to Symmetric Gauss-Siedel Conjugate Gradient Iterative. – 14 if Solver Type is set to SSOR Conjugate Gradient Iterative. – 15 if Solver Type is set to ILDLT0 Conjugate Gradient Iterative. – 16 if Solver Type is set to Modified ILDLT0 Conjugate Gradient Iterative. • PTYPE = Thermal problem type from Thermal Nonlinear Controls.

– 0 if Thermal problem type is set to Linear Problem. – 1 if Thermal problem type is set to Nonlinear problem Gauss Point Temperature. – 2 if Thermal problem type is set to Nonlinear problem Element Average Temperature. • FWORK = Fraction of Work Converted into Heat from Thermal Solver Controls (defaults to 1).

*CONTROL_THERMAL_NONLINEAR This keyword is written if the simulation is determined to be a thermal one (for example, Coupled Structural Thermal Analysis). See Solver Type from the Solver Controls section of the Analysis Settings.

Card • THLSTL = Line Search from Thermal Nonlinear Controls (defaults to 0.0) • TOL = Temperature Convergence from Thermal Nonlinear Controls (defaults to 0.0).

*CONTROL_TIMESTEP Specifies conditions for determining the computational time step.

Card • DTINIT = 0 Initial Time Step. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

259

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • TSSFAC = Time Step Safety Factor from the Step Controls section of the Analysis Settings. • ISDO = 0 (default). Basis of time size calculation for 4-node shell elements. • TSLIMT = 0 Minimum Element Timestep; the default value of 0.0 is used. • DT2MS = the negative value of Time Step Size specified in the Step Controls section of the Analysis Settings, if Automatic Mass Scaling is set to Yes. If Automatic Mass Scaling is set to No the default value of 0.0 is used. • LCTM = 0. • ERODE = 1 (constant). • MS1ST = 0 (default).

*DAMPING_GLOBAL Specifies the mass weighted nodal damping applied globally to the nodes of deformable bodies and the center of mass of rigid bodies.

Card • LCID = 0, a constant damping factor will be used as specified in VALDMP. • VALDMP = Magnitude from the Damping Controls section of the Analysis Settings ( defaults to zero if Global Damping is set to No).

8.4.4. Part Setup *PART Defines geometry bodies. Card1 • HEADING = name of the body specified in the Workbench environment. Card2 • PID = ID of the part. It is set in the LS-DYNA solver and does not reflect the ID specified in the mesh definition of the model. • SECID = ID of the section keyword associated with the part (see *SECTION). • MID = ID of the material keyword associated with the part (see *MAT). • EOSID = ID of the equation of state associated with the material of this part (*EOS and *MAT). If there is no EOS keyword associated with this part then this parameter is set to 0.

260

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • HGID = ID of the hourglass keyword associated with the part (see *HOURGLASS). If there is no hourglass keyword associated with this part then this parameter is set to 0.

*SECTION_BEAM Defines cross sectional properties for beam, truss, spot weld and cable elements. Card1 • SECID = ID of the section. • ELFORM = 1 or 2 (default). ELFORM = 2 is set for user defined cross sections. The default element formulation option can be changed using the Section object found under Part on the LSDYNA Pre tab of Workbench LS-DYNA. • SHRF = 0.833 (default). • QR = 0, which LS-DYNA defaults to 2, quadrature rule is 2x2 Gauss. If the cross sectional area of the beam is complex or user-defined, this parameter becomes IRID and is assigned the negative value of the IRID parameter in the corresponding *INTEGRATION_BEAM keyword (see above for details). • CST = 2 for solid cross sections nand hollow cross sections (arbitrary user defined integration rule). Card2 • for solid types or hollow cylinders – TS1 = width of beam. This refers specifically to the dimension at node 1. – TS2 = TS1. This refers specifically to the dimension at node 2. – TT1 = 1. Height of beam. This refers specifically to the dimension at node 1. Set to zero for circular solids. – TT2 = TT1. This refers specifically to the dimension at node 2. Set to zero for circular solids. These parameters are overwritten by the *INTEGRATION_BEAM defined for these types. • for general symmetric types – A = cross-sectional area. – ISS = Iyy, moment of inertia about the local s-axis. – ITT = Izz, moment of inertia about the local t-axis. – IST = Iyz. – J = Ixx. The Section object found under Part on the LSDYNA Pre tab of Workbench LS-DYNA allows you to modify the default generated values . In presence of line Bodies:

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

261

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

• ELFORM = LS-DYNA ID from the Definition section of the Section object. This field is read only; the actual value of the element formulation is set by the Formulation section of the Section object. If the formulation is one of the following, the Card is calculated similarly to the above definition for *SECTION_BEAM, and an *INTEGRATION_BEAM is written: • Hughes -Liu with cross section integration • Integrated warped beam • Belytschko Schwer full cross-section integration • Belytschko Schwer tubular beam with cross-section integration If the formulation is one of the following: • Belytschko Schwer resultant beam (resultant) • Truss (resultant) • Belytschko Schwer full cross-section integration Card 2 is modified and uses the syntax for the alternative form for formulations 2, 3, and 12. • STYPE is calculated from the section type defined in ANSYS DesignModeler or SpaceClaim. • D1 - D6 are calculated from the dimensions defined in ANSYS DesignModeler. If the formulation is Discrete/ Beam Cable, an additional panel is available: Figure 8.1: Discrete and Cable Controls when the Option is set to Discrete Beam

262

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA A material Card (*MAT_LINEAR_ELASTIC_DISCRETE_BEAM (p. 263)) is added to allow definition of properties for the discrete Beam.

*MAT_LINEAR_ELASTIC_DISCRETE_BEAM This card replaces the material defined in Engineering and its properties are calculated from it and the above panel. • MID = ID of material type, must be unique between the material keyword definitions. • RO = Density of the Material • TKR = Longitudinal Stiffness X from Discrete and Cable Controls • TKS = Longitudinal Stiffness Y from Discrete and Cable Controls • TKT = Longitudinal Stiffness Z from Discrete and Cable Controls • RKR = Torsional Stiffness X from Discrete and Cable Controls • RKS = Torsional Stiffness X from Discrete and Cable Controls • RKT = Torsional Stiffness X from Discrete and Cable Controls Figure 8.2: Discrete and Cable Controls when the Option is set to Cable

*MAT_CABLE_DISCRETE_BEAM This card replaces the material defined in Engineering Data and its properties are calculated from it, and the above panel. • MID = ID of material type, must be unique between the material keyword definitions. • RO = Density of the Material • E = Young Modulus of the Material A material Card (*MAT_CABLE_DISCRETE_BEAM) is added to allow definition of properties for the discrete Beam.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

263

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

*SECTION_SHELL Defines section properties for shell elements. Card1 • SECID = ID of the section. • ELFORM = 2 (default). • SHRF = 0.8333 (default). • NIP = 3 (default). Card2 • T1 = thickness of body. • T2-T4 = T1, shell thickness at nodes 2, 3 and 4. The Section object found under Part on the LSDYNA Pre tab of Workbench LS-DYNA allows you to modify the default generated values . In the presence of Surface Bodies:

• ELFORM = LS-DYNA ID from the Definition section of the Section object. This field is read only; the actual value of the element formulation is set by the Formulation section of the Section object. • NIP = Through Thickness Integration Points from the Definition section of the Section object.

*SECTION_SOLID Defines section properties for solid elements. Card • SECID = ID of the section. • ELFORM = – 1 (default). Also, used for first-order hexahedral elements, 5-noded pyramids, 6-noded wedges or bodies with mixed element types that include tetrahedrons together with hexahedrons, pyramids, or wedges. – 10 if elements are first-order tetrahedrons. – 16 if the elements are second-order tetrahedrons.

264

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA The Section object found under Part on the LSDYNA Pre tab of Workbench LS-DYNA allows you to modify the default generated values . In the presence of Solid Bodies:

• ELFORM = LS-DYNA ID from the Definition section of the Section object. This field is read only; the actual value of the element formulation is set by the Formulation section of the Section object.

*SECTION_SOLID_ALE This keyword is written when you use the Section object found under Part on the LSDYNA Pre tab of Workbench LS-DYNA, which allows you to modify the default generated values for the *SECTION keyword. If the ALE section from the Definition of the Section object is set to Yes.

• ELFORM = LS-DYNA ID from the Definition section of the Section object. This field is read only; the actual value of the element formulation is set by the Formulation section of the Section object. If LS-DYNA ID is zero, ELFORM is set to 5 (1 Point ALE ). Available Formulations are the following : • 1 point ALE : ELFORM = 5 • 1 point Eulerian : ELFORM = 6 • 1 point Eulerian ambient : ELFORM = 7 • 1 point ALE Multi-Material Element : ELFORM = 11 • 1 point Integration with single material and void : ELFORM = 12

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

265

Using Workbench LS-DYNA for an Explicit Dynamics Analysis Card 2 • AFAC = Simple Average from the ALE Controls of the Section object. Smoothing weight factor - Simple average. • BFAC = Volume Weighting from the ALE Controls of the Section object. Smoothing weight factor - Volume Weighting • CFAC = Isoparametric Weighting from the ALE Controls of the Section object. • DFAC = Equipotential Weighting from the ALE Controls of the Section object • AAFAC = Advection Factor from the ALE Controls of the Section object • START = start from the ALE Time Controls of the Section object. • END = end from the ALE Time Controls of the Section object.

*HOURGLASS Defines hourglass and bulk viscosity properties that are referenced in the *PART keyword via its HGID parameter (see *PART keyword). This keyword can be written using the Hourglass Control object found under Part on the LSDYNA Pre tab of Workbench LS-DYNA, which allows you to specify body scoped hourglass definition.

• HGID = ID of the part. It is set in the LS-DYNA solver and does not reflect the ID specified in the mesh definition of the model. • IHQ = Hourglass Control Type. • QM = Hourglass from the Coefficients section of the Hourglass Control object. • Q1 = Quadratic Bulk from the Coefficients section of the Hourglass Control object. • Q2 = Linear Bulk from the Coefficients section of the Hourglass Control object. • IBQ = 1 Standard LS-DYNA Bulk Viscosity This keyword can also be created using the Keyword Snippet(also, Commands objects) for the LS-DYNA solver. To use it, insert a Keyword Snippet under a Geometry body in the Tree Outline. The program

266

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA will automatically substitute the HGID parameter in accordance with the *PART keyword of the associated body. All other parameters in the Keyword Snippet are transcribed literally. If the keyword is entered in a Keyword Snippet anywhere else in the Tree Outline, it will be exported literally. This practice is not recommended, however, and a warning is provided in the header of Keyword Snippet objects when detected.

*CONSTRAINED_LAGRANGE_IN_SOLID This keyword is used for reinforcements body interactions. • SLAVE is set to the ID of the component containing line bodies • Master is set to the ID of the component containing solid bodies

*CONSTRAINED_RIGID_BODIES Specifies rigid bodies to be merged into one part. The resulting Part ID matches the ID of the rigid body designated as the master. By constraining the rigid bodies together using a single multibody part you avoid specifying conflicting motion on the nodes shared among the rigid bodies. All boundary conditions applied to the master body will also be applied to all the slave bodies as well. Any boundary conditions that were applied to the slaves will be ignored. The object Master Rigid Body allows you to specify the master rigid body. Card • PIDM = ID of the master rigid body. • PIDS = ID of the slave rigid body.

8.4.5. Engineering Data Materials and Equations of State Equation of State (EOS) Keywords The following are descriptions for *EOS keywords natively supported by Workbench LS-DYNA. More generally, any *EOS keyword may be introduced into the export file with the help of Commands objects in the Mechanical application (termed Keyword Snippet when referring to the LS-DYNA solver). To use it, insert a Keyword Snippet under a Geometry body in the Tree Outline. The program will automatically substitute the EOSID parameter, in accordance with the *PART keyword of the associated body. All other parameters in the Keyword Snippet are transcribed literally, overriding any values that would otherwise derive from the Engineering Data workspace. If the *EOS keyword is entered in a Keyword Snippet anywhere else in the Tree Outline, it will be exported literally and the Engineering Data EOS information will also be exported, if present. This practice is not recommended, however, and a warning is provided in the header of Keyword Snippet objects when detected.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

267

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

*EOS_GRUNEISEN Specifies a shock equation of state. This keyword is created when a Shock EOS linear equation of state is present in the properties of a material that is used in the simulation and the Johnson Cook plasticity model is also present. The bilinear version of this equation of state is not currently supported. Card1 • EOSID = ID of the keyword, must be unique between the *EOS keywords. • C = parameter C1 for a Linear Shock EOS property. • S1 = parameter S1 for a Linear Shock EOS property. • S2 = Parameter Quadratic S2 for a Linear Shock EOS property. • S3 = 0. • GAMAO = Gruneisen Coefficient for a Linear Shock EOS property. • A = 0. Card2 - mandatory, left blank.

*EOS_LINEAR_POLYNOMIAL Specifies the coefficients for a linear polynomial elastic EOS. The *EOS_LINEAR_POLYNOMIAL keyword is only created when the Johnson Cook strength property is added to the material model (which requires an EOS), but no other EOS has been specified. It is not directly available from the Engineering Data workspace, however. Card1 • EOSID = ID of the keyword, must be unique between the *EOS keywords. • C0 = 0. • C1 = Parameter A1. • C2 = Parameter A2. • C3 = Parameter A3. • C4 = Parameter A4. • C5 = Parameter A5. • C6 = Parameter A6. Card2 - mandatory, left blank.

Materials keywords The following are descriptions for *MAT keywords natively supported by projects that use the Workbench LS-DYNA extension. More generally, any *MAT keyword may be introduced into the project with the help of Commands objects in the Mechanical application (termed Keyword Snippet when referring to 268

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA the LS-DYNA solver). To use it, insert a Keyword Snippet under a Geometry body in the Tree Outline. The program will automatically substitute the MID parameter in accordance with the *PART keyword (see below) of the associated body. All other parameters in the Keyword Snippet are transcribed literally, overriding any values that would otherwise derive from the Engineering Data workspace. If the *MAT keyword is entered in a Keyword Snippet anywhere else in the Tree Outline, it will be exported literally and Engineering Data EOS information will also be exported, if present. This practice is not recommended, however, and a warning is provided in the header of Keyword Snippet objects when detected.

*MAT_3-PARAMETER_BARLAT This material law is used for the Bilinear 3 Parameter Barlat hardening and exponential 3 parameter Barlat hardening models. Card 1 • MID = ID of the material. Must be unique between the material keyword definitions. • RO = density of the material from the Engineering Data workspace. • E = Young's modulus of the material from the Engineering Data workspace, either specified directly or calculated from Bulk and Shear moduli. • PR = Poisson's Ratio of the material from the Engineering Data workspace, either specified directly or calculated from Bulk and Shear moduli. • HR = Hardening Type, set to 2 for Swift or 5 for Ghosh when the model is exponential, or to 1 when the model is bilinear. • P1 = Material Parameter, set to Hardening Constant K from Engineering Data when the model is exponential, or to the tangent modulus when the model is bilinear. • P2 = Material Parameter, set to Hardening Exponent n from Engineering Data when the model is exponential, or to the yield stress when the model is bilinear. • ITER = Iteration flag, set to 0. Card 2 • M = Barlat exponent from Engineering data. • R00 = Lankford parameter in 0 degree direction. • R45 = Lankford parameter in 45 degree direction. • R90 = Lankford parameter in 90 degree direction. Card 3 • AOPT = Coordinate System ID of body Coordinate System in Mechanical. • C = Strain Rate Constant. • P = Strain Rate Constant.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

269

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • EPSO = Reference Strain Rate.

*MAT_ADD_EROSION ADD_EROSION is added to a given material when a failure model is defined in Engineering Data, to a material that doesn't support the defined failure model. Card • MID = ID of material for which this failure model applies. • SIGP1 = Principal Stress Failure, if present. Otherwise it is 0. • MXEPS = Maximum Principal Strain, if present. Otherwise it is 0. • EPSSH = Maximum Shear Strain, if present. Otherwise it is 0. • EFFEPS = Maximum Equivalent Plastic Strain EPS, if present. Otherwise it is 0. • MNPRES = Maximum Tensile Pressure, if present. Otherwise it is 0.

*MAT_ARRUDA_BOYCE_RUBBER (or *MAT_127) • MID = ID of the material type. Must be unique between the material keyword definitions. • RO = Density of the material from the Engineering Data workspace. • K = Bulk modulus of the material, calculated from incompressibility parameter. • G = Initial shear modulus of the material from the Engineering Data workspace.

*MAT_BLATZ-KO_RUBBER (or *MAT_007) Blatz-Ko materials are only for rubber materials under compression. Poisson's ratio (NUXY) is automatically set to 0.463 by LS-DYNA, so only DENS and GXY are required. Card1 • MID = ID of the material type. Must be unique between the material keyword definitions. • RO = Density of the material. • G = Initial Shear modulus of material.

*MAT_ELASTIC (or *MAT_001) Specifies isotropic elastic materials. It is available for beam, shell and solid elements. This keyword is used if the selected material includes the Isotropic Elasticity strength model and the Stiffness Behavior is set to Deformable in the Definition section of the body. Card • MID = ID of material type. Must be unique between the material keyword definitions. • RO = density of the material from the Engineering Data workspace. 270

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • E = Young's modulus of the material from the Engineering Data workspace, either specified directly or calculated from Bulk and Shear moduli. • PR = Poisson's ratio of the material from the Engineering Data workspace, either specified directly or calculated from Bulk and Shear moduli.

*MAT_ENHANCED_COMPOSITE_DAMAGE (or *MAT_054) Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • EA = Young's Modulus X direction from the Orthotropic Elasticity model. • EB = Young's Modulus Y direction from the Orthotropic Elasticity model. • EC = Young's Modulus Z direction from the Orthotropic Elasticity model. • PRBA = Poisson's Ratio XY from the Orthotropic Elasticity model multiplied by Young's Modulus Y / Young's Modulus X. • PRCA = Poisson's Ratio YZ from the Orthotropic Elasticity model multiplied by Young's Modulus Z / Young's Modulus X. • PRCB = Poisson's Ratio XZ from the Orthotropic Elasticity model multiplied by Young's Modulus Z / Young's Modulus Y. Card2 • GAB = Shear Modulus XY from the Orthotropic Elasticity model. • GBC = Shear Modulus YZ from the Orthotropic Elasticity model. • GCA = Shear Modulus XZ from the Orthotropic Elasticity model. • AOPT = – 0 (default). When this parameter is set to zero the locally orthotropic material axes are determined from three element nodes. The first node specifies the local origin, the second specifies one of the axes and the third specifies the plane on which the axis rests. – - ID of local coordinate system assigned to the body with this material model. Card 3 is left blank Card 4 is left blank Card 5 is left blank Card 6 • XC = Compressive X of the Orthotropic Stress Limits definition, if present. Otherwise it is 0. • XT = Tensile X of the Orthotropic Stress Limits definition, if present. Otherwise it is 0. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

271

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • YC = Compressive Y of the Orthotropic Stress Limits definition, if present. Otherwise it is 0. • YT = Tensile Y of the Orthotropic Stress Limits definition, if present. Otherwise it is 0. • SC = Shear XY of the Orthotropic Stress Limits definition, if present. Otherwise it is 0.

*MAT_FLD_TRANSVERSELY_ANISOTROPIC This material law is used for the Bilinear transversely anisotropic hardening and multilinear transversely anisotropic hardening models. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of the material from the Engineering Data workspace. • E = Young's modulus of the material from the Engineering Data workspace, either specified directly or calculated from Bulk and Shear moduli. • PR = Poisson's ratio of the material from the Engineering Data workspace, either specified directly or calculated from Bulk and Shear moduli. • SIGY = Yield Strength. • ETAN = Tangent Modulus. • R = Anisotropic Hardening Parameter. • HLCID = 0 when the model is bilinear, or is set to the ID of the curve of effective stress versus plastic strain when the model is multilinear. • LCFLD is the ID of the curve describing the forming limit diagram.

*MAT_HYPERELASTIC_RUBBER (or *MAT_077_H) Specifies a general hyperelastic rubber model, optionally combined with viscoelasticity. This keyword is used if the material includes the Mooney-Rivlin, Polynomial or Yeoh hyperelastic strength model and the Stiffness Behavior is set to Deformable in the Definition section of the body. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of the material from the Engineering Data workspace. • PR = Poisson's ratio of the material from the Engineering Data workspace. Values higher than 0.49 are recommended. Smaller values may not work and should not be used. • N = 0, specifies that the constants in card 2 will be defined. • NV = 0. This parameter is not used if N = 0 above. • G = Shear modulus of the material from the Engineering Data workspace. • SIGF = 0. This parameter is not used if N = 0 above.

272

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA Card2 • C10 = constant C10 from the Engineering Data workspace. • C01 = constant C01 from the material properties in the Engineering Data. Set to zero for Yeoh models. • C11 = constant C11 from the Engineering Data workspace. Set to zero for Yeoh models. • C20 = constant C20 from the Engineering Data workspace. • C02 = constant C02 from the Engineering Data workspace. Set to zero for Yeoh models. • C30 = constant C30 from the Engineering Data workspace.

*MAT_JOHNSON_COOK (or *MAT_015) Defines a Johnson - Cook type of material. Such materials are useful for problems with large variations in strain rates where adiabatic temperature increases due to plastic heating cause material softening. This keyword is used if the material specified includes a Johnson Cook strength model. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • G = Shear modulus of material. • E = Young's modulus of the material (shell elements only). • PR = Poisson's ratio of the material (shell elements only). Card2 • A = Initial yield stress from the Johnson Cook strength parameters. • B = Hardening Constant from the Johnson Cook strength parameters. • N = Hardening Exponent from the Johnson Cook strength parameters. • C = Strain Rate Constant from the Johnson Cook strength parameters. • M = Thermal Softening Exponent from the Johnson Cook strength parameters. • TM = Melting Temperature from the Johnson Cook strength parameters. • TR = 15, room temperature. • EPSO = Reference Strain Rate from the Johnson Cook strength parameters. Card3 • CP = Specific Heat from the material properties. • PC = 0 (LS-DYNA default). • SPALL = 2.0 (LS-DYNA default). Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

273

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • IT = 0 (LS-DYNA default). • D1 = D1 parameter of the Johnson Cook failure model definition, if present. Otherwise it is 0. • D2 = D2 parameter of the Johnson Cook failure model definition, if present. Otherwise it is 0. • D3 = D3 parameter of the Johnson Cook failure model definition, if present. Otherwise it is 0. • D4 = D4 parameter of the Johnson Cook failure model definition, if present. Otherwise it is 0. Card4 • D5 = D5 parameter of the Johnson Cook failure model definition, if present. Otherwise it is 0. • C2/P = "Reference Strain Rate (/sec)" parameter of the Johnson Cook failure model definition, if present. Otherwise it is 0.

*MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY (or *MAT_123) Enhanced Piecewise Linear model (for shell elements only) that accounts for multiple failure methods: • Effective plastic strain. • Thinning (through-thickness) plastic strain. • Major principal in-plane strain. You can specify the number of through-thickness integration points that must fail before the shell element is deleted. This model is useful in pure bending applications where the center layer may never reach failure strain. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • E = Young's modulus of the material. • PR = Poisson's ratio of the material. • SIGY = Yield Strength from the BISO strength model. It is not required for MISO models. • ETAN = Tangent Modulus from the BISO strength model. It is not required for MISO models. • FAIL = Maximum Equivalent Plastic Strain EPS parameter of the Plastic Strain failure model, if present. Otherwise it is set to 10E+20. Card2 • C = Strain Rate Constant C. • P = Strain Rate Constant P. • LCSS = ID of the curve that defining effective stress versus effective plastic strain.

274

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • LCSR is left blank. • VP = Formulation for rate effects; set to 0 if the strain rate correction is set to scale yield stress, set to 1 if strain rate correction is set to viscoplastic. • EPSTHIN = Thinning Strain at Failure. • EPSMAJ = Major in Plane Strain At Failure. • NUMINT is left blank. Card3 is left blank. Card4 is left blank. Card5 is left blank.

*MAT_OGDEN_RUBBER (or *MAT_077_O) Specifies the Ogden rubber model, optionally combined with viscoelasticity. This keyword is used if the material includes the Ogden hyperelastic strength model and the Stiffness Behavior is set to Deformable in the Definition section of the body. For card 1 see *MAT_HYPERELASTIC_RUBBER (p. 272) Card2 • MU1 = Material Constant MU1 from the Ogden model. • MU2 = Material Constant MU2 from the Ogden model. • MU3 = Material Constant MU3 from the Ogden model. • MU4 = 0. • MU5 = 0. • MU6 = 0. • MU7 = 0. • MU8 = 0. Card3 • ALPHA1 = Material Constant A1 from the Ogden model. • ALPHA2 = Material Constant A2 from the Ogden model. • ALPHA3 = Material Constant A3 from the Ogden model. • ALPHA1 = 0. • ALPHA1 = 0. • ALPHA1 = 0.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

275

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • ALPHA1 = 0. • ALPHA8 = 0.

*MAT_ORTHOTROPIC_ELASTIC (or *MAT_002) Specifies the model for an elastic-orthotropic behavior of solids, shells, and thick shells. This keyword is created when the Orthotropic Elasticity property is present in a material that is used. The Poisson's ratios required with this keyword must be in their minor version, however Workbench requires their major versions hence they are converted by multiplying them by the relevant Young's modulus ratios. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • EA = Young's Modulus X direction from the Orthotropic Elasticity model. • EB = Young's Modulus Y direction from the Orthotropic Elasticity model. • EC = Young's Modulus Z direction from the Orthotropic Elasticity model. • PRBA = Poisson's Ratio XY from the Orthotropic Elasticity model multiplied by Young's Modulus Y / Young's Modulus X. • PRCA = Poisson's Ratio YZ from the Orthotropic Elasticity model multiplied by Young's Modulus Z / Young's Modulus X. • PRCB = Poisson's Ratio XZ from the Orthotropic Elasticity model multiplied by Young's Modulus Z / Young's Modulus Y. Card2 • GAB = Shear Modulus XY from the Orthotropic Elasticity model. • GBC = Shear Modulus YZ from the Orthotropic Elasticity model. • GCA = Shear Modulus XZ from the Orthotropic Elasticity model. • AOPT = – 0 (default). When this parameter is set to zero the locally orthotropic material axes are determined from three element nodes. The first node specifies the local origin, the second specifies one of the axes and the third specifies the plane on which the axis rests. – - ID of local coordinate system assigned to the body with this material model. Card3 - mandatory, left blank. Card4 - mandatory, left blank.

276

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA

*MAT_PIECEWISE_LINEAR_PLASTICITY (or *MAT_24) Defines elasto-plastic materials with arbitrary stress-strain curve and arbitrary strain rate dependency. This keyword is used if the material specified includes a Multilinear Isotropic Hardening (BISO or MISO) strength model. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • E = Young's modulus of the material. • PR = Poisson's ratio of the material. • SIGY = Yield Strength from the BISO strength model. It is not required for MISO models. • ETAN = Tangent Modulus from the BISO strength model. It is not required for MISO models. • FAIL = Maximum Equivalent Plastic Strain EPS parameter of the Plastic Strain failure model, if present. Otherwise it is set to 10E+20. Card2 • C = 0. • P = 0. • LCSS = ID of the curve that defining effective stress versus effective plastic strain. Card3 - mandatory, left blank. Card4 - mandatory, left blank.

*MAT_PLASTIC_KINEMATIC (or *MAT_003) Specifies isotropic and kinematic hardening plastic behavior in materials. This keyword is created when the Bilinear Kinematic Hardening (BKIN) strength model is present in a material. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • E = Young's modulus of the material. • PR = Poisson's ratio of the material. • SIGY = Yield Strength from the BKIN strength model. • ETAN = Tangent Modulus from the BKIN strength model. • BETA = 0.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

277

Using Workbench LS-DYNA for an Explicit Dynamics Analysis Card2 • SRC = left blank. • SRP = left blank. • FS = Maximum Equivalent Plastic Strain EPS parameter of the Plastic Strain failure model, if present. Otherwise it is left blank.

*MAT_POWER_LAW_PLASTICITY (or *MAT_018) Defines an isotropic plasticity model with rate affects modeled by a power hardening law. Power law hardening defined with strength coefficient k and hardening coefficient n. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • E = Young's modulus of the material. • PR = Poisson's ratio of the material. • K = Strength coefficient. • N = Hardening exponent. • SRC = Strain rate parameter C; if zero, rate effects are ignored. • SRP = Strain rate parameter, P; if zero, rate effects are ignored. Card 2 • SIGY = Initial yield stress. • EPSF = Maximum Equivalent Plastic Strain EPS parameter of the Plastic Strain failure model, if present. Otherwise it is left blank. • VP = Formulation for rate effects; set to 0 if the strain rate correction is set to scale yield stress, set to 1 if the strain rate correction is set to viscoplastic.

*MAT_RATE_SENSITIVE_POWERLAW_PLASTICITY (or *MAT_064) This specialized model is used specifically for superplastic forming. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • E = Young's modulus of the material. • PR = Poisson's ratio of the material.

278

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • K = Hardening Constant. • M = Hardening exponent. • N = Strain Rate Constant. • EO = Reference Strain Rate • VP = Formulation for rate effects; set to 0 if the strain rate correction is set to scale yield stress, set to 1 if strain rate correction is set to viscoplastic • EPSO is left blank

*MAT_RIGID (or *MAT_020) Specifies materials for rigid bodies. This keyword is created when the Stiffness Behavior is set to Rigid under the Definition section of the body. Any strength or EOS material properties defined are ignored. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • E = Young's modulus of the material. • PR = Poisson's ratio of the material. Card2 • CMO = – 0 if there are no constraints on the rigid body. – -1 if rigid body is constrained in any way. • CON1 = – 0 if there are no constraints on the rigid body. – = Local Coordinate System ID if associated with the constraint. Otherwise it is set to 0. • CON2 = – 0 if there are no constraints on the rigid body. – = 111111 if the body is constrained with a fixed support or with a combination of a simple support and a fixed rotation. – = 111000 if the body is constrained with a simple support. – = 000111 if the body is constrained with a fixed rotation. Card3 • LCO = CON1 if non-zero. Otherwise it will remain blank.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

279

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

*MAT_SIMPLIFIED_JOHNSON_COOK (or *MAT_098) Defines a Johnson - Cook type of material. Such materials are useful for problems with large variations in strain rates where adiabatic temperature increases due to plastic heating cause material softening. This keyword is used if the material specified includes a Johnson Cook strength model without an Equation Of State. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • E = Young's modulus of the material. • PR = Poisson's ratio of the material. Card2 • A= Initial yield stress from the Johnson Cook strength parameters. • B = Hardening Constant from the Johnson Cook strength parameters. • N = Hardening Exponent from the Johnson Cook strength parameters. • C = Strain Rate Constant from the Johnson Cook strength parameters. • PSFAIL = Maximum Equivalent Plastic Strain EPS parameter of the Plastic Strain failure model, if present. Otherwise it is set to 10E+20. • SIGMAX = 0. Not used. • SIGSAT = 0. Not used. • EPSO = Reference Strain Rate from the Johnson Cook strength parameters.

*MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC This material law is used for the Bilinear transversely anisotropic hardening and multilinear transversely anisotropic hardening models. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of the material from the Engineering Data workspace. • E = Young's modulus of the material from the Engineering Data workspace, either specified directly or calculated from Bulk and Shear moduli. • PR = Poisson's ratio of the material from the Engineering Data workspace, either specified directly or calculated from Bulk and Shear moduli. • SIGY = Yield Strength. • ETAN = Tangent Modulus.

280

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • R = Anisotropic Hardening Parameter. • HLCID = 0 when the model is bilinear, or is set to the ID of the curve of effective stress versus plastic strain when the model is multilinear.

8.4.6. Mesh Definition *NODE Defines nodes. All the parameters are obtained from mesh definitions of the model. Card • NID = ID of the node. • X = x coordinate. • Y = y coordinate. • Z = z coordinate.

*ELEMENT_BEAM Specifies beam elements. Card • EID = ID of the element. • PID = ID of the part it belongs to. • N1 = ID of nodal point 1. • N2 = ID of nodal point 2. • N3 = ID of nodal point 3, used for cross section orientation.

*ELEMENT_SHELL Specifies three, four, six and eight noded shell elements. Card • EID = ID of the element. • PID = ID of the part it belongs to. • N1 = ID of nodal point 1. • N2 = ID of nodal point 2. • N3 = ID of nodal point 3. • N4 = ID of nodal point 4. • N5-8 = ID of mid side nodes for six and eight noded shells. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

281

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

*ELEMENT_SHELL_THICKNESS_OFFSET Surface body thicknesses properties can be defined on faces of surface bodies using the Thickness object in the Geometry. This keyword defines scoped surface body thickness.

Card1 - the same as *ELEMENT_SHELL Card2 • THIC1 = Thickness field of the Thickness object. • THIC2 = Thickness field of the Thickness object. • THIC3 = Thickness field of the Thickness object. • THIC4 =Thickness field of the Thickness object. Card3 • OFFSET = value calculated from the Offset Type field of the Thickness object. if Offset Type = – Middle, it equals zero. – Top, it is equal to half of the thickness as a negative number. – Bottom, it is equal to half of the thickness. – User defined, it is equal to the value defined in the field Membrane offset.

*ELEMENT_SHELL_OFFSET_COMPOSITE Layered section properties can be defined on faces of surface bodies using the Layered Section object in the Geometry. This keyword defines layered section thickness.

Card1 - the same as *ELEMENT_SHELL

282

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA Card2 • OFFSET = value calculated from the Offset Type field of the Layered Section object. if Offset Type = – Middle, it equals zero. – Top, it is equal to half of the thickness as a negative number. – Bottom, it is equal to half of the thickness. – User defined, it is equal to the value defined in the field Membrane offset. Card3 Defines the property of two layers. Card3 is repeated as many times as required to specify all the layers in the section. The sequence is starting with the bottommost layer. • MID1= ID of material in Layer1. Must be unique between the material keyword definitions. • THICK1 = Thickness of the Layer1. • B1 = Angle defined in the worksheet for Layer1 projected onto the element surface. • MID2 = ID of material in Layer 2. Must be unique between the material keyword definitions. • THICK2 = Thickness of the Layer2 • B2 = Angle defined in the worksheet for Layer2 projected onto the element surface.

*ELEMENT_SOLID Specifies 3D solid elements including 10-noded tetrahedrons (second order). Apart from the second order case the two cards are combined into one. Card1 • EID = ID of the element. • PID = ID of the part it belongs to. Card2 • N1 = ID of nodal point 1. • N2 = ID of nodal point 2. • N3 = ID of nodal point 3. • N4 = ID of nodal point 4. • . • . • . Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

283

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • N10 = ID of nodal point 10.

8.4.7. Coordinate Systems *DEFINE_COORDINATE_SYSTEM Specifies a local coordinate system with three points: one at the local origin, one on the local x-axis and one on the local x-y plane. Card1 • CID = ID of the coordinate system, must be unique. • XO = global X-coordinate of the origin. • YO = global Y-coordinate of the origin. • ZO = global Z-coordinate of the origin. • XL = global X-coordinate of a point on the local x-axis. • YL = global Y-coordinate of a point on the local x-axis. • ZL = global Z-coordinate of a point on the local x-axis. Card2 • XP = global X-coordinate of a point on the local x-y plane. • YP = global Y-coordinate of a point on the local x-y plane. • ZP = global Z-coordinate of a point on the local x-y plane.

*DEFINE_VECTOR Specifies a vector by defining the coordinates of two points. This keyword defines the local coordinate system with respect to which a *BOUNDARY_PRESCRIBED_MOTION is prescribed. The ID of this coordinate system is specified with parameter CID. Card • VID = ID of the vector. • XT = 0, the local x-coordinate of the origin of the coordinate system specified with CID below. • YT = 0, the local y-coordinate of the origin of the coordinate system specified with CID below. • ZT = 0, the local z-coordinate of the origin of the coordinate system specified with CID below. • XH = 1 if the vector has a component in the x direction of the coordinate system specified with CID. Otherwise, this is set to 0. • YH = 1 if the vector has a component in the y direction of the coordinate system specified with CID. Otherwise, this is set to 0.

284

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • ZH = 1 if the vector has a component in the z direction of the coordinate system specified with CID. Otherwise, this is set to 0. • CID = ID of the coordinate system used to define the vector. If no coordinate system is specified this parameter is set to 0 to specify the global coordinate system.

8.4.8. Components and Named Selections *SET_NODE_LIST Defines a set of nodes. Card2 is repeated as many times as required to specify all the node IDs in the set. Card1 • SID = ID of the set. Card2 • NID1-NID8 = IDs for eight of the nodes in the set.

*SET_PART_LIST Defines a set of parts. Card2 is repeated as many times as required to specify all the part IDs in the set. Card1 • SID = ID of the set. Card2 • PID1-PID8 = IDs for eight of the parts in the set.

*SET_SEGMENT Defines triangular and quadrilateral segments. Card2 is repeated as many times as required to specify all the segments in the set. Card1 • SID = ID of the set. Card2 • N1-N4 = IDs of nodes that define one of the segments. For triangular segments N4=N3.

8.4.9. Remote Points and Point Masses *CONSTRAINED_NODAL_RIGID_BODY this keyword is generated for remote points. Remote points are a way of abstracting a connection to a solid model, be it a vertex, edge, face, body, or node, to a point in space (specified by Location). Remote Points are akin to the various remote loads available in the Mechanical application. Remote boundary conditions create remote points in space behind the scenes, or internally, whereas the Remote Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

285

Using Workbench LS-DYNA for an Explicit Dynamics Analysis Point objects define a specific point in space only. Remote point is converted to a rigid constraint ( nodal rigid body), independently of the stiffness behavior.

the location set in the Remote Point Scope is not used in the input file definition. Card1 • PID = ID of the Rigid Body. It is set in the LS-DYNA solver and does not reflect the ID specified in the remote point definition. • NSID identifies a set of nodes that are to be defined as a rigid body. This set of nodes is based on the scoped entities. The set consists of nodes from several different deformable parts. • PNODE = 0. This is not used in the exported file. • DRFLAG = the value is calculated from the translational active degrees of freedom when the DOF Selection in the Remote Point definition is set to Manual. It allows you to deactivate certain degrees of freedom in the rigid body definition. DRFLAG = – 1, when X Component is inactive. – 2, when Y Component is inactive. – 3, When Z Component is inactive. – 4, when X and Y Component are inactive. – 5, when Y and Z Component are inactive. – 6, when Z and X Component are inactive. – 7, when X, Y, and Z Components are inactive. 286

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • RRFLAG = the value calculated from the rotational active degrees of freedom when the DOF Selection in the Remote Point Definition is set to Manual. It allows you to deactivate certain degrees of freedom in the rigid body definition. RRFLAG = – 1, when Rotation X is inactive. – 2, when Rotation Y is inactive. – 3, when Rotation Z is inactive. – 4, when Rotation X and Y are inactive. – 5, when Rotation Y and Z are inactive. – 6, when Rotation Z and X are inactive. – 7, when Rotation X, Y, and Z are inactive.

*CONSTRAINED_NODAL_RIGID_BODY_INERTIA This keyword is generated for point masses. Point masses use a remote point for their definition, or can be applied on a remote point. See *CONSTRAINED_NODAL_RIGID_BODY for additional information. Card1 • PID = ID of the Rigid Body. It is set in the LS-DYNA solver and does not reflect the ID specified in the remote point/Point Mass definition. • NSID identifies a set of nodes that are to be defined as a rigid body. This set of nodes is based on the scoped entities. The set consists of nodes from several different deformable parts. • PNODE = 0. This is not used in the exported file. • DRFLAG = 0. All Translational degrees of freedom are active in the rigid body definition. • RRFLAG = 0. All Rotational degrees of freedom are active in the rigid body definition. Card2 • XC = X Coordinate from the Scope of the Point Mass object. • YC = Y Coordinate from the Scope of the Point Mass object. • ZC = Z Coordinate from the Scope of the Point Mass object. • TM = Mass from the Scope of the Point Mass object. Card3 • IXX= Mass Moment Of Inertia X from the Definition of the Point Mass object. • IXY = 0 • IXZ = 0 • IYY = Mass Moment Of Inertia Y from the Definition of the Point Mass object. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

287

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • IYZ = 0 • IZZ = Mass Moment Of Inertia Z from the Definition of the Point Mass object.

*INITIAL_VELOCITY_GENERATION Specifies initial translational and rotational velocities. Card1 • ID = ID of part where the initial velocity is applied. • STYP = 2, the velocity is applied to a whole part. In Workbench initial velocities can only be applied to whole parts. • OMEGA = angular velocity about the rotational axis. • VX = initial translational velocity in the x direction. • VY = initial translational velocity in the y direction. • VZ = initial translational velocity in the z direction. • IVATN = 0 (default) slave bodies of a multibody part are not assigned the initial velocities of the master part. • ICID = Local coordinate system ID. The specified velocities are in the local system. Card2 • XC = 0. x coordinate of the origin of the applied coordinate system. • YC = 0. y coordinate of the origin of the applied coordinate system. • ZC = 0. z coordinate of the origin of the applied coordinate system. • NX = x-direction cosine. • NY = y-direction cosine. • NZ = z-direction cosine. • PHASE = 0 (default), velocities are applied immediately. • IRIGID = 0: Option to overwrite or automatically set rigid body velocities defined on the *PART_INERTIA and *CONSTRAINED_NODAL_RIGID_BODY _INERTIA cards.

*INITIAL_VELOCITY_RIGID_BODY Specifies initial translational and rotational velocities at the center of gravity for rigid bodies. Card • PID = ID of the rigid body. • VX = initial translational velocity in the x direction.

288

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • VY = initial translational velocity in the y direction. • VZ = initial translational velocity in the z direction. • VXR = initial rotational velocity around the x-axis. • VYR = initial rotational velocity around the y-axis. • VZR = initial rotational velocity around the z-axis.

8.4.10. Contacts and Body Interactions *CONTACT_AUTOMATIC_GENERAL Specifies friction or frictionless contacts between line bodies (beams). This keyword is created if the contact is specified using Body Interactions and the geometry contains line bodies. All the parameter cards are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE.

*CONTACT_AUTOMATIC_NODES_TO_SURFACE Specifies nodes-to-surface friction or frictionless contacts. This keyword is created if the contact is specified using a Contact Region and the Behavior is set to Asymmetric. Card1 - mandatory • SSID = ID for the set of slave nodes involved in the contact. • MSID = ID for the set of master segments involved in the contact. • SSTYP = 4, the slave entities for the contact are nodes. • MSTYP = 0, the master entities for the contact are segments. • SBOXID, MBOXID, SPR and MPR are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Parameter Card2 and Card3 is the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE.

*CONTACT_AUTOMATIC_SINGLE_SURFACE Specifies friction or frictionless contacts between parts. This keyword is created if the contact is specified using Body Interactions. Card1 - mandatory • SSID = ID for the set of parts created for the bodies in the Body Interaction. If the contact is applied to all the bodies in the geometry then this parameter is set to 0. • MSID = 0. • SSTYP =2, the slave entities are parts. If the contact is applied to all the bodies in the geometry then this parameter is set to 5. • MSTYP = 2, the master entities are parts. If the contact is applied to all the bodies in the geometry then this parameter is set to 0. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

289

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • SBOXID = It is not used, will be left blank. • MBOXID = It is not used, will be left blank. • SPR = 1 (constant) requests that forces on the slave side of the contact be included in the results files NCFORC (ASCII) and INTFOR (binary). • MPR = 1 (constant) requests that forces on the master side of the contact be included in the results files NCFORC (ASCII) and INTFOR (binary). T Card2 - mandatory • FS = Friction Coefficient value from the inputs for frictional contact. • FD = Dynamic Coefficient value from the inputs for frictional contact. • DC = Decay Constant value from the inputs for frictional contact. • VC = 0 (LS-DYNA default). • VDC = 10 (constant). This parameter specifies the percentage of the critical viscous damping coefficient to be used in order to avoid undesirable oscillation in the contact. Card3 - mandatory, left blank for defaults to be used. Card A is the same as for *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE.

*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE Defines specific surface-to-surface friction or frictionless contacts. This keyword is created if the contact is specified using a Contact Region and the Behavior is set to Symmetric. Card1 - mandatory • SSID = ID for the set of slave segments involved in the contact. • MSID = ID for the set of master segments involved in the contact. • SSTYP = 0, the slave entities for the contact are segments. • MSTYP = 0, the master entities for the contact are segments. • SBOXID, MBOXID, SPR and MPR are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Parameter Card2 and Card3 are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Card A • SOFT = 2 except for asymmetric contacts like NODES_TO_SURFACE and unbreakable bonded contacts for which it is set to 1. • SOFSCL = left blank, the default value of 0.1 will be used. This scale factor is used to determine the stiffness of the interface when SOFT is set to 1. For SOFT = 2 scale factor SLSFAC (see *CONTROL_CONTACT) is used instead. • LCIDAB = left blank.

290

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • MAXPAR= left blank. • SBOPT = 3. • DEPTH = 5.

*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK Specifies breakable symmetric bonded contacts. This keyword is created for Bonded contact when the Breakable option is set to Stress Criteria and the contact Behavior is set to Symmetric. Card 1 is the same as in *CONTACT_TIED_SURFACE_TO_SURFACE_OFFSET. Card2 - mandatory • FS = Normal Stress Limit value for the bonded contact. • FD = Shear Stress Limit value for the bonded contact. • DC = 0 (LS-DYNA default). This parameter is not required for bonded contacts. • VC and VDC are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Card3 - mandatory, is left blank. Card A is the same as for *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE.

*CONTACT_ONEWAY_AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK Specifies breakable asymmetric bonded contacts. This keyword is created for Bonded contact when the Breakable option is set to Stress Criteria and the contact Behavior is set to Asymmetric. Parameter cards are the same as in *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK. Card A is not used for this keyword.

*CONTACT_TIED_NODES_TO_SURFACE_OFFSET Specifies non breakable asymmetric bonded contacts. This keyword is created for Bonded contacts that are not designated as Breakable whose Behavior is set to Asymmetric. This keyword is not used for Body Interactions as these types of contacts are always symmetric. Card1 - mandatory • SSID = ID for the set of slave nodes involved in the contact. • MSID = ID for the set of master segment or for the set of parts involved in the contact. • SSTYP = 4. SSID indicates the ID for a set of nodes. • MSTYP = 0, MSID indicates the ID for a set of segments. • SBOXID, MBOXID, SPR and MPR are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Card 2 left blank.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

291

Using Workbench LS-DYNA for an Explicit Dynamics Analysis Card 3 • SFS = left blank, the default value of 1.0 will be used. Default slave penalty stiffness scale factor for SLSFAC (see *CONTROL_CONTACT). • SFM= left blank, the default value of 1.0 will be used. Default master penalty stiffness scale factor for SLSFAC (see *CONTROL_CONTACT). • SST = the negative value of:

"Maximum Offset" is the Definition parameter available for bonded contacts and body interactions. "Maximum Offset" is obtained from the inputs of the Contact Region of Bonded type. • MST = SST.

*CONTACT_TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET Specifies non-breakable asymmetric bonded contacts. This keyword is created for Bonded contacts that are not designated as Breakable whose Behavior is set to Asymmetric and when the contact Formulation is set to MPC. This keyword is not used for Body Interactions as these types of contacts are always symmetric. The card is identical to CONTACT_TIED_NODES_TO_SURFACE_ OFFSET.

*CONTACT_TIED_SURFACE_TO_SURFACE_OFFSET Specifies general non-breakable bonded contacts that are symmetric. This keyword is created for Bonded and non-breakable contacts which are defined by Contact Regions that are Bonded, non-breakable and whose Behavior is set to Symmetric. Card1 - mandatory • SSID = ID for a set of slave segments or a set of parts involved in the contact. • MSID = ID for the set of master segments or the set of parts involved in the contact. • SSTYP = specifies whether the ID used in SSID represents parts or segments. It is set to 0 if SSID represents a set of segments and 2 if it represents a set of parts. • MSTYP = SSTYP. • SBOXID, MBOXID, SPR and MPR are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Cards 2 and 3 are the same as in *CONTACT_TIED_NODES_TO_SURFACE_OFFSET. Card A is the same as for *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE.

*CONTACT_TIED_SURFACE_TO_SURFACE_CONSTRAINED_OFFSET Specifies general non-breakable bonded contacts that are symmetric. This keyword is created for Bonded and non-breakable contacts which are defined by Contact Regions that are Bonded, non-breakable and whose Behavior is set to Symmetric and when the contact Formulation is set to MPC.

292

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA The card is identical to CONTACT_TIED_SURFACE_TO_SURFACE_ OFFSET.

*CONSTRAINED_SPOTWELD Specifies spot welds between non-contiguous nodal pairs of shell elements. This keyword is created when a spot weld contact is defined in the Mechanical application. Card • N1 = ID of the first node used in the weld. • N2 = ID of the second node present in the weld. • SN = Normal force at weld failure. • SS = Shear force at weld failure. • N = Exponent of normal force. • M = Exponent of shear force.

8.4.10.1. Keywords Created from the Contact Properties Object The Contact Properties object found under Part on the LSDYNA Pre tab of Workbench LS-DYNA allows you to modify the default generated values (the type of the contact) and specify additional values.

*CONTACT_ERODING_SINGLE_SURFACE is written if the contact is specified using a body interaction. The following keywords are written if the contact is specified using a contact region, and the indicated conditions exist. *CONTACT_ERODING_NODES_TO_SURFACE is written if the contact Properties Type Section is set to Eroding and the contact is asymmetric. *CONTACT_ERODING_SURFACE_TO_SURFACE is written if the contact Properties Type Section is set to Eroding and the contact is symmetric. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

293

Using Workbench LS-DYNA for an Explicit Dynamics Analysis *CONTACT_FORMING_SURFACE_TO_SURFACE is written if the contact Properties Type Section is set to Forming and the contact is symmetric. *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE is written if the contact Properties Type Section is set to Forming and the contact is asymmetric. *CONTACT_FORMING_NODES_TO_SURFACE is written if the contact Properties Type Section is set to Forming and the contact is asymmetric, and the scoped entities on the slave side are edges. *CONTACT_INTERFERENCE_SURFACE_TO_SURFACE is written if the contact Properties Type Section is set to Interference and the contact is symmetric. *CONTACT_INTERFERENCE_ONE_WAY_SURFACE_TO_SURFACE is written if the contact Properties Type Section is set to Interference and the contact is asymmetric. *CONTACT_INTERFERENCE_NODES_TO_SURFACE is written if the contact Properties Type Section is set to Interference and the contact is asymmetric, and the scoped entities on the slave side are edges. *CONTACT_TIED_SHELL_EDGE_TO_SURFACE is written if the contact Properties Type Section is set to Tied Shell Edge, the contact is asymmetric, and the contact formulation is set to MPC. *CONTACT_TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET is written if the contact Properties Type Section is set to Tied Shell Edge, the contact is asymmetric. This is the default behavior. The cards for these contact keywords are as follows: Card1 • BT = Birth Time from the Common Controls section of the Contact Properties object. • DT = Death Time from the Common Controls section of the Contact Properties object. • SFS = Slave Penalty Scale Factor from the Common Controls section of the Contact Properties object. • SFM = Master Penalty Scale Factor from the Common Controls section of the Contact Properties object. • SST = Optional Thickness for Slave Surface from the Advanced Controls section of the Contact Properties object. • MST = Optional Thickness for Master Surface from the Advanced Controls section of the Contact Properties object. • DEPTH = Depth from the Advanced Controls section of the Contact Properties object. Card A is also modified • SOFT = Soft Constraint Formulation from the Advanced Controls section of the Contact Properties object. • SOFTSCL = Soft Constraint Scale Factor from the Advanced Controls section of the Contact Properties object. If the contact type is set to Eroding, additional parameters are available to support this formulation. • ISYM = Symmetry Plane Option from the Erosion Controls section of the Contact Properties object. • IADJ = Erosion Node Option from the Erosion Controls section of the Contact Properties object.

294

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • EROSOP = Solid Elements Treatment from the Erosion Controls section of the Contact Properties object.

*CONTACT_FORCE_TRANSDUCER_PENALTY When single surface contacts are used, one or more force transducers are added via the *CONTACT_FORCE_TRANSDUCER_PENALTY command. A force transducer does not produce any contact forces and allows you to monitor the contact forces on a subset of parts of the models. A force transducer is added for each body involved in a body interaction (Frictionless or Frictional).

*CONSTRAINED_LAGRANGE_IN_SOLID

8.4.11. Magnitude and Tabular Data *DEFINE_CURVE Specifies magnitudes that are given in tabular format. Some keywords require magnitudes to be specified as a load curve. Should a constant be needed, it may be represented as a curve by repeating its value for time steps 0 and 1. Card1 • LCID = ID for load curve, is incremented every time a new load curve is defined. Card2, 3, 4... • A = abscissa value, usually time. • O = ordinate (function) value.

*DEFINE_CURVE_FUNCTION Specifies a time function where the magnitude is defined by a function expression. Card1 • LCID = ID for load curve, is incremented every time a new load curve is defined. Card2, 3 , 4 Lines of eighty characters used to form the text of the function.

8.4.12. Acceleration and Gravity *LOAD_BODY_X Specifies gravitational or other acceleration loads in the x direction. The load is applied to all nodes in the model. Card • LCID = ID of the load curve that represents the magnitude of the load (see *DEFINE_CURVE). • SF = 1.0 (default), load curve scale factor.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

295

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • LCIDDR = 0 (default), ID of load curve defined for dynamic relaxation. • XC = 0.0 (default), X-center of rotation needed for angular velocities. • YC = 0.0 (default), Y-center of rotation needed for angular velocities. • ZC = 0.0 (default), Z-center of rotation needed for angular velocities. • CID = ID of local coordinate system used. Set to 0 for the global coordinate system.

*LOAD_BODY_Y Specifies gravitational or other acceleration loads in the y direction. The load is applied to all nodes in the model. Card (see *LOAD_BODY_X).

*LOAD_BODY_Z Specifies gravitational or other acceleration loads in the z direction. The load is applied to all nodes in the model. Card (see *LOAD_BODY_X).

8.4.13. Supports *BOUNDARY_SPC_SET Specifies Fixed Support, Simply Supported, and Fixed Rotation constraints. Card • NSID = ID of set of nodes to which the boundary is applied. • CID = ID of the associated coordinate system. 0 specifies the global coordinate system. • DOFX = 0 or 1. 0 means that the translation is free and 1 that the translation is constrained along the x direction. It is set to 0 for the Fixed Rotation boundary condition and to 1 for the Simply Supported boundary condition. • DOFY = 0 or 1. 0 means that the translation is free and 1 that the translation is constrained along the y direction. It is set to 0 for the Fixed Rotation boundary condition and to 1 for the Simply Supported boundary condition. • DOFZ = 0 or 1. 0 means that the translation is free and 1 that the translation is constrained along the z direction. It is set to 0 for the Fixed Rotation boundary condition and to 1 for the Simply Supported boundary condition. • DOFRX = 0 or 1. 0 means that the rotation is free and 1 that the rotation is constrained along the x direction. It is set to 0 for the Simply Supported Boundary Condition and to 1 for the Fixed Rotation Boundary Condition when the degree of freedom is fixed in that direction.

296

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • DOFRY = 0 or 1. 0 means that the rotation is free and 1 that the rotation is constrained along the y direction. It is set to 0 for the Simply Supported Boundary Condition and to 1 for the Fixed Rotation Boundary Condition when the degree of freedom is fixed in that direction. • DOFRZ = 0 or 1. 0 means that the rotation is free and 1 that the rotation is constrained along the z direction. It is set to 0 for the Simply Supported Boundary Condition and to 1 for the Fixed Rotation Boundary Condition when the degree of freedom is fixed in that direction.

*BOUNDARY_PRESCRIBED_MOTION_RIGID See *BOUNDARY_PRESCRIBED_MOTION_SET

*BOUNDARY_PRESCRIBED_MOTION_SET Specifies velocity and displacement boundary conditions. Card1 • ID = ID of set of nodes or part (for rigid bodies) to which the boundary condition is applied. • DOF = 1, 2 or 3 depending on whether the boundary condition is in the x, y or z direction respectively, and is a translational boundary condition. DOF = 4, 5 or 6 depending on whether the boundary condition is in the x, y or z direction respectively, and is a rotational boundary condition. Setting 4 is used if the boundary is applied according to a local coordinate system. • VAD = 0 or 2 depending whether the boundary condition is velocity or displacement. • LCID = ID of the curve prescribing the magnitude of the boundary condition. Constant values of velocity are applied as a step function from time = 0. Constant values of displacement are ramped from zero at time = 0 to the constant value at termination time. This is done to make sure that displacements are applied in a transient fashion. • SF = 1.0 (default) scale factor for load curve. • VID = 0 (default). ID of vector that defines the local coordinate system the boundary condition is applied with. • DEATH = 0.0 (default), sets it to 1E28. • BIRTH = 0, the motion is applied from the beginning of the solution. Card2: not required.

8.4.14. Loads *LOAD_NODE_SET Applies a concentrated nodal force to a set of nodes. Card • NSID = the set of nodes where the force is applied. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

297

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • DOF = 1, 2 or 3 depending on the force direction x, y or z. • LCID = ID of the load curve that describes the magnitude of the force (see *DEFINE_CURVE). • SF = 1.0 (default), load curve scale factor. • CID = ID of local coordinate system used. Set to 0 for the global coordinate system.

*LOAD_RIGID_BODY Applies a concentrated nodal force to a rigid body. The force is applied at the center of mass. Card See *LOAD_NODE_SET. Note that parameter NSID is replaced by PID which is the ID of the part the force is applied to.

*LOAD_SEGMENT_SET Applies a distributed pressure load over each segment in a segment set. Card • LCID = ID of the load curve that describes the magnitude of the pressure (see *DEFINE_CURVE). • SSID = ID of set of nodes to which the pressure is applied. • SF = 1.0 (default), load curve scale factor. • AT = arrival time for pressure is assigned the time at load step 1 if pressure is given in tabular form or 0 if constant pressure.

8.4.15. Discrete Connections *SECTION_DISCRETE Defines section properties for solid elements. DRO is the Displacement/Rotation Option. • SECID = ID of the section. • DRO = – 0 for translational spring/damper. – 1 for torsional spring/damper.

*ELEMENT_DISCRETE Specifies spring elements. • EID = ID of the element. • PID = ID of the part it belongs to. • N1 = ID of nodal point 1.

298

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA • N2 = ID of nodal point 2.

*MAT_SPRING_ELASTIC This keyword is used in support of spring connections, the K parameter of this material keyword is the stiffness of the string. • MID = ID of material type. Must be unique between the material keyword definitions. • K = Elastic stiffness (force/displacement) or (moment/rotation).

*MAT_DAMPER_VISCOUS This keyword is used in support of spring connections. The damping constant DC of this material is the damping parameter of the spring, if this damping is non null. • MID = ID of material type. Must be unique between the material keyword definitions. • DC = Damping constant (force/displacement rate) or (moment/rotation rate).

8.4.16. Other Supports *BOUNDARY_NON_REFLECTING Specifies impedance boundaries. Impedance boundaries can only be applied on solid elements in LSDYNA. Card • SSID = ID of segment on whose nodes the boundary is applied (see *SET_SEGMENT bellow). • AD = 0.0 (default) for setting the activation flag for dilatational waves to on. • AS = 0.0 (default) for setting the activation flag for shear waves to on.

*BOUNDARY_SLIDING_PLANE Defines a boundary plane for sliding symmetry. • NSID = ID of the set of nodes to which the boundary is applied • VX = X component of vector defining normal. • VY = Y component of vector defining normal. • VZ = Z component of vector defining normal. • COPT = – 0 if the Option is set to node moves on normal plane. – 1 if the Option is set to node moves only in vector direction.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

299

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

*RIGID_WALL_PLANAR The RIGIDWALL option provides a simple way of treating contact between a rigid surface and nodal points of a deformable body, called slave nodes.

• NSID = ID of the set of nodes to which the boundary is applied. • XT, YT, ZT, XH, YH, ZH are calculated from the coordinate system definition; the normal Z of the coordinate system is the normal to the plane. • FRIC = Friction

8.4.17. Environment Temperature *INITIAL_TEMPERATURE_SET This keyword is added in coupled structural thermal analyses, where it defines the initial temperature of the environment. • NSID = 0. All nodes of the model are initialized with the temperature Temp. • Temp = temperature of the environment.

8.4.18. ASCII Files The following keywords specify time-history output (ASCII format) for an explicit dynamics analysis. The time history files output are requested through Time History Output Controls section of the Analysis Settings. Up to 10 ASCII files can be requested in the GUI. The sampling time is calculated from the number of values requested and from the end time of the simulation.

300

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA The results files (GLSTAT, BNDOUT, RCFORC, SPCFORC,MATSUM) are always output by Workbench LSDYNA. The sampling frequency can, however, be modified.

*DATABASE_HISTORY_NODE_SET Controls which nodes or elements are output into the binary history file and the ASCII file NODOUT for a particular result tracker. Card ID1 is set to the id of the component defined by the result tracker object.

*DATABASE_BNDOUT Specifies the sampling parameters for the BNDOUT results file (stores Boundary condition forces and energy). Card DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_DEFGEO Specifies the sampling parameters for the DEFGEO results file (stores Deformed Geometry Data). Card DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_DEFORC Specifies the sampling parameters for the DEFORC results file (Discrete Elements Data). Card DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_GCEOUT Specifies the sampling parameters for the GCEOUT results file (Geometric Contact Entities). Card DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_GLSTAT Specifies the sampling parameters for the GLSTAT results file (stores general energy results). Card

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

301

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_INTFORC Specifies the sampling parameters for the JNTFORC results file (stores Joint Forces). DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_MATSUM Specifies the sampling parameters for the MATSUM results file (stores general energy and velocity results as the GLSTAT file but it stores them per body. It is necessary for rigid bodies). Card • DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_NCFORC Specifies the sampling parameters for the NCFORC results file (stores Nodal Interface Forces). Card • DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_NODOUT Specifies the sampling parameters for the NODOUT results file (stores displacement and velocity results). Card • DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_RBDOUT Specifies the sampling parameters for the RBDOUT results file (stores Rigid Body Data ). Card DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_RCFORC Specifies the sampling parameters for the RCFORC results file (stores contact forces). Card DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_RWFORC Specifies the sampling parameters for the RWFORC results file (stores Rigid Wall forces). 302

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

LS-DYNA Keywords used by Workbench LS-DYNA Card DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_SLEOUT Specifies the sampling parameters for the SLEOUT results file (stores sliding interface forces). Card • DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_SPCFORC Specifies the sampling parameters for the SPCFORC results file (stores reaction forces). Card • DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

*DATABASE_SWFORC Specifies the sampling parameters for the SWFORC results file (stores the spotweld and rivet forces). Card • DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings.

8.4.19. Database Output Settings *DATABASE_EXTENT_BINARY Control to some extent the content of binary output databases d3plot, d3thdt, and d3part. four parameters are set by Workbench LS-DYNA : • SIGFLG: Flag for including the stress tensor for shells. • STRFLG: Flag for including the strain tensor for shells. • EPSFLG: Flag for including the effective plastic strains for shells. • MSSCL: Output nodal information related to mass scaling into the d3plot database.

*DATABASE_BINARY_D3PLOT Specifies the sampling parameters for the binary D3PLOT results plotting file. Card • DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings if Calculate Results At is set to Equally Spaced Time Points ( this value defaults to 20).

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

303

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

*DATABASE_BINARY_INTFOR Specifies the sampling parameters for the binary intfor results file. This file contains contact information ( pressure, nodal contact forces) Card • DT = End Time divided by Value from the Time History Output Controls section of the Analysis Settings if Calculate Results At is set to Equally Spaced Time Points ( this value defaults to 20).

8.4.20. End of Input File *END Terminates the keyword file. It has no parameter cards.

8.5. Material Models Available in Workbench LS-DYNA 8.5.1. Introduction Workbench LS-DYNA supports a large material library, and can, therefore, simulate nearly any application. Workbench LS-DYNA materials offer many features including: • Strain rate dependent plasticity models with strain failure criterion. • Temperature dependent and temperature sensitive plasticity models. • Equations of state and null material models (bird-strike analyses, etc.). The modeling of such phenomena can generally be broken down into three components: 8.5.1.1. Equation of State 8.5.1.2. Material Strength Model 8.5.1.3. Material Failure Model

8.5.1.1. Equation of State An equation of state describes the hydrodynamic response of a material. This is the primary response for gases and liquids, which can sustain no shear. Their response to dynamic loading is assumed hydrodynamic, with pressure varying as a function of density and internal energy. This is also the primary response for solids at high deformation rates, when the hydrodynamic pressure is far greater than the yield stress of the material.

8.5.1.2. Material Strength Model Solid materials may initially respond elastically, but under highly dynamic loadings, they can reach stress states that exceed their yield stress and deform plastically. Material strength laws describe this nonlinear elastic-plastic response.

304

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Material Models Available in Workbench LS-DYNA

8.5.1.3. Material Failure Model Solids usually fail under extreme loading conditions, resulting in crushed or cracked material. Material failure models simulate the various ways in which materials fail. Liquids will also fail in tension, a phenomenon usually referred to as cavitation.

8.5.2. Density See the description in Density (p. 171).

8.5.3. Linear Elastic See the description in Linear Elastic (p. 171).

8.5.3.1. Isotropic Elasticity See the description in Isotropic Elasticity (p. 171). This material behavior is written as *MAT_ELASTIC (p. 270).

8.5.3.2. Orthotropic Elasticity See the description in Orthotropic Elasticity (p. 172). This material behavior is written as *MAT_ORTHOTROPIC_ELASTIC (p. 276).

8.5.3.3. Anisotropic Elasticity This material description requires the full elasticity matrix. Because of symmetry, only 21 constants are required:

This material is only valid for solid elements. Material properties are locally orthotropic with material axes defined based on the mesh orientation defined in the Mechanical application (Body orientation).

8.5.4. Test Data See the description in Test Data (p. 173).

8.5.5. Hyperelasticity Following are several forms of strain energy potential (Ψ) provided for the simulation of nearly incompressible hyperelastic materials. The different models are generally applicable over different ranges of strain as illustrated in Hyperelasticity (p. 173), however these numbers are not definitive and users should verify the applicability of the model chosen prior to use.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

305

Using Workbench LS-DYNA for an Explicit Dynamics Analysis Hyperelastic materials may only be used in solid and shell elements for LS-DYNA simulations. See Hyperelasticity (p. 173) for additional information on the models discussed in this section.

8.5.5.1. Blatz-Ko Hyperelasticity Blatz-Ko materials are only for rubber materials under compression. Poisson's ratio (NUXY) is automatically set to 0.463 by LS-DYNA, so only density and initial shear modulus are required. This model uses the second Piola-Kirchhoff stress:

G is the shear modulus, V is the relative volume, ν is the Poisson's ratio, Cij is the right Cauchy-Green strain tensor, and δij is the Kronecker delta. This material behavior is written as *MAT_BLATZ-KO_RUBBER (p. 270).

8.5.5.2. Mooney-Rivlin The 2, 3, 5 parameter Mooney-Rivlin hyperelastic material models have been implemented. The 9 parameter version of this material model is not supported. This material behavior is written as *MAT_HYPERELASTIC_RUBBER (p. 272).

8.5.5.3. Polynomial This material behavior is written as *MAT_HYPERELASTIC _RUBBER (p. 272).

8.5.5.4. Yeoh The first order and second order of this material model have been implemented. This material behavior is written as *MAT_HYPERELASTIC_RUBBER (p. 272).

8.5.5.5. Ogden This material behavior is written as *MAT_OGDEN_RUBBER (p. 275).

8.5.6. Plasticity All stress-strain input should be in terms of true stress and true (or logarithmic) strain and result in all output as also true stress and true strain. For small-strain regions of response, true stress-strain and engineering stress-strain are approximately equal. If your stress-strain data is in the form of engineering stress and engineering strain you can convert: • strain from engineering strain to logarithmic strain using:

306

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Material Models Available in Workbench LS-DYNA • engineering stress to true stress using:

Note This stress conversion is only valid for incompressible materials. The following Plasticity models are discussed in this section: 8.5.6.1. Bilinear Isotropic Hardening 8.5.6.2. Multilinear Isotropic Hardening 8.5.6.3. Bilinear Kinematic Hardening 8.5.6.4. Johnson-Cook Strength 8.5.6.5. Cowper-Symonds Power Law Hardening 8.5.6.6. Rate Sensitive Power Law Hardening 8.5.6.7. Cowper-Symonds Piecewise Linear Hardening 8.5.6.8. Modified Cowper-Symonds Piecewise Linear Hardening

8.5.6.1. Bilinear Isotropic Hardening This plasticity material model is often used in large strain analyses. A bilinear stress-strain curve requires that you input the Yield Strength and Tangent Modulus. The slope of the first segment in the curve is equivalent to the Young's modulus of the material while the slope of the second segment is the tangent modulus. This material behavior is written as *MAT_PLASTIC_KINEMATIC (p. 277). The parameter beta of this keyword is set to 1. Custom results variables available for this model: Name Description

Solids Shells Beams

EPS

Yes

Effective Plastic Strain

Yes*

No

*Resultant value over shell/beam section.

8.5.6.2. Multilinear Isotropic Hardening This plasticity material model is often used in large strain analyses. Do not use this model for cyclic or highly nonproportional load histories in small-strain analyses. You must supply the data in the form of plastic strain vs. stress. The first point of the curve must be the yield point, that is, zero plastic strain and yield stress. The slope of the stress-strain curve is assumed to be zero beyond the last user-defined stress-strain data point. No segment of the curve can have a slope of less than zero.

Note You can define up to 10 stress strain pairs using this model in explicit dynamics systems. Temperature dependence of the curves is not directly supported. Temperature dependent plasticity can be represented using the Johnson-Cook plasticity model. Custom results variables available for this model: Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

307

Using Workbench LS-DYNA for an Explicit Dynamics Analysis Name Description

Solids Shells Beams

EPS

Yes

Effective Plastic Strain

Yes*

No

*Resultant value over shell/beam section.

8.5.6.3. Bilinear Kinematic Hardening This plasticity material model assumes that the total stress range is equal to twice the yield stress, to include the Bauschinger effect. This model may be used for materials that obey Von Mises yield criteria (includes most metals). The tangent modulus cannot be less than zero or greater than the elastic modulus. This material behavior is written as *MAT_PLASTIC_KINEMATIC (p. 277). The parameter beta of this keyword is set to 0. Custom results variables available for this model: Name Description

Solids Shells Beams

EPS

Yes

Effective Plastic Strain

Yes*

No

*Resultant value over shell/beam section.

8.5.6.4. Johnson-Cook Strength See Johnson-Cook Strength (p. 180) for information about this model. However, the strain rate correction parameter described in this material model is not used by LS-DYNA. This material behavior is written as *MAT_JOHNSON_COOK (p. 273) or *MAT_SIMPLIFIED_JOHNSON_COOK (p. 280) depending on whether it is used in combination with an equation of state or not. The simplified form is used when no equation of state is defined. The thermal terms are discarded in that scenario. Custom results variables available for this model: Name Description

Solids Shells Beams

EPS

Effective Plastic Strain

Yes

Yes*

No

TEMP

Temperature**

Yes

Yes*

No

*Resultant value over shell/beam section. **Temperature will be non-zero only if a specific heat capacity is defined.

8.5.6.5. Cowper-Symonds Power Law Hardening The Cowper-Symonds power law hardening lets you define plastic behavior with bilinear isotropic hardening and power law hardening defined with strength coefficient K and hardening coefficient n. Strain rate effects are accounted for by the Cowper-Symonds strain rate parameters, C and P.

308

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Material Models Available in Workbench LS-DYNA Yield surface can be scaled for strain rate dependence or the latter can be defined using a fully viscoplastic formation. This material behavior is written as *MAT_POWER_LAW_PLASTICITY (p. 278). Name

Symbol Units Notes

Initial Yield Stress

A

Stress

Hardening Constant

K

Stress

Hardening Exponent

n

None

Strain Rate Constant C

None Assumed 1/second in all cases

Strain Rate Constant P

None

Strain Rate Correction

None Option List:

-

Scale Yield Stress Viscoplastic Custom results variables available for this model: Name Description

Solids Shells Beams

EPS

Yes

Effective Plastic Strain

Yes*

Yes*

*Resultant value over shell/beam section.

8.5.6.6. Rate Sensitive Power Law Hardening Strain rate dependent plasticity model typically used for superplastic forming analyses. The material model follows a Ramburgh-Osgood constitutive relationship of the form:

where: k is the material coefficient, m is the hardening coefficient, n is the strain rate parameter. Name

Symbol Units Notes

Hardening Constant

K

Stress

Hardening Exponent

m

None

Strain Rate Constant

n

None

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

309

Using Workbench LS-DYNA for an Explicit Dynamics Analysis Name

Symbol Units Notes

Reference Strain Rate

None Units fixed at 1/sec Default = 0.0002

This material behavior is written as *MAT_RATE_SENSITIVE_POWERLAW_PLASTICITY (p. 278).

8.5.6.7. Cowper-Symonds Piecewise Linear Hardening This model is very efficient in solution and is most commonly used in crash simulations. It is similar to the multilinear isotropic hardening behavior. Stress-strain behavior is defined with a load curve of effective true stress versus effective plastic true strain. Failure strain can be input for which elements will be eliminated. Yield surface can be scaled for strain rate dependence by the Cowper-Symonds model. This material behavior is written as *MAT_ PIECEWISE_LINEAR_PLASTICITY (p. 277), where the parameter lcss is the curve id of the effective stress versus plastic strain. Name

Symbol Units Notes

Initial Yield Stress

A

Stress

Strain Rate Constant C

None Assumed 1/second in all cases

Strain Rate Constant P

None

Strain Rate Correction

None Option List:

-

Scale Yield Stress Viscoplastic

8.5.6.8. Modified Cowper-Symonds Piecewise Linear Hardening This model is an enhanced version of the Cowper Symonds Piecewise Linear model that accounts for multiple failure methods: • Effective plastic strain • Thinning (through-thickness) plastic strain • Major principal in-plane strain The plastic strain failure parameter of this material model is defined by adding a plastic strain failure behavior to it. Name

Symbol Units Notes

Initial Yield Stress

A

Stress

Strain Rate Constant

C

None Assumed 1/second in all cases

Strain Rate Constant

P

None

Thinning Strain At Failure

310

None

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Material Models Available in Workbench LS-DYNA Name

Symbol Units Notes

Major In Plane Strain At Failure Strain Rate Correction

None -

None Option List: Scale Yield Stress Viscoplastic

This material behavior is written as *MAT_ MODIFIED_PIECEWISE_LINEAR_PLASTICITY (p. 274), where the parameter lcss is the curve id of the effective stress versus plastic strain.

8.5.7. Forming Plasticity The following Forming Plasticity models are discussed in this section: 8.5.7.1. Bilinear Transversely Anisotropic Hardening 8.5.7.2. Multilinear Transversely Anisotropic Hardening 8.5.7.3. Bilinear FLD Transversely Anisotropic Hardening 8.5.7.4. Multilinear FLD Transversely Anisotropic Hardening 8.5.7.5. Bilinear 3 Parameter Barlat Hardening 8.5.7.6. Exponential 3 Parameter Barlat Hardening 8.5.7.7. Exponential Barlat Anisotropic Hardening

8.5.7.1. Bilinear Transversely Anisotropic Hardening This material model is most commonly used for sheet metal forming of anisotropic materials. It is a fully iterative anisotropic plasticity model available for shell and 2–D elements only. In this model the yield function given by Hill[3] is reduced to the following for the case of plane stress:

The anisotropic hardening parameter, R, is defined by the ratio of the in-plane plastic strain rate to the out-of-plane plastic strain rate:

Name

Symbol Units Notes

Yield Strength

Stress

Tangent Modulus

Stress

Anisotropic hardening Parameter

None

This material behavior is written as *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC (p. 280).

8.5.7.2. Multilinear Transversely Anisotropic Hardening This material model is most commonly used for sheet metal forming of anisotropic materials.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

311

Using Workbench LS-DYNA for an Explicit Dynamics Analysis It is a fully iterative anisotropic plasticity model available for shell and 2-D elements only. In this model the yield function given by Hill[3] is reduced to the following for the case of plane stress:

A load curve parameter is defined for the relationship between the effective yield stress and the effective plastic strain. Name

Symbol Units Notes

Anisotropic hardening Parameter

None

This material behavior is written as *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC (p. 280).

8.5.7.3. Bilinear FLD Transversely Anisotropic Hardening This material model is used for simulating the sheet metal forming of anisotropic materials. Only transversely anisotropic materials can be considered. For this model, the dependence of the flow stress with the effective plastic strain is modeled by defining a yield stress and a tangent modulus. In addition, you also define a forming limit diagram. This diagram will be used to compute the maximum strain ratio that the material can experience.

This plasticity model is only available for shell and 2-D elements. The model directly follows the plasticity theory introduced in the Transversely Anisotropic Elastic Plastic model described earlier in this section. You can refer to that model for the theoretical basis. Name Yield Strength

312

Symbol Units Notes Stress

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Material Models Available in Workbench LS-DYNA Name

Symbol Units Notes

Tangent Modulus

Stress

Anisotropic hardening Parameter

None

This material behavior is written as *MAT_FLD_TRANSVERSELY_ANISOTROPIC (p. 272).

8.5.7.4. Multilinear FLD Transversely Anisotropic Hardening This material model is used for simulating the sheet metal forming of anisotropic materials. Only transversely anisotropic materials can be considered. For this model, the dependence of the flow stress with the effective plastic strain is modeled using a curve. In addition, you also define a forming limit diagram. This diagram will be used to compute the maximum strain ratio that the material can experience. This plasticity model is only available for shell and 2-D elements. The model directly follows the plasticity theory introduced in the Transversely Anisotropic Elastic Plastic model described earlier in this section. You can refer to that model for the theoretical basis.

Name

Symbol Units Notes

Anisotropic hardening Parameter

None

This material behavior is written as *MAT_FLD_TRANSVERSELY_ANISOTROPIC (p. 272).

8.5.7.5. Bilinear 3 Parameter Barlat Hardening This is an anisotropic plasticity model developed by Barlat and Lian[1] used for modeling aluminum sheets under plane stress conditions. Both exponential and linear hardening rules are available. The anisotropic yield criterion for plane stress is defined as: Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

313

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

where σY is the yield stress, a and c are anisotropic material constants, m is Barlat exponent, and K1 and K2 are defined by:

Here, h and p are additional anisotropic material constants. For the exponential hardening option, the material yield strength is given by:

where k is the strength coefficient, ε0 is the initial strain at yield, εp is the plastic strain, and n is the hardening coefficient. All of the anisotropic material constants, excluding p which is determined implicitly, are determined from Barlat and Lian width to thickness strain ratio (R) values as shown:

c=2–a

The width to thickness strain ratio for any angle Φ can be calculated from:

The hardening rule is linear and requires input of yield strength and tangent modulus, in addition to the Barlat exponent. This material behavior is written as *MAT_3-PARAMETER_BARLAT (p. 269).

8.5.7.6. Exponential 3 Parameter Barlat Hardening The theory is identical to the bilinear 3 parameter Barlat model, but for this material model the hardening rule is exponential. It requires input of the hardening constant K, and hardening exponent, in addition to the Barlat exponent. This material behavior is written as *MAT_3-PARAMETER_BARLAT (p. 269).

8.5.7.7. Exponential Barlat Anisotropic Hardening This is an anisotropic plasticity model developed by Barlat, Lege, and Brem[2] used for modeling material behavior in forming processes. The anisotropic yield function Φ is defined as:

314

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Material Models Available in Workbench LS-DYNA

where m is the flow potential exponent and Si are the principal values of the symmetric matrix Sij.

where a, b, c, f, g, and h represent the anisotropic material constants. When a=b=c=f=g=h=1, isotropic material behavior is modeled and the yield surface reduces to the Tresca surface for m = 1 and the von Mises surface for m = 2 or 4. For this material option, the yield strength is given by:

where k is the strength coefficient, εP is the plastic strain, ε0 is the initial strain at yield, and n is the hardening coefficient. The stress-strain behavior can be specified at only one temperature. This material behavior is written as *MAT_3-PARAMETER_BARLAT (p. 269).

8.5.8. Foams 8.5.8.1. Rate Independent Low Density Foam This is a highly compressible (urethane) foam material model often used for padded materials such as seat cushions. In compression, the model assumes hysteresis unloading behavior with possible energy dissipation. In tension, the material model behaves linearly until tearing occurs. For uniaxial loading, the model assumes that there is no coupling in transverse directions. By using input shape factor controls (a hysteresis unloading factor (HU), a decay constant (β), and a shape factor for unloading), the observed unloading behavior of foams can be closely approximated. The stress-strain behavior can be specified at only one temperature. Input the curve for nominal stress vs. strain, the tension cutoff (tearing) stress, the hysteresis unloading factor, the decay constant, the viscous coefficient, and the shape factor for unloading,

8.5.9. Eulerian 8.5.9.1. Vacuum This model is a dummy material representing a vacuum in a multi-material Euler/ALE model. Instead of using ELFORM = 12 (under *SECTION_SOLID), you should use ELFORM = 11 with the void material defined as vacuum material instead.

8.5.10. Rigid Materials See the description in Rigid Materials (p. 227).

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

315

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

8.5.11. Equations of State Background information is discussed in this section along with available EOS models: 8.5.11.1. Background 8.5.11.2. Bulk Modulus 8.5.11.3. Shear Modulus 8.5.11.4. Polynomial EOS 8.5.11.5. Shock EOS Linear 8.5.11.6. Shock EOS Bilinear

8.5.11.1. Background A general material model requires equations that relate stress to deformation and internal energy (or temperature). In most cases, the stress tensor may be separated into a uniform hydrostatic pressure (all three normal stresses equal) and a stress deviatoric tensor associated with the resistance of the material to shear distortion. Then the relation between the hydrostatic pressure, the local density (or specific volume) and local specific energy (or temperature) is known as an equation of state. Hooke's law is the simplest form of an equation of state and is implicitly assumed when you use linear elastic material properties. Hooke's law is energy independent and is only valid if the material being modeled undergoes relatively small changes in volume (less than approximately 2%). One of the alternative equation of state properties should be used if the material is expected to experience high volume changes during an analysis. Before looking at the various equations of state available, it is good to understand some of the fundamental physics behind their formulations. See the links in the following sections.

8.5.11.2. Bulk Modulus See the description in Bulk Modulus (p. 200).

8.5.11.3. Shear Modulus See the description in Shear Modulus (p. 200).

8.5.11.4. Polynomial EOS See the description in Polynomial EOS (p. 201). They are written as *EOS_LINEAR_POLYNOMIAL (p. 268). See LS-DYNA Keywords used by Workbench LS-DYNA (p. 252) for more information.

8.5.11.5. Shock EOS Linear See the description in Shock EOS Linear (p. 203). They are written as *EOS_GRUNEISEN (p. 268). See LS-DYNA Keywords used by Workbench LS-DYNA (p. 252) for more information.

316

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Material Models Available in Workbench LS-DYNA

8.5.11.6. Shock EOS Bilinear See the description in Shock EOS Bilinear (p. 204). They are written as *EOS_GRUNEISEN (p. 268). See LS-DYNA Keywords used by Workbench LS-DYNA (p. 252) for more information.

8.5.12. Failure Background Materials are not able to withstand tensile stresses which exceed the material's local tensile strength. The computation of the dynamic motion of materials assuming that they always remain continuous, even if the predicted local stresses reach very large values, will lead to unphysical solutions. A model has to be constructed to recognize when tensile limits are reached to modify the computation to deal with this and to describe the properties of the material after this formulation has been applied. Several different modes of failure initiation can be represented in the explicit dynamics system. Element failure in the explicit dynamics system has two components, failure initiation and post failure response.

Failure Initiation A number of mechanisms are available to initiate failure in a material (see properties Plastic Strain Failure, Principal Stress Failure, Principal Strain Failure, Tensile Pressure Failure, Johnson-Cook Failure). When specified criteria are met within an element, a post failure response is activated.

Post Failure Response After failure initiation in an element, the subsequent strength characteristics of the element will change depending on the type of failure model. • Instantaneous Failure Upon failure initiation, the element deviatoric stress will be immediately set to zero and retained at this level. Subsequently, the element will only be able to support compressive pressures. By default, tensile failure models will produce an instantaneous post failure response. The following Failure models are discussed in this section: 8.5.12.1. Plastic Strain Failure 8.5.12.2. Principal Stress Failure 8.5.12.3. Principal Strain Failure 8.5.12.4. Johnson-Cook Failure

8.5.12.1. Plastic Strain Failure Plastic strain failure can be used to model ductile failure in materials. Failure initiation is based on the effective plastic strain in the material. The user inputs a maximum plastic strain value.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

317

Using Workbench LS-DYNA for an Explicit Dynamics Analysis If the material effective plastic strain is greater than the user defined maximum, failure initiation occurs. The material instantaneously fails.

Note This failure model must be used in conjunction with a plasticity or brittle strength model.

8.5.12.2. Principal Stress Failure Principal stress failure can be used to represent brittle failure in materials. Failure initiation is based on one of two criteria • Maximum principal tensile stress • Maximum shear stress (derived from the maximum difference in the principal stresses) Failure is initiated when either of the above criteria is met. The material instantaneously fails. If this model is used in conjunction with a plasticity model, it is often recommended to deactivate the Maximum Shear stress criteria by specifying a large value. In this case the shear response will be handled by the plasticity model. Name

Symbol Units Notes

Maximum Tensile Stress

Stress User must input a positive value. Default = +1e+20

Maximum Shear Stress

Stress User must input a positive value. Default = +1e+20

8.5.12.3. Principal Strain Failure Principal strain failure can be used to represent brittle or ductile failure in materials. Failure initiation is based on one of two criteria • Maximum principal tensile strain • Maximum shear strain (derived from the maximum difference in the principal strains) Failure is initiated when either of the above criteria is met. The material instantaneously fails. If this model is used in conjunction with a plasticity model, it is often recommended to deactivate the maximum shear strain criteria by specifying a large value. In this case the shear response will be treated by the plasticity model. Name

Symbol Units Notes

Maximum Principal Strain

None User must input a positive value. Default = +1e+20

Maximum Shear Strain

None User must input a positive value. Default = +1e+20

318

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Customizing Workbench LS-DYNA using ACT

8.5.12.4. Johnson-Cook Failure The Johnson-Cook failure model can be used to model ductile failure of materials experiencing large pressures, strain rates and temperatures.

This model is constructed in a similar way to the Johnson-Cook plasticity model in that it consists of three independent terms that define the dynamic fracture strain as a function of pressure, strain rate and temperature: Name

Symbol Units

Damage Constant D1

D1

None

Damage Constant D2

D2

None

Damage Constant D3

D3

None

Damage Constant D4

D4

None

Damage Constant D5

D5

None

Melting Temperature

Notes

Temperature

8.5.13. Thermal Properties Properties Isotropic Thermal Conductivity Specific Heat These properties are used when the LS-DYNA calculation is thermal-structural coupled, and are part of the definition of the *MAT_THERMAL_ISOTROPIC material.

8.6. Customizing Workbench LS-DYNA using ACT Workbench LS-DYNA can be customized with ACT (ANSYS Customization Toolkit). You can create interactions between user defined extensions and the Workbench LS-DYNA system. You can create objects or features for custom preprocessing in the context of ANSYS Mechanical. Custom postprocessing is not supported. This section assumes some degree of familiarity with ACT. Other ANSYS guides provide related information: • For an introduction to writing scripts for Mechanical, see the Scripting in Mechanical Guide. • For descriptions of all ACT API objects, methods, and properties, see the ANSYS ACT API Reference Guide. • For information on how to use ACT to create apps (extensions) that customize and automate ANSYS products, see the ANSYS ACT Developer's Guide. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

319

Using Workbench LS-DYNA for an Explicit Dynamics Analysis • For ACT usage, customization, and automation information specific to Mechanical, see the ANSYS ACT Customization Guide for Mechanical. An example of how to set up custom preprocessing is described here. The following is an example from an XML file that sets up Rigid Bodies and Flexible Bodies categories in the Data panel, each with a Geometry field. The resulting load and Details panel are shown.

[function(solver,solverdata,stream)]

320

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Customizing Workbench LS-DYNA using ACT The solverdata is a helper structure. It helps integrate user extensions with Workbench LS-DYNA, particularly when the solver commands generated by the extension add entities that have identifiers, like nodes, elements or components. Through the solverdata structure, ACT provides an efficient method to manage the newly created IDs of these entities with the existing IDs previously generated by Workbench LS-DYNA. It also enables reuse of internally implemented keywords like materials or elements.

Note The Workbench LS-DYNA extension is written in C# and the syntax shown for the methods is C#. The following table and sections describe the available solverdata methods. Table 8.1: Solverdata Methods CreateMaterial (p. 322)CreateMaterial (p. 322) Two different methods available to create materials for LS-DYNA. CreateNewElement (p. 322)

Method to create an element keyword.

GetNewPartId (p. 323)

Method to get an unused part identifier.

LSDynaSolverExtension.KeyWords.Part.Part CreateNewPart (p. 323)

Method to create a new part keyword.

CreateSection (p. 324)

Method to create a new section keyword.

GetComponent (p. 324)

Method to get the LS-DYNA equivalent of a mechanical Named Selection.

GetContactId (p. 324)

Method to get the solver contact identifier of the contact object.

GetContactTargetId (p. 325)

Method to get the solver contact identifier of the contact target object.

GetCoordinateSystemSolverId (p. 325)

Method to get the solver coordinate system identifier.

GetEndTime (p. 325)

Method to get the simulation end time.

GetMaterialSolverId (p. 325)

Method to get the material identifier of a body.

GetNamedSelectionLSDYNAId (p. 326)

Method to get the solver named selection identifier.

GetNewContact (p. 326)

Method to get an empty contact keyword.

GetNewCurveId (p. 326)

Method to get an unused curve identifier.

GetNewElementId (p. 326)

Method to get an unused element identifier.

GetNewElementType (p. 326)

Method to get an unused part identifier.

GetNewNodeId (p. 327)

Method to get an unused node identifier.

GetNewVectorId (p. 327)

Method to get an unused vector identifier.

GetRemotePointNodeId (p. 327)

Method to get the master node identifier for a remote point.

GetSolverUnitSystem (p. 327)

Method to get the solver unit system.

ContainsDynamicRelaxation (p. 327)

Method to determine if dynamic relaxation is used in the model.

CurrentStep (p. 328)

Method to get the current step.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

321

Using Workbench LS-DYNA for an Explicit Dynamics Analysis MaxElementId (p. 328)

Method to get the maximum element identifier.

MaxElementType (p. 328)

Method to get the maximum part identifier.

MaxNodeId (p. 328)

Method to get the maximum node identifier.

8.6.1. CreateMaterial This method tries to create a Workbench LS-DYNA material keyword based on the Engineering Data material object. For example. If the material is an elastic only material, this method will return *MAT_ELASTIC keyword.

Declaration Syntax public IMaterialKeyWord CreateMaterial(IMaterial materialClass, long materialId); Table 8.2: Properties Property

Type

Description

materialClass IMaterial The class of the Engineering Data material object. materialID

long

The ID of the Engineering Data material object.

8.6.2. CreateMaterial This method tries to create a Workbench LS-DYNA material keyword based on the Engineering Data material object and the material type. For example, if the material is compatible with an LS-DYNA spotweld material (has at least elastic properties) and *MAT_SPOTWELD is entered as the material type, this method will return *MAT_SPOTWELD keyword.

Declaration Syntax public IMaterialKeyWord CreateMaterial(IMaterial materialClass, string materialType, long materialId); Table 8.3: Properties Property

Type

Description

materialClass IMaterial The class of the Engineering Data material object. materialType string

The type of the Engineering Data material object.

materialID

The ID of the Engineering Data material object.

long

8.6.3. CreateNewElement This method creates an element keyword (solid, shell, beam, etc.) based elementType and will return the LS-DYNA keyword that represents the specified element type.

322

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Customizing Workbench LS-DYNA using ACT

Declaration Syntax public IKeyWord CreateNewElement(string elementType); The following element types are available: Table 8.4: Properties Property

Type Description

elementType string The following values are valid: • "*ELEMENT_SOLID": • "*ELEMENT_SHELL": • "*ELEMENT_BEAM": • "*ELEMENT_DISCRETE": • "*ELEMENT_INERTIA": • "*ELEMENT_MASS": • "*ELEMENT_TSHELL":

8.6.4. GetNewPartId This method returns an unused part identifier.

Declaration Syntax public long GetNewPartId() ;

8.6.5. LSDynaSolverExtension.KeyWords.Part.Part CreateNewPart This method will create a new part keyword with the identifier partId. By default, the material identifier and the section identifier are set to partId. This method should be used in conjunction with the method GetNewPartId() to avoid identifier clashes in the input file.

Declaration Syntax public LSDynaSolverExtension.KeyWords.Part.Part CreateNewPart(long partId); Table 8.5: Properties Property Type Description partId

long The ID of the newly created part.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

323

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

8.6.6. CreateSection This method will create a new section keyword based on the section type sectionName, on the section identifier secId, and the element formulation elform.

Declaration Syntax public IKeyWord CreateSection(string sectionName, long secId, long elform); The following section types are available: Table 8.6: Properties Property

Type Description

elementType string The following values are valid: • "*SECTION_SOLID" • "*SECTION_SECTION_ALE" • "*SECTION_SHELL" • "*SECTION_BEAM" • "SECTION_DISCRETE"

8.6.7. GetComponent This method returns a string containing the LS-DYNA text equivalent of a Mechanical Named Selection given an ACT selectionInfo. The identifier of the component identifier is automatically incremented by Workbench LS-DYNA.

Declaration Syntax public string GetComponent(ISelectionInfo info, out int nsid); Table 8.7: Properties Property Type

Description

info

ISelectionInfo An ACT selection object.

nsid

int

A new ID for the named selection created.

8.6.8. GetContactId This method returns the solver contact identifier given the tree identifier of the contact object.

324

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Customizing Workbench LS-DYNA using ACT

Declaration Syntax public string GetContactId(int treeId); Table 8.8: Properties Property Type Description treeId

int

Workbench ID of contact object.

8.6.9. GetContactTargetId This method returns the solver contact target identifier given the tree identifier of the contact object.

Declaration Syntax public string GetContactTargetId(int treeId); Table 8.9: Properties Property Type Description treeId

int

Workbench ID of contact target object.

8.6.10. GetCoordinateSystemSolverId This method returns the solver coordinate system identifier given the tree identifier of the coordinate system object.

Declaration Syntax public string GetCoordinateSystemSolverId(int id); Table 8.10: Properties Property Type Description id

int

Workbench ID of coordinate system object.

8.6.11. GetEndTime This method returns the simulation end time.

Declaration Syntax public double GetEndTime();

8.6.12. GetMaterialSolverId This method returns the material identifier given the body identifier the material is applied to.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

325

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

Declaration Syntax public string GetMaterialSolverId(int bodyId); Table 8.11: Properties Property Type Description bodyId

int

Workbench ID of the body to which the material is applied.

8.6.13. GetNamedSelectionLSDYNAId This method returns the LS-DYNA solver named selection identifier given an existing Workbench named selection.

Declaration Syntax public int GetNamedSelectionLSDYNAId(ISelectionInfo namedSelection); Table 8.12: Properties Property

Type

Description

namedSelection ISelectionInfo Workbench ID of named selection of interest.

8.6.14. GetNewContact This method returns a new empty contact keyword.

Declaration Syntax public IKeyWord GetNewContact();

8.6.15. GetNewCurveId This method returns an unused curve identifier.

Declaration Syntax public ulong GetNewCurveId();

8.6.16. GetNewElementId This method returns an unused element identifier.

Declaration Syntax public ulong GetNewElementId();

8.6.17. GetNewElementType This method returns an unused part identifier.

326

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Customizing Workbench LS-DYNA using ACT

Declaration Syntax public uint GetNewElementType();

8.6.18. GetNewNodeId This method returns an unused node identifier.

Declaration Syntax public ulong GetNewNodeId();

8.6.19. GetNewVectorId This method returns an unused vector identifier.

Declaration Syntax public ulong GetNewVectorId();

8.6.20. GetRemotePointNodeId This method returns the master node identifier for a given remote point (tree) identifier.

Declaration Syntax public int GetRemotePointNodeId(int remotePointId); Table 8.13: Properties Property

Type Description

remotePointId int

Workbench ID of remote point of interest.

8.6.21. GetSolverUnitSystem This method returns the solver unit system.

Declaration Syntax public string GetSolverUnitSystem() ;

8.6.22. ContainsDynamicRelaxation This method returns whether dynamic relaxation is used or not in the model.

Declaration Syntax public bool ContainsDynamicRelaxation { get; };

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

327

Using Workbench LS-DYNA for an Explicit Dynamics Analysis

8.6.23. CurrentStep This method returns the current step of the model. For LS-DYNA it is always 1.

Declaration Syntax public uint CurrentStep { get; };

8.6.24. MaxElementId This method returns the maximum element identifier in the model.

Declaration Syntax public ulong MaxElementId { get; } ;

8.6.25. MaxElementType This method returns the maximum part identifier in the model.

Declaration Syntax public uint MaxElementType { get; };

8.6.26. MaxNodeId This method returns the maximum node identifier in the model.

Declaration Syntax public ulong MaxNodeId { get; };

8.7. References The following references are cited in this section: 1. F. Barlat and J. Lian. "Plastic Behavior and Stretchability of Sheet Metals. Part I: A Yield Function for Orthotropic Sheets Under Plane Stress Conditions". Int. Journal of Plasticity, Vol. 5. pg. 51-66. 1989. 2. F. Barlat, D. J. Lege, and J. C. Brem. "A Six-Component Yield Function for Anistropic Materials". Int. Journal of Plasticity, Vol. 7. pg. 693-712. 1991. 3. R. Hill. "A Theory of the Yielding and Plastic Flow of Anisotropic Metals". Proceedings of the Royal Society of London, Series A., Vol. 193. pg. 281–197. 1948.

328

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 9: Using the Drop Test Wizard 9.1. What is the Drop Test Wizard The Drop Test Wizard allows a fully automated setup of a drop test analysis within an Explicit Dynamics analysis. You need only supply a file containing the geometry of the object to be dropped in the analysis. The wizard allows you to change the initial orientation of the geometry, and automatically creates a rigid, fixed target geometry within Mechanical which can also be oriented at an angle. The wizard applies impact velocity and standard earth gravity boundary conditions to the dropped geometry and defines contact behavior between the geometry and the target.

9.2. Loading and Opening the Drop Test Wizard The Drop Test Wizard must be first loaded into Mechanical, then opened using the icon in the Environment Context tab. 1. After starting Workbench, select Extensions Manage Extensions... 2. In the Extensions Manager window, select the check box next to MechanicalDropTest, then click Close. 3. Add an Explicit Dynamics analysis system to the project. 4. Using the Geometry cell, either create a new geometry or import a file containing the geometry of the object to be dropped during the analysis. 5. Once the geometry is specified, launch Mechanical by selecting Edit... from the Model cell of the analysis system in Workbench. 6. Ensure that the geometry is suitable to be used with the Drop Test Wizard (see Preparing the Geometry for Use in the Drop Test Wizard (p. 329)).

7. Select the Explicit Dynamics object in the outline. Launch the wizard by clicking tab.

on the Context

9.3. Preparing the Geometry for Use in the Drop Test Wizard Ensure that your geometry meets the following criteria in order for it to work properly with the Drop Test Wizard. • Before running the Drop Test Wizard, the geometry must be up-to-date. Therefore, all bodies need to have a material assigned and all shell bodies need to have a thickness assigned. • The geometry should not contain construction geometries, as construction geometries will not rotate with the remaining user geometry. Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

329

Using the Drop Test Wizard • Any point or distributed masses, and connections such as joints and springs defined on the user geometry need to be defined on associative coordinate systems (see for more information). Otherwise, these objects will not rotate with the user geometry when any rotations are defined using the Drop Test Wizard or the Rotate Geometry object. • It is important to ensure that the mesh is not in a Read Only state. This means that the Drop Test Wizard is not supported for geometries with imported thicknesses from ACP.

9.4. Setting up the Drop Parameters The Drop Test Wizard works by creating a rigid target geometry within Mechanical at the automatically detected first point of contact, making the target plane a fixed support and adding a Drop Height initial condition to the system. The analysis begins with the contact point of the geometry just touching the target, with an initial velocity determined from the specified drop height. You can choose to change the orientation of both the geometry and the automatically generated target plane. The Drop Test Wizard always creates an analysis simulating a dropped object in the -Y direction. The dropped geometry should therefore be oriented accordingly. The first page of the wizard shows the following input fields: Field

Description

Target Rotation (X) Enter the angle at which to rotate the target plane geometry about the global X axis. Drop Rotation (X)

Enter the angle at which to rotate the dropped geometry about its center of mass.

Drop Rotation (Y)

Enter the angle at which to rotate the dropped geometry about its center of mass.

Drop Rotation (Z)

Enter the angle at which to rotate the dropped geometry about its center of mass.

Define By

Define the impact magnitude by Drop Height or by Impact Velocity.

Drop Height

If you chose to define the drop test by drop height, enter the drop height value.

Impact Velocity

If you chose to define the drop test by impact velocity, enter the velocity value.

The target plane is automatically created if a non-zero angle is input into Target Rotation (X). The rotations are immediately updated on the dropped geometry in the graphical window when you enter the values, which allows you to inspect the setup of the model visually. The rotations are always applied in the order X, Y, Z irrespective of the order of entry into the Drop Rotation input fields. If you entered a drop height value, it is converted into an impact velocity with the relationship as shown below. With the energy balance:

The impact velocity is derived by:

If you choose to define the drop test by impact velocity, the drop height is calculated as follows: 330

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting up the Drop Parameters

Note Air resistance is not taken into account in determining impact velocity, which means the conversion is only valid for drop heights of approximately 5 meters. When going beyond this height, it is recommended that experimental data containing impact velocity be used to define the impact conditions. Once you have set all of these fields to your desired values, click Next to continue. This will display the second page of the wizard and initiate the creation of the objects associated with the fields on the first page of the wizard: • The rotations are stored in a Rotate Geometry object. • The size of the target geometry is calculated as 2.5 times the longest side of the dropped geometry’s bounding box, which gives the geometry room to deform or exhibit sliding behavior. The target is then added to the Geometry using a Construction Geometry object. • The target geometry is positioned such that no separation exists between the geometry to be dropped and the target geometry. Note that if there are shells in the model the target will be offset by the shell thickness to allow you to use shell thickness in contact. • A Drop Height initial condition is added to the analysis, scoped to the dropped geometry with the fields matching those in the wizard. The Drop Height initial condition is fully parameterizable. • The analysis settings Type Analysis Settings Preference Type called ‘Drop Test’ • Sets the analysis end time to a value equal to the time it would take for the geometry to move 10% of its own length in the -Y direction traveling at the impact velocity. If there is more than one step in the analysis, the End Time of the final step is set to this value. On the second page of the wizard, the following fields are available: Field

Description

Frictional Behavior

Specify whether the body interaction will be Frictional or Frictionless in the simulation.

Friction Coefficient

Set a value for μ, the coefficient of friction for the body interaction.

Dynamic Coefficient

Set the value of the dynamic coefficient of friction for the body interaction.

These fields are used to specify a global body interaction defining the contact behavior between the dropped geometry and the target. When you click Finish, the wizard does the following: • Creates the Body Interaction. • Creates the Standard Earth Gravity boundary condition and scopes it to the dropped geometry. • Creates a mesh for all the geometry and performs a check to see if any point on the mesh of the dropped geometry is penetrating the mesh of the target. If this is the case, a new target is created in a corrected Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

331

Using the Drop Test Wizard location and a new mesh is generated. If mesh penetration occurs, a warning message will be displayed in the Messages panel. • Creates a Fixed Support boundary condition and scopes it to the target. • Adds three result objects to the tree: Total Deformation, Equivalent Plastic Strain, and Total Acceleration. Once all of these steps are completed, the wizard will close.

Note You can return from page 2 of the wizard to page 1 using the Back button, and also Exit the wizard entirely from both pages, but note that any actions that the wizard has performed such as geometry rotations and object creation will not be undone.

9.5. Complete the Analysis Once the wizard has run to completion, the analysis is ready to be solved. However, you may wish to refine the default mesh generated and review contact definitions if the model contains multiple parts. You may also want to specify materials for the dropped geometry at this point. The target does not need a material specification as it is rigid and fully constrained. If you modify the Rotate Geometry object after running the wizard and the target will move accordingly. This is only the case with a target created through the drop test wizard; rotations can lead to mesh penetration in a custom geometry.

9.6. The Rotate Geometry Object The Rotate Geometry object created by the wizard is part of the MechanicalDropTest extension. When created by the wizard, it is put under the first Explicit Dynamics branch in the project tree. However, if there are multiple systems in the project tree, the geometry will be subject to the rotations in all of the analysis systems. Note that this means that if you have an analysis system (Explicit or otherwise) which shares the Geometry and Model with an Explicit system, and you run the Drop Test Wizard on the Explicit system, any results in the first analysis system will be cleared. You can make modifications to the orientation of the geometry to be dropped after the wizard has been run by directly modifying the Rotation Angle fields in the Rotate Geometry object. On modifying an angle the following happens: • Dropped geometry is rotated according to the new angles. • Target plane is regenerated to ensure that it is positioned such that no separation exists between the geometry to be dropped and the target plane. As a result of these actions, the mesh will be cleared and must be regenerated. Note that the analysis end time is not updated, and mesh penetrations are not checked once the user remeshes. If you modify the geometry after having run the Drop Test Wizard, only the original geometry will be scoped to the Rotation Object. You will need to manually scope any new geometry to the Rotation Object for it to be rotated by any subsequent runs of the Drop Test Wizard.

332

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Current Limitations

9.7. Current Limitations The following are known limitations of the Drop Test Wizard and the features it uses: • With the exception of the Rotate Geometry object, there is no synchronization of data between objects in the project tree and the Drop Test Wizard when the wizard is open. Therefore, if you modify the Drop Height or the rotation angle in the Collision Point coordinate system, these changes will not be reflected in the wizard unless the wizard is restarted. • The Drop Test Wizard can only be used for a 3D analysis. • You cannot use an implicit system to pre-stress the geometry when using the Drop Test Wizard. • When a geometry is rotated within Mechanical using the Rotate Geometry object, any present mesh information will be cleared and the mesh will have to be generated again. • When a geometry object is added in Mechanical using the Construction Geometry object, the entire mesh present in the analysis system will be cleared and the mesh will have to be generated again. • Mesh penetration is only tested at the end of the wizard execution. It will not be tested if you modify the Rotate Geometry angles or if you regenerate the mesh. • The Drop Test Wizard is not available on Linux. The Drop Height initial condition may be added manually to an analysis on Linux. • If you modify the thickness of any Surface Bodies after the wizard has been run, there is no check to ensure that the change in thickness has resulted in any penetrations of the geometry with the Drop Test Ground Plane. • You are advised not to rename any of the objects created by the Drop Test Wizard as any subsequent runs of the Drop Test Wizard may result in undesired behavior. • If you have multiple Explicit Dynamics systems in one project that share the Model cell, then the Drop Test Wizard can only be used on the first Explicit Dynamics system that appears in the project tree in Mechanical. • The Drop Test Wizard can only be run on projects in Mechanical where the Mesh is editable. This means that the Drop Test Wizard cannot be run on geometries with composite shell layups defined in ACP because for such geometries the Mesh is Read Only. • The Drop Test Wizard should not be run when construction geometries form part of the user geometry. In such cases, the construction geometry parts will not rotate with the remaining user geometry.

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

333

334

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

D

Index Symbols 2–parameter mooney-rivlin model, 174 3–parameter mooney-rivlin model, 174 5–parameter mooney-rivlin model, 175 9–parameter mooney-rivlin model, 175

A analysis settings for explicit dynamics analyses, 45 analysis types explicit dynamics, 3 applying pre-stress effects, 121

B body interaction types, 19 bonded, 20 frictional, 19 frictionless, 19 reinforcement, 24 body interactions folder properties body self contact, 17 contact detection, 11 edge on edge contact, 18 element self contact, 17 formulation, 13 limiting time step velocity, 18 listing, 11 pinball factor, 18 shell thickness, 14 time step safety factor, 18 tolerance, 17 body interactions in explicit dynamics analyses connections, 9 body scoped result tracker, 84 body self contact for body interactions, 17 bonded body interaction type, 20 boundary scoped result tracker, 87 breakable setting for body interaction object, 20 brittle strength, 186

C compaction EOS linear, 210 compaction EOS nonlinear, 211 contact detection for body interactions, 11 contact scoped result tracker, 87 cowper symonds strength, 182 crack softening, 222 crushable foam, 208

decay coefficient for body interaction object, 19 density, 171 detonation point, 72 display options for result tracker graphs, 86 dynamic coefficient for body interaction object, 19

E edge on edge contact for body interactions, 18 element self contact for body interactions, 17 Equation of state, 164 equations of state, 199 ideal gas, 200 eroded nodes, 89 Explicit Dynamics detonation point, 72 impedance boundary, 69 explicit dynamics analysis LSDYNA commands, 229, 252 explicit dynamics analysis settings, 45 explicit dynamics analysis type, 3 Explicit Dynamics system analysis settings, 145 body scoped result tracker, 84 boundary scoped result tracker, 87 elastic waves, 135 erosion controls, 158 Euler (Virtual) solutions, 140 Euler-Lagrange Coupling, 142 Eulerian reference frame, 136 explicit time integration, 132 force reaction result tracker, 87 implicit time integration, 132 Lagrangian reference frame, 136 mass scaling, 134 material properties, 142 moment reaction result tracker, 87 multiple material transport, 142 operation of , 130 plastic waves, 135 point scoped result tracker, 81, 87 shell coupling, 144 shock waves, 135 solver controls, 150 sub-cycling, 144 theory, 129 wave propagation, 134 Explicit Material Library, 165 explicit transient dynamic analysis, 131

F failure, 216

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

335

Index Grady Spall, 225 Johnson cook, 224 plastic strain, 218 post, 217 principal strain, 219 principal stress, 218 stochastic, 220 tensile pressure, 221 filtering result tracker graphs, 86 formulation for body interactions, 13 friction coefficient for body interaction object, 19 frictional body interaction type, 19 frictionless body interaction type, 19

I impedance boundary description, 69 implicit transient dynamic analysis, 131 isotropic elasticity, 171

J Johnson cook strength, 180 Johnson-holmquist strength, 189

L Library Explicit Material, 165 limiting time step velocity for body interactions, 18 Linear Elastic, 171 ls-dyna analyses , 3 LSDYNA commands, 229, 252

M material properties nonlinear, 173 maximum offset for body interaction object , 20 MO granular strength, 198 Model Material failure, 164 Material strength, 164 mooney-rivlin model, 174 2–parameter, 174 3–parameter, 174 5–parameter, 175 9–parameter, 175 multilinear kinematic hardening, 180

ogden, 177 orthotropic elasticity, 172

P p-alpha EOS, 213 pinball factor for body interactions, 18 plasticity, 178 point scoped result tracker, 81 polynomial, 175 polynomial EOS, 201 porous collapse damage, 196 porous materials, 209

R reinforcement body interaction type, 24 result tracker explicit dynamics, 81 resume capability for explicit dynamics, 78 RHT concrete strength, 193 rigid materials, 227

S shear damage, 195 shear stress exponent for body interaction object, 20 shear stress limit for body interaction object, 20 shell thickness for body interactions, 14 shock EOS linear, 203 State Equation of, 164 steinberg guinan strength, 183 strain hardening, 195 strain rate effects, 196 symmetry defining in explicit dynamics, 35

T tensile failure, 197 test data, 173 thermal specific heat, 227 time step safety factor for body interactions, 18 tolerance for body interactions, 17

V Viscoelastic, 172

Y

N neo-hookean, 173 normal stress exponent for body interaction object, 20 normal stress limit for body interaction object, 20

336

O

yeoh, 176

Z zerilli armstrong, 184

Release 2019 R2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.