Ansys 8.1 - Structural Analysis Guide
This document was uploaded by user and they confirmed that they have the permission to share it. If you are author or own the copyright of this book, please report to us by using this DMCA report form. Report DMCA
Overview
Download & View Ansys 8.1 - Structural Analysis Guide as PDF for free.
More details
- Words: 175,159
- Pages: 478
Structural Analysis Guide ANSYS Release 8.1
001972 April 2004
ANSYS, Inc. is a UL registered ISO 9001: 2000 Company
Structural Analysis Guide ANSYS Release 8.1
ANSYS, Inc. Southpointe 275 Technology Drive Canonsburg, PA 15317 [email protected] http://www.ansys.com (T) 724-746-3304 (F) 724-514-9494
Revision History Number 001612 001695* 001788* 001901* 001972*
Release ANSYS 6.1 ANSYS 7.0 ANSYS 7.1 ANSYS 8.0 ANSYS 8.1
Date April 2002 October 2002 May 2003 October 2003 April 2004
* ANSYS Documentation on CD.
Trademark Information ANSYS, DesignSpace, DesignModeler, ANSYS DesignXplorer VT, ANSYS DesignXplorer, ANSYS Emax, ANSYS Workbench environment, CFX, AI*Environment, CADOE and any and all ANSYS, Inc. product names referenced on any media, manual or the like, are registered trademarks or trademarks of subsidiaries of ANSYS, Inc. located in the United States or other countries. Copyright © 2004 SAS IP, Inc. All rights reserved. Unpublished rights reserved under the Copyright Laws of the United States. ANSYS, Inc. is a UL registered ISO 9001: 2000 Company ANSYS Inc. products may contain U.S. Patent No. 6,055,541 Microsoft, Windows, Windows 2000 and Windows XP are registered trademarks of Microsoft Corporation. Inventor and Mechanical Desktop are registered trademarks of Autodesk, Inc. SolidWorks is a registered trademark of SolidWorks Corporation. Pro/ENGINEER is a registered trademark of Parametric Technology Corporation. Unigraphics, Solid Edge and Parasolid are registered trademarks of Electronic Data Systems Corporation (EDS). ACIS and ACIS Geometric Modeler are registered trademarks of Spatial Technology, Inc. "FLEXlm License Manager" is a trademark of Macrovision Corporation. Other product and company names mentioned herein are the trademarks or registered trademarks of their respective owners. This ANSYS, Inc. software product and program documentation is ANSYS Confidential Information and are furnished by ANSYS, Inc. under an ANSYS software license agreement that contains provisions concerning non-disclosure, copying, length and nature of use, warranties, disclaimers and remedies, and other provisions. The Program and Documentation may be used or copied only in accordance with the terms of that license agreement. See the ANSYS, Inc. online documentation or the ANSYS, Inc. documentation CD for the complete Legal Notice. If this is a copy of a document published by and reproduced with the permission of ANSYS, Inc., it might not reflect the organization or physical appearance of the original. ANSYS, Inc. is not liable for any errors or omissions introduced by the copying process. Such errors are the responsibility of the party providing the copy.
Table of Contents 1. Overview of Structural Analyses ......................................................................................................... 1–1 1.1. Definition of Structural Analysis .................................................................................................... 1–1 1.2. Types of Structural Analysis ........................................................................................................... 1–1 1.3. Elements Used in Structural Analyses ............................................................................................ 1–2 1.4. Material Model Interface ............................................................................................................... 1–2 1.5. Types of Solution Methods ............................................................................................................ 1–2 2. Structural Static Analysis .................................................................................................................... 2–1 2.1. Definition of Static Analysis ........................................................................................................... 2–1 2.2. Linear vs. Nonlinear Static Analyses ............................................................................................... 2–1 2.3. Performing a Static Analysis .......................................................................................................... 2–1 2.3.1. Build the Model ................................................................................................................... 2–1 2.3.1.1. Points to Remember .................................................................................................... 2–1 2.3.2. Set Solution Controls ............................................................................................................ 2–2 2.3.2.1. Access the Solution Controls Dialog Box ...................................................................... 2–2 2.3.2.2. Using the Basic Tab ..................................................................................................... 2–2 2.3.2.3. The Transient Tab ........................................................................................................ 2–3 2.3.2.4. Using the Sol'n Options Tab ......................................................................................... 2–4 2.3.2.5. Using the Nonlinear Tab .............................................................................................. 2–4 2.3.2.6. Using the Advanced NL Tab ......................................................................................... 2–5 2.3.3. Set Additional Solution Options ........................................................................................... 2–5 2.3.3.1. Stress Stiffening Effects ................................................................................................ 2–5 2.3.3.2. Newton-Raphson Option ............................................................................................. 2–6 2.3.3.3. Prestress Effects Calculation ......................................................................................... 2–6 2.3.3.4. Mass Matrix Formulation ............................................................................................. 2–6 2.3.3.5. Reference Temperature ............................................................................................... 2–7 2.3.3.6. Mode Number ............................................................................................................. 2–7 2.3.3.7. Creep Criteria .............................................................................................................. 2–7 2.3.3.8. Printed Output ............................................................................................................ 2–7 2.3.3.9. Extrapolation of Results ............................................................................................... 2–7 2.3.4. Apply the Loads ................................................................................................................... 2–7 2.3.4.1. Load Types .................................................................................................................. 2–7 2.3.4.1.1. Displacements (UX, UY, UZ, ROTX, ROTY, ROTZ) ................................................... 2–7 2.3.4.1.2. Forces (FX, FY, FZ) and Moments (MX, MY, MZ) .................................................... 2–7 2.3.4.1.3. Pressures (PRES) .................................................................................................. 2–8 2.3.4.1.4. Temperatures (TEMP) .......................................................................................... 2–8 2.3.4.1.5. Fluences (FLUE) .................................................................................................. 2–8 2.3.4.1.6. Gravity, Spinning, Etc. ......................................................................................... 2–8 2.3.4.2. Apply Loads to the Model ............................................................................................ 2–8 2.3.4.2.1. Applying Loads Using TABLE Type Array Parameters ........................................... 2–8 2.3.4.3. Calculating Inertia Relief .............................................................................................. 2–9 2.3.4.3.1. Inertia Relief Output ............................................................................................ 2–9 2.3.4.3.2. Partial Inertia Relief Calculations .......................................................................... 2–9 2.3.4.3.3. Using a Macro to Perform Inertia Relief Calculations ........................................... 2–10 2.3.5. Solve the Analysis .............................................................................................................. 2–10 2.3.6. Review the Results ............................................................................................................. 2–10 2.3.6.1. Postprocessors .......................................................................................................... 2–11 2.3.6.2. Points to Remember .................................................................................................. 2–11 2.3.6.3. Reviewing Results Data .............................................................................................. 2–11 2.3.6.4. Typical Postprocessing Operations ............................................................................. 2–11 2.4. A Sample Static Analysis (GUI Method) ........................................................................................ 2–13 Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 2.4.1. Problem Description .......................................................................................................... 2–13 2.4.2. Problem Specifications ....................................................................................................... 2–13 2.4.3. Problem Sketch .................................................................................................................. 2–14 2.4.3.1. Set the Analysis Title .................................................................................................. 2–14 2.4.3.2. Set the System of Units .............................................................................................. 2–14 2.4.3.3. Define Parameters ..................................................................................................... 2–14 2.4.3.4. Define the Element Types .......................................................................................... 2–15 2.4.3.5. Define Material Properties ......................................................................................... 2–15 2.4.3.6. Create Hexagonal Area as Cross-Section ..................................................................... 2–15 2.4.3.7. Create Keypoints Along a Path ................................................................................... 2–16 2.4.3.8. Create Lines Along a Path .......................................................................................... 2–16 2.4.3.9. Create Line from Shank to Handle .............................................................................. 2–17 2.4.3.10. Cut Hex Section ....................................................................................................... 2–17 2.4.3.11. Set Meshing Density ................................................................................................ 2–17 2.4.3.12. Set Element Type for Area Mesh ............................................................................... 2–17 2.4.3.13. Generate Area Mesh ................................................................................................ 2–18 2.4.3.14. Drag the 2-D Mesh to Produce 3-D Elements ............................................................ 2–18 2.4.3.15. Select BOTAREA Component and Delete 2-D Elements ............................................. 2–18 2.4.3.16. Apply Displacement Boundary Condition at End of Wrench ...................................... 2–19 2.4.3.17. Display Boundary Conditions ................................................................................... 2–19 2.4.3.18. Apply Pressure on Handle ........................................................................................ 2–19 2.4.3.19. Write the First Load Step .......................................................................................... 2–21 2.4.3.20. Define Downward Pressure ...................................................................................... 2–21 2.4.3.21. Write Second Load Step ........................................................................................... 2–22 2.4.3.22. Solve from Load Step Files ....................................................................................... 2–22 2.4.3.23. Read First Load Step and Review Results .................................................................. 2–22 2.4.3.24. Read the Next Load Step and Review Results ............................................................ 2–23 2.4.3.25. Zoom in on Cross-Section ........................................................................................ 2–23 2.4.3.26. Exit ANSYS ............................................................................................................... 2–23 2.5. A Sample Static Analysis (Command or Batch Method) ................................................................ 2–24 2.6. Where to Find Other Examples .................................................................................................... 2–26 3. Modal Analysis .................................................................................................................................... 3–1 3.1. Definition of Modal Analysis .......................................................................................................... 3–1 3.2. Uses for Modal Analysis ................................................................................................................. 3–1 3.3. Overview of Steps in a Modal Analysis ........................................................................................... 3–1 3.4. Build the Model ............................................................................................................................ 3–1 3.5. Apply Loads and Obtain the Solution ............................................................................................ 3–2 3.5.1. Enter the Solution Processor ................................................................................................. 3–2 3.5.2. Define Analysis Type and Options ......................................................................................... 3–2 3.5.2.1. Option: New Analysis [ANTYPE] .................................................................................... 3–2 3.5.2.2. Option: Analysis Type: Modal [ANTYPE] ........................................................................ 3–3 3.5.2.3. Option: Mode-Extraction Method [MODOPT] ............................................................... 3–3 3.5.2.4. Option: Number of Modes to Extract [MODOPT] ........................................................... 3–4 3.5.2.5. Option: Number of Modes to Expand [MXPAND] .......................................................... 3–4 3.5.2.6. Option: Mass Matrix Formulation [LUMPM] .................................................................. 3–4 3.5.2.7. Option: Prestress Effects Calculation [PSTRES] .............................................................. 3–4 3.5.2.8. Additional Modal Analysis Options .............................................................................. 3–4 3.5.3. Define Master Degrees of Freedom ....................................................................................... 3–4 3.5.4. Apply Loads ......................................................................................................................... 3–5 3.5.4.1. Applying Loads Using Commands ............................................................................... 3–5 3.5.4.2. Applying Loads Using the GUI ..................................................................................... 3–5 3.5.4.3. Listing Loads ............................................................................................................... 3–6
vi
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 3.5.5. Specify Load Step Options .................................................................................................... 3–6 3.5.6. Participation Factor Table Output ......................................................................................... 3–6 3.5.7. Solve ................................................................................................................................... 3–7 3.5.7.1. Output ........................................................................................................................ 3–7 3.5.7.1.1. Output From Subspace Mode-Extraction Method ................................................ 3–7 3.5.8. Exit the Solution Processor ................................................................................................... 3–8 3.6. Expand the Modes ........................................................................................................................ 3–8 3.6.1. Points to Remember ............................................................................................................ 3–8 3.6.2. Expanding the Modes .......................................................................................................... 3–8 3.7. Review the Results ...................................................................................................................... 3–10 3.7.1. Points to Remember ........................................................................................................... 3–10 3.7.2. Reviewing Results Data ...................................................................................................... 3–10 3.7.3. Option: Listing All Frequencies ........................................................................................... 3–10 3.7.4. Option: Display Deformed Shape ........................................................................................ 3–11 3.7.5. Option: List Master DOF ...................................................................................................... 3–11 3.7.6. Option: Line Element Results .............................................................................................. 3–11 3.7.7. Option: Contour Displays ................................................................................................... 3–11 3.7.8. Option: Tabular Listings ...................................................................................................... 3–11 3.7.9. Other Capabilities .............................................................................................................. 3–12 3.8. A Sample Modal Analysis (GUI Method) ....................................................................................... 3–12 3.8.1. Problem Description .......................................................................................................... 3–12 3.8.2. Problem Specifications ....................................................................................................... 3–12 3.8.3. Problem Sketch .................................................................................................................. 3–12 3.9. A Sample Modal Analysis (Command or Batch Method) ............................................................... 3–13 3.10. Where to Find Other Examples .................................................................................................. 3–14 3.11. Prestressed Modal Analysis ....................................................................................................... 3–14 3.12. Prestressed Modal Analysis of a Large-Deflection Solution ......................................................... 3–15 3.13. Comparing Mode-Extraction Methods ....................................................................................... 3–16 3.13.1. Block Lanczos Method ...................................................................................................... 3–17 3.13.2. Subspace Method ............................................................................................................ 3–17 3.13.3. PowerDynamics Method .................................................................................................. 3–17 3.13.4. Reduced Method .............................................................................................................. 3–18 3.13.5. Unsymmetric Method ....................................................................................................... 3–18 3.13.6. Damped Method .............................................................................................................. 3–18 3.13.6.1. Damped Method-Real and Imaginary Parts of the Eigenvalue ................................... 3–18 3.13.6.2. Damped Method-Real and Imaginary Parts of the Eigenvector .................................. 3–18 3.13.7. QR Damped Method ........................................................................................................ 3–19 3.14. Matrix Reduction ...................................................................................................................... 3–19 3.14.1. Theoretical Basis of Matrix Reduction ................................................................................ 3–19 3.14.1.1. Guidelines for Selecting Master DOF ........................................................................ 3–19 3.14.1.2. A Note About Program-Selected Masters .................................................................. 3–21 4. Harmonic Response Analysis .............................................................................................................. 4–1 4.1. Definition of Harmonic Response Analysis ..................................................................................... 4–1 4.2. Uses for Harmonic Response Analysis ............................................................................................ 4–1 4.3. Commands Used in a Harmonic Response Analysis ........................................................................ 4–2 4.4. The Three Solution Methods ......................................................................................................... 4–2 4.4.1. The Full Method ................................................................................................................... 4–2 4.4.2. The Reduced Method ........................................................................................................... 4–2 4.4.3. The Mode Superposition Method ......................................................................................... 4–3 4.4.4. Restrictions Common to All Three Methods .......................................................................... 4–3 4.5. How to Do Harmonic Response Analysis ........................................................................................ 4–3 4.5.1. Full Harmonic Response Analysis .......................................................................................... 4–3
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
vii
Structural Analysis Guide 4.5.2. Build the Model ................................................................................................................... 4–4 4.5.2.1. Points to Remember .................................................................................................... 4–4 4.5.3. Apply Loads and Obtain the Solution ................................................................................... 4–4 4.5.3.1. Enter the ANSYS Solution Processor ............................................................................. 4–4 4.5.3.2. Define the Analysis Type and Options .......................................................................... 4–4 4.5.3.3. Apply Loads on the Model ........................................................................................... 4–5 4.5.3.3.1. Applying Loads Using Commands ....................................................................... 4–8 4.5.3.3.2. Applying Loads and Listing Loads Using the GUI ................................................. 4–9 4.5.3.4. Specify Load Step Options ........................................................................................... 4–9 4.5.3.4.1. General Options .................................................................................................. 4–9 4.5.3.4.2. Dynamics Options ............................................................................................. 4–10 4.5.3.4.3. Output Controls ................................................................................................ 4–10 4.5.3.5. Save a Backup Copy of the Database to a Named File ................................................. 4–11 4.5.3.6. Start Solution Calculations ......................................................................................... 4–11 4.5.3.7. Repeat for Additional Load Steps ............................................................................... 4–11 4.5.3.8. Leave SOLUTION ....................................................................................................... 4–11 4.5.4. Review the Results ............................................................................................................. 4–11 4.5.4.1. Postprocessors .......................................................................................................... 4–11 4.5.4.2. Points to Remember .................................................................................................. 4–11 4.5.4.3. Using POST26 ............................................................................................................ 4–12 4.5.4.4. Using POST1 .............................................................................................................. 4–12 4.6. Sample Harmonic Response Analysis (GUI Method) ..................................................................... 4–13 4.6.1. Problem Description .......................................................................................................... 4–13 4.6.2. Problem Specifications ....................................................................................................... 4–13 4.6.3. Problem Diagram ............................................................................................................... 4–14 4.6.3.1. Set the Analysis Title .................................................................................................. 4–14 4.6.3.2. Define the Element Types .......................................................................................... 4–14 4.6.3.3. Define the Real Constants .......................................................................................... 4–15 4.6.3.4. Create the Nodes ....................................................................................................... 4–15 4.6.3.5. Create the Spring Elements ........................................................................................ 4–15 4.6.3.6. Create the Mass Elements .......................................................................................... 4–16 4.6.3.7. Specify the Analysis Type, MDOF, and Load Step Specifications .................................. 4–16 4.6.3.8. Define Loads and Boundary Conditions ...................................................................... 4–16 4.6.3.9. Solve the Model ........................................................................................................ 4–17 4.6.3.10. Review the Results ................................................................................................... 4–17 4.6.3.11. Exit ANSYS ............................................................................................................... 4–18 4.7. Sample Harmonic Response Analysis (Command or Batch Method) ............................................. 4–18 4.8. Where to Find Other Examples .................................................................................................... 4–19 4.9. Reduced Harmonic Response Analysis ......................................................................................... 4–20 4.9.1. Apply Loads and Obtain the Reduced Solution ................................................................... 4–20 4.9.2. Review the Results of the Reduced Solution ........................................................................ 4–21 4.9.3. Expand the Solution (Expansion Pass) ................................................................................. 4–21 4.9.3.1. Points to Remember .................................................................................................. 4–21 4.9.3.2. Expanding the Modes ................................................................................................ 4–21 4.9.4. Review the Results of the Expanded Solution ...................................................................... 4–23 4.9.5. Sample Input ..................................................................................................................... 4–24 4.10. Mode Superposition Harmonic Response Analysis ..................................................................... 4–25 4.10.1. Obtain the Modal Solution ................................................................................................ 4–25 4.10.2. Obtain the Mode Superposition Harmonic Solution .......................................................... 4–25 4.10.3. Expand the Mode Superposition Solution ......................................................................... 4–27 4.10.4. Review the Results ........................................................................................................... 4–27 4.10.5. Sample Input ................................................................................................................... 4–27
viii
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 4.11. Other Analysis Details ............................................................................................................... 4–28 4.11.1. Prestressed Harmonic Response Analysis .......................................................................... 4–28 4.11.1.1. Prestressed Full Harmonic Response Analysis ........................................................... 4–28 4.11.1.2. Prestressed Reduced Harmonic Response Analysis ................................................... 4–29 4.11.1.3. Prestressed Mode Superposition Harmonic Response Analysis ................................. 4–29 5. Transient Dynamic Analysis ................................................................................................................ 5–1 5.1. Definition of Transient Dynamic Analysis ....................................................................................... 5–1 5.2. Preparing for a Transient Dynamic Analysis ................................................................................... 5–1 5.3. Three Solution Methods ................................................................................................................ 5–2 5.3.1. Full Method ......................................................................................................................... 5–2 5.3.2. Mode Superposition Method ................................................................................................ 5–2 5.3.3. Reduced Method ................................................................................................................. 5–3 5.4. Performing a Full Transient Dynamic Analysis ................................................................................ 5–3 5.4.1. Build the Model ................................................................................................................... 5–4 5.4.1.1. Points to Remember .................................................................................................... 5–4 5.4.2. Establish Initial Conditions ................................................................................................... 5–4 5.4.3. Set Solution Controls ............................................................................................................ 5–6 5.4.3.1. Access the Solution Controls Dialog Box ...................................................................... 5–6 5.4.3.2. Using the Basic Tab ..................................................................................................... 5–7 5.4.3.3. Using the Transient Tab ............................................................................................... 5–7 5.4.3.4. Using the Remaining Solution Controls Tabs ................................................................ 5–8 5.4.4. Set Additional Solution Options ........................................................................................... 5–8 5.4.4.1. Prestress Effects ........................................................................................................... 5–9 5.4.4.2. Damping Option ......................................................................................................... 5–9 5.4.4.3. Mass Matrix Formulation ............................................................................................. 5–9 5.4.5. Apply the Loads ................................................................................................................... 5–9 5.4.6. Save the Load Configuration for the Current Load Step ....................................................... 5–10 5.4.7. Repeat Steps 3-6 for Each Load Step ................................................................................... 5–10 5.4.8. Save a Backup Copy of the Database .................................................................................. 5–10 5.4.9. Start the Transient Solution ................................................................................................ 5–10 5.4.10. Exit the Solution Processor ............................................................................................... 5–11 5.4.11. Review the Results ........................................................................................................... 5–11 5.4.11.1. Postprocessors ........................................................................................................ 5–11 5.4.11.2. Points to Remember ................................................................................................ 5–11 5.4.11.3. Using POST26 .......................................................................................................... 5–11 5.4.11.4. Other Capabilities .................................................................................................... 5–12 5.4.11.5. Using POST1 ............................................................................................................ 5–12 5.4.12. Sample Input for a Full Transient Dynamic Analysis ........................................................... 5–12 5.5. Performing a Mode Superposition Transient Dynamic Analysis .................................................... 5–13 5.5.1. Build the Model .................................................................................................................. 5–13 5.5.2. Obtain the Modal Solution ................................................................................................. 5–13 5.5.3. Obtain the Mode Superposition Transient Solution ............................................................. 5–14 5.5.3.1. Points to Remember .................................................................................................. 5–14 5.5.3.2. Obtaining the Solution .............................................................................................. 5–14 5.5.4. Expand the Mode Superposition Solution ........................................................................... 5–18 5.5.5. Review the Results ............................................................................................................. 5–18 5.5.6. Sample Input for a Mode Superposition Transient Dynamic Analysis ................................... 5–18 5.6. Performing a Reduced Transient Dynamic Analysis ...................................................................... 5–19 5.6.1. Obtain the Reduced Solution .............................................................................................. 5–19 5.6.1.1. Define the Analysis Type and Options ........................................................................ 5–20 5.6.1.2. Define Master Degrees of Freedom ............................................................................ 5–20 5.6.1.3. Define Gap Conditions ............................................................................................... 5–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
ix
Structural Analysis Guide 5.6.1.3.1. Gap Conditions ................................................................................................. 5–20 5.6.1.4. Apply Initial Conditions to the Model ......................................................................... 5–21 5.6.1.4.1. Dynamics Options ............................................................................................. 5–22 5.6.1.4.2. General Options ................................................................................................ 5–22 5.6.1.4.3. Output Control Options .................................................................................... 5–23 5.6.1.5. Write the First Load Step to a Load Step File ............................................................... 5–23 5.6.1.6. Specify Loads and Load Step Options ......................................................................... 5–23 5.6.1.7. Obtaining the Solution .............................................................................................. 5–23 5.6.2. Review the Results of the Reduced Solution ........................................................................ 5–23 5.6.3. Expand the Solution (Expansion Pass) ................................................................................. 5–24 5.6.3.1. Points to Remember .................................................................................................. 5–24 5.6.3.2. Expanding the Solution ............................................................................................. 5–24 5.6.4. Review the Results of the Expanded Solution ...................................................................... 5–25 5.7. Sample Reduced Transient Dynamic Analysis (GUI Method) ......................................................... 5–26 5.7.1. Problem Description .......................................................................................................... 5–26 5.7.2. Problem Specifications ....................................................................................................... 5–26 5.7.3. Problem Sketch .................................................................................................................. 5–27 5.7.3.1. Specify the Title ......................................................................................................... 5–27 5.7.3.2. Define Element Types ................................................................................................ 5–27 5.7.3.3. Define Real Constants ................................................................................................ 5–27 5.7.3.4. Define Material Properties ......................................................................................... 5–28 5.7.3.5. Define Nodes ............................................................................................................ 5–28 5.7.3.6. Define Elements ........................................................................................................ 5–28 5.7.3.7. Define Analysis Type and Analysis Options ................................................................. 5–29 5.7.3.8. Define Master Degrees of Freedom ............................................................................ 5–29 5.7.3.9. Set Load Step Options ............................................................................................... 5–29 5.7.3.10. Apply Loads for the First Load Step .......................................................................... 5–29 5.7.3.11. Specify Output ........................................................................................................ 5–29 5.7.3.12. Solve the First Load Step .......................................................................................... 5–30 5.7.3.13. Apply Loads for the Next Load Step .......................................................................... 5–30 5.7.4. Solve the Next Load Step .................................................................................................... 5–30 5.7.4.1. Set the Next Time Step and Solve ............................................................................... 5–30 5.7.4.2. Run the Expansion Pass and Solve .............................................................................. 5–30 5.7.4.3. Review the Results in POST26 .................................................................................... 5–31 5.7.4.4. Review the Results in POST1 ...................................................................................... 5–31 5.7.4.5. Exit ANSYS ................................................................................................................. 5–31 5.8. Sample Reduced Transient Dynamic Analysis (Command or Batch Method) ................................. 5–31 5.9. Performing a Prestressed Transient Dynamic Analysis .................................................................. 5–32 5.9.1. Prestressed Full Transient Dynamic Analysis ........................................................................ 5–32 5.9.2. Prestressed Mode Superposition Transient Dynamic Analysis .............................................. 5–33 5.9.3. Prestressed Reduced Transient Dynamic Analysis ................................................................ 5–33 5.10. Other Analysis Details ............................................................................................................... 5–33 5.10.1. Guidelines for Integration Time Step ................................................................................. 5–33 5.10.2. Automatic Time Stepping ................................................................................................. 5–35 5.10.3. Damping .......................................................................................................................... 5–36 5.11. Where to Find Other Examples .................................................................................................. 5–40 6. Spectrum Analysis ............................................................................................................................... 6–1 6.1. Definition of Spectrum Analysis .................................................................................................... 6–1 6.2. What is a Spectrum? ..................................................................................................................... 6–1 6.2.1. Response Spectrum ............................................................................................................. 6–1 6.2.1.1. Single-Point Response Spectrum (SPRS) ....................................................................... 6–1 6.2.1.2. Multi-Point Response Spectrum (MPRS) ....................................................................... 6–1
x
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 6.2.2. Dynamic Design Analysis Method (DDAM) ............................................................................ 6–2 6.2.3. Power Spectral Density ........................................................................................................ 6–2 6.2.4. Deterministic vs. Probabilistic Analyses ................................................................................. 6–2 6.3. Steps in a Single-Point Response Spectrum (SPRS) Analysis ............................................................ 6–2 6.3.1. Build the Model ................................................................................................................... 6–3 6.3.1.1. Points to Remember .................................................................................................... 6–3 6.3.2. Obtain the Modal Solution ................................................................................................... 6–3 6.3.3. Obtain the Spectrum Solution .............................................................................................. 6–3 6.3.4. Expand the Modes ............................................................................................................... 6–6 6.3.5. Combine the Modes ............................................................................................................. 6–6 6.3.6. Review the Results ............................................................................................................... 6–8 6.4. Sample Spectrum Analysis (GUI Method) ..................................................................................... 6–10 6.4.1. Problem Description .......................................................................................................... 6–10 6.4.2. Problem Specifications ....................................................................................................... 6–10 6.4.3. Problem Sketch .................................................................................................................. 6–11 6.4.4. Procedure .......................................................................................................................... 6–11 6.4.4.1. Set the Analysis Title .................................................................................................. 6–11 6.4.4.2. Define the Element Type ............................................................................................ 6–11 6.4.4.3. Define the Real Constants .......................................................................................... 6–11 6.4.4.4. Define Material Properties ......................................................................................... 6–12 6.4.4.5. Define Keypoints and Line ......................................................................................... 6–12 6.4.4.6. Set Global Element Density and Mesh Line ................................................................. 6–12 6.4.4.7. Set Boundary Conditions ........................................................................................... 6–13 6.4.4.8. Specify Analysis Type and Options ............................................................................. 6–13 6.4.4.9. Solve the Modal Analysis ........................................................................................... 6–13 6.4.4.10. Set Up the Spectrum Analysis .................................................................................. 6–13 6.4.4.11. Define Spectrum Value vs. Frequency Table ............................................................. 6–14 6.4.4.12. Solve Spectrum Analysis .......................................................................................... 6–14 6.4.4.13. Set up the Expansion Pass ........................................................................................ 6–14 6.4.4.14. Expand the Modes ................................................................................................... 6–14 6.4.4.15. Start Expansion Pass Calculation .............................................................................. 6–15 6.4.4.16. Set Up Mode Combination for Spectrum Analysis ..................................................... 6–15 6.4.4.17. Select Mode Combination Method ........................................................................... 6–15 6.4.4.18. Combine the Modes ................................................................................................ 6–15 6.4.4.19. Postprocessing: Print Out Nodal, Element, and Reaction Solutions ............................ 6–15 6.4.4.20. Exit ANSYS ............................................................................................................... 6–16 6.5. Sample Spectrum Analysis (Command or Batch Method) ............................................................. 6–16 6.6. Where to Find Other Examples .................................................................................................... 6–17 6.7. How to Do a Random Vibration (PSD) Analysis ............................................................................. 6–18 6.7.1. Expand the Modes ............................................................................................................. 6–18 6.7.2. Obtain the Spectrum Solution ............................................................................................ 6–18 6.7.3. Combine the Modes ........................................................................................................... 6–21 6.7.4. Review the Results ............................................................................................................. 6–22 6.7.4.1. Reviewing the Results in POST1 ................................................................................. 6–22 6.7.4.1.1. Read the Desired Set of Results into the Database .............................................. 6–22 6.7.4.1.2. Display the Results ............................................................................................ 6–23 6.7.4.2. Calculating Response PSDs in POST26 ........................................................................ 6–23 6.7.4.3. Calculating Covariance in POST26 .............................................................................. 6–23 6.7.5. Sample Input ..................................................................................................................... 6–24 6.8. How to Do DDAM Spectrum Analysis .......................................................................................... 6–25 6.9. How to Do Multi-Point Response Spectrum (MPRS) Analysis ........................................................ 6–25 7. Buckling Analysis ................................................................................................................................ 7–1
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xi
Structural Analysis Guide 7.1. Definition of Buckling Analysis ...................................................................................................... 7–1 7.2. Types of Buckling Analyses ........................................................................................................... 7–1 7.2.1. Nonlinear Buckling Analysis .................................................................................................. 7–1 7.2.2. Eigenvalue Buckling Analysis ................................................................................................ 7–1 7.3. Commands Used in a Buckling Analysis ......................................................................................... 7–2 7.4. Procedure for Nonlinear Buckling Analysis ..................................................................................... 7–2 7.4.1. Applying Load Increments ................................................................................................... 7–2 7.4.2. Automatic Time Stepping ..................................................................................................... 7–2 7.4.3. Important ............................................................................................................................ 7–2 7.4.4. Points to Remember ............................................................................................................ 7–3 7.5. Procedure for Eigenvalue Buckling Analysis ................................................................................... 7–3 7.5.1. Build the Model ................................................................................................................... 7–3 7.5.1.1. Points to Remember .................................................................................................... 7–4 7.5.2. Obtain the Static Solution .................................................................................................... 7–4 7.5.3. Obtain the Eigenvalue Buckling Solution .............................................................................. 7–5 7.5.4. Expand the Solution ............................................................................................................. 7–6 7.5.4.1. Points to Remember .................................................................................................... 7–6 7.5.4.2. Expanding the Solution ............................................................................................... 7–6 7.5.5. Review the Results ............................................................................................................... 7–7 7.6. Sample Buckling Analysis (GUI Method) ........................................................................................ 7–8 7.6.1. Problem Description ............................................................................................................ 7–8 7.6.2. Problem Specifications ......................................................................................................... 7–8 7.6.3. Problem Sketch .................................................................................................................... 7–9 7.6.3.1. Set the Analysis Title .................................................................................................... 7–9 7.6.3.2. Define the Element Type ............................................................................................. 7–9 7.6.3.3. Define the Real Constants and Material Properties ...................................................... 7–10 7.6.3.4. Define Nodes and Elements ....................................................................................... 7–10 7.6.3.5. Define the Boundary Conditions ................................................................................ 7–11 7.6.3.6. Solve the Static Analysis ............................................................................................. 7–11 7.6.3.7. Solve the Buckling Analysis ........................................................................................ 7–11 7.6.3.8. Review the Results ..................................................................................................... 7–12 7.6.3.9. Exit ANSYS ................................................................................................................. 7–12 7.7. Sample Buckling Analysis (Command or Batch Method) ............................................................... 7–12 7.8. Where to Find Other Examples .................................................................................................... 7–12 8. Nonlinear Structural Analysis ............................................................................................................. 8–1 8.1. What is Structural Nonlinearity? .................................................................................................... 8–1 8.1.1. Causes of Nonlinear Behavior ............................................................................................... 8–1 8.1.1.1. Changing Status (Including Contact) ............................................................................ 8–2 8.1.1.2. Geometric Nonlinearities ............................................................................................. 8–2 8.1.1.3. Material Nonlinearities ................................................................................................. 8–2 8.1.2. Basic Information About Nonlinear Analyses ......................................................................... 8–2 8.1.2.1. Conservative versus Nonconservative Behavior; Path Dependency ............................... 8–5 8.1.2.2. Substeps ..................................................................................................................... 8–5 8.1.2.3. Load Direction in a Large-Deflection Analysis ............................................................... 8–6 8.1.2.4. Nonlinear Transient Analyses ....................................................................................... 8–6 8.2. Using Geometric Nonlinearities ..................................................................................................... 8–6 8.2.1. Stress-Strain ......................................................................................................................... 8–7 8.2.1.1. Large Deflections with Small Strain .............................................................................. 8–7 8.2.2. Stress Stiffening ................................................................................................................... 8–7 8.2.3. Spin Softening ..................................................................................................................... 8–8 8.3. Modeling Material Nonlinearities .................................................................................................. 8–8 8.3.1. Nonlinear Materials .............................................................................................................. 8–8
xii
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 8.3.1.1. Plasticity ..................................................................................................................... 8–9 8.3.1.1.1. Plastic Material Options ..................................................................................... 8–10 8.3.1.2. Multilinear Elasticity ................................................................................................... 8–16 8.3.1.3. User Defined Material ................................................................................................ 8–16 8.3.1.4. Hyperelasticity .......................................................................................................... 8–17 8.3.1.4.1. Mooney-Rivlin Hyperelastic Option (TB,HYPER) .................................................. 8–18 8.3.1.4.2. Ogden Hyperelastic Option ............................................................................... 8–18 8.3.1.4.3. Neo-Hookean Hyperelastic Option .................................................................... 8–19 8.3.1.4.4. Polynomial Form Hyperelastic Option ............................................................... 8–19 8.3.1.4.5. Arruda-Boyce Hyperelastic Option ..................................................................... 8–19 8.3.1.4.6. Gent Hyperelastic Option .................................................................................. 8–20 8.3.1.4.7. Yeoh Hyperelastic Option ................................................................................. 8–20 8.3.1.4.8. Blatz-Ko Foam Hyperelastic Option ................................................................... 8–20 8.3.1.4.9. Ogden Compressible Foam Hyperelastic Option ................................................ 8–20 8.3.1.4.10. User-Defined Hyperelastic Option ................................................................... 8–21 8.3.1.4.11. Mooney-Rivlin Hyperelastic Option (TB,MOONEY) ............................................ 8–21 8.3.1.5. Creep ........................................................................................................................ 8–29 8.3.1.5.1. Implicit Creep Procedure ................................................................................... 8–30 8.3.1.5.2. Explicit Creep Procedure ................................................................................... 8–31 8.3.1.6. Shape Memory Alloy .................................................................................................. 8–31 8.3.1.7. Viscoplasticity ........................................................................................................... 8–32 8.3.1.8. Viscoelasticity ............................................................................................................ 8–33 8.3.1.9. Swelling .................................................................................................................... 8–34 8.3.2. Material Model Combinations ............................................................................................. 8–35 8.3.2.1. BISO and CHAB Example ............................................................................................ 8–35 8.3.2.2. MISO and CHAB Example ........................................................................................... 8–35 8.3.2.3. NLISO and CHAB Example .......................................................................................... 8–35 8.3.2.4. BISO and RATE Example ............................................................................................. 8–36 8.3.2.5. MISO and RATE Example ............................................................................................ 8–36 8.3.2.6. NLISO and RATE Example ........................................................................................... 8–37 8.3.2.7. BISO and CREEP Example ........................................................................................... 8–37 8.3.2.8. MISO and CREEP Example .......................................................................................... 8–37 8.3.2.9. NLISO and CREEP Example ......................................................................................... 8–38 8.3.2.10. BKIN and CREEP Example ......................................................................................... 8–38 8.3.2.11. HILL and BISO Example ............................................................................................ 8–38 8.3.2.12. HILL and MISO Example ........................................................................................... 8–39 8.3.2.13. HILL and NLISO Example .......................................................................................... 8–39 8.3.2.14. HILL and BKIN Example ............................................................................................ 8–39 8.3.2.15. HILL and MKIN Example ........................................................................................... 8–40 8.3.2.16. HILL and KINH Example ............................................................................................ 8–40 8.3.2.17. HILL and CHAB Example .......................................................................................... 8–41 8.3.2.18. HILL and BISO and CHAB Example ............................................................................ 8–41 8.3.2.19. HILL and MISO and CHAB Example ........................................................................... 8–41 8.3.2.20. HILL and NLISO and CHAB Example .......................................................................... 8–42 8.3.2.21. HILL and RATE and BISO Example ............................................................................. 8–43 8.3.2.22. HILL and RATE and MISO Example ............................................................................ 8–44 8.3.2.23. HILL and RATE and NLISO Example ........................................................................... 8–44 8.3.2.24. HILL and CREEP Example .......................................................................................... 8–45 8.3.2.25. HILL and CREEP and BISO Example ........................................................................... 8–46 8.3.2.26. HILL and CREEP and MISO Example .......................................................................... 8–47 8.3.2.27. HILL and CREEP and NLISO Example ......................................................................... 8–47 8.3.2.28. HILL and CREEP and BKIN Example ........................................................................... 8–47
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xiii
Structural Analysis Guide 8.4. Running a Nonlinear Analysis in ANSYS ....................................................................................... 8–48 8.5. Performing a Nonlinear Static Analysis ........................................................................................ 8–48 8.5.1. Build the Model .................................................................................................................. 8–49 8.5.2. Set Solution Controls .......................................................................................................... 8–49 8.5.2.1. Using the Basic Tab: Special Considerations ............................................................... 8–49 8.5.2.2. Advanced Analysis Options You Can Set on the Solution Controls Dialog Box ............. 8–50 8.5.2.2.1. Equation Solver ................................................................................................ 8–50 8.5.2.3. Advanced Load Step Options You Can Set on the Solution Controls Dialog Box .......... 8–51 8.5.2.3.1. Automatic Time Stepping ................................................................................. 8–51 8.5.2.3.2. Convergence Criteria ........................................................................................ 8–51 8.5.2.3.3. Maximum Number of Equilibrium Iterations ...................................................... 8–52 8.5.2.3.4. Predictor-Corrector Option ............................................................................... 8–52 8.5.2.3.5. Line Search Option ........................................................................................... 8–53 8.5.2.3.6. Cutback Criteria ................................................................................................ 8–53 8.5.3. Set Additional Solution Options .......................................................................................... 8–53 8.5.3.1. Advanced Analysis Options You Cannot Set on the Solution Controls Dialog Box ........ 8–53 8.5.3.1.1. Stress Stiffness .................................................................................................. 8–53 8.5.3.1.2. Newton-Raphson Option .................................................................................. 8–54 8.5.3.2. Advanced Load Step Options You Cannot Set on the Solution Controls Dialog Box ..... 8–55 8.5.3.2.1. Creep Criteria .................................................................................................... 8–55 8.5.3.2.2. Time Step Open Control .................................................................................... 8–55 8.5.3.2.3. Solution Monitoring .......................................................................................... 8–55 8.5.3.2.4. Birth and Death ................................................................................................ 8–56 8.5.3.2.5. Output Control ................................................................................................. 8–56 8.5.4. Apply the Loads ................................................................................................................. 8–56 8.5.5. Solve the Analysis .............................................................................................................. 8–57 8.5.6. Review the Results ............................................................................................................. 8–57 8.5.6.1. Points to Remember .................................................................................................. 8–57 8.5.6.2. Reviewing Results in POST1 ....................................................................................... 8–57 8.5.6.3. Reviewing Results in POST26 ..................................................................................... 8–59 8.5.7. Terminating a Running Job; Restarting ............................................................................... 8–59 8.6. Performing a Nonlinear Transient Analysis ................................................................................... 8–59 8.6.1. Build the Model .................................................................................................................. 8–60 8.6.2. Apply Loads and Obtain the Solution .................................................................................. 8–60 8.6.3. Review the Results ............................................................................................................. 8–61 8.7. Sample Input for a Nonlinear Transient Analysis .......................................................................... 8–61 8.8. Restarts ...................................................................................................................................... 8–62 8.9. Using Nonlinear (Changing-Status) Elements ............................................................................... 8–63 8.9.1. Element Birth and Death .................................................................................................... 8–63 8.10. Tips and Guidelines for Nonlinear Analysis ................................................................................. 8–63 8.10.1. Starting Out with Nonlinear Analysis ................................................................................. 8–63 8.10.1.1. Be Aware of How the Program and Your Structure Behave ........................................ 8–63 8.10.1.2. Keep It Simple ......................................................................................................... 8–64 8.10.1.3. Use an Adequate Mesh Density ................................................................................ 8–64 8.10.1.4. Apply the Load Gradually ......................................................................................... 8–64 8.10.2. Overcoming Convergence Problems ................................................................................. 8–64 8.10.2.1. Performing Nonlinear Diagnostics ............................................................................ 8–65 8.10.2.2. Tracking Convergence Graphically ........................................................................... 8–66 8.10.2.3. Using Automatic Time Stepping ............................................................................... 8–67 8.10.2.4. Using Line Search .................................................................................................... 8–68 8.10.2.5. Using the Arc-Length Method .................................................................................. 8–68 8.10.2.6. Artificially Inhibit Divergence in Your Model's Response ........................................... 8–69
xiv
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 8.10.2.7. Turn Off Extra Element Shapes ................................................................................. 8–70 8.10.2.8. Using Birth and Death Wisely ................................................................................... 8–70 8.10.2.9. Read Your Output .................................................................................................... 8–70 8.10.2.10. Graph the Load and Response History .................................................................... 8–71 8.11. Sample Nonlinear Analysis (GUI Method) ................................................................................... 8–71 8.11.1. Problem Description ........................................................................................................ 8–72 8.11.2. Problem Specifications ..................................................................................................... 8–72 8.11.3. Problem Sketch ................................................................................................................ 8–73 8.11.3.1. Set the Analysis Title and Jobname .......................................................................... 8–73 8.11.3.2. Define the Element Types ........................................................................................ 8–73 8.11.3.3. Define Material Properties ........................................................................................ 8–74 8.11.3.4. Specify the Kinematic Hardening material model (KINH) ........................................... 8–74 8.11.3.5. Label Graph Axes and Plot Data Tables ..................................................................... 8–74 8.11.3.6. Create Rectangle ..................................................................................................... 8–74 8.11.3.7. Set Element Size ...................................................................................................... 8–75 8.11.3.8. Mesh the Rectangle ................................................................................................. 8–75 8.11.3.9. Assign Analysis and Load Step Options .................................................................... 8–75 8.11.3.10. Monitor the Displacement ..................................................................................... 8–75 8.11.3.11. Apply Constraints .................................................................................................. 8–76 8.11.3.12. Solve the First Load Step ........................................................................................ 8–76 8.11.3.13. Solve the Next Six Load Steps ................................................................................. 8–77 8.11.3.14. Review the Monitor File ......................................................................................... 8–77 8.11.3.15. Use the General Postprocessor to Plot Results. ........................................................ 8–77 8.11.3.16. Define Variables for Time-History Postprocessing ................................................... 8–78 8.11.3.17. Plot Time-History Results ....................................................................................... 8–78 8.11.3.18. Exit ANSYS ............................................................................................................. 8–79 8.12. Sample Nonlinear Analysis (Command or Batch Method) ........................................................... 8–79 8.13. Where to Find Other Examples .................................................................................................. 8–82 9. Material Curve Fitting ......................................................................................................................... 9–1 9.1. Applicable Material Behavior Types ............................................................................................... 9–1 9.2. Hyperelastic Material Curve Fitting ................................................................................................ 9–1 9.2.1. Using Curve Fitting to Determine Your Hyperelastic Material Behavior ................................. 9–1 9.2.1.1. Prepare Experimental Data .......................................................................................... 9–2 9.2.1.2. Input the Data into ANSYS ........................................................................................... 9–3 9.2.1.2.1. Batch .................................................................................................................. 9–3 9.2.1.2.2. GUI ..................................................................................................................... 9–3 9.2.1.3. Select a Material Model Option .................................................................................... 9–3 9.2.1.3.1. Batch .................................................................................................................. 9–4 9.2.1.3.2. GUI ..................................................................................................................... 9–4 9.2.1.4. Initialize the Coefficients .............................................................................................. 9–4 9.2.1.4.1. Batch .................................................................................................................. 9–4 9.2.1.4.2. GUI ..................................................................................................................... 9–5 9.2.1.5. Specify Control Parameters and Solve .......................................................................... 9–5 9.2.1.5.1. Batch .................................................................................................................. 9–5 9.2.1.5.2. GUI ..................................................................................................................... 9–5 9.2.1.6. Plot Your Experimental Data and Analyze ..................................................................... 9–6 9.2.1.6.1. Batch .................................................................................................................. 9–6 9.2.1.6.2. GUI ..................................................................................................................... 9–6 9.2.1.6.3. Review/Verify ..................................................................................................... 9–6 9.2.1.7. Write Data to TB Command ......................................................................................... 9–6 9.2.1.7.1. Batch .................................................................................................................. 9–6 9.2.1.7.2. GUI ..................................................................................................................... 9–7
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xv
Structural Analysis Guide 9.3. Creep Material Curve Fitting ......................................................................................................... 9–7 9.3.1. Using Curve Fitting to Determine Your Creep Material Behavior ........................................... 9–7 9.3.1.1. Prepare Experimental Data .......................................................................................... 9–7 9.3.1.2. Input the Data into ANSYS ........................................................................................... 9–9 9.3.1.2.1. Batch .................................................................................................................. 9–9 9.3.1.2.2. GUI ..................................................................................................................... 9–9 9.3.1.3. Select a Material Model Option .................................................................................... 9–9 9.3.1.3.1. Batch .................................................................................................................. 9–9 9.3.1.3.2. GUI ................................................................................................................... 9–10 9.3.1.4. Initialize the Coefficients ............................................................................................ 9–10 9.3.1.4.1. Batch ................................................................................................................ 9–10 9.3.1.4.2. GUI ................................................................................................................... 9–11 9.3.1.5. Specify Control Parameters and Solve ........................................................................ 9–11 9.3.1.5.1. Batch ................................................................................................................ 9–11 9.3.1.5.2. GUI ................................................................................................................... 9–11 9.3.1.6. Plot the Experimental Data and Analyze ..................................................................... 9–11 9.3.1.6.1. Batch ................................................................................................................ 9–12 9.3.1.6.2. GUI ................................................................................................................... 9–12 9.3.1.6.3. Analyze Your Curves for Proper Fit ..................................................................... 9–12 9.3.1.7. Write Data to TB Command ....................................................................................... 9–12 9.3.1.7.1. Batch ................................................................................................................ 9–12 9.3.1.7.2. GUI ................................................................................................................... 9–12 9.3.2. Tips For Curve Fitting Creep Models ................................................................................... 9–12 9.4. Viscoelastic Material Curve Fitting ............................................................................................... 9–14 9.4.1. Using Curve Fitting to Determine the Coefficients of Viscoelastic Material Model ................. 9–14 9.4.1.1. Prepare Experimental Data ........................................................................................ 9–15 9.4.1.2. Input the Data into ANSYS ......................................................................................... 9–16 9.4.1.2.1. Batch ................................................................................................................ 9–16 9.4.1.2.2. GUI ................................................................................................................... 9–16 9.4.1.3. Select a Material Model Option .................................................................................. 9–16 9.4.1.3.1. Batch ................................................................................................................ 9–17 9.4.1.3.2. GUI ................................................................................................................... 9–17 9.4.1.4. Initialize the Coefficients ............................................................................................ 9–17 9.4.1.4.1. Batch ................................................................................................................ 9–18 9.4.1.4.2. GUI ................................................................................................................... 9–18 9.4.1.5. Specify Control Parameters and Solve ........................................................................ 9–18 9.4.1.5.1. Batch ................................................................................................................ 9–19 9.4.1.5.2. GUI ................................................................................................................... 9–20 9.4.1.6. Plot the Experimental Data and Analyze ..................................................................... 9–20 9.4.1.6.1. Batch ................................................................................................................ 9–20 9.4.1.6.2. GUI ................................................................................................................... 9–20 9.4.1.6.3. Analyze Your Curves for Proper Fit ..................................................................... 9–20 9.4.1.7. Write Data to TB Command ....................................................................................... 9–20 9.4.1.7.1. Batch ................................................................................................................ 9–20 9.4.1.7.2. GUI ................................................................................................................... 9–21 10. Gasket Joints Simulation ................................................................................................................. 10–1 10.1. Overview of Gasket Joints ......................................................................................................... 10–1 10.2. Performing a Gasket Joint Analysis ............................................................................................ 10–1 10.3. Finite Element Formulation ....................................................................................................... 10–2 10.3.1. Element Topologies ......................................................................................................... 10–2 10.3.2. Thickness Direction .......................................................................................................... 10–2 10.4. ANSYS Family of Interface Elements .......................................................................................... 10–3
xvi
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 10.4.1. Element Selection ............................................................................................................ 10–3 10.4.2. Applications ..................................................................................................................... 10–3 10.5. Material Definition .................................................................................................................... 10–4 10.5.1. Material Characteristics .................................................................................................... 10–4 10.5.2. Input Format .................................................................................................................... 10–5 10.5.2.1. Define General Parameters ...................................................................................... 10–6 10.5.2.2. Define Compression Load Closure Curve .................................................................. 10–6 10.5.2.3. Define Linear Unloading Data .................................................................................. 10–6 10.5.2.4. Define Nonlinear Unloading Data ............................................................................. 10–7 10.5.3. Temperature Dependencies ............................................................................................. 10–8 10.5.4. Plotting Gasket Data ....................................................................................................... 10–11 10.6. Meshing Interface Elements .................................................................................................... 10–12 10.7. Solution Procedure and Result Output ..................................................................................... 10–16 10.7.1. Typical Gasket Solution Output Listing ............................................................................ 10–17 10.8. Reviewing the Results ............................................................................................................. 10–19 10.8.1. Points to Remember ....................................................................................................... 10–19 10.8.2. Reviewing Results in POST1 ............................................................................................ 10–19 10.8.3. Reviewing Results in POST26 .......................................................................................... 10–20 10.9. Sample Gasket Element Verification Analysis (Command or Batch Method) .............................. 10–20 11. Contact ............................................................................................................................................ 11–1 11.1. Contact Overview ..................................................................................................................... 11–1 11.1.1. Explicit Dynamics Contact Capabilities .............................................................................. 11–1 11.2. General Contact Classification ................................................................................................... 11–1 11.3. ANSYS Contact Capabilities ....................................................................................................... 11–2 11.3.1. Surface-to-Surface Contact Elements ................................................................................ 11–3 11.3.2. Node-to-Surface Contact Elements ................................................................................... 11–3 11.3.3. Node-to-Node Contact Elements ...................................................................................... 11–4 11.4. Performing a Surface-to-Surface Contact Analysis ...................................................................... 11–4 11.4.1. Using Surface-to-Surface Contact Elements ....................................................................... 11–4 11.4.2. Steps in a Contact Analysis ............................................................................................... 11–5 11.4.3. Creating the Model Geometry and Mesh ........................................................................... 11–5 11.4.4. Identifying Contact Pairs .................................................................................................. 11–5 11.4.5. Designating Contact and Target Surfaces .......................................................................... 11–6 11.4.5.1. Asymmetric Contact vs. Symmetric Contact ............................................................. 11–7 11.4.5.1.1. Background .................................................................................................... 11–7 11.4.5.1.2. Using KEYOPT(8) ............................................................................................. 11–7 11.4.6. Defining the Target Surface .............................................................................................. 11–7 11.4.6.1. Pilot Nodes .............................................................................................................. 11–8 11.4.6.2. Primitives ................................................................................................................ 11–8 11.4.6.3. Element Types and Real Constants ........................................................................... 11–8 11.4.6.3.1. Defining Target Element Geometry ................................................................. 11–8 11.4.6.4. Using Direct Generation to Create Rigid Target Elements .......................................... 11–9 11.4.6.5. Using ANSYS Meshing Tools to Create Rigid Target Elements .................................. 11–10 11.4.6.5.1. Some Modeling and Meshing Tips ................................................................. 11–12 11.4.6.5.2. Verifying Nodal Number Ordering (Contact Direction) of Target Surface ......... 11–13 11.4.7. Defining the Deformable Contact Surface ....................................................................... 11–14 11.4.7.1. Element Type ........................................................................................................ 11–14 11.4.7.2. Real Constants and Material Properties ................................................................... 11–15 11.4.7.3. Generating Contact Elements ................................................................................. 11–16 11.4.8. Set the Real Constants and Element KEYOPTS ................................................................. 11–17 11.4.8.1. Real Constants ....................................................................................................... 11–17 11.4.8.1.1. Positive and Negative Real Constant Values ................................................... 11–19
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xvii
Structural Analysis Guide 11.4.8.2. Element KEYOPTS .................................................................................................. 11–20 11.4.8.3. Selecting a Contact Algorithm (KEYOPT(2)) ............................................................. 11–21 11.4.8.3.1. Background .................................................................................................. 11–21 11.4.8.4. Determining Contact Stiffness and Allowable Penetration ...................................... 11–22 11.4.8.4.1. Background .................................................................................................. 11–22 11.4.8.4.2. Using FKN and FTOLN ................................................................................... 11–23 11.4.8.4.3. Using FKT and SLTO ...................................................................................... 11–23 11.4.8.4.4. Using KEYOPT(10) ......................................................................................... 11–24 11.4.8.4.5. Chattering Control Parameters ...................................................................... 11–25 11.4.8.5. Choosing a Friction Model ..................................................................................... 11–25 11.4.8.5.1. Background .................................................................................................. 11–25 11.4.8.5.2. Using TAUMAX, FACT, DC, and COHE ............................................................. 11–26 11.4.8.5.3. Static and Dynamic Friction Coefficients ........................................................ 11–26 11.4.8.6. Selecting Location of Contact Detection ................................................................. 11–28 11.4.8.6.1. Background .................................................................................................. 11–28 11.4.8.6.2. Using KEYOPT(4) and TOLS ............................................................................ 11–28 11.4.8.7. Adjusting Initial Contact Conditions ....................................................................... 11–30 11.4.8.7.1. Background .................................................................................................. 11–30 11.4.8.7.2. Using PMIN, PMAX, CNOF, ICONT, KEYOPT(5), and KEYOPT(9) ......................... 11–30 11.4.8.8. Physically Moving Contact Nodes Towards the Target Surface ................................ 11–37 11.4.8.9. Determining Contact Status and the Pinball Region ................................................ 11–38 11.4.8.9.1. Background .................................................................................................. 11–38 11.4.8.9.2. Using PINB .................................................................................................... 11–39 11.4.8.10. Avoiding Spurious Contact in Self Contact Problems ............................................. 11–39 11.4.8.11. Selecting Surface Interaction Models .................................................................... 11–40 11.4.8.11.1. Background ................................................................................................ 11–40 11.4.8.11.2. Using KEYOPT(12) and FKOP ........................................................................ 11–40 11.4.8.12. Modeling Contact with Superelements ................................................................. 11–41 11.4.8.12.1. Background ................................................................................................ 11–41 11.4.8.12.2. Using KEYOPT(3) ......................................................................................... 11–41 11.4.8.13. Accounting for Thickness Effect ............................................................................ 11–42 11.4.8.13.1. Background ................................................................................................ 11–42 11.4.8.13.2. Using KEYOPT(11) ....................................................................................... 11–42 11.4.8.14. Using Time Step Control ...................................................................................... 11–42 11.4.8.14.1. Background ................................................................................................ 11–42 11.4.8.14.2. Using KEYOPT(7) ......................................................................................... 11–42 11.4.8.15. Using the Birth and Death Option ......................................................................... 11–42 11.4.9. Controlling the Motion of the Rigid Target Surface (Rigid-to-Flexible Contact) ................. 11–43 11.4.10. Modeling Thermal Contact ........................................................................................... 11–44 11.4.10.1. Thermal Contact Behavior vs. Contact Status ........................................................ 11–44 11.4.10.2. Free Thermal Surface ........................................................................................... 11–44 11.4.10.3. Temperature on Target Surface ............................................................................ 11–45 11.4.10.4. Modeling Conduction .......................................................................................... 11–45 11.4.10.4.1. Using TCC ................................................................................................... 11–45 11.4.10.4.2. Using the Quasi Solver Option ..................................................................... 11–46 11.4.10.5. Modeling Convection ........................................................................................... 11–46 11.4.10.6. Modeling Radiation ............................................................................................. 11–46 11.4.10.6.1. Background ................................................................................................ 11–46 11.4.10.6.2. Using SBCT and RDVF .................................................................................. 11–47 11.4.10.7. Modeling Heat Generation Due to Friction ........................................................... 11–47 11.4.10.7.1. Background ................................................................................................ 11–47 11.4.10.7.2. Using FHTG and FWGT ................................................................................ 11–47
xviii
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 11.4.10.8. Modeling External Heat Flux ................................................................................. 11–48 11.4.11. Modeling Electric Contact ............................................................................................. 11–48 11.4.11.1. Modeling Surface Interaction ............................................................................... 11–48 11.4.11.1.1. Background ................................................................................................ 11–48 11.4.11.1.2. Using ECC ................................................................................................... 11–49 11.4.11.2. Modeling Heat Generation Due to Electric Current ................................................ 11–49 11.4.12. Modeling Magnetic Contact .......................................................................................... 11–50 11.4.12.1. Using MCC ........................................................................................................... 11–50 11.4.12.2. Modeling Perfect Magnetic Contact ..................................................................... 11–51 11.4.13. Applying Necessary Boundary Conditions to the Deformable Elements ......................... 11–51 11.4.14. Defining Solution and Load Step Options ...................................................................... 11–51 11.4.15. Solving the Problem ..................................................................................................... 11–52 11.4.16. Reviewing the Results ................................................................................................... 11–53 11.4.16.1. Points to Remember ............................................................................................ 11–53 11.4.16.2. Reviewing Results in POST1 .................................................................................. 11–53 11.4.16.3. Reviewing Results in POST26 ................................................................................ 11–54 11.5. GUI Aids for Contact Analyses .................................................................................................. 11–54 11.5.1. The Contact Manager ..................................................................................................... 11–54 11.5.2. The Contact Wizard ........................................................................................................ 11–55 11.5.3. Managing Contact Pairs .................................................................................................. 11–56 11.6. Performing a Node-to-Surface Contact Analysis ....................................................................... 11–57 11.6.1. Using the Node-to-Surface Contact Elements .................................................................. 11–57 11.6.1.1. CONTA175 KEYOPTS .............................................................................................. 11–59 11.6.1.1.1. KEYOPT(3) ..................................................................................................... 11–59 11.6.1.1.2. KEYOPT(4) ..................................................................................................... 11–59 11.6.1.2. CONTA175 Real Constants ..................................................................................... 11–60 11.6.1.3. Multiphysics Contact ............................................................................................. 11–60 11.7. Using the Internal MPC Approach for Assemblies and Kinematic Constraints ............................ 11–60 11.7.1. Modeling Solid-solid and Shell-shell Assemblies .............................................................. 11–61 11.7.2. Modeling a Shell-solid Assembly ..................................................................................... 11–62 11.7.3. Surface-based Constraints .............................................................................................. 11–66 11.7.3.1. Defining Surface-based Constraints ........................................................................ 11–67 11.7.3.2. Modeling a Beam-solid Assembly ........................................................................... 11–68 11.7.4. Restrictions and Recommendations for Internal MPC ....................................................... 11–69 11.8. Performing a Node-to-Node Contact Analysis .......................................................................... 11–70 11.8.1. Creating Geometry and Meshing the Model .................................................................... 11–71 11.8.2. Generating Contact Elements ......................................................................................... 11–71 11.8.2.1. Generating Contact Elements Automatically at Coincident Nodes ........................... 11–72 11.8.2.2. Generating Contact Elements Automatically at Offset Nodes .................................. 11–72 11.8.2.3. Node Ordering ...................................................................................................... 11–72 11.8.3. Defining the Contact Normal .......................................................................................... 11–73 11.8.4. Defining the Initial Interference or Gap ........................................................................... 11–74 11.8.5. Selecting the Contact Algorithm ..................................................................................... 11–74 11.8.6. Applying Necessary Boundary Conditions ....................................................................... 11–74 11.8.7. Defining the Solution Options ........................................................................................ 11–75 11.8.8. Solving the Problem ....................................................................................................... 11–76 11.8.9. Reviewing the Results ..................................................................................................... 11–76 12. Fracture Mechanics .......................................................................................................................... 12–1 12.1. Definition of Fracture Mechanics ............................................................................................... 12–1 12.2. Solving Fracture Mechanics Problems ....................................................................................... 12–1 12.2.1. Modeling the Crack Region ............................................................................................... 12–1 12.2.1.1. 2-D Fracture Models ................................................................................................ 12–3
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xix
Structural Analysis Guide 12.2.1.2. 3-D Fracture Models ................................................................................................ 12–4 12.2.2. Calculating Fracture Parameters ....................................................................................... 12–5 12.2.2.1. Stress Intensity Factors ............................................................................................ 12–5 12.2.2.2. J-Integral ................................................................................................................. 12–6 12.2.2.3. Energy Release Rate ................................................................................................. 12–8 13. Composites ...................................................................................................................................... 13–1 13.1. Definition of Composites ........................................................................................................... 13–1 13.2. Modeling Composites ............................................................................................................... 13–1 13.2.1. Choosing the Proper Element Type ................................................................................... 13–1 13.2.2. Defining the Layered Configuration .................................................................................. 13–2 13.2.2.1. Specifying Individual Layer Properties ...................................................................... 13–3 13.2.2.2. Defining the Constitutive Matrices ........................................................................... 13–4 13.2.2.3. Sandwich and Multiple-Layered Structures ............................................................... 13–4 13.2.2.4. Node Offset ............................................................................................................. 13–5 13.2.3. Specifying Failure Criteria ................................................................................................. 13–5 13.2.4. Additional Modeling and Postprocessing Guidelines ......................................................... 13–6 14. Fatigue ............................................................................................................................................. 14–1 14.1. Definition of Fatigue ................................................................................................................. 14–1 14.1.1. What the ANSYS Program Does ........................................................................................ 14–1 14.1.2. Basic Terminology ............................................................................................................ 14–1 14.2. Doing a Fatigue Evaluation ....................................................................................................... 14–2 14.2.1. Enter POST1 and Resume Your Database .......................................................................... 14–2 14.2.2. Establish the Size, Fatigue Material Properties, and Locations ............................................ 14–2 14.2.3. Store Stresses and Assign Event Repetitions and Scale Factors ........................................... 14–4 14.2.3.1. Storing Stresses ....................................................................................................... 14–4 14.2.3.1.1. Manually Stored Stresses ................................................................................. 14–4 14.2.3.1.2. Nodal Stresses from Jobname.RST ................................................................... 14–5 14.2.3.1.3. Stresses at a Cross-Section ............................................................................... 14–5 14.2.3.2. Listing, Plotting, or Deleting Stored Stresses ............................................................. 14–6 14.2.3.3. Assigning Event Repetitions and Scale Factors ......................................................... 14–6 14.2.3.4. Guidelines for Obtaining Accurate Usage Factors ..................................................... 14–7 14.2.4. Activate the Fatigue Calculations ...................................................................................... 14–9 14.2.5. Review the Results ........................................................................................................... 14–9 14.2.6. Other Approaches to Range Counting .............................................................................. 14–9 14.2.7. Sample Input ................................................................................................................... 14–9 15. p-Method Structural Static Analysis ................................................................................................ 15–1 15.1. Definition of p-Method Analysis ................................................................................................ 15–1 15.2. Benefits of Using the p-Method ................................................................................................. 15–1 15.3. Using the p-Method .................................................................................................................. 15–1 15.3.1. Select the p-Method Procedure ........................................................................................ 15–1 15.3.2. Build the Model ................................................................................................................ 15–2 15.3.2.1. Define the Element Types ........................................................................................ 15–2 15.3.2.1.1. Specifying a p-Level Range .............................................................................. 15–2 15.3.2.2. Specify Material Properties and/or Real Constants .................................................... 15–3 15.3.2.2.1. Material Properties .......................................................................................... 15–3 15.3.2.2.2. Real Constants ................................................................................................ 15–3 15.3.2.3. Define the Model Geometry ..................................................................................... 15–4 15.3.2.4. Mesh the Model into Solid or Shell Elements ............................................................ 15–4 15.3.2.4.1. Using Program Defaults .................................................................................. 15–4 15.3.2.4.2. Specifying Mesh Controls ................................................................................ 15–4 15.3.2.4.3. Guidelines for Creating a Good Mesh ............................................................... 15–5 15.3.3. Additional Information for Building Your Model ................................................................ 15–5
xx
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 15.3.3.1. Viewing your element model ................................................................................... 15–5 15.3.3.2. Coupling ................................................................................................................. 15–6 15.3.3.2.1. Coupling of Corner Nodes ............................................................................... 15–6 15.3.3.2.2. Midside Node Coupling ................................................................................... 15–7 15.3.4. Apply Loads and Obtain the Solution ................................................................................ 15–7 15.3.5. Helpful Hints for Common Problems ............................................................................... 15–12 15.3.6. Review the Results .......................................................................................................... 15–12 15.3.6.1. The p-Element Subgrid .......................................................................................... 15–13 15.3.7. Querying Subgrid Results ............................................................................................... 15–13 15.3.8. Printing and Plotting Node and Element Results ............................................................. 15–14 15.3.8.1. Specialized p-Method Displays and Listings ............................................................ 15–14 15.4. Sample p-Method Analysis (GUI Method) ................................................................................. 15–14 15.4.1. Problem Description ....................................................................................................... 15–15 15.4.2. Problem Specifications ................................................................................................... 15–15 15.4.3. Problem Diagram ........................................................................................................... 15–15 15.4.3.1. Set the Analysis Title .............................................................................................. 15–15 15.4.3.2. Select p-Method .................................................................................................... 15–15 15.4.3.3. Define the Element Type and Options .................................................................... 15–15 15.4.3.4. Define the Real Constants ...................................................................................... 15–16 15.4.3.5. Define Material Properties ...................................................................................... 15–16 15.4.3.6. Create Plate with Hole ............................................................................................ 15–16 15.4.3.7. Mesh the Areas ...................................................................................................... 15–16 15.4.3.8. Define Symmetry Boundary Conditions .................................................................. 15–17 15.4.3.9. Define Pressure Load along Right Edge. .................................................................. 15–17 15.4.3.10. Define Convergence Criteria ................................................................................ 15–17 15.4.3.11. Solve the Problem ................................................................................................ 15–17 15.4.3.12. Review the Results and Exit ANSYS ....................................................................... 15–18 15.5. Sample p-Method Analysis (Command or Batch Method) ......................................................... 15–18 16. Beam Analysis and Cross Sections .................................................................................................. 16–1 16.1. An Overview of Beams .............................................................................................................. 16–1 16.2. What Are Cross Sections? .......................................................................................................... 16–1 16.3. How to Create Cross Sections .................................................................................................... 16–2 16.3.1. Defining a Section and Associating a Section ID Number ................................................... 16–3 16.3.2. Defining Cross Section Geometry and Setting the Section Attribute Pointer ...................... 16–3 16.3.2.1. Determining the Number of Cells to Define .............................................................. 16–4 16.3.3. Meshing a Line Model with BEAM44, BEAM188, or BEAM189 Elements .............................. 16–4 16.4. Creating Cross Sections ............................................................................................................. 16–5 16.4.1. Using the Beam Tool to Create Common Cross Sections .................................................... 16–5 16.4.2. Creating Custom Cross Sections with a User-defined Mesh ................................................ 16–6 16.4.3. Creating Custom Cross Sections with Mesh Refinement and Multiple Materials .................. 16–7 16.4.4. Defining Composite Cross Sections ................................................................................... 16–8 16.4.5. Defining a Tapered Beam ................................................................................................. 16–8 16.5. Managing Cross Section and User Mesh Libraries ....................................................................... 16–9 16.6. Sample Lateral Torsional Buckling Analysis (GUI Method) ........................................................... 16–9 16.6.1. Problem Description ....................................................................................................... 16–10 16.6.2. Problem Specifications ................................................................................................... 16–10 16.6.3. Problem Sketch .............................................................................................................. 16–11 16.6.4. Eigenvalue Buckling and Nonlinear Collapse ................................................................... 16–11 16.6.5. Set the Analysis Title and Define Model Geometry ........................................................... 16–12 16.6.6. Define Element Type and Cross Section Information ....................................................... 16–12 16.6.7. Define the Material Properties and Orientation Node ...................................................... 16–12 16.6.8. Mesh the Line and Verify Beam Orientation ..................................................................... 16–13
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xxi
Structural Analysis Guide 16.6.9. Define the Boundary Conditions ..................................................................................... 16–13 16.6.10. Solve the Eigenvalue Buckling Analysis ......................................................................... 16–14 16.6.11. Solve the Nonlinear Buckling Analysis ........................................................................... 16–15 16.6.12. Plot and Review the Results .......................................................................................... 16–15 16.7. Sample Problem with Cantilever Beams, Command Method .................................................... 16–16 16.8. Where to Find Other Examples ................................................................................................ 16–17 17. Shell Analysis and Cross Sections .................................................................................................... 17–1 17.1. An Overview of Shells ................................................................................................................ 17–1 17.2. What Are Cross Sections? .......................................................................................................... 17–1 17.3. How to Create Cross Sections .................................................................................................... 17–1 17.3.1. Defining a Section and Associating a Section ID Number ................................................... 17–2 17.3.2. Defining Layer Data .......................................................................................................... 17–2 17.3.3. Overriding Program Calculated Section Properties ............................................................ 17–3 17.3.4. Specifying a Shell Thickness Variation (Tapered Shells) ...................................................... 17–3 17.3.5. Setting the Section Attribute Pointer ................................................................................ 17–3 17.3.6. Associating an Area with a Section .................................................................................... 17–3 17.3.7. Using the Shell Tool to Create Sections ............................................................................. 17–3 17.3.8. Managing Cross Section Libraries ..................................................................................... 17–5 Index ................................................................................................................................................. Index–1
List of Figures 2.1. Diagram of Allen Wrench .................................................................................................................. 2–14 3.1. Diagram of a Model Airplane Wing .................................................................................................... 3–12 3.2. Choose Master DOF .......................................................................................................................... 3–20 3.3. Choosing Master DOFs ...................................................................................................................... 3–20 3.4. Choosing Masters in an Axisymmetric Shell Model ............................................................................. 3–21 4.1. Harmonic Response Systems ............................................................................................................... 4–1 4.2. Relationship Between Real/Imaginary Components and Amplitude/Phase Angle ................................. 4–6 4.3. An Unbalanced Rotating Antenna ....................................................................................................... 4–7 4.4. Two-Mass-Spring-System .................................................................................................................. 4–14 5.1. Examples of Load-Versus-Time Curves ................................................................................................. 5–4 5.2. Examples of Gap Conditions .............................................................................................................. 5–21 5.3. Model of a Steel Beam Supporting a Concentrated Mass .................................................................... 5–27 5.4. Effect of Integration Time Step on Period Elongation ......................................................................... 5–34 5.5. Transient Input vs. Transient Response .............................................................................................. 5–35 5.6. Rayleigh Damping ............................................................................................................................ 5–38 6.1. Single-Point and Multi-Point Response Spectra ................................................................................... 6–2 6.2. Simply Supported Beam with Vertical Motion of Both Supports ......................................................... 6–11 7.1. Buckling Curves .................................................................................................................................. 7–1 7.2. Adjusting Variable Loads to Find an Eigenvalue of 1.0 .......................................................................... 7–4 7.3. Bar with Hinged Ends .......................................................................................................................... 7–9 8.1. Common Examples of Nonlinear Structural Behavior ........................................................................... 8–1 8.2. A Fishing Rod Demonstrates Geometric Nonlinearity ........................................................................... 8–2 8.3. Newton-Raphson Approach ................................................................................................................ 8–3 8.4. Traditional Newton-Raphson Method vs. Arc-Length Method .............................................................. 8–4 8.5. Load Steps, Substeps, and Time .......................................................................................................... 8–4 8.6. Nonconservative (Path-Dependent) Behavior ...................................................................................... 8–5 8.7. Load Directions Before and After Deflection ........................................................................................ 8–6 8.8. Stress-Stiffened Beams ........................................................................................................................ 8–8 8.9. Elastoplastic Stress-Strain Curve .......................................................................................................... 8–9 xxii
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 8.10. Kinematic Hardening ...................................................................................................................... 8–10 8.11. Bauschinger Effect .......................................................................................................................... 8–11 8.12. NLISO Stress-Strain Curve ................................................................................................................ 8–14 8.13. Cast Iron Plasticity ........................................................................................................................... 8–16 8.14. Hyperelastic Structure ..................................................................................................................... 8–17 8.15. Typical Hyperelastic Stress-Strain Curves ......................................................................................... 8–23 8.16. Data Locations in Stress and Strain Input Arrays ............................................................................... 8–25 8.17. Typical Evaluated Hyperelastic Stress-Strain Curve ........................................................................... 8–27 8.18. Stress Relaxation and Creep ............................................................................................................ 8–29 8.19. Time Hardening Creep Analysis ....................................................................................................... 8–30 8.20. Shape Memory Alloy Phases ............................................................................................................ 8–32 8.21. Viscoplastic Behavior in a Rolling Operation .................................................................................... 8–33 8.22. Viscoelastic Behavior (Maxwell Model) ............................................................................................. 8–34 8.23. Linear Interpolation of Nonlinear Results Can Introduce Some Error ................................................. 8–58 8.24. Convergence Norms Displayed By the Graphical Solution Tracking (GST) Feature ............................. 8–67 8.25. Typical Nonlinear Output Listing ..................................................................................................... 8–70 8.26. Cyclic Point Load History ................................................................................................................. 8–73 10.1. Element Topology of a 3-D 8-Node Interface Element ...................................................................... 10–2 10.2. Pressure vs. Closure Behavior of a Gasket Material ............................................................................ 10–5 10.3. Gasket Material Input: Linear Unloading Curves ............................................................................... 10–7 10.4. Gasket Material Input: Nonlinear Unloading Curves ......................................................................... 10–8 10.5. Gasket Compression and Unloading Curves at Two Temperatures .................................................. 10–11 10.6. Gasket Finite Element Model Geometry ......................................................................................... 10–14 10.7. Whole Model Mesh with Brick Element .......................................................................................... 10–14 10.8. Interface Layer Mesh ..................................................................................................................... 10–15 10.9. Whole Model Tetrahedral Mesh ..................................................................................................... 10–15 10.10. Interface Layer Mesh with Degenerated Wedge Elements ............................................................ 10–16 11.1. Localized Contact Zones ................................................................................................................. 11–6 11.2. ANSYS Geometric Entities and Their Corresponding Rigid Target Elements .................................... 11–10 11.3. A Single Circular Target Segment Created From Arc Line Segments ................................................ 11–11 11.4. Meshing Patterns for Arbitrary Target Surfaces .............................................................................. 11–12 11.5. Smoothing Convex Corner ............................................................................................................ 11–13 11.6. Correct Node Ordering .................................................................................................................. 11–13 11.7. Contact Element Types .................................................................................................................. 11–15 11.8. Specification of the Contact Surface's Outward Normal .................................................................. 11–17 11.9. Depth of the Underlying Element .................................................................................................. 11–20 11.10. Sliding Contact Resistance ........................................................................................................... 11–26 11.11. Friction Decay ............................................................................................................................. 11–27 11.12. Contact Detection Located at Gauss Point ................................................................................... 11–28 11.13. Contact Detection Point Location at Nodal Point ......................................................................... 11–29 11.14. Node Slippage Using Nodal Integration KEYOPT(4) = 1 or 2 .......................................................... 11–29 11.15. Contact Surface Adjustment With ICONT ..................................................................................... 11–32 11.16. Contact Surface Adjustment (PMIN, PMAX) .................................................................................. 11–33 11.17. A Scenario in Which Initial Adjustment Will Fail ............................................................................ 11–34 11.18. Ignoring Initial Penetration, KEYOPT(9) = 1 .................................................................................. 11–35 11.19. Components of True Penetration ................................................................................................. 11–36 11.20. Ramping Initial Interference ........................................................................................................ 11–37 11.21. Effect of Moving Contact Nodes .................................................................................................. 11–38 11.22. Auto Spurious Prevention ............................................................................................................ 11–39 11.23. Target Temperature .................................................................................................................... 11–45 11.24. Contact Manager Toolbar ............................................................................................................ 11–54 11.25. Example of a Contact Wizard Dialog ............................................................................................ 11–56
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xxiii
Structural Analysis Guide 11.26. Node-to-Surface Contact Elements .............................................................................................. 11–58 11.27. Example of Shell-solid Assembly .................................................................................................. 11–62 11.28. Shell-solid Assembly (Original Mesh) ........................................................................................... 11–63 11.29. Shell-solid Assembly with Solid-solid Constraint Option ............................................................... 11–64 11.30. Shell-solid Assembly with Shell-shell Constraint Option ............................................................... 11–64 11.31. Shell-solid Assembly with Shell-solid Constraint Option ............................................................... 11–65 11.32. Rigid Constraint Surface .............................................................................................................. 11–66 11.33. Force-distributed Surface ............................................................................................................ 11–67 11.34. Beam-solid Assembly Defined by Rigid Constraint Surface ........................................................... 11–69 11.35. Beam-solid Assembly Defined by Force-distributed Surface ......................................................... 11–69 11.36. Node-to-Node Contact Elements ................................................................................................. 11–70 11.37. Contact Between Two Concentric Pipes ....................................................................................... 11–72 11.38. Two Concentric Pipes, Normals Rotated Properly ......................................................................... 11–73 11.39. Example of Overconstrained Contact Problem ............................................................................. 11–75 12.1. Crack Tip and Crack Front ................................................................................................................ 12–2 12.2. Examples of Singular Elements ........................................................................................................ 12–3 12.3. A Fracture Specimen and 2-D FE Model ........................................................................................... 12–4 12.4. Taking Advantage of Symmetry ...................................................................................................... 12–4 12.5. Crack Coordinate Systems ............................................................................................................... 12–5 12.6. Typical Path Definitions ................................................................................................................... 12–6 12.7. J-Integral Contour Path Surrounding a Crack-Tip ............................................................................. 12–7 12.8. Examples of Paths for J-integral Calculation ..................................................................................... 12–7 13.1. Layered Model Showing Dropped Layer .......................................................................................... 13–3 13.2. Sandwich Construction ................................................................................................................... 13–4 13.3. Layered Shell With Nodes at Midplane ............................................................................................. 13–5 13.4. Layered Shell With Nodes at Bottom Surface ................................................................................... 13–5 13.5. Example of an Element Display ........................................................................................................ 13–7 13.6. Sample LAYPLOT Display for [45/-45/ - 45/45] Sequence .................................................................. 13–8 14.1. Cylinder Wall with Stress Concentration Factors (SCFs) .................................................................... 14–4 14.2. Three Loadings in One Event ........................................................................................................... 14–5 14.3. Surface Nodes are Identified by PPATH Prior to Executing FSSECT .................................................... 14–6 15.1. Fan Model Showing p-Element vs. h-Element Meshes ...................................................................... 15–5 15.2. Coupled Nodes on One Element ...................................................................................................... 15–6 15.3. Nodes Coupled Between Adjacent Elements ................................................................................... 15–6 15.4. Both Corner Nodes are Coupled ...................................................................................................... 15–7 15.5. All Coupled Nodes are Midside Nodes ............................................................................................. 15–7 15.6. Constraints on Rotated Nodes ......................................................................................................... 15–9 15.7. p-Element Subgrids for Quadrilateral Elements .............................................................................. 15–13 15.8. Steel Plate With a Hole .................................................................................................................. 15–15 16.1. Plot of a Z Cross Section .................................................................................................................. 16–2 16.2. Types of Solid Section Cell Mesh ...................................................................................................... 16–4 16.3. BeamTool with Subtypes Drop Down List Displayed ........................................................................ 16–6 16.4. Lateral-Torsional Buckling of a Cantilever I-Beam ........................................................................... 16–10 16.5. Diagram of a Beam With Deformation Indicated ............................................................................ 16–11 17.1. Plot of a Shell Section ...................................................................................................................... 17–2 17.2. Shell Tool With Layup Page Displayed ............................................................................................. 17–4 17.3. Shell Tool With Section Controls Page Displayed .............................................................................. 17–4 17.4. Shell Tool With Summary Page Displayed ........................................................................................ 17–5
xxiv
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide
List of Tables 1.1. Structural Element Types .................................................................................................................... 1–2 2.1. Basic Tab Options ............................................................................................................................... 2–3 2.2. Sol'n Options Tab Options ................................................................................................................... 2–4 2.3. Nonlinear Tab Options ........................................................................................................................ 2–4 2.4. Advanced NL Tab Options ................................................................................................................... 2–5 2.5. Loads Applicable in a Static Analysis ................................................................................................... 2–8 3.1. Analysis Types and Options ................................................................................................................. 3–2 3.2. Loads Applicable in a Modal Analysis .................................................................................................. 3–5 3.3. Load Commands for a Modal Analysis ................................................................................................. 3–5 3.4. Load Step Options .............................................................................................................................. 3–6 3.5. Expansion Pass Options ...................................................................................................................... 3–8 3.6. Symmetric System Eigensolver Choices ............................................................................................. 3–17 4.1. Analysis Types and Options ................................................................................................................. 4–4 4.2. Applicable Loads in a Harmonic Response Analysis .............................................................................. 4–7 4.3. Load Commands for a Harmonic Response Analysis ............................................................................ 4–8 4.4. Load Step Options .............................................................................................................................. 4–9 4.5. Expansion Pass Options .................................................................................................................... 4–22 5.1. Transient Tab Options ......................................................................................................................... 5–8 5.2. Options for the First Load Step-Mode Superposition Analysis ............................................................. 5–15 5.3. Options for the First Load Step-Reduced Analysis .............................................................................. 5–22 5.4. Expansion Pass Options .................................................................................................................... 5–24 5.5. Damping for Different Analysis Types ................................................................................................ 5–36 5.6. Damping Matrix Formulation with Different Damping Coefficients .................................................... 5–39 6.1. Analysis Types and Options ................................................................................................................. 6–4 6.2. Load Step Options .............................................................................................................................. 6–4 6.3. Solution Items Available in a PSD Analysis ......................................................................................... 6–21 6.4. Organization of Results Data from a PSD Analysis .............................................................................. 6–22 8.1. Suggested Mooney-Rivlin Constants ................................................................................................. 8–23 8.2. Data Locations in Stress and Strain Input Arrays ................................................................................. 8–24 9.1. Experimental Details for Case 1 and 2 Models and Blatz-Ko .................................................................. 9–2 9.2. Experimental Details for Case 3 Models ............................................................................................... 9–2 9.3. Hyperelastic Curve Fitting Model Types ............................................................................................... 9–3 9.4. Creep Data Types and Abbreviations ................................................................................................... 9–8 9.5. Creep Model and Data/Type Attribute ................................................................................................. 9–8 9.6. Creep Models and Abbreviations ....................................................................................................... 9–10 9.7. Viscoelastic Data Types and Abbreviations ........................................................................................ 9–15 11.1. ANSYS Contact Capabilities ............................................................................................................. 11–2 11.2. Summary of Real Constant Defaults in Different Environments ....................................................... 11–18 11.3. Summary of KEYOPT Defaults in Different Environments ................................................................ 11–21 16.1. ANSYS Cross Section Commands ..................................................................................................... 16–2 17.1. ANSYS Cross Section Commands ..................................................................................................... 17–1
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xxv
xxvi
Chapter 1: Overview of Structural Analyses 1.1. Definition of Structural Analysis Structural analysis is probably the most common application of the finite element method. The term structural (or structure) implies not only civil engineering structures such as bridges and buildings, but also naval, aeronautical, and mechanical structures such as ship hulls, aircraft bodies, and machine housings, as well as mechanical components such as pistons, machine parts, and tools.
1.2. Types of Structural Analysis The seven types of structural analyses available in the ANSYS family of products are explained below. The primary unknowns (nodal degrees of freedom) calculated in a structural analysis are displacements. Other quantities, such as strains, stresses, and reaction forces, are then derived from the nodal displacements. Structural analyses are available in the ANSYS Multiphysics, ANSYS Mechanical, ANSYS Structural, and ANSYS Professional programs only. You can perform the following types of structural analyses. Each of these analysis types are discussed in detail in this manual. Static Analysis--Used to determine displacements, stresses, etc. under static loading conditions. Both linear and nonlinear static analyses. Nonlinearities can include plasticity, stress stiffening, large deflection, large strain, hyperelasticity, contact surfaces, and creep. Modal Analysis--Used to calculate the natural frequencies and mode shapes of a structure. Different mode extraction methods are available. Harmonic Analysis--Used to determine the response of a structure to harmonically time-varying loads. Transient Dynamic Analysis--Used to determine the response of a structure to arbitrarily time-varying loads. All nonlinearities mentioned under Static Analysis above are allowed. Spectrum Analysis--An extension of the modal analysis, used to calculate stresses and strains due to a response spectrum or a PSD input (random vibrations). Buckling Analysis--Used to calculate the buckling loads and determine the buckling mode shape. Both linear (eigenvalue) buckling and nonlinear buckling analyses are possible. Explicit Dynamic Analysis--This type of structural analysis is only available in the ANSYS LS-DYNA program. ANSYS LS-DYNA provides an interface to the LS-DYNA explicit finite element program. Explicit dynamic analysis is used to calculate fast solutions for large deformation dynamics and complex contact problems. Explicit dynamic analysis is described in the ANSYS LS-DYNA User's Guide. In addition to the above analysis types, several special-purpose features are available: •
Fracture mechanics
•
Composites
•
Fatigue
•
p-Method
•
Beam Analyses Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 1: Overview of Structural Analyses
1.3. Elements Used in Structural Analyses Most ANSYS element types are structural elements, ranging from simple spars and beams to more complex layered shells and large strain solids. Most types of structural analyses can use any of these elements. Note — Explicit dynamics analysis can use only the explicit dynamic elements (LINK160, BEAM161, PLANE162, SHELL163, SOLID164, COMBI165, MASS166, LINK167, and SOLID168).
Table 1.1 Structural Element Types Category
Element Name(s)
Spars
LINK1, LINK8, LINK10, LINK180
Beams
BEAM3, BEAM4, BEAM23, BEAM24, BEAM44, BEAM54, BEAM188, BEAM189
Pipes
PIPE16, PIPE17, PIPE18, PIPE20, PIPE59, PIPE60
2-D Solids
PLANE2, PLANE25, PLANE42, HYPER56, HYPER74, PLANE82, PLANE83, HYPER84, VISCO88, VISCO106, VISCO108, PLANE145, PLANE146, PLANE182, PLANE183
3-D Solids
SOLID45, SOLID46, HYPER58, SOLID64, SOLID65, HYPER86, VISCO89, SOLID92, SOLID95, VISCO107, SOLID147, SOLID148, HYPER158, SOLID185, SOLID186, SOLID187, SOLID191
Shells
SHELL28, SHELL41, SHELL43, SHELL51, SHELL61, SHELL63, SHELL91, SHELL93, SHELL99, SHELL150, SHELL181
Interface
INTER192, INTER193, INTER194, INTER195
Contact
CONTAC12, CONTAC52, TARGE169, TARGE170, CONTA171, CONTA172, CONTA173, CONTA174, CONTA175
Coupled-Field
SOLID5, PLANE13, FLUID29, FLUID30, FLUID38, SOLID62, FLUID79, FLUID80, FLUID81, SOLID98, FLUID129, INFIN110, INFIN111, FLUID116, FLUID130
Specialty
COMBIN7, LINK11, COMBIN14, MASS21, MATRIX27, COMBIN37, COMBIN39, COMBIN40, MATRIX50, SURF153, SURF154
Explicit Dynamics
LINK160, BEAM161, PLANE162, SHELL163, SOLID164, COMBI165, MASS166, LINK167, SOLID168
1.4. Material Model Interface For analyses described in this guide, if you are using the GUI, you must specify the material you will be simulating using an intuitive material model interface. This interface uses a hierarchical tree structure of material categories, which is intended to assist you in choosing the appropriate model for your analysis. See Section 1.2.4.4: Material Model Interface in the ANSYS Basic Analysis Guide for details on the material model interface.
1.5. Types of Solution Methods Two solution methods are available for solving structural problems in the ANSYS family of products: the hmethod and the p-method. The h-method can be used for any type of analysis, but the p-method can be used only for linear structural static analyses. Depending on the problem to be solved, the h-method usually requires a finer mesh than the p-method. The p-method provides an excellent way to solve a problem to a desired level of accuracy while using a coarse mesh. In general, the discussions in this manual focus on the procedures required for the h-method of solution. Chapter 15, “p-Method Structural Static Analysis” discusses procedures specific to the p-method.
1–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 2: Structural Static Analysis 2.1. Definition of Static Analysis A static analysis calculates the effects of steady loading conditions on a structure, while ignoring inertia and damping effects, such as those caused by time-varying loads. A static analysis can, however, include steady inertia loads (such as gravity and rotational velocity), and time-varying loads that can be approximated as static equivalent loads (such as the static equivalent wind and seismic loads commonly defined in many building codes). Static analysis is used to determine the displacements, stresses, strains, and forces in structures or components caused by loads that do not induce significant inertia and damping effects. Steady loading and response conditions are assumed; that is, the loads and the structure's response are assumed to vary slowly with respect to time. The kinds of loading that can be applied in a static analysis include: •
Externally applied forces and pressures
•
Steady-state inertial forces (such as gravity or rotational velocity)
•
Imposed (nonzero) displacements
•
Temperatures (for thermal strain)
•
Fluences (for nuclear swelling)
More information about the loads that you can apply in a static analysis appears in Section 2.3.4: Apply the Loads.
2.2. Linear vs. Nonlinear Static Analyses A static analysis can be either linear or nonlinear. All types of nonlinearities are allowed - large deformations, plasticity, creep, stress stiffening, contact (gap) elements, hyperelastic elements, and so on. This chapter focuses on linear static analyses, with brief references to nonlinearities. Details of how to handle nonlinearities are described in Chapter 8, “Nonlinear Structural Analysis”.
2.3. Performing a Static Analysis The procedure for a static analysis consists of these tasks: 1.
Section 2.3.1: Build the Model
2.
Section 2.3.2: Set Solution Controls
3.
Section 2.3.3: Set Additional Solution Options
4.
Section 2.3.4: Apply the Loads
5.
Section 2.3.5: Solve the Analysis
6.
Section 2.3.6: Review the Results
2.3.1. Build the Model See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details, see the ANSYS Modeling and Meshing Guide.
2.3.1.1. Points to Remember Keep the following points in mind when doing a static analysis: Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 2: Structural Static Analysis •
You can use both linear and nonlinear structural elements.
•
Material properties can be linear or nonlinear, isotropic or orthotropic, and constant or temperature-dependent. –
You must define stiffness in some form (for example, Young's modulus (EX), hyperelastic coefficients, and so on).
–
For inertia loads (such as gravity), you must define the data required for mass calculations, such as density (DENS).
–
For thermal loads (temperatures), you must define the coefficient of thermal expansion (ALPX).
Note the following information about mesh density: •
Regions where stresses or strains vary rapidly (usually areas of interest) require a relatively finer mesh than regions where stresses or strains are nearly constant (within an element).
•
While considering the influence of nonlinearities, remember that the mesh should be able to capture the effects of the nonlinearities. For example, plasticity requires a reasonable integration point density (and therefore a fine element mesh) in areas with high plastic deformation gradients.
2.3.2. Set Solution Controls Setting solution controls involves defining the analysis type and common analysis options for an analysis, as well as specifying load step options for it. When you are doing a structural static analysis, you can take advantage of a streamlined solution interface (called the Solution Controls dialog box) for setting these options. The Solution Controls dialog box provides default settings that will work well for many structural static analyses, which means that you may need to set only a few, if any, of the options. Because the streamlined solution interface is the recommended tool for setting solution controls in a structural static analysis, it is the method that is presented in this chapter. If you prefer not to use the Solution Controls dialog box (Main Menu> Solution> Analysis Type> Sol'n Controls), you can set solution controls for your analysis using the standard set of ANSYS solution commands and the standard corresponding menu paths (Main Menu> Solution> Unabridged Menu> option). For a general overview of the Solution Controls dialog box, see Section 3.11: Using Special Solution Controls for Certain Types of Structural Analyses in the ANSYS Basic Analysis Guide.
2.3.2.1. Access the Solution Controls Dialog Box To access the Solution Controls dialog box, choose menu path Main Menu> Solution> Analysis Type> Sol'n Controls. The following sections provide brief descriptions of the options that appear on each tab of the dialog box. For details about how to set these options, select the tab that you are interested in (from within the ANSYS program), and then click the Help button. Chapter 8, “Nonlinear Structural Analysis” also contains details about the nonlinear options introduced in this chapter.
2.3.2.2. Using the Basic Tab The Basic tab is active when you access the dialog box. The controls that appear on the Basic tab provide the minimum amount of data that ANSYS needs for the analysis. Once you are satisfied with the settings on the Basic tab, you do not need to progress through the remaining tabs unless you want to adjust the default settings for the more advanced controls. As soon as you click OK on any tab of the dialog box, the settings are applied to the ANSYS database and the dialog box closes.
2–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.3: Performing a Static Analysis You can use the Basic tab to set the options listed in Table 2.1: “Basic Tab Options”. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Basic tab, and click the Help button.
Table 2.1 Basic Tab Options Option
For more information on this option, see: •
Section 1.2.6.1: Defining the Analysis Type and Analysis Options in the ANSYS Basic Analysis Guide
•
Chapter 8, “Nonlinear Structural Analysis” in the ANSYS Structural Analysis Guide
•
Section 3.16: Restarting an Analysis in the ANSYS Basic Analysis Guide
Control time settings, including: time at end of load step [TIME], automatic time stepping [AUTOTS], and number of substeps to be taken in a load step [NSUBST or DELTIM]
•
Section 2.4: The Role of Time in Tracking in the ANSYS Basic Analysis Guide
•
Section 2.7.1: General Options in the ANSYS Basic Analysis Guide
Specify solution data to write to database [OUTRES]
•
Section 2.7.4: Output Controls in the ANSYS Basic Analysis Guide
Specify analysis type [ANTYPE, NLGEOM]
Special considerations for setting these options in a static analysis include: •
When setting ANTYPE and NLGEOM, choose Small Displacement Static if you are performing a new analysis and you want to ignore large deformation effects such as large deflection, large rotation, and large strain. Choose Large Displacement Static if you expect large deflections (as in the case of a long, slender bar under bending) or large strains (as in a metal-forming problem). Choose Restart Current Analysis if you want to restart a failed nonlinear analysis, or you have previously completed a static analysis, and you want to specify additional loads.
•
When setting TIME, remember that this load step option specifies time at the end of the load step. The default value is 1.0 for the first load step. For subsequent load steps, the default is 1.0 plus the time specified for the previous load step. Although time has no physical meaning in a static analysis (except in the case of creep, viscoplasticity, or other rate-dependent material behavior), it is used as a convenient way of referring to load steps and substeps (see Chapter 2, “Loading” in the ANSYS Basic Analysis Guide).
•
When setting OUTRES, keep this caution in mind: Caution: By default, only 1000 results sets can be written to the results file (Jobname.RST). If this number is exceeded (based on your OUTRES specification), the program will terminate with an error. Use the command /CONFIG,NRES to increase the limit (see Chapter 19, “Memory Management and Configuration” in the ANSYS Basic Analysis Guide).
2.3.2.3. The Transient Tab The Transient tab contains transient analysis controls; it is available only if you choose a transient analysis and remains grayed out when you choose a static analysis. For these reasons, it is not described here.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–3
Chapter 2: Structural Static Analysis
2.3.2.4. Using the Sol'n Options Tab You can use the Sol'n Options tab to set the options listed in Table 2.2: “Sol'n Options Tab Options”. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Sol'n Options tab, and click the Help button.
Table 2.2 Sol'n Options Tab Options Option
For more information about this option, see the following section(s) in the ANSYS Basic Analysis Guide:
Specify equation solver [EQSLV]
•
Section 3.2: Selecting a Solver through Section 3.10: Using the Automatic Iterative (Fast) Solver Option
Specify parameters for multiframe restart [RESCONTROL]
•
Section 3.16.2: Multiframe Restart
Special considerations for setting these options in a static analysis include: •
When setting EQSLV, specify one of these solvers: –
Program chosen solver (ANSYS selects a solver for you, based on the physics of the problem)
–
Sparse direct solver (default for linear and nonlinear, static and full transient analyses)
–
Preconditioned Conjugate Gradient (PCG) solver (recommended for large models/high wavefronts, bulky structures)
–
Algebraic Multigrid (AMG) solver (applicable in the same situations as the PCG solver, but provides parallel processing; for faster turnaround times when used in a multiprocessor environment)
–
Distributed Domain Solver (DDS) provides parallel processing on multiple systems across a network
–
Iterative solver (auto-select; for linear static/full transient structural or steady-state thermal analyses only; recommended)
–
Frontal direct solver
Note — The AMG and DDS solvers are part of Parallel Performance for ANSYS, which is a separately-licensed product. See Chapter 13, “Improving ANSYS Performance and Parallel Performance for ANSYS” in the ANSYS Advanced Analysis Techniques Guide for more information about these solvers.
2.3.2.5. Using the Nonlinear Tab You can use the Nonlinear tab to set the options listed in Table 2.3: “Nonlinear Tab Options”. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Nonlinear tab, and click the Help button.
Table 2.3 Nonlinear Tab Options Option Activate line search [LNSRCH]
2–4
For more information about this option, see the following section(s) in the ANSYS Structural Analysis Guide: •
Section 8.5.2.3.5: Line Search Option
•
Section 8.10.2.4: Using Line Search
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.3: Performing a Static Analysis Option
For more information about this option, see the following section(s) in the ANSYS Structural Analysis Guide:
Activate a predictor on the DOF solution [PRED]
•
Section 8.5.2.3.4: Predictor-Corrector Option
Specify the maximum number of iterations allowed per substep [NEQIT]
•
Section 8.5.2.3.3: Maximum Number of Equilibrium Iterations
Specify whether you want to include creep calculation [RATE]
•
Section 8.3.1.5: Creep
•
Section 8.5.3.2.1: Creep Criteria
Set convergence criteria [CNVTOL]
•
Section 8.5.2.3.2: Convergence Criteria
Control bisections [CUTCONTROL]
•
Section 8.5.2.3.6: Cutback Criteria
2.3.2.6. Using the Advanced NL Tab You can use the Advanced NL tab to set the options listed in Table 2.4: “Advanced NL Tab Options”. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Advanced NL tab, and click the Help button.
Table 2.4 Advanced NL Tab Options Option
For more information about this option, see the following section(s) in the ANSYS Structural Analysis Guide:
Specify analysis termination criteria [NCNV]
•
Section 8.5.2.3.3: Maximum Number of Equilibrium Iterations
Control activation and termination of the arc-length method [ARCLEN, ARCTRM]
•
Section 8.10.2.5: Using the Arc-Length Method
•
Chapter 2, “Loading” in the ANSYS Basic Analysis Guide
2.3.3. Set Additional Solution Options This section discusses additional options that you can set for the solution. These options do not appear on the Solution Controls dialog box because they are used very infrequently, and their default settings rarely need to be changed. ANSYS menu paths are provided in this section to help you access these options for those cases in which you choose to override the ANSYS-assigned defaults. Many of the options that appear in this section are nonlinear options, and are described further in Chapter 8, “Nonlinear Structural Analysis”.
2.3.3.1. Stress Stiffening Effects Some elements, including those in the 18x family of elements, include stress stiffening effects regardless of the SSTIF command setting. To determine whether an element includes stress stiffening, refer to the appropriate element description in the ANSYS Elements Reference. By default, stress stiffening effects are ON when NLGEOM is ON. Specific situations in which you can turn OFF stress stiffening effects include:
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–5
Chapter 2: Structural Static Analysis •
Stress stiffening is relevant only in nonlinear analyses. If you are performing a linear analysis [NLGEOM,OFF], you can turn stress stiffening OFF.
•
Prior to the analysis, you know that the structure is not likely to fail because of buckling (bifurcation, snap through).
Including stress stiffness terms, in general, accelerates nonlinear convergence characteristics. Keeping in mind the points listed above, you may choose to turn stress stiffening OFF for specific problems in which convergence difficulties are seen; for example, local failures. Command(s): SSTIF GUI: Main Menu> Solution> Unabridged Menu> Analysis Options
2.3.3.2. Newton-Raphson Option Use this analysis option only in a nonlinear analysis. This option specifies how often the tangent matrix is updated during solution. You can specify one of these values: •
Program-chosen (default)
•
Full
•
Modified
•
Initial stiffness
•
Full with unsymmetric matrix Command(s): NROPT GUI: Main Menu> Solution> Unabridged Menu> Analysis Options
2.3.3.3. Prestress Effects Calculation Use this analysis option to perform a prestressed analysis on the same model, such as a prestressed modal analysis. The default is OFF. Note — The stress stiffening effects and the prestress effect calculation both control the generation of the stress stiffness matrix, and therefore should not be used together in an analysis. If both are specified, the last option specified will override the previous setting. Command(s): PSTRES GUI: Main Menu> Solution> Unabridged Menu> Analysis Options
2.3.3.4. Mass Matrix Formulation Use this analysis option if you plan to apply inertial loads on the structure (such as gravity and spinning loads). You can specify one of these values: •
Default (depends on element type)
•
Lumped mass approximation Note — For a static analysis, the mass matrix formulation you use does not significantly affect the solution accuracy (assuming that the mesh is fine enough). However, if you want to do a prestressed dynamic analysis on the same model, the choice of mass matrix formulation may be important; see the appropriate dynamic analysis section for recommendations. Command(s): LUMPM GUI: Main Menu> Solution> Unabridged Menu> Analysis Options
2–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.3: Performing a Static Analysis
2.3.3.5. Reference Temperature This load step option is used for thermal strain calculations. Reference temperature can be made material-dependent with the MP,REFT command. Command(s): TREF GUI: Main Menu> Solution> Load Step Opts> Other> Reference Temp
2.3.3.6. Mode Number This load step option is used for axisymmetric harmonic elements. Command(s): MODE GUI: Main Menu> Solution> Load Step Opts> Other> For Harmonic Ele
2.3.3.7. Creep Criteria This nonlinear load step option specifies the creep criterion for automatic time stepping. Command(s): CRPLIM GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Creep Criterion
2.3.3.8. Printed Output Use this load step option to include any results data on the output file (Jobname.OUT). Command(s): OUTPR GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Output Ctrls> Solu Printout Caution: Proper use of multiple OUTPR commands can sometimes be a little tricky. See Section 2.7.4: Output Controls in the ANSYS Basic Analysis Guide for more information on how to use this command.
2.3.3.9. Extrapolation of Results Use this load step option to review element integration point results by copying them to the nodes instead of extrapolating them (default when no material nonlinearities are present). Command(s): ERESX GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Output Ctrls> Integration Pt
2.3.4. Apply the Loads After you set the desired solution options, you are ready to apply loads to the model.
2.3.4.1. Load Types All of the following load types are applicable in a static analysis.
2.3.4.1.1. Displacements (UX, UY, UZ, ROTX, ROTY, ROTZ) These are DOF constraints usually specified at model boundaries to define rigid support points. They can also indicate symmetry boundary conditions and points of known motion. The directions implied by the labels are in the nodal coordinate system.
2.3.4.1.2. Forces (FX, FY, FZ) and Moments (MX, MY, MZ) These are concentrated loads usually specified on the model exterior. The directions implied by the labels are in the nodal coordinate system. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–7
Chapter 2: Structural Static Analysis
2.3.4.1.3. Pressures (PRES) These are surface loads, also usually applied on the model exterior. Positive values of pressure act towards the element face (resulting in a compressive effect).
2.3.4.1.4. Temperatures (TEMP) These are applied to study the effects of thermal expansion or contraction (that is, thermal stresses). The coefficient of thermal expansion must be defined if thermal strains are to be calculated. You can read in temperatures from a thermal analysis [LDREAD], or you can specify temperatures directly, using the BF family of commands.
2.3.4.1.5. Fluences (FLUE) These are applied to study the effects of swelling (material enlargement due to neutron bombardment or other causes) or creep. They are used only if you input a swelling or creep equation.
2.3.4.1.6. Gravity, Spinning, Etc. These are inertia loads that affect the entire structure. Density (or mass in some form) must be defined if inertia effects are to be included.
2.3.4.2. Apply Loads to the Model Except for inertia loads, which are independent of the model, you can define loads either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). You can also apply boundary conditions via TABLE type array parameters (see Section 2.3.4.2.1: Applying Loads Using TABLE Type Array Parameters) or as function boundary conditions (see Section 2.6.15: Applying Loads Using Function Boundary Conditions). Table 2.5: “Loads Applicable in a Static Analysis” summarizes the loads applicable to a static analysis. In an analysis, loads can be applied, removed, operated on, or listed.
Table 2.5 Loads Applicable in a Static Analysis Load Type
Category
For details on commands and menu paths for defining these loads, see...
Displacement (UX, UY, UZ, ROTX, ROTY, Constraints ROTZ)
Section 2.6.3: DOF Constraints in the ANSYS Basic Analysis Guide
Force, Moment (FX, FY, FZ, MX, MY, MZ) Forces
Section 2.6.6: Forces (Concentrated Loads) in the ANSYS Basic Analysis Guide
Pressure (PRES)
Surface Loads
Section 2.6.7: Surface Loads in the ANSYS Basic Analysis Guide
Temperature (TEMP), Fluence (FLUE)
Body Loads
Section 2.6.8: Body Loads in the ANSYS Basic Analysis Guide
Gravity, Spinning, and so on
Inertia Loads
Section 2.6.9: Inertia Loads in the ANSYS Basic Analysis Guide
2.3.4.2.1. Applying Loads Using TABLE Type Array Parameters You can also apply loads using TABLE type array parameters. For details on using tabular boundary conditions, see Section 2.6.14: Applying Loads Using TABLE Type Array Parameters in the ANSYS Basic Analysis Guide. In a structural analysis, valid primary variables are TIME, TEMP, and location (X, Y, Z). 2–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.3: Performing a Static Analysis When defining the table, TIME must be in ascending order in the table index (as in any table array). You can define a table array parameter via command or interactively. For more information on defining table array parameters, see the ANSYS APDL Programmer's Guide.
2.3.4.3. Calculating Inertia Relief You can use a static analysis to perform inertia relief calculations, which calculate the accelerations that will counterbalance the applied loads. You can think of inertia relief as an equivalent free-body analysis. Issue this command before SOLVE as part of the inertia load commands. Your model should meet the following requirements: •
The model should not contain axisymmetric elements, substructures, or nonlinearities. Models with a mixture of 2-D and 3-D element types are not recommended.
•
The effects of offsets and tapering are ignored for beam elements (BEAM23, BEAM24, BEAM44, and BEAM54) as well as for layered elements (SHELL91, SHELL99, SOLID46, and SOLID191). The effects of unsymmetrical layups for layered elements are also ignored. (Breaking up each tapered element into several elements will give a more accurate solution.)
•
Data required for mass calculations (such as density) must be specified.
•
Specify only the minimum number of displacement constraints - those required to prevent rigid-body motion. Three constraints (or fewer, depending on the element type) are necessary for 2-D models and six (or fewer) are necessary for 3-D models. Additional constraints, such as those required to impose symmetry conditions, are permitted, but check for zero reaction forces at all the constraints to make sure that the model is not overconstrained for inertia relief.
•
The loads for which inertia relief calculations are desired should be applied. Command(s): IRLF,1 GUI: Main Menu> Solution> Load Step Opts> Other> Inertia Relief
2.3.4.3.1. Inertia Relief Output Use the IRLIST command to print the output from inertia relief calculations. This output consists of the translational and rotational accelerations required to balance the applied loads and can be used by other programs to perform kinematics studies. The summary listing of mass and moments of inertia (produced during solution) is accurate, not approximate. The reaction forces at the constraints will be zero because the calculated inertia forces balance the applied forces. Inertia relief output is stored in the database rather than in the results file (Jobname.RST). When you issue IRLIST, ANSYS pulls the information from the database, which contains the inertia relief output from the most recent solution [SOLVE or PSOLVE]. Command(s): IRLIST GUI: No GUI equivalent.
2.3.4.3.2. Partial Inertia Relief Calculations You can also do a partial inertia relief calculation. Use the partial solution method [PSOLVE], as shown in the command input below: /PREP7 ... ... MP,DENS,... ... ...
! Generate model, define density
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–9
Chapter 2: Structural Static Analysis FINISH /SOLU D,... F,... SF,... OUTPR,ALL,ALL IRLF,1 PSOLVE,ELFORM PSOLVE,ELPREP IRLIST FINISH
! Specify only minimum no. of constraints ! Other loads ! ! ! ! ! ! !
Activates printout of all items Can also be set to -1 for precise mass and load summary only, no inertia relief Calculates element matrices Modifies element matrices and calculates inertia relief terms Lists the mass summary and total load summary tables
See the ANSYS Commands Reference for discussions of the OUTPR, IRLF, IRLIST, and PSOLVE commands.
2.3.4.3.3. Using a Macro to Perform Inertia Relief Calculations If you need to do inertia relief calculations frequently, you can write a macro containing the above commands. Macros are described in the ANSYS APDL Programmer's Guide.
2.3.5. Solve the Analysis You are now ready to solve the analysis. 1.
Save a backup copy of the database to a named file. You can then retrieve your model by reentering the ANSYS program and issuing RESUME. Command(s): SAVE GUI: Utility Menu> File> Save as
2.
Start solution calculations. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
3.
If you want the analysis to include additional loading conditions (that is, multiple load steps), you will need to repeat the process of applying loads, specifying load step options, saving, and solving for each load step. (Other methods for handling multiple load steps are described in Chapter 2, “Loading” in the ANSYS Basic Analysis Guide.)
4.
Leave SOLUTION. Command(s): FINISH GUI: Close the Solution menu.
2.3.6. Review the Results Results from a static analysis are written to the structural results file, Jobname.RST. They consist of the following data: •
Primary data: –
•
2–10
Nodal displacements (UX, UY, UZ, ROTX, ROTY, ROTZ)
Derived data: –
Nodal and element stresses
–
Nodal and element strains
–
Element forces Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.3: Performing a Static Analysis –
Nodal reaction forces
–
and so on
2.3.6.1. Postprocessors You can review these results using POST1, the general postprocessor, and POST26, the time-history processor. •
POST1 is used to review results over the entire model at specific substeps (time-points). Some typical POST1 operations are explained below.
•
POST26 is used in nonlinear static analyses to track specific result items over the applied load history. See Chapter 8, “Nonlinear Structural Analysis” for the use of POST26 in a nonlinear static analysis. For a complete description of all postprocessing functions, see Chapter 4, “An Overview of Postprocessing” in the ANSYS Basic Analysis Guide.
2.3.6.2. Points to Remember •
To review results in POST1 or POST26, the database must contain the same model for which the solution was calculated.
•
The results file (Jobname.RST) must be available.
2.3.6.3. Reviewing Results Data 1.
Read in the database from the database file. Command(s): RESUME GUI: Utility Menu> File> Resume from
2.
Read in the desired set of results. Identify the data set by load step and substep numbers or by time. (If you specify a time value for which no results are available, the ANSYS program will perform linear interpolation on all the data to calculate the results at that time.) Command(s): SET GUI: Main Menu> General Postproc> Read Results> By Load Step
3.
Perform the necessary POST1 operations. Typical static analysis POST1 operations are explained below.
2.3.6.4. Typical Postprocessing Operations Option: Display Deformed Shape Use the PLDISP command to display a deformed shape (Main Menu> General Postproc> Plot Results> Deformed Shape). The KUND field on PLDISP gives you the option of overlaying the undeformed shape on the display. Option: List Reaction Forces and Moments The PRRSOL command lists reaction forces and moments at the constrained nodes (Main Menu> General Postproc> List Results> Reaction Solu). To display reaction forces, issue /PBC,RFOR,,1 and then request a node or element display [NPLOT or EPLOT]. (Use RMOM instead of RFOR for reaction moments.) Option: List Nodal Forces and Moments
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–11
Chapter 2: Structural Static Analysis Use the PRESOL,F (or M) command to list nodal forces and moments (Main Menu> General Postproc> List Results> Element Solution). You can list the sum of all nodal forces and moments for a selected set of nodes. Select a set of nodes and use this feature to find out the total force acting on those nodes: Command(s): FSUM GUI: Main Menu> General Postproc> Nodal Calcs> Total Force Sum You can also check the total force and total moment at each selected node. For a body in equilibrium, the total load is zero at all nodes except where an applied load or reaction load exists: Command(s): NFORCE GUI: Main Menu> General Postproc> Nodal Calcs> Sum @ Each Node The FORCE command (Main Menu> General Postproc> Options for Outp) dictates which component of the forces is being reviewed: •
Total (default)
•
Static component
•
Damping component
•
Inertia component
For a body in equilibrium, the total load (using all FORCE components) is zero at all nodes except where an applied load or reaction load exists. Option: Line Element Results For line elements, such as beams, spars, and pipes, use ETABLE to gain access to derived data (stresses, strains, and so on) (Main Menu> General Postproc> Element Table> Define Table). Results data are identified by a combination of a label and a sequence number or component name on the ETABLE command. See the ETABLE discussion in The General Postprocessor (POST1) in the ANSYS Basic Analysis Guide for details. Option: Error Estimation For linear static analyses using solid or shell elements, use the PRERR command to list the estimated solution error due to mesh discretization (Main Menu> General Postproc> List Results> Percent Error). This command calculates and lists the percent error in structural energy norm (SEPC), which represents the error relative to a particular mesh discretization. Option: Structural Energy Error Estimation Use PLESOL,SERR to contour the element-by-element structural energy error (SERR) (Main Menu> General Postproc> Plot Results> Contour Plot> Element Solu). Regions of high SERR on the contour display are good candidates for mesh refinement. (You can activate automatic mesh refinement by means of the ADAPT command - see the ANSYS Modeling and Meshing Guide for more information.) See Section 5.3.6: Estimating Solution Error in the ANSYS Basic Analysis Guide for more details about error estimation. Option: Contour Displays Use PLNSOL and PLESOL to contour almost any result item, such as stresses (SX, SY, SZ...), strains (EPELX, EPELY, EPELZ...), and displacements (UX, UY, UZ...) (Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu). The KUND field on PLNSOL and PLESOL gives you the option of overlaying the undeformed shape on the display. 2–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.4: A Sample Static Analysis (GUI Method) Use PLETAB and PLLS to contour element table data and line element data (Main Menu> General Postproc> Element Table> Plot Element Table and Main Menu> General Postproc> Plot Results> Contour Plot> Line Elem Res). Caution: Derived data, such as stresses and strains, are averaged at the nodes by the PLNSOL command. This averaging results in "smeared" values at nodes where elements of different materials, different shell thicknesses, or other discontinuities meet. To avoid the smearing effect, use selecting (described in Chapter 7, “Selecting and Components” in the ANSYS Basic Analysis Guide) to select elements of the same material, same shell thickness, and so on before issuing PLNSOL. Alternatively, use PowerGraphics with the AVRES command (Main Menu> General Postproc> Options for Outp) to not average results across different materials and/or different shell thicknesses. Option: Vector Displays Use PLVECT to view vector displays (Main Menu> General Postproc> Plot Results> Vector Plot> Predefined) and PRVECT to view vector listings (Main Menu> General Postproc> List Results> Vector Data). Vector displays (not to be confused with vector mode) are an effective way of viewing vector quantities, such as displacement (DISP), rotation (ROT), and principal stresses (S1, S2, S3). Option: Tabular Listings Use these commands to produce tabular listings: Command(s): PRNSOL (nodal results), PRESOL (element-by-element results) PRRSOL (reaction data), and so on GUI: Main Menu> General Postproc> List Results> solution option Use the NSORT and ESORT commands to sort the data before listing them (Main Menu> General Postproc> List Results> Sorted Listing> Sort Nodes or Sort Elems). Other Postprocessing Capabilities Many other postprocessing functions - mapping results onto a path, load case combinations, and so on - are available in POST1. See Chapter 4, “An Overview of Postprocessing” in the ANSYS Basic Analysis Guide for details.
2.4. A Sample Static Analysis (GUI Method) In this sample analysis, you will run a static analysis of an Allen wrench.
2.4.1. Problem Description An Allen wrench (10 mm across the flats) is torqued by means of a 100 N force at its end. Later, a 20 N downward force is applied at the same end, at the same time retaining the original 100 N torquing force. The objective is to determine the stress intensity in the wrench under these two loading conditions.
2.4.2. Problem Specifications The following dimensions are used for this problem: Width across flats = 10 mm Configuration = hexagonal Length of shank = 7.5 cm Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–13
Chapter 2: Structural Static Analysis Length of handle = 20 cm Bend radius = 1 cm Modulus of elasticity = 2.07 x 1011 Pa Applied torquing force = 100 N Applied downward force = 20 N
2.4.3. Problem Sketch Figure 2.1 Diagram of Allen Wrench
2.4.3.1. Set the Analysis Title 1.
Choose menu path Utility Menu> File> Change Title.
2.
Type the text "Static Analysis of an Allen Wrench" and click on OK.
2.4.3.2. Set the System of Units 1.
Click once in the Input Window to make it active for text entry.
2.
Type the command /UNITS,SI and press ENTER. Notice that the command is stored in the history buffer, which can be accessed by clicking on the down arrow at the right of the input window.
3.
Choose menu path Utility Menu> Parameters> Angular Units. The Angular Units for Parametric Functions dialog box appears.
4.
In the drop down menu for Units for angular parametric functions, select "Degrees DEG."
5.
Click on OK.
2.4.3.3. Define Parameters 1.
Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.
2.
Type the following parameters and their values in the Selection field. Click on Accept after you define each parameter. For example, first type “exx = 2.07e11” in the Selection field and then click on Accept. Continue entering the remaining parameters and values in the same way. Parameter EXX
2–14
Value 2.07E11
Description Young's modulus is 2.07E11 Pa
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.4: A Sample Static Analysis (GUI Method) Parameter
Value
Description
W_HEX
.01
Width of hex across flats = .01 m
W_FLAT
W_HEX* TAN(30)
Width of flat = .0058 m
L_SHANK
.075
Length of shank (short end) .075 m
L_HANDLE
.2
Length of handle (long end) .2 m
BENDRAD
.01
Bend radius .01 m
L_ELEM
.0075
Element length .0075 m
NO_D_HEX
2
Number of divisions along hex flat = 2
TOL
25E-6
Tolerance for selecting node = 25E-6 m
Note — You can type the labels in upper- or lowercase; ANSYS always displays the labels in uppercase. 3.
Click on Close.
4.
Click on SAVE_DB on the ANSYS Toolbar.
2.4.3.4. Define the Element Types 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
In the scroll box on the left, click once on "Structural Solid."
4.
In the scroll box on the right, click once on "Brick 8node 45."
5.
Click on Apply to define it as element type 1.
6.
Scroll up the list on the right to "Quad 4node 42." Click once to select it.
7.
Click on OK to define Quad 4node42 as element type 2. The Library of Element Types dialog box closes.
8.
Click on Close in the Element Types dialog box.
2.4.3.5. Define Material Properties 1.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
2.
In the Material Models Available window, double-click on the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
3.
Type the text EXX in the EX field (for Young's modulus), and .3 for PRXY. Click on OK. This sets Young's modulus to the parameter specified above. Material Model Number 1 appears in the Material Models Defined window on the left.
4.
Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
2.4.3.6. Create Hexagonal Area as Cross-Section 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Areas> Polygon> By Side Length. The Polygon by Side Length dialog box appears.
2.
Enter 6 for number of sides.
3.
Enter W_FLAT for length of each side. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–15
Chapter 2: Structural Static Analysis 4.
Click on OK. A hexagon appears in the ANSYS Graphics window.
2.4.3.7. Create Keypoints Along a Path 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Keypoints> In Active CS. The Create Keypoints in Active Coordinate System dialog box appears.
2.
Enter 7 for keypoint number. Type a 0 in each of the X, Y, Z location fields.
3.
Click on Apply.
4.
Enter 8 for keypoint number.
5.
Enter 0,0,-L_SHANK for the X, Y, Z location, and click on Apply.
6.
Enter 9 for keypoint number.
7.
Enter 0,L_HANDLE,-L_SHANK for the X, Y, Z location, and click on OK.
2.4.3.8. Create Lines Along a Path 1.
Choose menu path Utility Menu> PlotCtrls> Window Controls> Window Options. The Window Options dialog box appears.
2.
In the Location of triad drop down menu, select "At top left."
3.
Click on OK.
4.
Choose menu path Utility Menu> PlotCtrls> Pan/Zoom/Rotate. The Pan-Zoom-Rotate dialog box appears.
5.
Click on "Iso" to generate an isometric view and click on Close.
6.
Choose menu path Utility Menu> PlotCtrls> View Settings> Angle of Rotation. The Angle of Rotation dialog box appears.
7.
Enter 90 for angle in degrees.
8.
In the Axis of rotation drop down menu, select "Global Cartes X."
9.
Click on OK.
10. Choose menu path Utility Menu> PlotCtrls> Numbering. The Plot Numbering Controls dialog box appears. 11. Click the Keypoint numbers radio button to turn keypoint numbering on. 12. Click the Line numbers radio button to turn line numbering on. 13. Click on OK. 14. Choose menu path Main Menu> Preprocessor> Modeling> Create> Lines> Lines> Straight Line. The Create Straight Line picking menu appears. 15. Click once on keypoints 4 and 1 to create a line between keypoints 1 and 4. (If you have trouble reading the keypoint numbers in the ANSYS Graphics window, use the controls on the Pan-Zoom-Rotate dialog box (Utility Menu> PlotCtrls> Pan/Zoom/Rotate) to zoom in.) 16. Click once on keypoints 7 and 8 to create a line between keypoints 7 and 8. 17. Click once on keypoints 8 and 9 to create a line between keypoints 8 and 9. 18. Click on OK.
2–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.4: A Sample Static Analysis (GUI Method)
2.4.3.9. Create Line from Shank to Handle 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Lines> Line Fillet. The Line Fillet picking menu appears.
2.
Click once on lines 8 and 9.
3.
Click on OK in the picking menu. The Line Fillet dialog box appears.
4.
Enter BENDRAD for Fillet radius and click on OK.
5.
Click on SAVE_DB on the ANSYS Toolbar.
2.4.3.10. Cut Hex Section In this step, you cut the hex section into two quadrilaterals. This step is required to satisfy mapped meshing. 1.
Choose menu path Utility Menu> PlotCtrls> Numbering. The Plot Numbering Controls dialog box appears.
2.
Click the Keypoint numbers radio button to Off.
3.
Click on OK.
4.
Choose menu path Utility Menu> Plot> Areas.
5.
Choose menu path Main Menu> Preprocessor> Modeling> Operate> Booleans> Divide> With Options> Area by Line. The Divide Area by Line picking menu appears.
6.
Click once on the shaded area, and click on OK.
7.
Choose menu path Utility Menu> Plot> Lines.
8.
Click once on line 7. (If you have trouble reading the line numbers in the ANSYS Graphics window, use the controls on the Pan-Zoom-Rotate dialog box (Utility Menu> PlotCtrls> Pan/Zoom/Rotate) to zoom in.)
9.
Click on OK. The Divide Area by Line with Options dialog box appears. In the Subtracted lines will be drop down menu, select Kept. Click OK.
10. Choose menu path Utility Menu> Select> Comp/Assembly> Create Component. The Create Component dialog box appears. 11. Enter BOTAREA for component name. 12. In the Component is made of drop down menu, select "Areas." 13. Click on OK.
2.4.3.11. Set Meshing Density 1.
Choose menu path Main Menu> Preprocessor> Meshing> Size Cntrls> Lines> Picked Lines. The Element Size on Picked Lines picking menu appears.
2.
Enter 1,2,6 in the picker, then press ENTER.
3.
Click on OK in the picking menu. The Element Sizes on Picked Lines dialog box appears.
4.
Enter NO_D_HEX for number of element divisions and click on OK.
2.4.3.12. Set Element Type for Area Mesh In this step, set the element type to PLANE42, all quadrilaterals for the area mesh.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–17
Chapter 2: Structural Static Analysis 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes. The Element Attributes dialog box appears.
2.
In the Element type number drop down menu, select “2 PLANE42” and click on OK.
3.
Choose menu path Main Menu> Preprocessor> Meshing> Mesher Opts. The Mesher Options dialog box appears.
4.
In the Mesher Type field, click on the Mapped radio button and then click on OK. The Set Element Shape dialog box appears.
5.
Click on OK to accept the default of Quad for 2-D shape key.
6.
Click on SAVE_DB on the ANSYS Toolbar.
2.4.3.13. Generate Area Mesh In this step, generate the area mesh you will later drag. 1.
Choose menu path Main Menu> Preprocessor> Meshing> Mesh> Areas> Mapped> 3 or 4 sided. The Mesh Areas picking box appears.
2.
Click on Pick All.
3.
Choose menu path Utility Menu> Plot> Elements.
2.4.3.14. Drag the 2-D Mesh to Produce 3-D Elements 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes. The Element Attributes dialog box appears.
2.
In the Element type number drop down menu, select “1 SOLID45” and click on OK.
3.
Choose menu path Main Menu> Preprocessor> Meshing> Size Cntrls> Global> Size. The Global Element Sizes dialog box appears.
4.
Enter L_ELEM for element edge length and click on OK.
5.
Choose menu path Utility Menu> PlotCtrls> Numbering.
6.
Click the Line numbers radio button to on if it is not already selected.
7.
Click on OK.
8.
Choose menu path Utility Menu> Plot> Lines.
9.
Choose menu path Main Menu> Preprocessor> Modeling> Operate> Extrude> Areas> Along Lines. The Sweep Areas along Lines picking box appears.
10. Click on Pick All. A second picking box appears. 11. Click once on lines 8, 10, and 9 (in that order). 12. Click on OK. The 3-D model appears in the ANSYS Graphics window. 13. Choose menu path Utility Menu> Plot> Elements. 14. Click on SAVE_DB on the ANSYS Toolbar.
2.4.3.15. Select BOTAREA Component and Delete 2-D Elements 1.
Choose menu path Utility Menu> Select> Comp/Assembly> Select Comp/Assembly. The Select Component or Assembly dialog appears.
2.
Click on OK to accept the default of select BOTAREA component.
2–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.4: A Sample Static Analysis (GUI Method) 3.
Choose menu path Main Menu> Preprocessor> Meshing> Clear> Areas. The Clear Areas picking menu appears.
4.
Click on Pick All.
5.
Choose menu path Utility Menu> Select> Everything.
6.
Choose menu path Utility Menu> Plot> Elements.
2.4.3.16. Apply Displacement Boundary Condition at End of Wrench 1.
Choose menu path Utility Menu> Select> Comp/Assembly> Select Comp/Assembly. The Select Component or Assembly dialog appears.
2.
Click on OK to accept the default of select BOTAREA component.
3.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears.
4.
In the top drop down menu, select "Lines."
5.
In the second drop down menu, select "Exterior."
6.
Click on Apply.
7.
In the top drop down menu, select "Nodes."
8.
In the second drop down menu, select "Attached to."
9.
Click on the "Lines, all" radio button to select it.
10. Click on OK. 11. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears. 12. Click on Pick All. The Apply U,ROT on Nodes dialog box appears. 13. In the scroll list for DOFs to be constrained, click on "ALL DOF." 14. Click on OK. 15. Choose menu path Utility Menu> Select> Entities. 16. In the top drop down menu, select "Lines." 17. Click on the "Sele All" button, then click on Cancel.
2.4.3.17. Display Boundary Conditions 1.
Choose menu path Utility Menu> PlotCtrls> Symbols. The Symbols dialog box appears.
2.
Click on the "All Applied BCs" radio button for Boundary condition symbol.
3.
In the Surface Load Symbols drop down menu, select "Pressures."
4.
In the “Show pres and convect as” drop down menu, select "Arrows."
5.
Click on OK.
2.4.3.18. Apply Pressure on Handle In this step, apply pressure on the handle to represent 100 N finger force. 1.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog appears.
2.
In the top drop down menu, select "Areas."
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–19
Chapter 2: Structural Static Analysis 3.
In the second drop down menu, select "By Location."
4.
Click on the "Y coordinates" radio button to select it.
5.
Enter BENDRAD,L_HANDLE for Min, Max, and click on Apply.
6.
Click on "X coordinates" to select it.
7.
Click on Reselect.
8.
Enter W_FLAT/2,W_FLAT for Min, Max, and click on Apply.
9.
In the top drop down menu, select "Nodes."
10. In the second drop down menu, select "Attached to." 11. Click on the "Areas, all" radio button to select it. 12. Click on the "From Full" radio button to select it. 13. Click on Apply. 14. In the second drop down menu, select "By Location." 15. Click on the "Y coordinates" radio button to select it. 16. Click on the "Reselect" radio button. 17. Enter L_HANDLE+TOL,L_HANDLE-(3.0*L_ELEM)-TOL for Min, Max. 18. Click on OK. 19. Choose menu path Utility Menu> Parameters> Get Scalar Data. The Get Scalar Data dialog box appears. 20. In the scroll box on the left, scroll to "Model Data" and select it. 21. In the scroll box on the right, scroll to "For selected set" and select it. 22. Click on OK. The Get Data for Selected Entity Set dialog box appears. 23. Enter "minyval" for the name of the parameter to be defined. 24. In the scroll box on the left, click once on "Current node set" to select it. 25. In the scroll box on the right, click once on "Min Y coordinate" to select it. 26. Click on Apply. 27. Click on OK again to select the default settings. The Get Data for Selected Entity Set dialog box appears. 28. Enter "maxyval" for the name of the parameter to be defined. 29. In the scroll box on the left, click once on "Current node set" to select it. 30. In the scroll box on the right, click once on "Max Y coordinate" to select it. 31. Click on OK. 32. Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears. 33. Type the text PTORQ=100/(W_HEX*(MAXYVAL-MINYVAL)) in the Selection text box and click on Accept. 34. Click on Close. 35. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Pressure> On Nodes. The Apply PRES on Nodes picking menu appears. 36. Click on Pick All. The Apply PRES on Nodes dialog box appears. 37. Enter PTORQ for Load PRES value and click on OK. 38. Choose menu path Utility Menu> Select> Everything. 2–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.4: A Sample Static Analysis (GUI Method) 39. Choose menu path Utility Menu> Plot> Nodes. 40. Click on SAVE_DB on the ANSYS Toolbar.
2.4.3.19. Write the First Load Step 1.
Choose menu path Main Menu> Solution> Load Step Opts> Write LS File. The Write Load Step File dialog appears.
2.
Enter 1 for load step file number n.
3.
Click on OK.
2.4.3.20. Define Downward Pressure In this step, you define the downward pressure on top of the handle, representing 20N (4.5 lb) of force. 1.
Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.
2.
Type the text PDOWN=20/(W_FLAT*(MAXYVAL-MINYVAL)) in the Selection text box and click on Accept.
3.
Click on Close.
4.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog appears.
5.
In the top drop down menu, select "Areas."
6.
In the second drop down menu, select "By Location."
7.
Click on the "Z coordinates" radio button to select it.
8.
Click on the "From Full" radio button to select it.
9.
Enter -(L_SHANK+(W_HEX/2)) for Min, Max.
10. Click on Apply. 11. In the top drop down menu, select "Nodes." 12. In the second drop down menu, select "Attached to." 13. Click on the Areas, all radio button to select it, and click on Apply. 14. In the second drop down menu, select "By Location." 15. Click on the "Y coordinates" radio button to select it. 16. Click on the "Reselect" radio button. 17. Enter L_HANDLE+TOL,L_HANDLE-(3.0*L_ELEM)-TOL for Min, Max. 18. Click on OK. 19. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Pressure> On Nodes. The Apply PRES on Nodes picking menu appears. 20. Click on Pick All. The Apply PRES on Nodes dialog box appears. 21. Enter PDOWN for Load PRES value and click on OK. 22. Choose menu path Utility Menu> Select> Everything. 23. Choose menu path Utility Menu> Plot> Nodes.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–21
Chapter 2: Structural Static Analysis
2.4.3.21. Write Second Load Step 1.
Choose menu path Main Menu> Solution> Load Step Opts> Write LS File. The Write Load Step File dialog box appears.
2.
Enter 2 for Load step file number n, and click on OK.
3.
Click on SAVE_DB on the ANSYS Toolbar.
2.4.3.22. Solve from Load Step Files 1.
Choose menu path Main Menu> Solution> Solve> From LS Files. The Solve Load Step Files dialog box appears.
2.
Enter 1 for Starting LS file number.
3.
Enter 2 for Ending LS file number, and click on OK.
4.
Click on the Close button after the Solution is done! window appears.
2.4.3.23. Read First Load Step and Review Results 1.
Choose menu path Main Menu> General Postproc> Read Results> First Set.
2.
Choose menu path Main Menu> General Postproc> List Results> Reaction Solu. The List Reaction Solution dialog box appears.
3.
Click on OK to accept the default of All Items.
4.
Review the information in the status window, and click on Close.
5.
Choose menu path Utility Menu> PlotCtrls> Symbols. The Symbols dialog box appears.
6.
Click on the "None" radio button for Boundary condition symbol, and click on OK.
7.
Choose menu path Utility Menu> PlotCtrls> Style> Edge Options. The Edge Options dialog box appears.
8.
In the Element outlines for non-contour/contour plots drop down menu, select "Edge Only/All."
9.
Click on OK.
10. Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears. 11. Click on the "Def + undeformed" radio button and click on OK. 12. Choose menu path Utility Menu> PlotCtrls> Save Plot Ctrls. The Save Plot Controls dialog box appears. 13. Type "pldisp.gsa" in the Selection box, and click on OK. 14. Choose menu path Utility Menu> PlotCtrls> View Settings> Angle of Rotation. The Angle of Rotation dialog box appears. 15. Enter 120 for Angle in degrees. 16. In the Relative/absolute drop down menu, select "Relative angle." 17. In the Axis of rotation drop down menu, select "Global Cartes Y." 18. Click on OK. 19. Choose menu path Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu. The Contour Nodal Solution Data dialog box appears. 20. In the scroll box on the left, click on "Stress." In the scroll box on the right, click on "Intensity SINT." 21. Click on OK. 2–22
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.4: A Sample Static Analysis (GUI Method) 22. Choose menu path Utility Menu> PlotCtrls> Save Plot Ctrls. The Save Plot Controls dialog box appears. 23. Type "plnsol.gsa" in the Selection box, and click on OK.
2.4.3.24. Read the Next Load Step and Review Results 1.
Choose menu path Main Menu> General Postproc> Read Results> Next Set.
2.
Choose menu path Main Menu> General Postproc> List Results> Reaction Solu. The List Reaction Solution dialog box appears.
3.
Click on OK to accept the default of All Items.
4.
Review the information in the status window, and click on Close.
5.
Choose menu path Utility Menu> PlotCtrls> Restore Plot Ctrls.
6.
Type "pldisp.gsa" in the Selection box, and click on OK.
7.
Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears.
8.
Click on the "Def + undeformed" radio button if it is not already selected and click on OK.
9.
Choose menu path Utility Menu> PlotCtrls> Restore Plot Ctrls.
10. Type "plnsol.gsa" in the Selection box, and click on OK. 11. Choose menu path Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu. The Contour Nodal Solution Data dialog box appears. 12. In the scroll box on the left, click on "Stress." In the scroll box on the right, scroll to "Intensity SINT" and select it. 13. Click on OK.
2.4.3.25. Zoom in on Cross-Section 1.
Choose menu path Utility Menu> WorkPlane> Offset WP by Increments. The Offset WP tool box appears.
2.
Enter 0,0,-0.067 for X, Y, Z Offsets and click on OK.
3.
Choose menu path Utility Menu> PlotCtrls> Style> Hidden Line Options. The Hidden-Line Options dialog box appears.
4.
In the drop down menu for Type of Plot, select "Capped hidden."
5.
In the drop down menu for Cutting plane is, select "Working plane."
6.
Click on OK.
7.
Choose menu path Utility Menu> PlotCtrls> Pan-Zoom-Rotate. The Pan-Zoom-Rotate tool box appears.
8.
Click on "WP."
9.
Drag the Rate slider bar to 10.
10. On the Pan-Zoom-Rotate dialog box, click on the large round dot several times to zoom in on the cross section.
2.4.3.26. Exit ANSYS 1.
Choose QUIT from the ANSYS Toolbar.
2.
Choose Quit - No Save! Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–23
Chapter 2: Structural Static Analysis 3.
Click on OK.
2.5. A Sample Static Analysis (Command or Batch Method) You can perform the example static analysis of an Allen wrench using the ANSYS commands shown below instead of GUI choices. Items prefaced with an exclamation point (!) are comments. /FILNAME,pm02! Jobname to use for all subsequent files /TITLE,Static analysis of an Allen wrench /UNITS,SI ! Reminder that the SI system of units is used /SHOW ! Specify graphics driver for interactive run; for batch ! run plots are written to pm02.grph ! Define parameters for future use EXX=2.07E11 ! Young's modulus (2.07E11 Pa = 30E6 psi) W_HEX=.01 ! Width of hex across flats (.01m=.39in) *AFUN,DEG ! Units for angular parametric functions W_FLAT=W_HEX*TAN(30) ! Width of flat L_SHANK=.075 ! Length of shank (short end) (.075m=3.0in) L_HANDLE=.2 ! Length of handle (long end) (.2m=7.9 in) BENDRAD=.01 ! Bend radius of Allen wrench (.01m=.39 in) L_ELEM=.0075 ! Element length (.0075 m = .30 in) NO_D_HEX=2 ! Number of divisions on hex flat TOL=25E-6 ! Tolerance for selecting nodes (25e-6 m = .001 in) /PREP7 ET,1,SOLID45 ! Eight-node brick element ET,2,PLANE42 ! Four-node quadrilateral (for area mesh) MP,EX,1,EXX ! Young's modulus for material 1 MP,PRXY,1,0.3 ! Poisson's ratio for material 1 RPOLY,6,W_FLAT ! Hexagonal area K,7 ! Keypoint at (0,0,0) K,8,,,-L_SHANK ! Keypoint at shank-handle intersection K,9,,L_HANDLE,-L_SHANK ! Keypoint at end of handle L,4,1 ! Line through middle of hex shape L,7,8 ! Line along middle of shank L,8,9 ! Line along handle LFILLT,8,9,BENDRAD ! Line along bend radius between shank and handle /VIEW,,1,1,1 ! Isometric view in window 1 /ANGLE,,90,XM ! Rotates model 90 degrees about X /PNUM,LINE,1 ! Line numbers turned on LPLOT /PNUM,LINE,0 ! Line numbers off L,1,4 ! Hex section is cut into two quadrilaterals ASBL,1,7,,,KEEP ! to satisfy mapped meshing requirements for bricks CM,BOTAREA,AREA ! Component name BOTAREA for the two areas ! Generate area mesh for later drag LESIZE,1,,,NO_D_HEX ! Number of divisions along line 1 LESIZE,2,,,NO_D_HEX LESIZE,6,,,NO_D_HEX TYPE,2 ! PLANE42 elements to be meshed first MSHAPE,0,2D ! Mapped quad mesh MSHKEY,1 SAVE ! Save database before meshing AMESH,ALL /TITLE,Meshed hex wrench end to be used in vdrag EPLOT ! Now drag the 2-D mesh to produce 3-D elements TYPE,1 ! ESIZE,L_ELEM ! VDRAG,2,3,,,,,8,10,9 ! /TYPE,,HIDP ! /TITLE,Meshed hex wrench EPLOT CMSEL,,BOTAREA !
2–24
Type pointer set to SOLID45 Element size Drag operation to create 3-D mesh Precise hidden line display
Select BOTAREA component and
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.5: A Sample Static Analysis (Command or Batch Method) ACLEAR,ALL ASEL,ALL FINISH
!
delete the 2-D elements
! Apply loads and obtain the solution /SOLU ANTYPE,STATIC ! Static analysis (default) /TITLE,Allen wrench -- Load step 1 ! First fix all nodes around bottom of shank CMSEL,,BOTAREA ! Bottom areas of shank LSEL,,EXT ! Exterior lines of those areas NSLL,,1 ! Nodes on those lines D,ALL,ALL ! Displacement constraints LSEL,ALL /PBC,U,,1 ! Displacement symbols turned on /TITLE,Boundary conditions on end of wrench NPLOT !Now apply pressure on handle to represent 100-N (22.5-lb) finger force ASEL,,LOC,Y,BENDRAD,L_HANDLE ! Areas on handle ASEL,R,LOC,X,W_FLAT/2,W_FLAT ! Two areas on one side of handle... NSLA,,1 ! ...and all corresponding nodes NSEL,R,LOC,Y,L_HANDLE+TOL,L_HANDLE-(3.0*L_ELEM)-TOL ! Reselects nodes at ! back end of handle (3 element lengths) *GET,MINYVAL,NODE,,MNLOC,Y ! Get minimum Y value of selected nodes *GET,MAXYVAL,NODE,,MXLOC,Y ! Get maximum Y value of selected nodes PTORQ=100/(W_HEX*(MAXYVAL-MINYVAL)) ! Pressure equivalent to 100 N SF,ALL,PRES,PTORQ ! PTORQ pressure on all selected nodes ALLSEL ! Restores full set of all entities /PSF,PRES,,2 ! Pressure symbols turned on /TITLE,Boundary conditions on wrench for load step 1 NPLOT LSWRITE ! Writes first load step /TITLE, Allen wrench -- load step 2 ! Downward pressure on top of handle, representing 20-N (4.5 -lb) force PDOWN=20/(W_FLAT*(MAXYVAL-MINYVAL)) ASEL,,LOC,Z,-(L_SHANK+(W_HEX/2)) ! Area on top flat of handle... NSLA,,1 ! ...and all corresponding nodes NSEL,R,LOC,Y,L_HANDLE+TOL,L_HANDLE-(3.0*L_ELEM)-TOL ! Reselects nodes at ! back end of handle (3 element lengths) SF,ALL,PRES,PDOWN ! PDOWN pressure at all selected nodes ALLSEL /TITLE,Boundary conditions on wrench for load step 2 NPLOT LSWRITE ! Writes second load step SAVE ! Save database before solution LSSOLVE,1,2 ! Initiates solution for load step files 1 and 2 FINISH !Review the results /POST1 SET,1 ! Reads load step 1 results PRRSOL ! Reaction solution listing /PBC,DEFA ! No BC symbols /PSF,DEFA ! No surface load symbols /EDGE,,1 ! Edges only, no interior element outlines /TITLE,Deformed allen wrench caused by torque PLDISP,2 ! Deformed shape overlaid with undeformed edge plot /GSAVE,pldisp,gsav ! Saves graphics specifications on pldisp.gsav /PLOPTS,INFO,ON ! Turns on entire legend column /PLOPTS,LEG1,OFF ! Turns off legend header /ANGLE,,120,YM,1 ! Additional rotation about model Y (to see high stress areas) /TITLE,Stress intensity contours caused by torque PLNSOL,S,INT ! Stress intensity contours
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–25
Chapter 2: Structural Static Analysis /GSAVE,plnsol,gsav ! Saves graphics specifications to plnsol.gsav SET,2 ! Reads load step 2 results PRRSOL ! Reaction solution listing /GRESUME,pldisp,gsav ! Resumes graphics specifications from pldisp.gsav /TITLE,Deformed allen wrench caused by torque and force PLDISP,2 /GRESUME,plnsol,gsav ! Resumes graphics specifications from plnsol.gsav /TITLE,Stress intensity contours caused by torque and force PLNSOL,S,INT WPOF,,,-0.067 ! Offset the working plane for cross-section view /TYPE,1,5 ! Capped hidden display /CPLANE,1 ! Cutting plane defined to use the WP /VIEW, 1 ,WP ! View will be normal to the WP /DIST,1,.01 ! Zoom in on the cross section /TITLE,Cross section of the allen wrench under torque and force loading PLNSOL,S,INT FINISH /EXIT,ALL
2.6. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual and the ANSYS Tutorials, describe additional structural static analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS family of products. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual includes the following structural static analysis test cases: VM1 - Statically Indeterminate Reaction Force Analysis VM2 - Beam Stresses and Deflections VM4 - Deflection of a Hinged Support VM11 - Residual Stress Problem VM12 - Combined Bending and Torsion VM13 - Cylindrical Shell Under Pressure VM16 - Bending of a Solid Beam VM18 - Out-of-plane Bending of a Curved Bar VM20 - Cylindrical Membrane Under Pressure VM25 - Stresses in a Long Cylinder VM29 - Friction on a Support Block VM31 - Cable Supporting Hanging Loads VM36 - Limit Moment Analysis VM39 - Bending of a Circular Plate with a Center Hole VM41 - Small Deflection of a Rigid Beam VM44 - Bending of an Axisymmetric Thin Pipe Under Gravity Loading VM53 - Vibration of a String Under Tension VM59 - Lateral Vibration of an Axially Loaded Bar VM63 - Static Hertz Contact Problem VM78 - Transverse Shear Stresses in a Cantilever Beam VM82 - Simply Supported Laminated Plate Under Pressure VM127 - Buckling of a Bar with Hinged Ends VM135 - Bending of a Beam on an Elastic Foundation VM141 - Diametric Compression of a Disk VM148 - Bending of a Parabolic Beam VM183 - Harmonic Response of a Spring-Mass System 2–26
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.6: Where to Find Other Examples VM199 - Viscoplastic Analysis of a Body Undergoing Shear Deformation VM201 - Rubber Cylinder Pressed Between Two Plates VM206 - Stranded Coil with Voltage Excitation VM211 - Rubber Cylinder Pressed Between Two Plates VM216 - Lateral Buckling of a Right-Angle Frame
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–27
2–28
Chapter 3: Modal Analysis 3.1. Definition of Modal Analysis You use modal analysis to determine the vibration characteristics (natural frequencies and mode shapes) of a structure or a machine component while it is being designed. It also can be a starting point for another, more detailed, dynamic analysis, such as a transient dynamic analysis, a harmonic response analysis, or a spectrum analysis.
3.2. Uses for Modal Analysis You use modal analysis to determine the natural frequencies and mode shapes of a structure. The natural frequencies and mode shapes are important parameters in the design of a structure for dynamic loading conditions. They are also required if you want to do a spectrum analysis or a mode superposition harmonic or transient analysis. You can do modal analysis on a prestressed structure, such as a spinning turbine blade. Another useful feature is modal cyclic symmetry, which allows you to review the mode shapes of a cyclically symmetric structure by modeling just a sector of it. Modal analysis in the ANSYS family of products is a linear analysis. Any nonlinearities, such as plasticity and contact (gap) elements, are ignored even if they are defined. You can choose from several mode-extraction methods: Block Lanczos (default), subspace, PowerDynamics, reduced, unsymmetric, damped, and QR damped. The damped and QR damped methods allow you to include damping in the structure. Details about mode-extraction methods are covered later in this section.
3.3. Overview of Steps in a Modal Analysis The procedure for a modal analysis consists of four main steps: 1.
Build the model.
2.
Apply loads and obtain the solution.
3.
Expand the modes.
4.
Review the results.
3.4. Build the Model See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details, see the ANSYS Modeling and Meshing Guide. When building your model, remember these points: •
Only linear behavior is valid in a modal analysis. If you specify nonlinear elements, they are treated as linear. For example, if you include contact elements, their stiffnesses are calculated based on their initial status and never change.
•
Material properties can be linear, isotropic or orthotropic, and constant or temperature-dependent. You must define both Young's modulus (EX) (or stiffness in some form) and density (DENS) (or mass in some form) for a modal analysis. Nonlinear properties are ignored. If applying element damping, you must define the required real constants for the specific element type (COMBIN7, COMBIN14, COMBIN37, and so on). Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 3: Modal Analysis
3.5. Apply Loads and Obtain the Solution In this step you define the analysis type and options, apply loads, specify load step options, and begin the finite element solution for the natural frequencies.
3.5.1. Enter the Solution Processor 1.
Enter the ANSYS solution processor. Command(s): /SOLU GUI: Main Menu> Solution
3.5.2. Define Analysis Type and Options After you have entered the solution processor, you define the analysis type and analysis options. ANSYS offers the options listed in Table 3.1: “Analysis Types and Options” for a modal analysis. Each of the options is explained in detail below.
Table 3.1 Analysis Types and Options Option
Command
GUI Path
New Analysis
ANTYPE
Main Menu> Solution> Analysis Type> New Analysis
Analysis Type: Modal (see Note below)
ANTYPE
Main Menu> Solution> Analysis Type> New Analysis> Modal
mode-extraction Method
MODOPT
Main Menu> Solution> Analysis Type> Analysis Options
Number of Modes to Extract
MODOPT
Main Menu> Solution> Analysis Type> Analysis Options
No. of Modes to Expand (see Note below) MXPAND
Main Menu> Solution> Analysis Type> Analysis Options
Mass Matrix Formulation
LUMPM
Main Menu> Solution> Analysis Type> Analysis Options
Prestress Effects Calculation
PSTRES
Main Menu> Solution> Analysis Type> Analysis Options
Note — When you specify a modal analysis, a Solution menu that is appropriate for modal analyses appears. The Solution menu will be either “abridged” or “unabridged,” depending on the actions you took prior to this step in your ANSYS session. The abridged menu contains only those solution options that are valid and/or recommended for modal analyses. If you are on the abridged Solution menu and you want to access other solution options (that is, solution options that are valid for you to use, but their use may not be encouraged for this type of analysis), select the Unabridged Menu option. For details, see Section 3.11.1: Using Abridged Solution Menus in the ANSYS Basic Analysis Guide. Note — In the single point response spectrum (SPOPT,SPRS) and Dynamic Design analysis method (SPOPT,DDAM), the modal expansion can be performed after the spectrum analysis, based on the significance factor SIGNIF on the MXPAND command. If you want to perform modal expansion after the spectrum analysis, choose NO for mode expansion (MXPAND) on the dialog box for the modal analysis options (MODOPT).
3.5.2.1. Option: New Analysis [ANTYPE] Choose New Analysis. Note — Restarts are not valid in a modal analysis. If you need to apply different sets of boundary conditions, do a new analysis each time (or use the "partial solution" procedure described in Chapter 3, “Solution” in the ANSYS Basic Analysis Guide). 3–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.5: Apply Loads and Obtain the Solution
3.5.2.2. Option: Analysis Type: Modal [ANTYPE] Use this option to specify a modal analysis.
3.5.2.3. Option: Mode-Extraction Method [MODOPT] Choose one of the extraction methods listed below. (For more detailed information, see Section 3.13: Comparing Mode-Extraction Methods.) •
Block Lanczos method (default) The Block Lanczos method is used for large symmetric eigenvalue problems. You can use this method for the same types of problems for which you use the subspace method, but you achieve a faster convergence rate. The Block Lanczos method uses the sparse matrix solver, overriding any solver specified via the EQSLV command.
•
Subspace method The subspace method is used for large symmetric eigenvalue problems. Several solution controls are available to control the subspace iteration process. When doing a modal analysis with a large number of constraint equations, use the subspace method with the frontal solver instead of the JCG solver, or use the Block Lanczos mode-extraction method.
•
PowerDynamics method The PowerDynamics method is used for very large models (100,000+ DOFs), and is especially useful to obtain a solution for the first several modes to learn how the model will behave. You can then choose the most appropriate extraction method (subspace or Block Lanczos) for running the final solution. This method automatically uses the lumped mass approximation (LUMPM,ON) To use the PowerDynamics method when running in batch or command mode, you first issue MODOPT,SUBSPACE, followed by EQSLV,PCG. (The PCGOUT solver can also be used, but it is very slow.)
•
Reduced (Householder) method The reduced method is faster than the subspace method because it uses reduced (condensed) system matrices to calculate the solution. However, it is less accurate because the reduced mass matrix is approximate. (See Section 3.13: Comparing Mode-Extraction Methods.)
•
Unsymmetric method The unsymmetric method is used for problems with unsymmetric matrices, such as fluid-structure interaction problems.
•
Damped method The damped method is used for problems where damping cannot be ignored, such as bearing problems.
•
QR Damped method The QR damped method is faster and achieves better calculation efficiency than the damped method. It uses the reduced modal damped matrix to calculate complex damped frequencies in modal coordinates.
For most applications, you will use the Block Lanczos, subspace, reduced, or PowerDynamics method. The unsymmetric, damped, and QR damped methods are meant for special applications. When you specify a mode-extraction method, ANSYS automatically chooses the appropriate equation solver. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–3
Chapter 3: Modal Analysis Note — The damped, unsymmetric, and QR damped methods are not available in the ANSYS Professional program.
3.5.2.4. Option: Number of Modes to Extract [MODOPT] This option is required for all mode-extraction methods except the reduced method. For the unsymmetric and damped methods, requesting a larger number of modes than necessary reduces the possibility of missed modes, but results in more solution time.
3.5.2.5. Option: Number of Modes to Expand [MXPAND] This option is required for the reduced, unsymmetric, and damped methods only. However, if you want element results, you need to turn on the "Calculate elem results" option, regardless of the mode-extraction method. In the single point response spectrum (SPOPT,SPRS) and Dynamic Design analysis method (SPOPT,DDAM), the modal expansion can be performed after the spectrum analysis, based on the significance factor SIGNIF on the MXPAND command. If you want to perform modal expansion after the spectrum analysis, choose NO for mode expansion (MXPAND) on the dialog box for the modal analysis options (MODOPT). If you want the mode shapes normalized to unity for the Block Lanczos or subspace methods, you will need to expand the modes as well.
3.5.2.6. Option: Mass Matrix Formulation [LUMPM] Use this option to specify the default formulation (which is element-dependent) or lumped mass approximation. We recommend the default formulation for most applications. However, for some problems involving "skinny" structures such as slender beams or very thin shells, the lumped mass approximation often yields better results. Also, the lumped mass approximation can result in a shorter run time and lower memory requirements.
3.5.2.7. Option: Prestress Effects Calculation [PSTRES] Use this option to calculate the modes of a prestressed structure. By default, no prestress effects are included; that is, the structure is assumed to be stress-free. To include prestress effects, element files from a previous static (or transient) analysis must be available; see Section 3.11: Prestressed Modal Analysis. If prestress effects are turned on, the lumped mass setting [LUMPM] in this and subsequent solutions must be the same as it was in the prestress static analysis. Note — You can use only axisymmetric loads for prestressing harmonic elements such as PLANE25 and SHELL61.
3.5.2.8. Additional Modal Analysis Options After you complete the fields on the Modal Analysis Options dialog box, click OK. A dialog box specific to the selected extraction method appears. You see some combination of the following fields: FREQB, FREQE, PRMODE, Nrmkey, RIGID, SUBOPT. Refer to the MODOPT and RIGID command descriptions for the meaning of these fields.
3.5.3. Define Master Degrees of Freedom In a modal analysis, you also need to define master degrees of freedom. These are required only for the reduced mode-extraction method. Master degrees of freedom (MDOF) are significant degrees of freedom that characterize the dynamic behavior of the structure. You should choose at least twice as many MDOF as the number of modes of interest. We recommend that you define as many MDOF as you can based on your knowledge of the dynamic characteristics of the 3–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.5: Apply Loads and Obtain the Solution structure [M,MGEN], and also let the program choose a few additional masters based on stiffness-to-mass ratios [TOTAL]. You can list the defined MDOF [MLIST], and delete extraneous MDOF [MDELE]. For more details about master degrees of freedom, see Section 3.14: Matrix Reduction. Command(s): M GUI: Main Menu> Solution> Master DOFs> User Selected> Define
3.5.4. Apply Loads After defining master degrees of freedom, apply loads on the model. The only "loads" valid in a typical modal analysis are zero-value displacement constraints. (If you input a nonzero displacement constraint, the program assigns a zero-value constraint to that DOF instead.) Other loads can be specified, but are ignored (see Note below). For directions in which no constraints are specified, the program calculates rigid-body (zero-frequency) as well as higher (nonzero frequency) free body modes. Table 3.2: “Loads Applicable in a Modal Analysis” shows the commands to apply displacement constraints. Notice that you can apply them either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). For a general discussion of solid-model loads versus finite-element loads, see Chapter 2, “Loading” in the ANSYS Basic Analysis Guide. Note — Other loads - forces, pressures, temperatures, accelerations, and so on - can be specified in a modal analysis, but they are ignored for the mode-extraction. However, the program will calculate a load vector and write it to the mode shape file (Jobname.MODE) so that it can be used in a subsequent modesuperposition harmonic or transient analysis.
Table 3.2 Loads Applicable in a Modal Analysis Load Type
Category
Cmd Family
Displacement (UX, UY, UZ, ROTX, Constraints D ROTY, ROTZ)
GUI Path Main Menu> Solution> Define Loads> Apply> Structural> Displacement
In an analysis, loads can be applied, removed, operated on, or listed.
3.5.4.1. Applying Loads Using Commands Table 3.3: “Load Commands for a Modal Analysis” lists all the commands you can use to apply loads in a modal analysis.
Table 3.3 Load Commands for a Modal Analysis Load Type Displacement
Solid Model or FE
Entity
Apply
Delete
List
Operate
Apply Settings
Solid Model
Keypoints
DK
DKDELE
DKLIST
DTRAN
-
Solid Model
Lines
DL
DLDELE
DLLIST
DTRAN
-
Solid Model
Areas
DA
DADELE
DALIST
DTRAN
-
Finite Elem
Nodes
D
DDELE
DLIST
DSCALE
DSYM, DCUM
3.5.4.2. Applying Loads Using the GUI All loading operations (except List; see Section 3.5.4.3: Listing Loads) are accessed through a series of cascading menus. From the Solution menu, you select the operation (apply, delete, and so on), then the load type (displacement, force, and so on), and then the object to which you are applying the load (keypoint, line, node, and so on).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–5
Chapter 3: Modal Analysis For example, to apply a displacement load to a line, follow this GUI path: GUI: Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On lines
3.5.4.3. Listing Loads To list existing loads, follow this GUI path: GUI: Utility Menu> List>Loads> load type
3.5.5. Specify Load Step Options The only load step options available for a modal analysis are damping options.
Table 3.4 Load Step Options Option
Command
Damping (Dynamics) Options Alpha (mass) Damping
ALPHAD
Beta (stiffness) Damping
BETAD
Material-Dependent Damping Ratio
MP,DAMP
Element Damping (applied via element real constant) R Constant Material Damping Coefficient
MP,DMPR
Damping is valid only for the damped and QR damped mode-extraction methods. Damping is ignored for the other mode-extraction methods; see the Note below. If you include damping and specify the damped mode-extraction method, the calculated eigenvalues and eigenvectors are complex. If you include damping and specify the QR damped mode-extraction method, the eigenvalues are complex. However, the real eigenvectors are used for the mode superposition analysis. See Section 3.13: Comparing Mode-Extraction Methods for details. Also see the section Section 5.10.3: Damping in Chapter 5, “Transient Dynamic Analysis” for more information on damping. Only the QR damped method supports the constant material damping coefficient application in a downstream mode superposition harmonic analysis. The QR damped eigen analysis itself, however, does not include the effect of the constant material damping coefficient. The corresponding modal damping matrix is formulated during modal harmonic analysis. Note — Damping can be specified in a non-damped modal analysis if a single-point response spectrum analysis is to follow the modal analysis. Although the damping does not affect the eigenvalue solution, it is used to calculate an effective damping ratio for each mode, which is then used to calculate the response to the spectrum. Spectrum analyses are discussed in Chapter 6, “Spectrum Analysis”.
3.5.6. Participation Factor Table Output The participation factor table lists participation factors, mode coefficients, and mass distribution percentages for each mode extracted. The participation factors and mode coefficients are calculated based on an assumed unit displacement spectrum in each of the global Cartesian directions and rotation about each of these axes.
3–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.5: Apply Loads and Obtain the Solution The reduced mass distribution is also listed. Rotational participation factors will be calculated when a real eigensolver mode-extraction method (such as Block Lanczos, subspace, or QRDAMP) is used. Note — You can retrieve a participation factor or mode coefficient by issuing a *GET command. The factor or coefficient is valid for the excitation (assumed unit displacement spectrum) directed along the last of the applicable coordinates (rotation about the Z axis for a 3-D analysis). To retrieve a participation factor or mode coefficient for another direction, perform a spectrum analysis with the excitation set (SED) to the desired direction, then issue another *GET command.
3.5.7. Solve Before you solve, you should save (SAVE) a back-up copy of the database to a named file. You can then retrieve your model by reentering the ANSYS program and issuing RESUME. Now start the solution calculations. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
3.5.7.1. Output The output from the solution consists mainly of the natural frequencies, which are printed as part of the printed output (Jobname.OUT) and also written to the mode shape file (Jobname.MODE). The printed output may include reduced mode shapes and the participation factor table, depending on your analysis options and output controls. No mode shapes are written to the database or to the results file, so you cannot postprocess the results yet. To do this, you need to expand the modes (explained next).
3.5.7.1.1. Output From Subspace Mode-Extraction Method If you use the subspace mode-extraction method, you might see the following warning in the solution printout: "STURM number = n should be m," where n and m are integer numbers. This indicates that a mode has been missed, or that the mthand nth mode gave the same frequencies and only m modes were requested. There are two methods that you can use to investigate the missed mode: use more iteration vectors, or change the shift point used in the eigenvalue extraction. Both methods are briefly described below. (See the ANSYS, Inc. Theory Reference for more information.) To use more iteration vectors, you can issue the SUBOPT,,NPAD command. If you prefer to use the GUI to adjust the number of iteration vectors, follow these steps: 1.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Modal Analysis dialog box appears.
2.
Choose “Subspace” as the mode-extraction method and specify the number of modes to extract; then click OK. The Subspace Modal Analysis dialog box appears.
3.
Change the value of the NPAD field and click OK.
To change the shift point that was used in the eigenvalue extraction, you can issue the MODOPT,,,FREQB command. If you prefer to use the GUI to change the shift point, follow these steps: 1.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Modal Analysis dialog box appears.
2.
Choose “Subspace” as the mode-extraction method and specify the number of modes to extract; then click OK. The Subspace Modal Analysis dialog box appears. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–7
Chapter 3: Modal Analysis 3.
Change the value of the FREQB field and click OK.
If you use the damped mode-extraction method, the eigenvalues and eigenvectors are complex. The imaginary part of the eigenvalue represents the natural frequency, and the real part is a measure of the stability of the system. If you use the QR damped mode-extraction method, the eigenvalues are complex. However, the real eigenvectors are used for the mode superposition analysis.
3.5.8. Exit the Solution Processor You must now exit the solution processor. Command(s): FINISH GUI: Main Menu> Finish
3.6. Expand the Modes In its strictest sense, the term "expansion" means expanding the reduced solution to the full DOF set. The "reduced solution" is usually in terms of master DOF. In a modal analysis, however, we use the term "expansion" to mean writing mode shapes to the results file. That is, "expanding the modes" applies not just to reduced mode shapes from the reduced mode-extraction method, but to full mode shapes from the other mode-extraction methods as well. Thus, if you want to review mode shapes in the postprocessor, you must expand them (that is, write them to the results file). Expanded modes are also required for subsequent spectrum analyses. In the single point response spectrum (SPOPT,SPRS) and Dynamic Design analysis method (SPOPT,DDAM), the modal expansion can be performed after the spectrum analysis, based on the significance factor SIGNIF on the MXPAND command. If you want to perform modal expansion after the spectrum analysis, choose NO for mode expansion (MXPAND) on the dialog box for the modal analysis options (MODOPT). No expansion is necessary for subsequent mode superposition analyses.
3.6.1. Points to Remember •
The mode shape file (Jobname.MODE), Jobname.EMAT, Jobname.ESAV, and Jobname.TRI (if reduced method) must be available.
•
The database must contain the same model for which the modal solution was calculated.
3.6.2. Expanding the Modes 1.
Reenter the ANSYS solution processor. Command(s): /SOLU GUI: Main Menu> Solution Note — You must explicitly leave SOLUTION (using the FINISH command) and reenter (/SOLU) before performing the expansion pass.
2.
Activate the expansion pass and its options. ANSYS offers these options for the expansion pass:
Table 3.5 Expansion Pass Options Option Expansion Pass On/Off
Command EXPASS
No. of Modes to Expand MXPAND
3–8
GUI Path Main Menu> Solution> Analysis Type> ExpansionPass Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> Expand Modes
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.6: Expand the Modes Option
Command
GUI Path
Freq. Range for Expansion MXPAND
Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> Expand Modes
MXPAND
Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> Expand Modes
Stress Calc. On/Off
Each of these options is explained in detail below. Expansion Pass On/Off [EXPASS] Choose ON. Number of Modes to Expand [MXPAND, NMODE] Specify the number. Remember that only expanded modes can be reviewed in the postprocessor. Default is no modes expanded. Frequency Range for Expansion [MXPAND,, FREQB, FREQE] This is another way to control the number of modes expanded. If you specify a frequency range, only modes within that range are expanded. Stress Calculations On/Off [MXPAND,,,, Elcalc] Choose ON only if you plan to do a subsequent spectrum analysis and are interested in stresses or forces to do the spectrum. "Stresses" from a modal analysis do not represent actual stresses in the structure, but give you an idea of the relative stress distributions for each mode. Default is no stresses calculated. 3.
Specify load step options. The only options valid in a modal expansion pass are output controls: •
Printed output Use this option to include any results data (expanded mode shapes, stresses, and forces) on the printed output file (Jobname.OUT). Command(s): OUTPR GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout
•
Database and results file output Use this option to control the data on the results file (Jobname.RST). The FREQ field on OUTRES can be only ALL or NONE; that is, the data are written for all modes or no modes. For example, you cannot write information for every other mode. Command(s): OUTRES GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> DB/Results File
4.
Start expansion pass calculations. The output consists of expanded mode shapes and, if requested, relative stress distributions for each mode. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
5.
Repeat steps 2, 3, and 4 for additional modes to be expanded (in different frequency ranges, for example). Each expansion pass is stored as a separate load step on the results file.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–9
Chapter 3: Modal Analysis Caution: Spectrum analyses expect all expanded modes to be in one load step. In the single point response spectrum (SPOPT,SPRS) and Dynamic Design analysis method (SPOPT,DDAM), the modal expansion can be performed after the spectrum analysis, based on the significance factor SIGNIF on the MXPAND command. If you want to perform modal expansion after the spectrum analysis, choose NO for mode expansion (MXPAND) on the dialog box for the modal analysis options (MODOPT). 6.
Leave SOLUTION. You can now review results in the postprocessor. Command(s): FINISH GUI: Close the Solution menu.
Note — The expansion pass has been presented here as a separate step. However, if you include the MXPAND command in the modal solution step, the program not only extracts the eigenvalues and eigenvectors, but also expands the specified mode shapes.
3.7. Review the Results Results from a modal analysis (that is, the modal expansion pass) are written to the structural results file, Jobname.RST. Results consist of: •
Natural frequencies
•
Expanded mode shapes
•
Relative stress and force distributions (if requested).
You can review these results in POST1 [/POST1], the general postprocessor. Some typical postprocessing operations for a modal analysis are described below. For a complete description of all postprocessing functions, see Chapter 4, “An Overview of Postprocessing” in the ANSYS Basic Analysis Guide.
3.7.1. Points to Remember •
If you want to review results in POST1, the database must contain the same model for which the solution was calculated.
•
The results file (Jobname.RST) must be available.
3.7.2. Reviewing Results Data 1.
Read in results data from the appropriate substep. Each mode is stored on the results file as a separate substep. If you expand six modes, for instance, your results file will have one load step consisting of six substeps. Command(s): SET,SBSTEP GUI: Main Menu> General Postproc> Read Results> substep
2.
Perform any desired POST1 operations. Typical modal analysis POST1 operations are explained below:
3.7.3. Option: Listing All Frequencies You may want to list the frequencies of all modes expanded. A sample output from this command is shown below. ***** INDEX OF DATA SETS ON RESULTS FILE ***** SET TIME/FREQ LOAD STEP SUBSTEP CUMULATIVE 1 22.973 1 1 1 2 40.476 1 2 2
3–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.7: Review the Results 3 4
78.082 188.34
1 1
3 4
3 4
Command(s): SET,LIST GUI: Main Menu> General Postproc> List Results
3.7.4. Option: Display Deformed Shape Command(s): PLDISP GUI: Main Menu> General Postproc> Plot Results> Deformed Shape Use the KUND field on PLDISP to overlay the nondeformed shape on the display.
3.7.5. Option: List Master DOF Command(s): MLIST,ALL GUI: Main Menu> Solution> Master DOFs> User Selected> List All Note — To display the master DOFs graphically, plot the nodes (Utility Menu> Plot> Nodes or command NLIST).
3.7.6. Option: Line Element Results Command(s): ETABLE GUI: Main Menu> General Postproc> Element Table> Define Table For line elements, such as beams, spars, and pipes, use the ETABLE command to access derived data (stresses, strains, and so on). Results data are identified by a combination of a label and a sequence number or component name on the ETABLE command. See the ETABLE discussion in The General Postprocessor (POST1) in the ANSYS Basic Analysis Guide for details.
3.7.7. Option: Contour Displays Command(s): PLNSOL or PLESOL GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu Use these options to contour almost any result item, such as stresses (SX, SY, SZ...), strains (EPELX, EPELY, EPELZ...), and displacements (UX, UY, UZ...). The KUND field on PLNSOL and PLESOL gives you the option of overlaying the nondeformed shape on the display. You can also contour element table data and line element data: Command(s): PLETAB, PLLS GUI: Main Menu> General Postproc> Element Table> Plot Element Table Main Menu> General Postproc> Plot Results> Contour Plot> Line Elem Res Caution: Derived data, such as stresses and strains, are averaged at the nodes by the PLNSOL command. This averaging results in "smeared" values at nodes where elements of different materials, different shell thicknesses, or other discontinuities meet. To avoid the smearing effect, use selecting (described in Chapter 7, “Selecting and Components” in the ANSYS Basic Analysis Guide) to select elements of the same material, same shell thickness, and so on before issuing PLNSOL.
3.7.8. Option: Tabular Listings Command(s): PRNSOL (nodal results) PRESOL (element-by-element results) PRRSOL (reaction data), and so on NSORT, ESORT GUI: Main Menu> General Postproc> List Results> solution option Main Menu> General Postproc> List Results> Sorted Listing> Sort Nodes Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–11
Chapter 3: Modal Analysis Main Menu> General Postproc> List Results> Sorted Listing> Sort Elems Use the NSORT and ESORT commands to sort the data before listing them.
3.7.9. Other Capabilities Many other postprocessing functions - mapping results onto a path, load case combinations, and so on - are available in POST1. See The General Postprocessor (POST1) in the ANSYS Basic Analysis Guide for details. See the ANSYS Commands Reference for a discussion of the ANTYPE, MODOPT, M, TOTAL, EXPASS, MXPAND, SET, and PLDISP commands.
3.8. A Sample Modal Analysis (GUI Method) In this example, you perform a modal analysis on the wing of a model plane to demonstrate the wing's modal degrees of freedom.
3.8.1. Problem Description This is a modal analysis of a wing of a model plane. The wing is of uniform configuration along its length, and its cross-sectional area is defined to be a straight line and a spline, as shown. It is held fixed to the body on one end and hangs freely at the other. The objective of the problem is to demonstrate the wing's modal degrees of freedom.
3.8.2. Problem Specifications The dimensions of the wing are shown in the problem sketch. The wing is made of low density polyethylene with the following values: Young's modulus = 38x103 psi Poisson's ratio = .3 Density = 8.3e-5 lb-sec2/in4
3.8.3. Problem Sketch Figure 3.1 Diagram of a Model Airplane Wing
3–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.9: A Sample Modal Analysis (Command or Batch Method) The detailed step-by-step procedure for this example, Modal Analysis of a Model Airplane Wing, is included in the Modal Tutorial.
3.9. A Sample Modal Analysis (Command or Batch Method) You can perform the example modal analysis of a model airplane wing using the ANSYS commands shown below instead of GUI choices. Items prefaced with an exclamation point (!) are comments. You may receive warning messages when you run this problem. The version of the problem that appears in the Modal Tutorial contains an explanation of the warnings. /FILNAM,MODAL /TITLE,Modal Analysis of a Model Airplane Wing /PREP7 ET,1,PLANE42 ! Define PLANE42 as element type ET,2,SOLID45 ! Define SOLID45 as element type MP,EX,1,38000 MP,DENS,1,8.3E-5 MP,NUXY,1,.3 K,1 ! Define keypoint 1 at 0,0,0 K,2,2 ! Define keypoint 2 at 2,0,0 K,3,2.3,.2 ! Define keypoint 3 at 2.3,.2,0 K,4,1.9,.45 ! Define keypoint 4 at 1.9,.45,0 K,5,1,.25 ! Define keypoint 5 at 1,.25,0 LSTR,1,2 ! Create a straight line between LSTR,5,1 ! Create a straight line between BSPLIN,2,3,4,5,,,-1,,,-1,-.25 ! Create a B-spline AL,1,3,2 ESIZE,.25 AMESH,1 ESIZE,,10 TYPE,2 VEXT,ALL,,,,,10 /VIEW,,1,1,1 /ANG,1 /REP EPLOT FINISH /SOLU ANTYPE,MODAL MODOPT,SUBSP,5 ESEL,U,TYPE,,1 NSEL,S,LOC,Z,0 D,ALL,ALL NSEL,ALL MXPAND,5 SOLVE FINISH
! ! ! !
1 2
keypoints 1 and 2 keypoints 5 and 1
Choose modal analysis type Choose the subspace mode-extraction method, extracting 5 modes Unselect element type 1
/POST1 SET,LIST,2 SET,FIRST PLDISP,0 ANMODE,10,.5E-1 SET,NEXT PLDISP,0 ANMODE,10,.5E-1 SET,NEXT PLDISP,0 ANMODE,10,.5E-1 SET,NEXT PLDISP,0 ANMODE,10,.5E-1 SET,NEXT PLDISP,0 ANMODE,10,.5E-1 Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–13
Chapter 3: Modal Analysis FINISH /EXIT
3.10. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional modal analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS family of products. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual includes variety of modal analysis test cases: VM45 - Natural Frequency of a Spring-mass System VM47 - Torsional Frequency of a Suspended Disk VM48 - Natural Frequency of a Motor-generator VM50 - Fundamental Frequency of a Simply Supported Beam VM52 - Automobile Suspension System Vibrations VM53 - Vibration of a String Under Tension VM54 - Vibration of a Rotating Cantilever Blade VM55 - Vibration of a Stretched Circular Membrane VM57 - Torsional Frequencies of a Drill Pipe VM59 - Lateral Vibration of an Axially-loaded Bar VM60 - Natural Frequency of a Cross-ply Laminated Spherical Shell VM61 - Longitudinal Vibration of a Free-free Rod VM62 - Vibration of a Wedge VM66 - Vibration of a Flat Plate VM67 - Radial Vibrations of a Circular Ring from an Axisymmetric Model VM68 - PSD Response of a Two DOF Spring-mass System VM69 - Seismic Response VM70 - Seismic Response of a Beam Structure VM76 - Harmonic Response of a Guitar String VM89 - Natural Frequencies of a Two-mass-spring System VM151 - Nonaxisymmetric Vibration of a Circular Plate VM152 - Nonaxisymmetric Vibration of a Stretched Circular Membrane (Harmonic Els) VM153 - Nonaxisymmetric Vibration of a Stretched Circular Membrane (Modal) VM154 - Vibration of a Fluid Coupling VM175 - Natural Frequency of a Piezoelectric Transducer VM181 - Natural Frequency of a Flat Circular Plate with a Clamped Edge VM182 - Transient Response of a Spring-mass System VM183 - Harmonic Response of a Spring-mass System VM202 - Transverse Vibrations of a Shear Beam VM203 - Dynamic Load Effect on Simply-supported Thick Square Plate VM212 - Modal Analysis of a Rectangular Cavity
3.11. Prestressed Modal Analysis Use a prestressed modal analysis to calculate the frequencies and mode shapes of a prestressed structure, such as a spinning turbine blade. The procedure to do a prestressed modal analysis is essentially the same as a regular modal analysis, except that you first need to prestress the structure by doing a static analysis:
3–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.12: Prestressed Modal Analysis of a Large-Deflection Solution 1.
Build the model and obtain a static solution with prestress effects turned on [PSTRES,ON]. The same lumped mass setting [LUMPM] used here must also be used in the later prestress modal analysis. Chapter 2, “Structural Static Analysis” describes the procedure to obtain a static solution.
2.
Reenter SOLUTION and obtain the modal solution, also with prestress effects turned on (reissue PSTRES,ON). Files Jobname.EMAT (if ANSYS creates it) and Jobname.ESAV from the static analysis must be available. If the model is spinning, include spin-softening effects (via the OMEGA command's KSPIN option) if necessary.
3.
Expand the modes and review them in the postprocessor.
Step 1 above can also be a transient analysis. In such a case, save the EMAT and ESAV files at the desired time point. If the deformed shape from the static solution differs significantly from its nondeformed shape, you can perform a prestressed modal analysis of a large-deflection solution instead.
3.12. Prestressed Modal Analysis of a Large-Deflection Solution You can also perform a prestressed modal analysis following a large deflection (NLGEOM,ON) static analysis in order to calculate the frequencies and mode shapes of a highly deformed structure. Use the prestressed modal analysis procedure, but use the PSOLVE command (rather than the SOLVE command) to obtain the modal solution, as shown in the sample input listing below. Along with the PSOLVE command, you must issue the UPCOORD command to update the coordinates necessary for obtaining the correct stresses. This procedure uses the element matrices and element load vectors (for example, from pressures, temperature or acceleration loads) from a previous static analysis. These loads will be passed through to a subsequent mode superposition analysis if specified (LVSCALE command). Prestress must be applied (PSTRES,ON) during the static portion of the analysis. However, in cases where stressstiffening helps convergence: •
Stress-stiffening (SSTIF,ON) must be applied instead. (This requirement applies to elements outside of the 18x family of elements only.)
•
The EMATWRITE,YES command is also necessary to write the element matrices to File.EMAT.
Issuing either a PSTRES,OFF or SSTIF,OFF command prevents all previously specified prestressing from being applied. If the model is spinning, include spin-softening effects (via the OMEGA command's KSPIN option) in the modal solution if necessary. ! Initial, large deflection static analysis ! /PREP7 ... FINISH /SOLU ANTYPE,STATIC ! Static analysis NLGEOM,ON ! Large deflection analysis PSTRES,ON ! Flag to calculate the prestress matrix ... SOLVE FINISH ! ! Prestressed modal analysis ! Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–15
Chapter 3: Modal Analysis /SOLU ANTYPE,MODAL UPCOORD,1.0,ON PSTRES,ON MODOPT,... MXPAND,... PSOLVE,EIGxxxx FINISH /SOLU EXPASS,ON PSOLVE,EIGEXP
! ! ! ! ! ! ! !
Modal analysis Display mode shapes relative to deformed geometry in the postprocessor. Prestress effects ON Select eigensolver Specify the number of modes to expand, if desired. Calculate the eigenvalues and eigenvectors. Use EIGLANB or EIGFULL to match MODOPT command.
!Additional solution step for expansion. ! Expand the eigenvector solution. (Required if you ! want to review mode shapes in the postprocessor.)
FINISH
Note — You may also use one of the other eigensolvers (PSOLVE,EIGSYM, PSOLVE,EIGUNSY, PSOLVE,EIGDAMP or PSOLVE,EIGREDUC). In such a case, a PSOLVE,TRIANG command must precede the PSOLVE,EIGxxx command.
3.13. Comparing Mode-Extraction Methods The basic equation solved in a typical undamped modal analysis is the classical eigenvalue problem:
[K ]{φ i} = ω2i [M]{φ i} where: [K] = stiffness matrix {Φi} = mode shape vector (eigenvector) of mode i ω2 Ωi = natural circular frequency of mode i ( i is the eigenvalue) [M] = mass matrix Many numerical methods are available to solve the above equation. ANSYS offers these methods: •
Block Lanczos method (default)
•
Subspace method
•
PowerDynamics method
•
Reduced (Householder) method
•
Unsymmetric method
•
Damped method (The damped method solves a different equation; see the ANSYS, Inc. Theory Reference for more information.)
•
QR damped method (The QR damped method solves a different equation; see the ANSYS, Inc. Theory Reference for more information.) Note — The damped, unsymmetric, and QR damped methods are not available in the ANSYS Professional program.
The first four methods (Block Lanczos, subspace, PowerDynamics, and reduced) are the most commonly used. Table 3.6: “Symmetric System Eigensolver Choices” compares these four mode-extraction methods. Following the table is a brief description of each mode-extraction method.
3–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.13: Comparing Mode-Extraction Methods
Table 3.6 Symmetric System Eigensolver Choices Eigensolver
Application
Memory Required
Disk Required
Block Lanczos
Default. To find many modes (about 40+) of large models. Recommended when the model consists of poorly shaped solid and shell elements. This solver performs well when the model consists of shells or a combination of shells and solids. Works faster but requires about 50% more memory than subspace.
Medium
Low
Subspace
To find few modes (up to about 40) of large models. Recommended when the model consists of well-shaped solid and shell elements. Works well if memory availability is limited.
Low
High
Power Dynamics To find few modes (up to about 20) of large models. Recommended for fast computation of eigenvalues of over 100K DOF models. On coarse mesh models, the frequencies are approximate. Missed modes are possible when repeated frequencies are present.
High
Low
Reduced
Low
Low
To find all modes of small to medium models (less than 10K DOF). Can be used to find few modes (up to about 40) of large models with proper selection of master DOF, but accuracy of frequencies depends on the master DOF selected.
3.13.1. Block Lanczos Method The Block Lanczos eigenvalue solver is the default. It uses the Lanczos algorithm where the Lanczos recursion is performed with a block of vectors. This method is as accurate as the subspace method, but faster. The Block Lanczos method uses the sparse matrix solver, overriding any solver specified via the EQSLV command. The Block Lanczos method is especially powerful when searching for eigenfrequencies in a given part of the eigenvalue spectrum of a given system. The convergence rate of the eigenfrequencies will be about the same when extracting modes in the midrange and higher end of the spectrum as when extracting the lowest modes. Therefore, when you use a shift frequency (FREQB) to extract n modes beyond the starting value of FREQB, the algorithm extracts the n modes beyond FREQB at about the same speed as it extracts the lowest n modes.
3.13.2. Subspace Method The subspace method uses the subspace iteration technique, which internally uses the generalized Jacobi iteration algorithm. It is highly accurate because it uses the full [K] and [M] matrices. For the same reason, however, the subspace method is slower than the reduced method. This method is typically used in cases where high accuracy is required or where selecting master DOF is not practical. When doing a modal analysis with a large number of constraint equations, use the subspace method with the frontal solver instead of the JCG solver, or use the Block Lanczos mode-extraction method. Using the JCG solver when your analysis has many constraint equations could result in an internal element stiffness assembly that requires large amounts of memory.
3.13.3. PowerDynamics Method The PowerDynamics method internally uses the subspace iterations, but uses the PCG iterative solver. This method may be significantly faster than either the subspace or the Block Lanczos methods, but may not converge if the model contains poorly-shaped elements, or if the matrix is ill-conditioned. This method is especially useful in very large models (100,000+ DOFs) to obtain a solution for the first few modes. Do not use this method if you will be running a subsequent spectrum analysis.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–17
Chapter 3: Modal Analysis The PowerDynamics method does not perform a Sturm sequence check (that is, it does not check for missing modes), which might affect problems with multiple repeated frequencies. This method always uses lumped mass approximation. Note — If you use PowerDynamics to solve a model that includes rigid body modes, be sure to issue the RIGID command or choose one of its GUI equivalents (Main Menu> Solution> Analysis Options or Main Menu> Preprocessor> Loads> Analysis Options).
3.13.4. Reduced Method The reduced method uses the HBI algorithm (Householder-Bisection-Inverse iteration) to calculate the eigenvalues and eigenvectors. It is relatively fast because it works with a small subset of degrees of freedom called master DOF. Using master DOF leads to an exact [K] matrix but an approximate [M] matrix (usually with some loss in mass). The accuracy of the results, therefore, depends on how well [M] is approximated, which in turn depends on the number and location of masters. Section 3.14: Matrix Reduction presents guidelines to select master DOFs.
3.13.5. Unsymmetric Method The unsymmetric method, which also uses the full [K] and [M] matrices, is meant for problems where the stiffness and mass matrices are unsymmetric (for example, acoustic fluid-structure interaction problems). It uses the Lanczos algorithm which calculates complex eigenvalues and eigenvectors if the system is non-conservative (for example, a shaft mounted on bearings). The real part of the eigenvalue represents the natural frequency and the imaginary part is a measure of the stability of the system - a negative value means the system is stable, whereas a positive value means the system is unstable. Sturm sequence checking is not available for this method. Therefore, missed modes are a possibility at the higher end of the frequencies extracted.
3.13.6. Damped Method The damped method is meant for problems where damping cannot be ignored, such as rotor dynamics applications. It uses full matrices ([K], [M], and the damping matrix [C]). It uses the Lanczos algorithm and calculates complex eigenvalues and eigenvectors (as described below). Sturm sequence checking is not available for this method. Therefore, missed modes are a possibility at the higher end of the frequencies extracted.
3.13.6.1. Damped Method-Real and Imaginary Parts of the Eigenvalue The imaginary part of the eigenvalue, Ω, represents the steady-state circular frequency of the system. The real part of the eigenvalue, σ, represents the stability of the system. If σ is less than zero, then the displacement amplitude will decay exponentially, in accordance with EXP(σ). If σ is greater than zero, then the amplitude will increase exponentially. (Or, in other words, negative σ gives an exponentially decreasing, or stable, response; and positive σ gives an exponentially increasing, or unstable, response.) If there is no damping, the real component of the eigenvalue will be zero. Note — The eigenvalue results reported by ANSYS are actually divided by 2* π. This gives the frequency in Hz (cycles/second). In other words: Imaginary part of eigenvalue, as reported = Ω/(2* π) Real part of eigenvalue, as reported = σ/(2* π)
3.13.6.2. Damped Method-Real and Imaginary Parts of the Eigenvector In a damped system, the response at different nodes can be out of phase. At any given node, the amplitude will be the vector sum of the real and imaginary components of the eigenvector.
3–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.14: Matrix Reduction
3.13.7. QR Damped Method The QR damped method combines the advantages of the Block Lanczos method with the complex Hessenberg method. The key concept is to approximately represent the first few complex damped eigenvalues by a linear combination of a small number of eigenvectors of the undamped system. After the undamped mode shapes are evaluated by using the real eigensolution (Block Lanczos method), the equations of motion are transformed to these modal coordinates. Using the QR algorithm, a smaller eigenvalue problem is then solved in the modal subspace. This approach gives good results for lightly damped systems and can also be applicable to any arbitrary damping type (proportional or non-proportional symmetric damping or unsymmetric gyroscopic damping matrix). Because the accuracy of this method is dependent on the number of modes used in the calculations, a sufficient number of fundamental modes are recommended, especially for highly damped systems to provide good results. This method is not recommended for critically damped or overdamped systems. This method outputs both the real and imaginary eigenvalues (frequencies), but outputs only the real eigenvectors (mode shapes).
3.14. Matrix Reduction Matrix reduction is a way to reduce the size of the matrices of a model and perform a quicker and cheaper analysis. It is mainly used in dynamic analyses such as modal, harmonic, and transient analyses. Matrix reduction is also used in substructure analyses to generate a superelement. Matrix reduction allows you to build a detailed model, as you would for a static stress analysis, and use only a "dynamic" portion of it for a dynamic analysis. You choose the "dynamic" portion by identifying key degrees of freedom, called master degrees of freedom, that characterize the dynamic behavior of the model. The ANSYS program then calculates reduced matrices and the reduced DOF solution in terms of the master DOF. You can then expand the solution to the full DOF set by performing an expansion pass. The main advantage of this procedure is the savings in CPU time to obtain the reduced solution, especially for dynamic analyses of large problems.
3.14.1. Theoretical Basis of Matrix Reduction The ANSYS program uses the Guyan Reduction procedure to calculate the reduced matrices. The key assumption in this procedure is that for the lower frequencies, inertia forces on the slave DOF (those DOF being reduced out) are negligible compared to elastic forces transmitted by the master DOF. Therefore, the total mass of the structure is apportioned among only the master DOF. The net result is that the reduced stiffness matrix is exact, whereas the reduced mass and damping matrices are approximate. For details about how the reduced matrices are calculated, refer to the ANSYS, Inc. Theory Reference.
3.14.1.1. Guidelines for Selecting Master DOF Choosing master DOF is an important step in a reduced analysis. The accuracy of the reduced mass matrix (and hence the accuracy of the solution) depends on the number and location of masters. For a given problem, you can choose many different sets of master DOF and will probably obtain acceptable results in all cases. You can choose masters using M and MGEN commands, or you can have the program choose masters during solution using the TOTAL command. We recommend that you do both: choose a few masters yourself, and also have the ANSYS program choose masters. This way, the program can pick up any modes that you may have missed. The following list summarizes the guidelines for selecting master DOF: •
The total number of master DOF should be at least twice the number of modes of interest.
•
Choose master DOF in directions in which you expect the structure or component to vibrate. For a flat plate, for example, you should choose at least a few masters in the out-of-plane direction (see Fig-
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–19
Chapter 3: Modal Analysis ure 3.2: “Choose Master DOF” (a)). In cases where motion in one direction induces a significant motion in another direction, choose master DOF in both directions (see Figure 3.2: “Choose Master DOF” (b)).
Figure 3.2 Choose Master DOF
(a) Possible out-of-plane masters for a flat plate(b) Motion in X induces motion in Y •
Choose masters at locations having relatively large mass or rotary inertia and relatively low stiffness (see Figure 3.3: “Choosing Master DOFs”). Examples of such locations are overhangs and "loosely" connected structures. Conversely, do not choose masters at locations with relatively small mass, or at locations with high stiffness (such as DOF close to constraints).
Figure 3.3 Choosing Master DOFs
Choose masters at locations with (a) large rotary inertia, (b) large mass •
If your primary interest is in bending modes, you can neglect rotational and "stretching" DOF.
•
If the degree of freedom to be chosen belongs to a coupled set, choose only the first (primary) DOF of the coupled set.
•
Choose master DOF at locations where forces or nonzero displacements are to be applied.
•
For axisymmetric shell models (SHELL51 or SHELL61), choose as masters the global UX degree of freedom at all nodes on those sections of the model that are parallel to or nearly parallel to the center line, so oscillatory motions between master DOF can be avoided (see Figure 3.4: “Choosing Masters in an Axisymmetric Shell Model”). This recommendation can be relaxed if the motion is primarily parallel to the centerline. For axisymmetric harmonic elements with MODE = 2 or greater, choose as masters both UX and UZ degrees of freedom.
3–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.14: Matrix Reduction
Figure 3.4 Choosing Masters in an Axisymmetric Shell Model
The best way to check the validity of the master DOF set is to rerun the analysis with twice (or half) the number of masters and to compare the results. Another way is to review the reduced mass distribution printed during a modal solution. The reduced mass should be, at least in the dominant direction of motion, within 10-15 percent of the total mass of the structure.
3.14.1.2. A Note About Program-Selected Masters If you let the ANSYS program select masters [TOTAL], the distribution of masters selected will depend on the order in which elements are processed during the solution. For example, different master DOF sets may be selected depending on whether the elements are processed from left to right or from right to left. However, this difference usually yields insignificant differences in the results. For meshes with uniform element sizes and properties (for example, a flat plate), the distribution of masters will, in general, not be uniform. In such cases, you should specify some master DOF of your own [M, MGEN]. The same recommendation applies to structures with an irregular mass distribution, where the program-selected master DOF may be concentrated in the higher-mass regions.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–21
3–22
Chapter 4: Harmonic Response Analysis 4.1. Definition of Harmonic Response Analysis Any sustained cyclic load will produce a sustained cyclic response (a harmonic response) in a structural system. Harmonic response analysis gives you the ability to predict the sustained dynamic behavior of your structures, thus enabling you to verify whether or not your designs will successfully overcome resonance, fatigue, and other harmful effects of forced vibrations.
4.2. Uses for Harmonic Response Analysis Harmonic response analysis is a technique used to determine the steady-state response of a linear structure to loads that vary sinusoidally (harmonically) with time. The idea is to calculate the structure's response at several frequencies and obtain a graph of some response quantity (usually displacements) versus frequency. "Peak" responses are then identified on the graph and stresses reviewed at those peak frequencies. This analysis technique calculates only the steady-state, forced vibrations of a structure. The transient vibrations, which occur at the beginning of the excitation, are not accounted for in a harmonic response analysis (see Figure 4.1: “Harmonic Response Systems”).
Figure 4.1 Harmonic Response Systems
!#" %$
34 ! 2!!*
"56#7 ' % $
ω
&
"' $
& ' ( )'!!*
+-,.+ /0 -" ω21 φ $ <= @ =>?
;<
, 0 '9!!*
8"5: ' ( (# 7 ' % $
% "6!$
Typical harmonic response system. Fo and Ω are known. uo and Φ are unknown (a). Transient and steady-state dynamic response of a structural system (b). Harmonic response analysis is a linear analysis. Some nonlinearities, such as plasticity will be ignored, even if they are defined. You can, however, have unsymmetric system matrices such as those encountered in a fluidstructure interaction problem (see Chapter 15, “Acoustics” in the ANSYS Coupled-Field Analysis Guide). Harmonic analysis can also be performed on a prestressed structure, such as a violin string (assuming the harmonic stresses are much smaller than the pretension stress). See Section 4.11.1.1: Prestressed Full Harmonic Response Analysis for more information on prestressed harmonic analyses.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 4: Harmonic Response Analysis
4.3. Commands Used in a Harmonic Response Analysis You use the same set of commands to build a model and perform a harmonic response analysis that you use to do any other type of finite element analysis. Likewise, you choose similar options from the graphical user interface (GUI) to build and solve models no matter what type of analysis you are doing. Section 4.6: Sample Harmonic Response Analysis (GUI Method) and Section 4.7: Sample Harmonic Response Analysis (Command or Batch Method) show a sample harmonic response analysis done via the GUI and via commands, respectively. For detailed, alphabetized descriptions of the ANSYS commands, see the ANSYS Commands Reference.
4.4. The Three Solution Methods Three harmonic response analysis methods are available: full, reduced, and mode superposition. (A fourth, relatively expensive method is to do a transient dynamic analysis with the harmonic loads specified as time-history loading functions; see Chapter 5, “Transient Dynamic Analysis” for details.) The ANSYS Professional program allows only the mode superposition method. Before we study the details of how to implement each of these methods, let's explore the advantages and disadvantages of each method.
4.4.1. The Full Method The full method is the easiest of the three methods. It uses the full system matrices to calculate the harmonic response (no matrix reduction). The matrices may be symmetric or unsymmetric. The advantages of the full method are: •
It is easy to use, because you don't have to worry about choosing master degrees of freedom or mode shapes.
•
It uses full matrices, so no mass matrix approximation is involved.
•
It allows unsymmetric matrices, which are typical of such applications as acoustics and bearing problems.
•
It calculates all displacements and stresses in a single pass.
•
It accepts all types of loads: nodal forces, imposed (nonzero) displacements, and element loads (pressures and temperatures).
•
It allows effective use of solid-model loads.
A disadvantage is that this method usually is more expensive than either of the other methods when you use the frontal solver. However, when you use the JCG solver or the ICCG solver, the full method can be very efficient.
4.4.2. The Reduced Method The reduced method enables you to condense the problem size by using master degrees of freedom and reduced matrices. After the displacements at the master DOF have been calculated, the solution can be expanded to the original full DOF set. (See Section 3.14: Matrix Reduction, for a more detailed discussion of the reduction procedure.) The advantages of this method are: •
It is faster and less expensive compared to the full method when you are using the frontal solver.
•
Prestressing effects can be included.
The disadvantages of the reduced method are:
4–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.5: How to Do Harmonic Response Analysis •
The initial solution calculates only the displacements at the master DOF. A second step, known as the expansion pass, is required for a complete displacement, stress, and force solution. (However, the expansion pass might be optional for some applications.)
•
Element loads (pressures, temperatures, etc.) cannot be applied.
•
All loads must be applied at user-defined master degrees of freedom. (This limits the use of solid-model loads.)
4.4.3. The Mode Superposition Method The mode superposition method sums factored mode shapes (eigenvectors) from a modal analysis to calculate the structure's response. Its advantages are: •
It is faster and less expensive than either the reduced or the full method for many problems.
•
Element loads applied in the preceding modal analysis can be applied in the harmonic response analysis via the LVSCALE command, unless the modal analysis was done using PowerDynamics.
•
It allows solutions to be clustered about the structure's natural frequencies. This results in a smoother, more accurate tracing of the response curve.
•
Prestressing effects can be included.
•
It accepts modal damping (damping ratio as a function of frequency).
Disadvantages of the mode superposition method are: •
Imposed (nonzero) displacements cannot be applied.
•
When you are using PowerDynamics for the modal analysis, initial conditions cannot have previouslyapplied loads.
4.4.4. Restrictions Common to All Three Methods All three methods are subject to certain common restrictions: •
All loads must be sinusoidally time-varying.
•
All loads must have the same frequency.
•
No nonlinearities are permitted.
•
Transient effects are not calculated.
You can overcome any of these restrictions by performing a transient dynamic analysis, with harmonic loads expressed as time-history loading functions. Chapter 5, “Transient Dynamic Analysis” describes the procedure for a transient dynamic analysis.
4.5. How to Do Harmonic Response Analysis We will first describe how to do a harmonic response analysis using the full method, and then list the steps that are different for the reduced and mode superposition methods.
4.5.1. Full Harmonic Response Analysis The procedure for a full harmonic response analysis consists of three main steps: 1.
Build the model. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–3
Chapter 4: Harmonic Response Analysis 2.
Apply loads and obtain the solution.
3.
Review the results.
4.5.2. Build the Model See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details, see the ANSYS Modeling and Meshing Guide.
4.5.2.1. Points to Remember •
Only linear behavior is valid in a harmonic response analysis. Nonlinear elements, if any, will be treated as linear elements. If you include contact elements, for example, their stiffnesses are calculated based on their initial status and are never changed.
•
Both Young's modulus (EX) (or stiffness in some form) and density (DENS) (or mass in some form) must be defined. Material properties may be linear, isotropic or orthotropic, and constant or temperature-dependent. Nonlinear material properties, if any, are ignored.
4.5.3. Apply Loads and Obtain the Solution In this step, you define the analysis type and options, apply loads, specify load step options, and initiate the finite element solution. Details of how to do these tasks are explained below. Note — Peak harmonic response occurs at forcing frequencies that match the natural frequencies of your structure. Before obtaining the harmonic solution, you should first determine the natural frequencies of your structure by obtaining a modal solution (as explained in Chapter 3, “Modal Analysis”).
4.5.3.1. Enter the ANSYS Solution Processor Command(s): /SOLU GUI: Main Menu> Solution
4.5.3.2. Define the Analysis Type and Options ANSYS offers these options for a harmonic response analysis:
Table 4.1 Analysis Types and Options Option
Command
GUI Path
New Analysis
ANTYPE
Main Menu> Solution> Analysis Type> New Analysis
Analysis Type: Harmonic Response ANTYPE
Main Menu> Solution> Analysis Type> New Analysis> Harmonic
Solution Method
HROPT
Main Menu> Solution> Analysis Type> Analysis Options
Solution Listing Format
HROUT
Main Menu> Solution> Analysis Type> Analysis Options
Mass Matrix Formulation
LUMPM
Main Menu> Solution> Analysis Type> Analysis Options
Equation Solver
EQSLV
Main Menu> Solution> Analysis Type> Analysis Options
4–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.5: How to Do Harmonic Response Analysis Each of these options is explained in detail below. •
Option: New Analysis (ANTYPE) Choose New Analysis. Restarts are not valid in a harmonic response analysis; if you need to apply additional harmonic loads, do a new analysis each time.
•
Option: Analysis Type: Harmonic Response (ANTYPE) Choose Harmonic Response as the analysis type.
•
Option: Solution Method (HROPT) Choose one of the following solution methods: – Full method – Reduced method – Mode superposition method
•
Option: Solution Listing Format (HROUT) This option determines how the harmonic displacement solution is listed in the printed output (Jobname.OUT). You can choose between real and imaginary parts (default), and amplitudes and phase angles.
•
Option: Mass Matrix Formulation (LUMPM) Use this option to specify the default formulation (which is element dependent) or lumped mass approximation. We recommend the default formulation for most applications. However, for some problems involving "skinny" structures such as slender beams or very thin shells, the lumped mass approximation often yields better results. Also, the lumped mass approximation can result in a shorter run time and lower memory requirements. After you complete the fields on the Harmonic Analysis Options dialog box, click on OK to reach a second Harmonic Analysis dialog box, where you choose an equation solver.
•
Option: Equation Solver (EQSLV) You can choose the frontal solver (default), the sparse direct solver (SPARSE), the Jacobi Conjugate Gradient (JCG) solver, or the Incomplete Cholesky Conjugate Gradient (ICCG) solver. The frontal direct solver or sparse direct solver is recommended for most structural models. When using a direct solver to solve a relatively large problem, choose the sparse solver over the frontal solver.
4.5.3.3. Apply Loads on the Model A harmonic analysis, by definition, assumes that any applied load varies harmonically (sinusoidally) with time. To completely specify a harmonic load, three pieces of information are usually required: the amplitude, the phase angle, and the forcing frequency range (see Figure 4.2: “Relationship Between Real/Imaginary Components and Amplitude/Phase Angle”).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–5
Chapter 4: Harmonic Response Analysis
Figure 4.2 Relationship Between Real/Imaginary Components and Amplitude/Phase Angle
2
* /.10 2 +-, 1 2 +@0
!#"$&% ACB10D% %
'( !)"$% 5 !
34% 6!79 >:? 8: ;< =
2
The amplitude is the maximum value of the load, which you specify using the commands shown in Table 4.2: “ Applicable Loads in a Harmonic Response Analysis”. The phase angle is a measure of the time by which the load lags (or leads) a frame of reference. On the complex plane (see Figure 4.2: “Relationship Between Real/Imaginary Components and Amplitude/Phase Angle”), it is the angle measured from the real axis. The phase angle is required only if you have multiple loads that are out of phase with each other. For example, the unbalanced rotating antenna shown in Figure 4.3: “An Unbalanced Rotating Antenna” will produce out-of-phase vertical loads at its four support points. The phase angle cannot be specified directly; instead, you specify the real and imaginary components of the out-of-phase loads using the VALUE and VALUE2 fields of the appropriate displacement and force commands. Pressures and other surface and body loads can only be specified with a phase angle of 0 (no imaginary component) with the following exceptions: nonzero imaginary components of pressures can be applied using the SURF153 and SURF154 elements in a full harmonic response analysis, or using a mode superposition harmonic response analysis if the mode-extraction method is Block Lanczos (see the SF and SFE commands). Figure 4.2: “Relationship Between Real/Imaginary Components and Amplitude/Phase Angle” shows how to calculate the real and imaginary components. The forcing frequency range is the frequency range of the harmonic load (in cycles/time). It is specified later as a load step option with the HARFRQ command.
4–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.5: How to Do Harmonic Response Analysis
Figure 4.3 An Unbalanced Rotating Antenna !
" # $&% "$& '$$("
,
)( # $ (*) )( +
+ "./'0 (1 ! '(1 '+ '$( '
+ "./'0 (1 ! '(1 '+ '$( '
: 6 "$
2"$(342 .5# '3/1 +(6 "+ # 7& 8 9
An unbalanced rotating antenna will produce out-of-phase vertical loads at its four support points. Note — A harmonic analysis cannot calculate the response to multiple forcing functions acting simultaneously with different frequencies (for example, two machines with different rotating speeds running at the same time). However, POST1 can superimpose multiple load cases to obtain the total response. Table 4.2: “ Applicable Loads in a Harmonic Response Analysis” summarizes the loads applicable to a to a harmonic response analysis. Except for inertia loads, you can define loads either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). For a general discussion of solid-model loads versus finite element loads, see Chapter 2, “Loading” in the ANSYS Basic Analysis Guide.
Table 4.2 Applicable Loads in a Harmonic Response Analysis Load Type
Category
Cmd Family
GUI Path
Displacement (UX, UY, Constraints UZ, ROTX, ROTY, ROTZ)
D
Main Menu> Solution> Define Loads> Apply> Structural> Displacement
Force, Moment (FX, FY, Forces FZ, MX, MY, MZ)
F
Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment
Pressure (PRES)
SF
Main Menu> Solution> Define Loads> Apply> Structural> Pressure
Surface Loads
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–7
Chapter 4: Harmonic Response Analysis Load Type Temperature (TEMP), Fluence (FLUE)
Category Body Loads
Gravity, Spinning, etc. Inertia Loads
Cmd Family
GUI Path
BF
Main Menu> Solution> Define Loads> Apply> Structural> Temperature
-
Main Menu> Solution> Define Loads> Apply> Structural> Other
In an analysis, loads can be applied, removed, operated on, or listed.
4.5.3.3.1. Applying Loads Using Commands Table 4.3: “Load Commands for a Harmonic Response Analysis” lists all the commands you can use to apply loads in a harmonic response analysis.
Table 4.3 Load Commands for a Harmonic Response Analysis Load Type Solid Model or FE Displacement
Force
Pressure
Temperature, Fluence
4–8
Entity
Apply
Delete
List
Operate
Apply Settings
Solid Mod- Keypoints el
DK
DKDELE
DKLIST
DTRAN
-
Solid Mod- Lines el
DL
DLDELE
DLLIST
DTRAN
-
Solid Mod- Areas el
DA
DADELE
DALIST
DTRAN
-
Finite Elem Nodes
D
DDELE
DLIST
DSCALE
Solid Mod- Keypoints el
FK
FKDELE
FKLIST
FTRAN
Finite Elem Nodes
F
FDELE
FLIST
FSCALE
FCUM
Solid Mod- Lines el
SFL
SFLDELE
SFLLIST
SFTRAN
SFGRAD
Solid Mod- Areas el
SFA
SFADELE
SFALIST
SFTRAN
SFGRAD
Finite Elem Nodes
SF
SFDELE
SFLIST
SFSCALE
SFGRAD, SFCUM
Finite Elem Elements
SFE
SFEDELE
SFELIST
SFSCALE
SFGRAD, SFBEAM, SFFUN, SFCUM
Solid Mod- Keypoints el
BFK
BFKDELE
BFKLIST
BFTRAN
-
Solid Mod- Lines el
BFL
BFLDELE
BFLLIST
BFTRAN
-
Solid Mod- Areas el
BFA
BFADELE
BFALIST
BFTRAN
-
Solid Mod- Volumes el
BFV
BFVDELE
BFVLIST
BFTRAN
-
Finite Elem Nodes
BF
BFDELE
BFLIST
BFSCALE
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
DSYM, DCUM -
BFCUM , BFUNIF , TBUNIF
Section 4.5: How to Do Harmonic Response Analysis Finite Elem Elements Load Type Solid Model or FE Inertia
-
BFE
BFEDELE
BFELIST
BFSCALE
BFCUM
Entity
Apply
Delete
List
Operate
Apply Settings
-
ACEL, OMEGA, DOMEGA, CGLOC, CGOMGA, DCGOMG
-
-
-
-
4.5.3.3.2. Applying Loads and Listing Loads Using the GUI These steps for a harmonic analysis are the same as those for most other analyses. See Section 3.5.4.2: Applying Loads Using the GUI and Section 3.5.4.3: Listing Loads for more information.
4.5.3.4. Specify Load Step Options The following options are available for a harmonic response analysis:
Table 4.4 Load Step Options Option
Command
GUI Path
General Options Number of Harmonic Solutions NSUBST
Main Menu> Solution> Load Step Opts> Time/Frequenc> Freq and Substeps
Stepped or Ramped Loads
KBC
Main Menu> Solution> Load Step Opts> Time/Frequenc> Time - Time Step or Freq and Substeps
Forcing Frequency Range
HARFRQ
Main Menu> Solution> Load Step Opts> Time/Frequenc> Freq and Substeps
Damping
ALPHAD, BETAD, DMPRAT
Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
Dynamics Options
MP,DAMP, MP,DM- Main Menu> Solution> Load Step Opts> Other> PR Change Mat Props> Material Models> Structural> Damping Output Control Options Printed Output
OUTPR
Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout
Database and Results File Output OUTRES
Main Menu> Solution> Load Step Opts> Output Ctrls> DB/ Results File
Extrapolation of Results
Main Menu> Solution> Load Step Opts> Output Ctrls> Integration Pt
ERESX
4.5.3.4.1. General Options General options include the following: •
Number of Harmonic Solutions (NSUBST)
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–9
Chapter 4: Harmonic Response Analysis You can request any number of harmonic solutions to be calculated. The solutions (or substeps) will be evenly spaced within the specified frequency range (HARFRQ). For example, if you specify 10 solutions in the range 30 to 40 Hz, the program will calculate the response at 31, 32, 33, ..., 39, and 40 Hz. No response is calculated at the lower end of the frequency range. •
Stepped or Ramped Loads (KBC) The loads may be stepped or ramped. By default, they are ramped, that is, the load amplitude is gradually increased with each substep. By stepping the loads (KBC,1), the same load amplitude will be maintained for all substeps in the frequency range. Note — Surface and body loads do not ramp from their previous load step values, except for those applied to PLANE2, SOLID45, SOLID92, and SOLID95 element types. The remaining element types always ramp from zero or from the value specified via BFUNIF.
4.5.3.4.2. Dynamics Options Dynamics options include the following: •
Forcing Frequency Range (HARFRQ) The forcing frequency range must be defined (in cycles/time) for a harmonic analysis. Within this range, you then specify the number of solutions to be calculated.
•
Damping Damping in some form should be specified; otherwise, the response will be infinity at the resonant frequencies. ALPHAD and BETAD result in a frequency-dependent damping ratio, whereas DMPRAT specifies a constant damping ratio to be used at all frequencies. Damping can also be specified for individual materials using MP,DAMP and MP,DMPR. See Section 5.10.3: Damping for further details. Note — If no damping is specified in a direct harmonic analysis (full or reduced), the program uses zero damping by default.
•
Alpha (Mass) Damping (ALPHAD)
•
Beta (Stiffness) Damping (BETAD)
•
Constant Damping Ratio (DMPRAT)
•
Material Dependent Damping Multiplier (MP,DAMP)
•
Constant Material Damping Coefficient (MP,DMPR)
4.5.3.4.3. Output Controls Output control options include the following: •
Printed Output (OUTPR) Use this option to include any results data on the output file (Jobname.OUT).
•
Database and Results File Output (OUTRES) This option controls the data on the results file (Jobname.RST).
• 4–10
Extrapolation of Results (ERESX) Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.5: How to Do Harmonic Response Analysis Use this option to review element integration point results by copying them to the nodes instead of extrapolating them (default).
4.5.3.5. Save a Backup Copy of the Database to a Named File You can then retrieve your model by reentering the ANSYS program and issuing RESUME. Command(s): SAVE GUI: Utility Menu> File> Save as
4.5.3.6. Start Solution Calculations Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
4.5.3.7. Repeat for Additional Load Steps Repeat the process for any additional loads and frequency ranges (that is, for additional load steps). If you plan to do time-history postprocessing (POST26), the frequency ranges should not overlap from one load step to the next. Another method for multiple load steps, which allows you to store the load steps on files and then solve them at once using a macro, is described in the ANSYS Basic Analysis Guide.
4.5.3.8. Leave SOLUTION Command(s): FINISH GUI: Close the Solution menu.
4.5.4. Review the Results The results data for a harmonic analysis are the same as the data for a basic structural analysis with the following additions: If you defined damping in the structure, the response will be out-of-phase with the loads. All results are then complex in nature and are stored in terms of real and imaginary parts. Complex results will also be produced if out-of-phase loads were applied. See Section 2.3.6: Review the Results in Chapter 2, “Structural Static Analysis”.
4.5.4.1. Postprocessors You can review these results using either POST26 or POST1. The normal procedure is to first use POST26 to identify critical forcing frequencies - frequencies at which the highest displacements (or stresses) occur at points of interest in the model - and to then use POST1 to postprocess the entire model at these critical forcing frequencies. •
POST1 is used to review results over the entire model at specific frequencies.
•
POST26 allows you to review results at specific points in the model over the entire frequency range.
Some typical postprocessing operations for a harmonic response analysis are explained below. For a complete description of all postprocessing functions, see Chapter 4, “An Overview of Postprocessing” in the ANSYS Basic Analysis Guide.
4.5.4.2. Points to Remember The points to remember for a harmonic analysis are the same as those for most structural analyses. See Section 2.3.6.2: Points to Remember in Chapter 2, “Structural Static Analysis”. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–11
Chapter 4: Harmonic Response Analysis
4.5.4.3. Using POST26 POST26 works with tables of result item versus frequency, known as variables. Each variable is assigned a reference number, with variable number 1 reserved for frequency. 1.
Define the variables using these options: Command(s): NSOL, ESOL, RFORCE GUI: Main Menu> TimeHist Postpro> Define Variables Note — The NSOL command is for primary data (nodal displacements), the ESOL command for derived data (element solution data, such as stresses), and the RFORCE command for reaction force data. To specify the total force, static component of the total force, damping component, or the inertia component, use the FORCE command.
2.
Graph the variables (versus frequency or any other variable). Then use PLCPLX to work with just the amplitude, phase angle, real part, or imaginary part. Command(s): PLVAR, PLCPLX GUI: Main Menu> TimeHist Postpro> Graph Variables Main Menu> TimeHist Postpro> Settings> Graph
3.
Get a listing of the variable. To list just the extreme values, use the EXTREM command. Then use the PRCPLX command to work with amplitude and phase angle or real and imaginary part. Command(s): PRVAR, EXTREM, PRCPLX GUI: Main Menu> TimeHist Postpro> List Variables> List Extremes Main Menu> TimeHist Postpro> List Extremes Main Menu> TimeHist Postpro> Settings> List
Many other functions, such as performing math operations among variables (in complex arithmetic), moving variables into array parameters, moving array parameters into variables, etc., are available in POST26; see Chapter 6, “The Time-History Postprocessor (POST26)” in the ANSYS Basic Analysis Guide for details. By reviewing the time-history results at strategic points throughout the model, you can identify the critical frequencies for further POST1 postprocessing.
4.5.4.4. Using POST1 1.
Read in results for the desired harmonic solution. You can use the SET command for this purpose, but it will read in either the real component or the imaginary component, not both at the same time. The true magnitude of the results is given by an SRSS (square-root-of-sum-of-squares) combination of the real and imaginary components (see Figure 4.2: “Relationship Between Real/Imaginary Components and Amplitude/Phase Angle”) and can be done for specific points in the model in POST26.
2.
Display the deformed shape of the structure, contours of stresses, strains, etc., or vector plots of vector items (PLVECT). To obtain tabular listings of data, use PRNSOL, PRESOL, PRRSOL, etc.
4–12
•
Option: Display Deformed Shape Command(s): PLDISP GUI: Main Menu> General Postproc> Plot Results> Deformed Shape
•
Option: Contour Displays Command(s): PLNSOL or PLESOL GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.6: Sample Harmonic Response Analysis (GUI Method) Use these options to contour almost any result item, such as stresses (SX, SY, SZ...), strains (EPELX, EPELY, EPELZ...), and displacements (UX, UY, UZ...). The KUND field on PLNSOL and PLESOL gives you the option of overlaying the undeformed shape on the display. •
Option: Vector Plots Command(s): PLVECT GUI: Main Menu> General Postproc> Plot Results> Vector Plot> Predefined Use PLNSOL or PLESOL to contour almost any result item, such as stresses (SX, SY, SZ...), strains (EPELX, EPELY, EPELZ...), and displacements (UX, UY, UZ...).
•
Option: Tabular Listings Command(s): PRNSOL (nodal results) PRESOL (element-by-element results) PRRSOL (reaction data) etc. NSORT, ESORT GUI: Main Menu> General Postproc> List Results> Nodal Solution Main Menu> General Postproc> List Results> Element Solution Main Menu> General Postproc> List Results> Reaction Solution Use the NSORT and ESORT commands to sort the data before listing them.
Many other functions, such as mapping results on to a path, transforming results to different coordinate systems, load case combinations, etc., are available in POST1; see Chapter 3, “Solution” in the ANSYS Basic Analysis Guide for details. See the ANSYS Commands Reference for a discussion of the ANTYPE, HROPT, HROUT, HARFRQ, DMPRAT, NSUBST, KBC, NSOL, ESOL, RFORCE, PLCPLX, PLVAR, PRCPLX, PRVAR, PLDISP, PRRSOL, and PLNSOL commands.
4.6. Sample Harmonic Response Analysis (GUI Method) In this sample problem, you will determine the harmonic response of a two-mass-spring system.
4.6.1. Problem Description Determine the response amplitude (Xi) and phase angle (Φi) for each mass (mi) of the system shown below when excited by a harmonic force (F1sin Ωt) acting on mass m1.
4.6.2. Problem Specifications Material properties for this problem are: m1 = m2 = 0.5 lb-sec2/in k1 = k2 = kc = 200 lb/in Loading for this problem is: F1 = 200 lb The spring lengths are arbitrarily selected and are used only to define the spring direction. Two master degrees of freedom are selected at the masses in the spring direction. A frequency range from zero to 7.5 Hz with a Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–13
Chapter 4: Harmonic Response Analysis solution at 7.5/30 = 0.25 Hz intervals is chosen to give an adequate response curve. POST26 is used to get an amplitude versus frequency display.
4.6.3. Problem Diagram Figure 4.4 Two-Mass-Spring-System
4.6.3.1. Set the Analysis Title 1.
Choose menu path Utility Menu> File> Change Title.
2.
Type the text "Harmonic Response of Two-Mass-Spring System" and click on OK.
4.6.3.2. Define the Element Types 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
Scroll down the list on the left to "Combination" and select it.
4.
Click once on "Spring-damper 14" in the list on the right.
5.
Click on Apply.
4–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.6: Sample Harmonic Response Analysis (GUI Method) 6.
Scroll up the list on the left to "Structural Mass" and select it.
7.
Click once on "3D mass 21" in the list on the right.
8.
Click on OK. The Library of Element Types dialog box closes.
9.
Click on Close in the Element Types dialog box.
4.6.3.3. Define the Real Constants 1.
Choose menu path Main Menu> Preprocessor> Real Constants.
2.
Click on Add. The Element Type for Real Constants dialog box appears.
3.
Click once on Type 1 to highlight it.
4.
Click on OK. The Real Constants for COMBIN14 dialog box appears.
5.
Enter 200 for the spring constant (K) and 0.1 for the damping coefficient (CV1). Click on OK.
6.
Repeat steps 2-4 for Type 2, MASS21.
7.
Enter .5 for mass in X direction and click on OK.
8.
Click on Close to close the Real Constants dialog box.
4.6.3.4. Create the Nodes 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Nodes> In Active CS.
2.
Enter 1 for node number.
3.
Enter 0, 0, 0 for the X, Y, and Z coordinates, respectively.
4.
Click on Apply.
5.
Enter 4 for node number.
6.
Enter 1, 0, 0 for the X, Y, and Z coordinates, respectively.
7.
Click on OK.
8.
Choose menu path Utility Menu> PlotCtrls> Numbering. The Plot Numbering Controls dialog box appears.
9.
Click once on "Node numbers" to turn node numbers on.
10. Click on OK. 11. Choose menu path Main Menu> Preprocessor> Modeling> Create> Nodes> Fill between Nds. A picking menu appears. 12. In the ANSYS Graphics window, click once on nodes 1 and 4 (on the left and right sides of the screen). A small box appears around each node. 13. Click on OK on the picking menu. The Create Nodes Between 2 Nodes dialog box appears. 14. Click on OK to accept the default of 2 nodes to fill. Nodes 2 and 3 appear in the graphics window.
4.6.3.5. Create the Spring Elements 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Thru Nodes. A picking menu appears.
2.
In the graphics window, click once on nodes 1 and 2.
3.
Click on Apply. A line appears between the selected nodes. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–15
Chapter 4: Harmonic Response Analysis 4.
Click once on nodes 2 and 3.
5.
Click on Apply. A line appears between the selected nodes.
6.
Click once on nodes 3 and 4.
7.
Click on OK. A line appears between the selected nodes.
4.6.3.6. Create the Mass Elements 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes.
2.
Enter 2 for element type number.
3.
Enter 2 for real constant set number and click on OK.
4.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Thru Nodes. A picking menu appears.
5.
In the graphics window, click once on node 2.
6.
Click on Apply.
7.
Click once on node 3 and click on OK.
4.6.3.7. Specify the Analysis Type, MDOF, and Load Step Specifications 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis.
2.
Click once on "Harmonic" and click on OK.
3.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options.
4.
Click once on "Full" to select the solution method.
5.
Click once on "Amplitud + phase" to select the DOF printout format and click on OK.
6.
Click OK in the Full Harmonic Analysis dialog box.
7.
Choose menu path Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout.
8.
Click on "Last substep" to set the print frequency and click on OK.
9.
Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Freq and Substeps.
10. Enter 0 and 7.5 for the harmonic frequency range. 11. Enter 30 for the number of substeps. 12. Click once on "Stepped" to specify stepped boundary conditions. 13. Click on OK.
4.6.3.8. Define Loads and Boundary Conditions 1.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. A picking menu appears.
2.
Click on Pick All. The Apply U, ROT on Nodes dialog box appears.
3.
In the scroll box for DOFs to be constrained, click once on "UY" to highlight it (make sure no other selections are highlighted).
4.
Click on OK.
5.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. A picking menu appears.
4–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.6: Sample Harmonic Response Analysis (GUI Method) 6.
In the graphics window, click once on nodes 1 and 4.
7.
Click on OK. The Apply U, ROT on Nodes dialog box appears.
8.
In the scroll box for DOFs to be constrained, click once on "UX" to highlight it and click once on "UY" to deselect it.
9.
Click on OK.
10. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Force/ Moment> On Nodes. A picking menu appears. 11. In the graphics window, click once on node 2. 12. Click on OK. The Apply F/M on Nodes dialog box appears. 13. In the scroll box for direction of force/moment, click once on "FX." 14. Enter 200 for the real part of force/moment and click on OK.
4.6.3.9. Solve the Model 1.
Choose menu path Main Menu> Solution> Solve> Current LS.
2.
Review the information in the status window and click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to begin the solution.
4.
When the solution is finished, a dialog box stating "Solution is done!" appears. Click on Close.
4.6.3.10. Review the Results For this sample, you will review the time-history results of nodes 2 and 3. 1.
Choose menu path Main Menu> TimeHist Postpro> Define Variables. The Defined Time-History Variables dialog box appears.
2.
Click on Add. The Add Time-History Variable dialog box appears.
3.
Click on OK to accept the default of Nodal DOF result. The Define Nodal Data dialog box appears.
4.
Enter 2 for reference number of variable.
5.
Enter 2 for node number.
6.
Enter 2UX for the user-specified label.
7.
In the scroll box on the right, click once on "Translation UX" to highlight it.
8.
Click on OK.
9.
Click on Add in the Defined Time-History Variables dialog box. The Add Time-History Variable dialog box appears.
10. Click on OK to accept the default of Nodal DOF result. The Define Nodal Data dialog box appears. 11. Enter 3 for reference number of variable. 12. Enter 3 for node number. 13. Enter 3UX for the user-specified label. 14. In the scroll box on the right, click once on "Translation UX" to highlight it. 15. Click on OK. 16. Click on Close.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–17
Chapter 4: Harmonic Response Analysis 17. Choose menu path Utility Menu> PlotCtrls> Style> Graphs. The Graph Controls dialog box appears. 18. In the scroll box for type of grid, scroll to "X and Y lines" to select it. 19. Click on OK. 20. Choose menu path Main Menu> TimeHist Postpro> Graph Variables. The Graph Time-History Variables dialog box appears. Your graph should look like this:
21. Enter 2 for 1st variable to graph. 22. Enter 3 for 2nd variable to graph. 23. Click on OK. A graph appears in the graphic window.
4.6.3.11. Exit ANSYS You are now finished with this sample problem. 1.
In the ANSYS Toolbar, click on Quit.
2.
Choose the save option you want and click on OK.
4.7. Sample Harmonic Response Analysis (Command or Batch Method) You can perform the example harmonic response analysis of a two-mass-spring system by using the following ANSYS commands instead of the GUI. /PREP7 /TITLE, Harmonic response of a two-mass-spring system ET,1,COMBIN14,,,2
4–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.8: Where to Find Other Examples ET,2,MASS21,,,4 R,1,200 R,2,.5 N,1 N,4,1 FILL E,1,2 E,2,3 E,3,4 TYPE,2 REAL,2 E,2 E,3 FINISH /SOLU ANTYPE,HARMIC HROPT,FULL HROUT,OFF OUTPR,BASIC,1 NSUBST,30 HARFRQ,,7.5 KBC,1 D,1,UY,,,4 D,1,UX,,,4,3 F,2,FX,200 SOLVE FINISH /POST26 NSOL,2,2,U,X,2UX NSOL,3,3,U,X,3UX /GRID,1 /AXLAB,Y,DISP PLVAR,2,3 FINISH
! Spring constant = 200 ! Mass = 0.5
! Spring element ! Spring element
! Mass element ! Mass element
! Harmonic response analysis ! Full harmonic response ! Print results as amplitudes and phase angles ! ! ! ! !
30 Intervals within freq. range Frequency range from 0 to 7.5 HZ Step boundary condition Constrain all 44 DOF Constrain nodes 1 and 4 in UX
! Store UX Displacements ! Turn grid on ! Y-axis label disp ! Display variables 2 and 3
4.8. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional harmonic analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS family of products. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual includes a variety of harmonic analysis test cases: VM19 - Random Vibration Analysis of a Deep Simply-Supported Beam VM76 - Harmonic Response of a Guitar String VM86 - Harmonic Response of a Dynamic System VM87 - Equivalent Structural Damping VM88 - Response of an Eccentric Weight Exciter VM90 - Harmonic Response of a Two-Mass-Spring System VM176 - Frequency Response of Electrical Input Admittance for a Piezoelectric Transducer VM177 - Natural Frequency of a Submerged Ring VM183 - Harmonic Response of a Spring-Mass System VM203 - Dynamic Load Effect on Simply-Supported Thick Square Plate
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–19
Chapter 4: Harmonic Response Analysis
4.9. Reduced Harmonic Response Analysis The reduced method, as its name implies, uses reduced matrices to calculate the harmonic solution. The procedure for a reduced harmonic analysis consists of five main steps: 1.
Build the model.
2.
Apply the loads and obtain the reduced solution.
3.
Review the results of the reduced solution.
4.
Expand the solution (expansion pass).
5.
Review the results of the expanded solution.
Of these, the first step is the same as for the full method. Details of the other steps are explained below.
4.9.1. Apply Loads and Obtain the Reduced Solution By reduced solution, we mean the degree of freedom solution calculated at the master DOF. The tasks required to obtain the reduced solution are as follows: 1.
Enter the ANSYS solution processor. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define the analysis type and options. Options for the reduced solution are the same as described for the full method except for the following differences: •
Choose the reduced solution method.
•
You can include prestress effects (PSTRES). This requires element files from a previous static (or transient) analysis that also included prestress effects. See Section 4.11.1: Prestressed Harmonic Response Analysis for details.
3.
Define master degrees of freedom. Master DOF are essential or dynamic degrees of freedom that characterize the dynamic behavior of the structure. For a reduced harmonic response dynamic analysis, master DOF are also required at locations where you want to apply forces or nonzero displacements. See Section 3.14: Matrix Reduction for guidelines to choose master DOF.
4.
Apply loads on the model. Harmonic loading is the same as described for the full method, except for the following restrictions: •
Only displacements and forces are valid. Element loads such as pressures, temperatures, and accelerations are not allowed.
•
Forces and nonzero displacements must be applied only at master DOF.
5.
Specify load step options. These are the same as described for the full method except that the OUTRES and ERESX commands are not available, and the constant material damping coefficient (MP,DMPR) is not applicable for the reduced method. The OUTPR command controls the printout of the nodal solution at the master DOF (OUTPR,NSOL,ALL (or NONE)).
6.
Save a copy of the database. Command(s): SAVE GUI: Utility Menu> File> Save as
7.
Start solution calculations.
4–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.9: Reduced Harmonic Response Analysis Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS 8.
Repeat steps 4 through 7 for any additional loads and frequency ranges (that is, for additional load steps). If you plan to do time-history postprocessing (POST26), the frequency ranges should not overlap from one load step to the next. Another method for multiple load steps, which allows you to store the load steps on files and then solve them at once using a macro, is described in the ANSYS Basic Analysis Guide.
9.
Leave SOLUTION. Command(s): FINISH GUI: Close the Solution menu.
4.9.2. Review the Results of the Reduced Solution Results from the reduced harmonic solution are written to the reduced harmonic displacement file, Jobname.RFRQ. They consist of displacements at the master DOF, which vary harmonically at each forcing frequency for which the solution was calculated. As with the full method, these displacements will be complex in nature if damping was defined or if out-of-phase loads were applied. You can review the master DOF displacements as a function of frequency using POST26. (POST1 cannot be used, because the complete solution at all DOF is not available.) The procedure to use POST26 is the same as described for the full method, except for the following differences: •
Before defining the POST26 variables, use the FILE command to specify that data are to be read from Jobname.RFRQ. For example, if HARMONIC is the jobname, the FILE command would be: FILE,HARMONIC,RFRQ. (By default, POST26 looks for a results file, which is not written by a reduced harmonic solution.)
•
Only nodal degree of freedom data (at master DOF) are available for processing, so you can use only the NSOL command to define variables.
4.9.3. Expand the Solution (Expansion Pass) The expansion pass starts with the reduced solution and calculates the complete displacement, stress, and force solution at all degrees of freedom. These calculations are done only at frequencies and phase angles that you specify. Therefore, before you begin the expansion pass, you should review the results of the reduced solution (using POST26) and identify the critical frequencies and phase angles. An expansion pass is not always required. For instance, if you are interested mainly in displacements at specific points on the structure, then the reduced solution could satisfy your requirements. However, if you want to determine displacements at non-master DOF, or if you are interested in the stress solution, then you must perform an expansion pass.
4.9.3.1. Points to Remember •
The .RFRQ, .TRI, .EMAT, and .ESAV files from the reduced solution must be available.
•
The database must contain the same model for which the reduced solution was calculated.
4.9.3.2. Expanding the Modes 1.
Reenter the ANSYS solution processor. Command(s): /SOLU GUI: Main Menu> Solution
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–21
Chapter 4: Harmonic Response Analysis Note — You must explicitly leave SOLUTION (using the FINISH command) and reenter (/SOLU) before performing the expansion pass. 2.
Activate the expansion pass and its options. ANSYS offers these options for the expansion pass:
Table 4.5 Expansion Pass Options Option
Command
GUI Path
Expansion Pass On/Off
EXPASS
Main Menu> Solution> Analysis Type> ExpansionPass
No. of Solutions to Expand
NUMEXP
Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> Range of Solu's
Freq. Range for Expansion
NUMEXP
Main Menu> Solution> Load Step Opts> ExpansionPass> Singe Expand> Range of Solu's
Phase Angle for Expansion
HREXP
Main Menu> Solution> Load Step Opts> ExpansionPass> Singe Expand> Range of Solu's
Stress Calculations On/Off
NUMEXP, EXPSOL
Main Menu> Solution> Load Step Opts> ExpansionPass> Singe Expand> Range of Solu's
Nodal Solution Listing Format
HROUT
Main Menu> Solution> Analysis Type> Analysis Options
Each of these options is explained in detail below. •
Option: Expansion Pass On/Off (EXPASS) Choose ON.
•
Option: Number of Solutions to Expand (NUMEXP,NUM) Specify the number. This number of evenly spaced solutions will be expanded over a frequency range (specified next). For example, NUMEXP,4,1000,2000 specifies four solutions in the frequency range 1000 to 2000 (that is, expanded solutions at 1250, 1500, 1750, and 2000).
•
Option: Frequency Range for Expansion (NUMEXP, BEGRNG, ENDRNG) Specify the frequency range. See the example above. If you do not need to expand multiple solutions, you can use EXPSOL to identify a single solution for expansion (either by its load step and substep numbers or by its frequency value).
•
Option: Phase Angle for Expansion (HREXP) If multiple solutions are to be expanded over a frequency range (NUMEXP), we suggest that you request both the real and imaginary parts to be expanded (HREXP,ALL). This way, you can easily combine the two parts in POST26 to review the peak values of displacements, stresses, and other results. If, on the other hand, a single solution is to be expanded (EXPSOL), you can specify the phase angle at which peak displacements occurred using HREXP,angle.
•
Option: Stress Calculations On/Off (NUMEXP or EXPSOL) You can turn off stress and force calculations if you are not interested in them. Default is to calculate stresses and forces.
• 4–22
Option: Nodal Solution Listing Format (HROUT) Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.9: Reduced Harmonic Response Analysis Determines how the harmonic displacement solution is listed in the printed output (Jobname.OUT). You can choose between real and imaginary parts (default), and amplitudes and phase angles. 3.
Specify load step options. The only options valid for a harmonic expansion pass are output controls: •
Printed Output Use this option to include any results data on the printed output file (Jobname.OUT). Command(s): OUTPR GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout
•
Database and Results File Output Use this option to control the data on the results file (Jobname.RST). Command(s): OUTRES GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> DB/Results File
•
Extrapolation of Results Use this option to review element integration point results by copying them to the nodes instead of extrapolating them (default). Note — The FREQ field on OUTPR and OUTRES can be only ALL or NONE. Command(s): ERESX GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> Integration Pt
4.
Start expansion pass calculations. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
5.
Repeat steps 2, 3, and 4 for additional solutions to be expanded. Each expansion pass is stored as a separate load step on the results file. Caution: Subsequent spectrum analyses expect all expanded modes to be in one load step.
6.
Leave SOLUTION. You can now review results in the postprocessor. Command(s): FINISH GUI: Close the Solution menu.
4.9.4. Review the Results of the Expanded Solution This step is the same as the corresponding step in a basic structural analysis with the following additions: You can review the results using POST1. (If you expanded solutions at several frequencies, you can also use POST26 to obtain graphs of stress versus frequency, strain versus frequency, etc.) The procedure to use POST1 (or POST26) is the same as described for the full method, except for one difference: if you requested expansion at a specific phase angle (HREXP,angle), there is only one solution available for each frequency. Use the SET command to read in the results. See Section 2.3.6: Review the Results in Chapter 2, “Structural Static Analysis”.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–23
Chapter 4: Harmonic Response Analysis
4.9.5. Sample Input A sample input listing for a reduced harmonic response analysis is shown below: ! Build the Model /FILNAM,... ! Jobname /TITLE,... ! Title /PREP7 ! Enter PREP7 -----! Generate model --FINISH ! Apply Loads and Obtain the Reduced Solution /SOLU ! Enter SOLUTION ANTYPE,HARMIC ! Harmonic analysis HROPT,REDU ! Reduced method HROUT,... ! Harmonic analysis output options M,... ! Master DOF TOTAL,... D,... ! Constraints F,... ! Loads (real and imaginary components) HARFRQ,... ! Forcing frequency range DMPRAT,... ! Damping ratio NSUBST,... ! Number of harmonic solutions KBC,... ! Ramped or stepped loads SAVE SOLVE ! Initiate multiple load step solution FINISH ! Review the Results of the Reduced Solution /POST26 FILE,,RFRQ ! Postprocessing file is Jobname.RFRQ NSOL,... ! Store nodal result as a variable PLCPLX,... ! Define how to plot complex variables PLVAR,... ! Plot variables PRCPLX,... ! Define how to list complex variables PRVAR,... ! List variables FINISH ! Expand the Solution /SOLU EXPASS,ON EXPSOL,... HREXP,... OUTRES,... SOLVE FINISH
! ! ! !
Reenter SOLUTION Expansion pass Expand a single solution Phase angle for expanded solution
! Review the Results of the Expanded Solution /POST1 SET,... ! Read results for desired frequency PLDISP,... ! Deformed shape PRRSOL,... ! List reactions PLNSOL,... ! Contour plot of nodal results -----! Other postprocessing as desired --FINISH
See the ANSYS Commands Reference for a discussion of the ANTYPE, HROPT, HROUT, M, TOTAL, HARFRQ, DMPRAT, NSUBST, KBC, FILE, NSOL, PLCPLX, PLVAR, PRCPLX, PRVAR, EXPASS, EXPSOL, HREXP, PLDISP, PRRSOL, and PLNSOL commands.
4–24
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.10: Mode Superposition Harmonic Response Analysis
4.10. Mode Superposition Harmonic Response Analysis The mode superposition method sums factored mode shapes (obtained from a modal analysis) to calculate the harmonic response. It is the only method allowed in the ANSYS Professional program. The procedure to use the method consists of five main steps: 1.
Build the model.
2.
Obtain the modal solution.
3.
Obtain the mode superposition harmonic solution.
4.
Expand the mode superposition solution.
5.
Review the results.
Of these, the first step is the same as described for the full method. The remaining steps are described below.
4.10.1. Obtain the Modal Solution Chapter 3, “Modal Analysis” describes how to obtain a modal solution. Following are some additional hints: •
The mode-extraction method should be Block Lanczos (default), subspace, reduced, PowerDynamics, or QR damped. (The other methods, unsymmetric and damped, do not apply to mode superposition.)
•
Be sure to extract all modes that may contribute to the harmonic response.
•
If PowerDynamics was used for the modal solution, no nonzero loads or displacements are allowed (that is, only u = 0 is valid as the initial condition). PowerDynamics does not create a load vector; therefore, the LVSCALE command is not valid unless the scale factor is set to zero.
•
For the reduced mode-extraction method, include those master degrees of freedom at which harmonic loads will be applied.
•
If you use the QR damped mode-extraction method, you must specify any damping (ALPHAD, BETAD, MP,DAMP, or element damping including gyroscopic) that you want to include during preprocessing or in the modal analysis. (ANSYS ignores damping specified during the mode superposition harmonic analysis.) You can set a constant damping ratio (DMPRAT), define constant material damping coefficients (MP,DMPR), or define the damping ratio as a function of mode (MDAMP) in a modal superposition harmonic analysis.
•
If you need to apply harmonically varying element loads (pressures, temperatures, accelerations, and so on), specify them in the modal analysis. ANSYS ignores the loads for the modal solution, but calculates a load vector and writes it to the mode shape file (Jobname.MODE). You can then use the load vector for the harmonic solution. The imaginary component of the load vector calculated from element loads will always be zero with only one exception: in a full harmonic response analysis or a mode superposition harmonic response analysis with the Block Lanczos mode-extraction method, you can apply imaginary pressures via SURF153 or SURF154.
•
The modes need not be expanded for the mode superposition solution. (If you want to review mode shapes, however, you must expand the mode shapes.)
•
Do not change the model data (for example, nodal rotations) between the modal and harmonic analyses.
4.10.2. Obtain the Mode Superposition Harmonic Solution In this step, the program uses mode shapes extracted by the modal solution to calculate the harmonic response. The mode shape file (Jobname.MODE) must be available, and the database must contain the same model for which the modal solution was obtained. If the modal solution was performed using the subspace or Block Lanczos Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–25
Chapter 4: Harmonic Response Analysis method using the default mass formulation (not the lumped mass approximation), the full file (Jobname.FULL) must also be available. The following tasks are involved: 1.
Enter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define the analysis type and analysis options. These are the same as described for the full method, except for the following differences:
3.
4.
•
Choose the mode superposition method of solution (HROPT).
•
Specify the modes you want to use for the solution (HROPT). This determines the accuracy of the harmonic solution. Generally, the number of modes specified should cover about 50 percent more than the frequency range of the harmonic loads.
•
Optionally, cluster the solutions about the structure's natural frequencies (HROUT) for a smoother and more accurate tracing of the response curve.
•
Optionally, at each frequency, print a summary table that lists the contributions of each mode to the response (HROUT). Note, OUTPR,NSOL must be specified to print mode contributions at each frequency.
Apply loads on the model. Harmonic loading is the same as described for the full method, except for the following restrictions: •
Only forces, accelerations, and the load vector created in the modal analysis are valid. Use the LVSCALE command to apply the load vector from the modal solution. Note that ALL loads from the modal analysis are scaled, including forces and accelerations. To avoid load duplication, delete any loads that were applied in the modal analysis.
•
If mode shapes from a reduced modal solution are being used, forces may be applied only at master DOF.
Specify load step options. These are the same as described for the reduced method except that you can also specify modal damping (MDAMP). In addition, if the QR damped method is specified, constant material damping coefficients (MP,DMPR) can be defined. The NSUBST command specifies the number of solutions on each side of a natural frequency if the clustering option (HROUT) is chosen. The default is to calculate four solutions, but you can specify any number of solutions from 2 through 20. (Any value over this range defaults to 10 and any value below this range defaults to 4.)
5.
If you used either the Block Lanczos (default) or the subspace option for the modal analysis (MODOPT,LANB or SUBSP), you may use a nodal component with the OUTRES,NSOL command to limit the displacement data written to the reduced displacement file Jobname.RFRQ. The expansion pass will only produce valid results for those nodes and for those elements in which all of the nodes of the elements have been written to the .RFRQ file. To use this option, first suppress all writing by invoking OUTRES,NSOL,NONE, then specify the item(s) of interest by invoking OUTRES,NSOL,ALL,component. Repeat the OUTRES command for any additional nodal components that you want to write to the .RFRQ file.
6.
Save a copy of the database. Command(s): SAVE GUI: Utility Menu> File> Save as
7.
Start solution calculations.
4–26
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.10: Mode Superposition Harmonic Response Analysis Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS 8.
Repeat steps 3 to 7 for any additional loads and frequency ranges (that is, for additional load steps). If you plan to do time-history postprocessing (POST26), the frequency ranges should not overlap from one load step to the next.
9.
Leave SOLUTION. Command(s): FINISH GUI: Close the Solution menu.
The mode superposition harmonic solution is written to the reduced displacement file, Jobname.RFRQ, regardless of whether the subspace, Block Lanczos, reduced, PowerDynamics, or QR damped method was used for the modal solution. You will therefore need to expand the solution if you are interested in stress results.
4.10.3. Expand the Mode Superposition Solution The procedure for the expansion pass is the same as described for the reduced method. Jobname.TRI from the modal analysis is needed only if the reduced eigenvalue extraction method was used. The output from the expansion pass includes the structural results file, Jobname.RST, containing expanded results. See Section 4.9.3: Expand the Solution (Expansion Pass).
4.10.4. Review the Results Results consist of harmonically varying displacements, stresses, and reaction forces at each forcing frequency for which the solution was calculated. You can review these results using POST26 or POST1, as explained for the reduced method.
4.10.5. Sample Input A sample input listing for a mode superposition harmonic response analysis is shown below: ! Build the Model /FILNAM,... /TITLE,... /PREP7 ------FINISH
! Jobname ! Title ! Enter PREP7 ! Generate model
! Obtain the Modal Solution /SOLU ! Enter SOLUTION ANTYPE,MODAL ! Modal analysis MODOPT,REDU ! Reduced method M,... ! Masters TOTAL,.. D,... ! Constraints SF,... ! Element loads SAVE SOLVE ! Initiate modal solution FINISH ! Obtain the Mode Superposition Harmonic Solution /SOLU ! Enter SOLUTION ANTYPE,HARMIC HROPT,MSUP,... HROUT,... LVSCALE,... F,... HARFRQ,...
! ! ! ! ! !
Harmonic analysis Mode superposition method; number of modes to use Harmonic analysis output options; cluster option Scale factor for loads from modal analysis Nodal loads Forcing frequency range
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–27
Chapter 4: Harmonic Response Analysis DMPRAT,... MDAMP,... NSUBST,... KBC,... SAVE SOLVE FINISH
! ! ! !
Damping ratio Modal damping ratios Number of harmonic solutions Ramped or stepped loads
! Initiate solution
! Review the Results of the Mode Superposition Solution /POST26 FILE,,RFRQ ! Postprocessing file is Jobname.RFRQ NSOL,... ! Store nodal result as a variable PLCPLX,... ! Define how to plot complex variables PLVAR,... ! Plot variables FINISH ! Expand the Solution (for Stress Results) /SOLU! Re-enter SOLUTION EXPASS,ON ! Expansion pass EXPSOL,... ! Expand a single solution HREXP,... ! Phase angle for expanded solution SOLVE FINISH ! Review the Results of the Expanded Solution /POST1 SET,... ! Read results for desired frequency PLDISP,... ! Deformed shape PLNSOL,... ! Contour plot of nodal results --FINISH
See the ANSYS Commands Reference for a discussion of the ANTYPE, MODOPT, M, TOTAL, HROPT, HROUT, LVSCALE, F, HARFRQ, DMPRAT, MDAMP, NSUBST, KBC, FILE, NSOL, PLCPLX, PLVAR, EXPASS, EXPSOL, HREXP, SET, and PLNSOL commands.
4.11. Other Analysis Details 4.11.1. Prestressed Harmonic Response Analysis A prestressed harmonic response analysis calculates the dynamic response of a prestressed structure, such as a violin string. It is assumed that the harmonically varying stresses (which are superimposed on the prestress) are much smaller than the prestress itself.
4.11.1.1. Prestressed Full Harmonic Response Analysis The procedure to do a prestressed full harmonic analysis is essentially the same as that for any other full harmonic analysis except that you first need to prestress the structure by doing a static analysis: 1.
Build the model and obtain a static solution with prestress effects turned on (PSTRES,ON). The procedure to obtain the static solution is explained in Chapter 2, “Structural Static Analysis”.
2.
Reenter SOLUTION and obtain the full harmonic solution, also with prestress effects turned on (reissue PSTRES,ON). Files Jobname.EMAT and Jobname.ESAV from the static analysis must be available. If thermal body forces were present during the static prestress analysis, these thermal body forces must not be deleted during the full harmonic analysis or else the thermal prestress will vanish. Hence, any temperature loads used to define the thermal prestress must also be used in the full harmonic response analysis as sinusoidally time-varying temperature loads. You should be aware of this limitation and exercise some judgement about whether or not to include temperature loads in their static prestress analysis.
4–28
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.11: Other Analysis Details
4.11.1.2. Prestressed Reduced Harmonic Response Analysis The procedure to do a prestressed reduced harmonic analysis is essentially the same as that for any other reduced harmonic analysis except that you first need to prestress the structure by doing a static analysis: 1.
Build the model and obtain a static solution with prestress effects turned on (PSTRES,ON). The procedure to obtain the static solution is explained in Chapter 2, “Structural Static Analysis”.
2.
Reenter SOLUTION and obtain the reduced harmonic solution, also with prestress effects turned on (reissue PSTRES,ON). Files Jobname.EMAT and Jobname.ESAV from the static analysis must be available.
4.11.1.3. Prestressed Mode Superposition Harmonic Response Analysis To include prestress effects in a mode superposition analysis, you must first perform a prestressed modal analysis. See Chapter 3, “Modal Analysis” for details. Once prestressed modal analysis results are available, proceed as for any other mode superposition analysis.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–29
4–30
Chapter 5: Transient Dynamic Analysis 5.1. Definition of Transient Dynamic Analysis Transient dynamic analysis (sometimes called time-history analysis) is a technique used to determine the dynamic response of a structure under the action of any general time-dependent loads. You can use this type of analysis to determine the time-varying displacements, strains, stresses, and forces in a structure as it responds to any combination of static, transient, and harmonic loads. The time scale of the loading is such that the inertia or damping effects are considered to be important. If the inertia and damping effects are not important, you might be able to use a static analysis instead (see Chapter 2, “Structural Static Analysis”). The basic equation of motion solved by a transient dynamic analysis is && } + (C){ u& } + (K){u} = {F(t)} (M){ u where: (M) = mass matrix (C) = damping matrix (K) = stiffness matrix && } = nodal acceleration vector {u { u& } = nodal velocity vector {u} = nodal displacement vector {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 && }) and damping forces ((C){ u& }). The ANSYS program uses the Newmark time into account inertia forces ((M){ u integration method or an improved method called HHT to solve these equations at discrete time points. The time increment between successive time points is called the integration time step.
5.2. Preparing for a Transient Dynamic Analysis A transient dynamic analysis is more involved than a static analysis because it generally requires more computer resources and more of your resources, in terms of the “engineering” time involved. You can save a significant amount of these resources by doing some preliminary work to understand the physics of the problem. For example, you can: 1.
Analyze a simpler model first. A model of beams, masses, and springs can provide good insight into the problem at minimal cost. This simpler model may be all you need to determine the dynamic response of the structure.
2.
If you are including nonlinearities, try to understand how they affect the structure's response by doing a static analysis first. In some cases, nonlinearities need not be included in the dynamic analysis.
3.
Understand the dynamics of the problem. By doing a modal analysis, which calculates the natural frequencies and mode shapes, you can learn how the structure responds when those modes are excited. The natural frequencies are also useful for calculating the correct integration time step.
4.
For a nonlinear problem, consider substructuring the linear portions of the model to reduce analysis costs. Substructuring is described in the ANSYS Advanced Analysis Techniques Guide.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 5: Transient Dynamic Analysis
5.3. Three Solution Methods Three methods are available to do a transient dynamic analysis: full, mode superposition, and reduced. The ANSYS Professional program allows only the mode superposition method. Before we study the details of how to implement each of these methods, we will examine the advantages and disadvantages of each.
5.3.1. Full Method The full method uses the full system matrices to calculate the transient response (no matrix reduction). It is the most general of the three methods because it allows all types of nonlinearities to be included (plasticity, large deflections, large strain, and so on). Note — If you do not want to include any nonlinearities, you should consider using one of the other methods because the full method is also the most expensive method of the three. The advantages of the full method are: •
It is easy to use, because you do not have to worry about choosing master degrees of freedom or mode shapes.
•
It allows all types of nonlinearities.
•
It uses full matrices, so no mass matrix approximation is involved.
•
All displacements and stresses are calculated in a single pass.
•
It accepts all types of loads: nodal forces, imposed (nonzero) displacements (although not recommended), and element loads (pressures and temperatures) and allows tabular boundary condition specification via TABLE type array parameters.
•
It allows effective use of solid-model loads.
The main disadvantage of the full method is that it is more expensive than either of the other methods. For procedural information about using the full method, see Section 5.4: Performing a Full Transient Dynamic Analysis.
5.3.2. Mode Superposition Method The mode superposition method sums factored mode shapes (eigenvectors) from a modal analysis to calculate the structure's response. This is the only method available in the ANSYS Professional program. Its advantages are: •
It is faster and less expensive than the reduced or the full method for many problems.
•
Element loads applied in the preceding modal analysis can be applied in the transient dynamic analysis via the LVSCALE command, unless the modal analysis was done using PowerDynamics.
•
It accepts modal damping (damping ratio as a function of mode number).
The disadvantages of the mode superposition method are: •
The time step must remain constant throughout the transient, so automatic time stepping is not allowed.
•
The only nonlinearity allowed is simple node-to-node contact (gap condition).
•
It does not accept imposed (nonzero) displacements.
5–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.4: Performing a Full Transient Dynamic Analysis For procedural information about using the mode superposition method, see Section 5.5: Performing a Mode Superposition Transient Dynamic Analysis.
5.3.3. Reduced Method The reduced method condenses the problem size by using master degrees of freedom and reduced matrices. After the displacements at the master DOF have been calculated, ANSYS expands the solution to the original full DOF set. (See Section 3.14: Matrix Reduction for a more detailed discussion of the reduction procedure.) The advantage of the reduced method is: •
It is faster and less expensive than the full method.
The disadvantages of the reduced method are: •
The initial solution calculates only the displacements at the master DOF. A second step, known as the expansion pass, is required for a complete displacement, stress, and force solution. (However, the expansion pass might not be needed for some applications.)
•
Element loads (pressures, temperatures, and so on) cannot be applied. Accelerations, however, are allowed.
•
All loads must be applied at user-defined master degrees of freedom. (This limits the use of solid-model loads.)
•
The time step must remain constant throughout the transient, so automatic time stepping is not allowed.
•
The only nonlinearity allowed is simple node-to-node contact (gap condition).
For procedural information about using the reduced method, see Section 5.6: Performing a Reduced Transient Dynamic Analysis.
5.4. Performing a Full Transient Dynamic Analysis Note - Before reading this section, you are encouraged to become familiar with the concepts presented in Chapter 2, “Structural Static Analysis”. We will first describe how to do a transient dynamic analysis using the full method. We will then list the steps that are different for the mode superposition and reduced methods. The procedure for a full transient dynamic analysis (available in the ANSYS Multiphysics, ANSYS Mechanical, and ANSYS Structural products) consists of these steps: 1.
Section 5.4.1: Build the Model
2.
Section 5.4.2: Establish Initial Conditions
3.
Section 5.4.3: Set Solution Controls
4.
Section 5.4.4: Set Additional Solution Options
5.
Section 5.4.5: Apply the Loads
6.
Section 5.4.6: Save the Load Configuration for the Current Load Step
7.
Section 5.4.7: Repeat Steps 3-6 for Each Load Step
8.
Section 5.4.8: Save a Backup Copy of the Database
9.
Section 5.4.9: Start the Transient Solution
10. Section 5.4.10: Exit the Solution Processor 11. Section 5.4.11: Review the Results Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–3
Chapter 5: Transient Dynamic Analysis
5.4.1. Build the Model See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details, see the ANSYS Modeling and Meshing Guide.
5.4.1.1. Points to Remember Keep the following points in mind when building a model for a full transient dynamic analysis: •
You can use both linear and nonlinear elements.
•
Both Young's modulus (EX) (or stiffness in some form) and density (DENS) (or mass in some form) must be defined. Material properties may be linear or nonlinear, isotropic or orthotropic, and constant or temperature-dependent.
Some comments on mesh density: •
The mesh should be fine enough to resolve the highest mode shape of interest.
•
Regions where stresses or strains are of interest require a relatively finer mesh than regions where only displacements are of interest.
•
If you want to include nonlinearities, the mesh should be able to capture the effects of the nonlinearities. For example, plasticity requires a reasonable integration point density (and therefore a fine element mesh) in areas with high plastic deformation gradients.
•
If you are interested in wave propagation effects (for example, a bar dropped exactly on its end), the mesh should be fine enough to resolve the wave. A general guideline is to have at least 20 elements per wavelength along the direction of the wave.
5.4.2. Establish Initial Conditions Before you can perform a full transient dynamic analysis on a model, you need to understand how to establish initial conditions and use load steps. A transient analysis, by definition, involves loads that are functions of time. To specify such loads, you need to divide the load-versus-time curve into suitable load steps. Each "corner" on the load-time curve may be one load step, as shown in Figure 5.1: “Examples of Load-Versus-Time Curves”.
Figure 5.1 Examples of Load-Versus-Time Curves
5–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.4: Performing a Full Transient Dynamic Analysis The first load step you apply is usually to establish initial conditions. You then specify the loads and load step options for the second and subsequent transient load steps. For each load step, you need to specify both load values and time values, along with other load step options such as whether to step or ramp the loads, use automatic time stepping, and so on. You then write each load step to a file and solve all load steps together. Establishing initial conditions is described below; the remaining tasks are described later in this chapter. The first step in applying transient loads is to establish initial conditions (that is, the condition at Time = 0). A transient dynamic analysis requires two sets of initial conditions (because the equations being solved are of
u& u& second order): initial displacement (uo) and initial velocity ( o ). If no special action is taken, both uo and o are && u
assumed to be zero. Initial accelerations ( o ) are always assumed to be zero, but you can specify nonzero initial accelerations by applying appropriate acceleration loads over a small time interval. The following paragraphs describe how to apply different combinations of initial conditions.
u&
Zero initial displacement and zero initial velocity - These are the default conditions, that is, if uo = o = 0, you do not need to specify anything. You may apply the loads corresponding to the first corner of the load-versus-time curve in the first load step. Nonzero initial displacement and/or nonzero initial velocity - You can set these initial conditions with the IC command. Command(s): IC GUI: Main Menu> Solution> Define Loads> Apply> Initial Condit'n> Define Caution: Be careful not to define inconsistent initial conditions. For instance, if you define an initial velocity at a single DOF, the initial velocity at every other DOF will be 0.0, potentially leading to conflicting initial conditions. In most cases, you will want to define initial conditions at every unconstrained DOF in your model. If these conditions are not the same at every DOF, it is usually much easier to define initial conditions explicitly, as documented below (rather than by using the IC command). See the ANSYS Commands Reference for a discussion of the TIMINT and IC commands. Zero initial displacement and nonzero initial velocity - The nonzero velocity is established by applying small displacements over a small time interval on the part of the structure where velocity is to be specified. For example if
u& o = 0.25, you can apply a displacement of 0.001 over a time interval of 0.004, as shown below. ... TIMINT,OFF D,ALL,UY,.001 TIME,.004 LSWRITE DDEL,ALL,UY TIMINT,ON ...
! ! ! ! ! !
Time integration effects off Small UY displ. (assuming Y-direction velocity) Initial velocity = 0.001/0.004 = 0.25 Write load data to load step file (Jobname.S01) Remove imposed displacements Time integration effects on
Nonzero initial displacement and nonzero initial velocity - This is similar to the above case, except that the imposed displacements are actual values instead of "small" values. For example, if uo = 1.0 and a displacement of 1.0 over a time interval of 0.4: ... TIMINT,OFF D,ALL,UY,1.0 TIME,.4 LSWRITE DDELE,ALL,UY
! ! ! ! !
u& o = 2.5, you would apply
Time integration effects off Initial displacement = 1.0 Initial velocity = 1.0/0.4 = 2.5 Write load data to load step file (Jobname.S01) Remove imposed displacements
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–5
Chapter 5: Transient Dynamic Analysis TIMINT,ON ...
! Time integration effects on
Nonzero initial displacement and zero initial velocity - This requires the use of two substeps (NSUBST,2) with a step change in imposed displacements (KBC,1). Without the step change (or with just one substep), the imposed displacements would vary directly with time, leading to a nonzero initial velocity. The example below shows how
u& to apply uo = 1.0 and o = 0.0: ... TIMINT,OFF ! Time integration effects off for static solution D,ALL,UY,1.0 ! Initial displacement = 1.0 TIME,.001 ! Small time interval NSUBST,2 ! Two substeps KBC,1 ! Stepped loads LSWRITE ! Write load data to load step file (Jobname.S01) ! Transient solution TIMINT,ON ! Time-integration effects on for transient solution TIME,... ! Realistic time interval DDELE,ALL,UY ! Remove displacement constraints KBC,0 ! Ramped loads (if appropriate) ! Continue with normal transient solution procedures ...
Nonzero initial acceleration - This can be approximated by specifying the required acceleration (ACEL) over a small interval of time. For example, the commands to apply an initial acceleration of 9.81 would look like this: ... ACEL,,9.81 ! Initial Y-direction acceleration TIME,.001 ! Small time interval NSUBST,2 ! Two substeps KBC,1 ! Stepped loads ! The structure must be unconstrained in the initial load step, or ! else the initial acceleration specification will have no effect. DDELE, ... ! Remove displacement constraints (if appropriate) LSWRITE ! Write load data to load step file (Jobname.S01) ! Transient solution TIME, ... ! Realistic time interval NSUBST, ... ! Use appropriate time step KBC,0 ! Ramped loads (if appropriate) D, ... ! Constrain structure as desired ! Continue with normal transient solution procedures LSWRITE ! Write load data to load step file (Jobname.S02) ...
See the ANSYS Commands Reference for discussions of the ACEL, TIME, NSUBST, KBC, LSWRITE, DDELE, and KBC commands.
5.4.3. Set Solution Controls This step for a transient dynamic analysis is the same as for a basic structural analysis (see Section 2.3.2: Set Solution Controls in Chapter 2, “Structural Static Analysis”) with the following additions: If you need to establish initial conditions for the full transient dynamic analysis (as described in Section 5.4.2: Establish Initial Conditions), you must do so for the first load step of the analysis. You can then cycle through the Solution Controls dialog box additional times to set individual load step options for the second and subsequent load steps (as described in Section 5.4.7: Repeat Steps 3-6 for Each Load Step).
5.4.3.1. Access the Solution Controls Dialog Box To access the Solution Controls dialog box, choose menu path Main Menu> Solution> Analysis Type> Sol'n Control. The following sections provide brief descriptions of the options that appear on each tab of the dialog 5–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.4: Performing a Full Transient Dynamic Analysis box. For details about how to set these options, select the tab that you are interested in (from within the ANSYS program), and then click the Help button. Chapter 8, “Nonlinear Structural Analysis” also contains details about the nonlinear options introduced in this chapter.
5.4.3.2. Using the Basic Tab The Basic tab is active when you access the dialog box. The controls that appear on the Basic tab provide the minimum amount of data that ANSYS needs for the analysis. Once you are satisfied with the settings on the Basic tab, you do not need to progress through the remaining tabs unless you want to adjust the default settings for the more advanced controls. As soon as you click OK on any tab of the dialog box, the settings are applied to the ANSYS database and the dialog box closes. You can use the Basic tab to set the options listed in Table 2.1: “Basic Tab Options”. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Basic tab, and click the Help button. Special considerations for setting these options in a full transient analysis include: •
When setting ANTYPE and NLGEOM, choose Small Displacement Transient if you are performing a new analysis and you want to ignore large deformation effects such as large deflection, large rotation, and large strain. Choose Large Displacement Transient if you expect large deflections (as in the case of a long, slender bar under bending) or large strains (as in a metal-forming problem). Choose Restart Current Analysis if you want to restart a failed nonlinear analysis, or you have previously completed a static prestress or a full transient dynamic analysis, and you want to extend the time-history.
•
When setting AUTOTS, remember that this load step option (which is also known as time-step optimization in a transient analysis) increases or decreases the integration time step based on the response of the structure. For most problems, we recommend that you turn on automatic time stepping, with upper and lower limits for the integration time step. These limits, specified using DELTIM or NSUBST, help to limit the range of variation of the time step; see Section 5.10.2: Automatic Time Stepping for more information. The default is ON.
•
NSUBST and DELTIM are load step options that specify the integration time step for a transient analysis. The integration time step is the time increment used in the time integration of the equations of motion. You can specify the time increment directly or indirectly (that is, in terms of the number of substeps). The time step size determines the accuracy of the solution: the smaller its value, the higher the accuracy. You should consider several factors in order to calculate a "good" integration time step; see Section 5.10.1: Guidelines for Integration Time Step for details.
•
When setting OUTRES, keep this caution in mind: Caution: By default, only the last substep (time-point) is written to the results file (Jobname.RST) in a full transient dynamic analysis. To write all substeps, set the Frequency so that it writes all of the substeps. Also, by default, only 1000 results sets can be written to the results file. If this number is exceeded (based on your OUTRES specification), the program will terminate with an error. Use the command /CONFIG,NRES to increase the limit (see Chapter 19, “Memory Management and Configuration” in the ANSYS Basic Analysis Guide).
5.4.3.3. Using the Transient Tab You can use the Transient tab to set the options listed in Table 5.1: “Transient Tab Options”. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Transient tab, and click the Help button. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–7
Chapter 5: Transient Dynamic Analysis
Table 5.1 Transient Tab Options Option
For more information about this option, see:
Specify whether time integration effects are on or off (TIMINT)
•
Section 8.6: Performing a Nonlinear Transient Analysis in the ANSYS Structural Analysis Guide
Specify whether to ramp the load change over the load step or to step-apply the load change (KBC)
•
Section 2.5: Stepped Versus Ramped Loads in the ANSYS Basic Analysis Guide
•
Section 2.7.1.5: Stepping or Ramping Loads in the ANSYS Basic Analysis Guide
Specify mass and stiffness damping (ALPHAD, BETAD)
•
Section 5.10.3: Damping in the ANSYS Structural Analysis Guide
Choose the time integration method, Newmark or HHT (TRNOPT)
•
Section 17.2: Transient Analysis in the ANSYS, Inc. Theory Reference
Define integration parameters (TINTP)
•
ANSYS, Inc. Theory Reference
Special considerations for setting these options in a full transient analysis include: •
TIMINT is a dynamic load step option that specifies whether time integration effects are on or off. Time integration effects must be turned on for inertia and damping effects to be included in the analysis (otherwise a static solution is performed), so the default is to include time integration effects. This option is useful when beginning a transient analysis from an initial static solution; that is, the first load steps are solved with the time integration effects off.
•
ALPHAD (alpha, or mass, damping) and BETAD (beta, or stiffness, damping) are dynamic load step options for specifying damping options. Damping in some form is present in most structures and should be included in your analysis. See Section 5.4.4.2: Damping Option for other damping options.
•
TRNOPT (TINTOPT) specifies the time integration method to be used. The default is Newmark method.
•
TINTP is a dynamic load step option that specifies transient integration parameters. Transient integration parameters control the nature of the Newmark and HHT time integration techniques.
5.4.3.4. Using the Remaining Solution Controls Tabs The options on the remaining tabs in the Solution Controls dialog box for a full transient analysis are the same as the ones you can set for a static structural analysis. See the following sections of Chapter 2, “Structural Static Analysis” for a list of these options: •
Section 2.3.2.4: Using the Sol'n Options Tab
•
Section 2.3.2.5: Using the Nonlinear Tab
•
Section 2.3.2.6: Using the Advanced NL Tab. Exception: You cannot use arc-length options in a full transient analysis.
5.4.4. Set Additional Solution Options The additional solution options that you can set for a full transient analysis are mostly the same as the ones you can set for a static structural analysis. For a general description of what additional solution options are, along with descriptions of those options that are the same, see the following sections of Chapter 2, “Structural Static Analysis”: 5–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.4: Performing a Full Transient Dynamic Analysis •
Section 2.3.3: Set Additional Solution Options
•
Section 2.3.3.1: Stress Stiffening Effects
•
Section 2.3.3.2: Newton-Raphson Option
•
Section 2.3.3.7: Creep Criteria
•
Section 2.3.3.8: Printed Output
•
Section 2.3.3.9: Extrapolation of Results
Additional solution options for a full transient analysis that differ from those for a static analysis, or have different descriptions are presented in the following sections.
5.4.4.1. Prestress Effects You may include prestress effects in your analysis. This requires element files from a previous static (or transient) analysis; see Section 5.9: Performing a Prestressed Transient Dynamic Analysis for details. Command(s): PSTRES GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options
5.4.4.2. Damping Option Use this load step option to include damping. Damping in some form is present in most structures and should be included in your analysis. In addition to setting ALPHAD and BETAD on the Solution Controls dialog box (as described in Section 5.4.3.3: Using the Transient Tab), you can specify the following additional forms of damping for a full transient dynamic analysis: •
Material-dependent beta damping (MP,DAMP)
•
Element damping (COMBIN7, and so on)
To use the MP form of damping: Command(s): MP,DAMP GUI: Main Menu> Solution> Load Step Opts> Other> Change Mat Props> Material Models> Structural> Damping Note that constant material damping coefficient (MP,DMPR) is not applicable in transient analysis. See Section 5.10.3: Damping for further details.
5.4.4.3. Mass Matrix Formulation Use this analysis option to specify a lumped mass matrix formulation. We recommend the default formulation for most applications. However, for some problems involving "skinny" structures, such as slender beams or very thin shells, the lumped mass approximation might provide better results. Also, the lumped mass approximation can result in a shorter run time and lower memory requirements. To use this option: Command(s): LUMPM GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options
5.4.5. Apply the Loads You are now ready to apply loads for the analysis. Table 2.5: “Loads Applicable in a Static Analysis” summarizes the loads applicable to a transient dynamic analysis. Except for inertia loads, you can define loads either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). Section 2.3.4: Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–9
Chapter 5: Transient Dynamic Analysis Apply the Loads describes the types of loads that are applicable. In an analysis, loads can be applied, removed, operated on, or deleted. For a general discussion of solid-model loads versus finite-element loads, see Chapter 2, “Loading” in the ANSYS Basic Analysis Guide. You can also apply time-dependent boundary conditions by defining a one-dimensional table (TABLE type array parameter). See Section 2.3.4.2.1: Applying Loads Using TABLE Type Array Parameters.
5.4.6. Save the Load Configuration for the Current Load Step As described in Section 5.4.2: Establish Initial Conditions, you need to apply loads and save the load configuration to a load step file for each corner of the load-versus-time curve. You may also want to have an additional load step that extends past the last time point on the curve to capture the response of the structure after the transient loading. Command(s): LSWRITE GUI: Main Menu> Solution> Load Step Opts> Write LS File
5.4.7. Repeat Steps 3-6 for Each Load Step For each load step that you want to define for a full transient dynamic analysis, you need to repeat steps 3-6. That is, for each load step, reset any desired solution controls and options, apply loads, and write the load configuration to a file. For each load step, you can reset any of these load step options: TIMINT, TINTP, ALPHAD, BETAD, MP,DAMP, TIME, KBC, NSUBST, DELTIM, AUTOTS, NEQIT, CNVTOL, PRED, LNSRCH, CRPLIM, NCNV, CUTCONTROL, OUTPR, OUTRES, ERESX, and RESCONTROL. An example load step file is shown below: TIME, ... Loads ... KBC, ... LSWRITE TIME, ... Loads ... KBC, ... LSWRITE TIME, ... Loads ... KBC, ... LSWRITE Etc.
! Time at the end of 1st transient load step ! Load values at above time ! Stepped or ramped loads ! Write load data to load step file ! Time at the end of 2nd transient load step ! Load values at above time ! Stepped or ramped loads ! Write load data to load step file ! Time at the end of 3rd transient load step ! Load values at above time ! Stepped or ramped loads ! Write load data to load step file
5.4.8. Save a Backup Copy of the Database Save a copy of the database to a named file. You can then retrieve your model by reentering the ANSYS program and issuing RESUME. Command(s): SAVE GUI: Utility Menu> File> Save as
5.4.9. Start the Transient Solution Use one of these methods to start the transient solution: Command(s): LSSOLVE GUI: Main Menu> Solution> Solve> From LS Files For additional ways to create and solve multiple load steps (the array parameter method and the multiple SOLVE method), see Section 3.14: Solving Multiple Load Steps in the ANSYS Basic Analysis Guide. 5–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.4: Performing a Full Transient Dynamic Analysis
5.4.10. Exit the Solution Processor Use one of these methods to exit the solution processor: Command(s): FINISH GUI: Close the Solution menu.
5.4.11. Review the Results You review results for a full transient analysis in the same way that you review results for most structural analyses. See Section 2.3.6: Review the Results in Chapter 2, “Structural Static Analysis”.
5.4.11.1. Postprocessors You can review these results using either POST26, which is the time-history postprocessor, or POST1, which is the general postprocessor. •
POST26 is used to review results at specific points in the model as functions of time.
•
POST1 is used to review results over the entire model at specific time points.
Some typical postprocessing operations for a transient dynamic analysis are explained below. For a complete description of all postprocessing functions, see Section 4.1: What Is Postprocessing? in the ANSYS Basic Analysis Guide.
5.4.11.2. Points to Remember The points to remember for a full transient analysis are the same as those for most structural analyses. See Section 2.3.6.2: Points to Remember in Chapter 2, “Structural Static Analysis”.
5.4.11.3. Using POST26 POST26 works with tables of result item versus time, known as variables. Each variable is assigned a reference number, with variable number 1 reserved for time. 1.
Define the variables. Command(s): NSOL (primary data, that is, nodal displacements) ESOL (derived data, that is, element solution data, such as stresses) RFORCE (reaction force data) FORCE (total force, or static, damping, or inertia component of total force) SOLU (time step size, number of equilibrium iterations, response frequency, and so on) GUI: Main Menu> TimeHist Postpro> Define Variables Note — In the mode superposition or reduced methods, only static force is available with the FORCE command.
2.
Graph or list the variables. By reviewing the time-history results at strategic points throughout the model, you can identify the critical time points for further POST1 postprocessing. Command(s): PLVAR (graph variables) PRVAR, EXTREM (list variables) GUI: Main Menu> TimeHist Postpro> Graph Variables Main Menu> TimeHist Postpro> List Variables Main Menu> TimeHist Postpro> List Extremes
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–11
Chapter 5: Transient Dynamic Analysis
5.4.11.4. Other Capabilities Many other postprocessing functions, such as performing math operations among variables, moving variables into array parameters, and moving array parameters into variables, are available in POST26. See Chapter 6, “The Time-History Postprocessor (POST26)” in the ANSYS Basic Analysis Guide for details.
5.4.11.5. Using POST1 1.
Read in model data from the database file. Command(s): RESUME GUI: Utility Menu> File> Resume from
2.
Read in the desired set of results. Use the SET command to identify the data set by load step and substep numbers or by time. Command(s): SET GUI: Main Menu> General Postproc> Read Results> By Time/Freq
3.
Perform the necessary POST1 operations. The typical POST1 operations that you perform for a transient dynamic analysis are the same as those that you perform for a static analysis. See Section 2.3.6.4: Typical Postprocessing Operations for a list of these operations. Note — If you specify a time for which no results are available, the results that are stored will be a linear interpolation between the two nearest time points.
5.4.12. Sample Input for a Full Transient Dynamic Analysis A sample input listing for a full transient analysis is shown below: ! Build the Model /FILNAM,... /TITLE,... /PREP7 -----! Generate model --FINISH
! Jobname ! Title ! Enter PREP7
! Apply Loads and Obtain the Solution /SOLU ! Enter SOLUTION ANTYPE,TRANS ! Transient analysis TRNOPT,FULL ! Full method D,... ! Constraints F,... ! Loads SF,... ALPHAD,... ! Mass damping BETAD,... ! Stiffness damping KBC,... ! Ramped or stepped loads TIME,... ! Time at end of load step AUTOTS,ON ! Auto time stepping DELTIM,... ! Time step size OUTRES,... ! Results file data options LSWRITE ! Write first load step -----! Loads, time, etc. for 2nd load step --LSWRITE ! Write 2nd load step SAVE LSSOLVE,1,2 ! Initiate multiple load step solution FINISH ! ! Review the Results /POST26 SOLU,... ! Store solution summary data
5–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.5: Performing a Mode Superposition Transient Dynamic Analysis NSOL,... ESOL,,,, RFORCE,... PLVAR,... PRVAR,... FINISH
! ! ! ! !
/POST1 SET,... ! PLDISP,... ! PRRSOL,... ! PLNSOL,... ! PRERR ! -----! Other postprocessing as --FINISH
Store nodal result as a variable Store element result as a variable Store reaction as a variable Plot variables List variables
Read desired set of results into database Deformed shape Reaction loads Contour plot of nodal results Global percent error (a measure of mesh adequacy) desired
See the ANSYS Commands Reference for discussions of the ANTYPE, TRNOPT, ALPHAD, BETAD, KBC, TIME, AUTOTS, DELTIM, OUTRES, LSWRITE, LSSOLVE, SOLU, NSOL, ESOL, RFORCE, PLVAR, PRVAR, PLDISP, PRRSOL, PLNSOL, and PRERR commands.
5.5. Performing a Mode Superposition Transient Dynamic Analysis The mode superposition method sums factored mode shapes (obtained from a modal analysis) to calculate the dynamic response. This method is available in the ANSYS Multiphysics, ANSYS Mechanical, ANSYS Structural, and ANSYS Professional products. The procedure to use the method consists of five main steps: 1.
Build the model.
2.
Obtain the modal solution.
3.
Obtain the mode superposition transient solution.
4.
Expand the mode superposition solution.
5.
Review the results.
5.5.1. Build the Model Building the model for a mode superposition transient dynamic analysis is the same as that described for the full method. See Section 5.4.1: Build the Model for more information.
5.5.2. Obtain the Modal Solution Chapter 3, “Modal Analysis” describes how to obtain a modal solution. Following are some additional hints: •
The mode-extraction method should be Block Lanczos (default), reduced, subspace, PowerDynamics, or QR damped. (The other methods, unsymmetric and damped, do not apply to mode superposition.) PowerDynamics does not create a load vector.
•
Be sure to extract all modes that may contribute to the dynamic response.
•
If PowerDynamics was used for the modal solution, no nonzero loads or displacements are allowed (that is, only u = 0 is valid as the initial condition). PowerDynamics does not create a load vector; therefore, the LVSCALE command is not valid unless the scale factor is set to zero.
•
For the reduced mode-extraction method, include those master degrees of freedom at those nodes at which forces and gap conditions are to be defined.
•
If you use the QR damped mode-extraction method, you must specify any damping (ALPHAD, BETAD, MP,DAMP, or element damping including gyroscopic) that you want to include during preprocessing or Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–13
Chapter 5: Transient Dynamic Analysis in the modal analysis. (ANSYS ignores damping specified during the mode superposition harmonic analysis.) You can set a constant damping ratio (DMPRAT) or define the damping ratio as a function of mode (MDAMP) in a modal superposition harmonic analysis. Note that constant material damping coefficient (MP,DMPR) is not applicable in transient analysis. •
Specify displacement constraints, if any. These constraints will be ignored if they are specified in the mode superposition transient solution instead of in the modal solution.
•
If you need to apply element loads (pressures, temperatures, accelerations, and so on) in the transient dynamic analysis, you must specify them in the modal analysis. The loads are ignored for the modal solution, but a load vector will be calculated and written to the mode shape file (Jobname.MODE). You can then use this load vector for the transient solution.
•
The modes need not be expanded for the mode superposition solution. (If you want to review mode shapes from a reduced modal solution, however, you must expand the mode shapes.)
•
The model data (for example, nodal rotations) should not be changed between the modal and transient analyses.
5.5.3. Obtain the Mode Superposition Transient Solution In this step, the program uses mode shapes extracted by the modal solution to calculate the transient response.
5.5.3.1. Points to Remember •
The mode shape file (Jobname.MODE) must be available.
•
The database must contain the same model for which the modal solution was obtained.
5.5.3.2. Obtaining the Solution The procedure to obtain the mode superposition transient solution is described below: 1.
Enter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define the analysis type and analysis options. These are the same as the analysis options that are described for the full method (in Section 5.4.3: Set Solution Controls and Section 5.4.4: Set Additional Solution Options), except for the following differences:
5–14
•
You cannot use the Solution Controls dialog box to define analysis type and analysis options for a mode superposition transient analysis. Instead, you must set them using the standard set of ANSYS solution commands (which are listed in Section 5.4.3: Set Solution Controls and Section 5.4.4: Set Additional Solution Options) and the standard corresponding menu paths.
•
Restarts are not available (ANTYPE).
•
Choose the mode superposition method of solution (TRNOPT).
•
When you specify a mode superposition transient analysis, a Solution menu that is appropriate for that specific type of analysis appears. The Solution menu will be either “abridged” or “unabridged,” depending on the actions you took prior to this step in your ANSYS session. The abridged menu contains only those solution options that are valid and/or recommended for mode superposition transient analyses. If you are on the abridged Solution menu and you want to access other solution options (that is, solution options that are valid for you to use, but their use may not be encouraged for this type of analysis), select the Unabridged Menu option from the Solution menu. For details, see Section 3.11.1: Using Abridged Solution Menus in the ANSYS Basic Analysis Guide. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.5: Performing a Mode Superposition Transient Dynamic Analysis •
Specify the number of modes you want to use for the solution (TRNOPT). This determines the accuracy of the transient solution. At a minimum, you should use all modes that you think will contribute to the dynamic response. If you expect higher frequencies to be excited, for example, the number of modes specified should include the higher modes. The default is to use all modes calculated in the modal solution.
•
If you do not want to use rigid body (0 frequency) modes, use MINMODE on the TRNOPT command to skip over them.
•
Nonlinear options (NLGEOM, SSTIF, NROPT) are not available.
3.
Define gap conditions, if any. They can only be defined between two master degree of freedom (DOF) nodes or between master DOF nodes and ground. When a non-reduced mode-extraction method is used, a master DOF implies an unconstrained, active DOF. If you used the QR damped mode-extraction method, gap conditions are not supported. More details about gap conditions are presented in Section 5.6.1.3.1: Gap Conditions. Command(s): GP GUI: Main Menu> Solution> Dynamic Gap Cond> Define
4.
Apply loads to the model. The following loading restrictions apply in a mode superposition transient dynamic analysis: •
Only forces, accelerations, and a load vector created in the modal analysis are valid. Imposed nonzero displacements are ignored. Use the LVSCALE command (Main Menu> Solution> Define Loads> Apply> Load Vector> For Mode Super) to apply the load vector from the modal solution.
•
If mode shapes from a reduced modal solution are being used, forces may be applied only at master DOF.
Multiple load steps are usually required to specify the load history in a transient analysis. The first load step is used to establish initial conditions, and second and subsequent load steps are used for the transient loading, as explained next. 5.
Establish initial conditions. In modal superposition transient analyses, a first solution is done at TIME = 0. This establishes the initial condition and time step size for the entire transient analysis. Generally, the only load applicable for the first load step is initializing nodal forces. For this pseudo-static analysis, the mode superposition method may yield poor results at TIME = 0 if nonzero loads are applied. The following load step options are available for the first load step:
Table 5.2 Options for the First Load Step-Mode Superposition Analysis Option
Command
GUI Path
Dynamics Options Transient Integration Paramet- TINTP ers
Main Menu> Solution> Load Step Opts> Time/Frequenc> Time Integration
Load Vector
LVSCALE
Main Menu> Solution> Define Loads> Apply> Load Vector> For Mode Super
Damping
ALPHAD, BETAD, DMPRAT, MP, MDAMP
Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping Main Menu> Solution> Load Step Opts> Other> Change Mat Props> Material Models> Structural> Damping
General Options
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–15
Chapter 5: Transient Dynamic Analysis Option Integration Time Step
Command
GUI Path
DELTIM
Main Menu> Solution> Load Step Opts> Time/Frequenc> Time-Time Step
OUTPR
Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout
Output Control Options Printed Output
•
Dynamics options include the following: – Transient Integration Parameters (TINTP) Transient integration parameters control the nature of the Newmark time integration technique. The default is to use the constant average acceleration scheme; see your ANSYS, Inc. Theory Reference for further details. –
Load Vector (LVSCALE) The load vector option allows you to apply a load vector created by the modal solution as one of the loads. You can use such a load vector to apply element loads (pressures, temperatures, and so on) on the model.
–
Damping Damping in some form is present in most structures and should be included in your analysis. You can specify five forms of damping in a mode superposition transient dynamic analysis: → Alpha (mass) damping (ALPHAD) → Beta (stiffness) damping (BETAD) → Constant damping ratio (DMPRAT) → Material-dependent beta damping (MP,DAMP) → Modal damping (MDAMP) Remember that, as described earlier in Section 5.5.2: Obtain the Modal Solution, any damping that you specify in the mode superposition transient analysis is ignored if you used the QR damped mode-extraction method. Constant material damping coefficient (MP,DMPR) is not applicable in transient analysis. See Section 5.10.3: Damping for further details.
•
The only valid general option for the first load step is integration time step (DELTIM), which is assumed to be constant throughout the transient. By default, the integration time step is assumed to be 1/(20f), where f is the highest frequency chosen for the solution. The DELTIM command is valid only in the first load step and is ignored in subsequent load steps. Note — If you do issue the TIME command in the first load step, it will be ignored. The first solution is always a static solution at TIME = 0.
•
6.
5–16
The output control option for the first load step is printed output (OUTPR). Use this option to control printout of the displacement solution at the master DOF.
Write the first load step to a load step file (Jobname.S01) by issuing the LSWRITE command. Command(s): LSWRITE Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.5: Performing a Mode Superposition Transient Dynamic Analysis GUI: Main Menu> Solution> Load Step Opts> Write LS File 7.
Specify loads and load step options for the transient loading portion, writing each load step to a load step file (LSWRITE). •
General options include the following: –
Time Option (TIME) This option specifies time at the end of the load step.
–
Load Vector (LVSCALE) The load vector option allows you to apply a load vector created by the modal solution as one of the loads.
–
Stepped or Ramped Loads (KBC) This option indicates whether to ramp the load change over the load step (KBC) or to step-apply the load change (KBC,1). The default is ramped.
•
Output control options include the following: –
Printed Output (OUTPR) Use this option to control printed output.
–
Database and Results File Output (OUTRES) This option controls the data on the reduced displacement file.
The only valid label on these commands is NSOL (nodal solution). The default for OUTRES is to write the solution for every fourth time-point to the reduced displacement file (unless there are gap conditions defined, in which case the default is to write every solution). 8.
If you used either the Block Lanczos (default) or subspace option for the modal analysis (MODOPT,LANB or MODOPT,SUBSP), you may use a nodal component with the OUTRES,NSOL command to limit the displacement data written to the reduced displacement file Jobname.RDSP. The expansion pass will only produce valid results for those nodes and for those elements in which all of the nodes of the elements have been written to the .RDSP file. To use this option, first suppress all writing by invoking OUTRES,NSOL,NONE, then specify the item(s) of interest by invoking OUTRES,NSOL,FREQ,COMP. Repeat the OUTRES command for any additional nodal components that you want to write to the .RDSP file. Only one output frequency is allowed - ANSYS uses the last frequency specified by OUTRES.
9.
Save a backup copy of the database to a named file. Command(s): SAVE GUI: Utility Menu> File> Save as
10. Start the transient solution. Command(s): LSSOLVE GUI: Main Menu> Solution> Solve> From LS Files 11. Leave SOLUTION. Command(s): FINISH GUI: Close the Solution menu.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–17
Chapter 5: Transient Dynamic Analysis The mode superposition transient solution is written to the reduced displacement file, Jobname.RDSP, regardless of whether the subspace, Block Lanczos, reduced, PowerDynamics, or QR damped method was used for the modal solution. You will therefore need to expand the solution if you are interested in stress results.
5.5.4. Expand the Mode Superposition Solution The procedure for the expansion pass is the same as described for the reduced method (see Section 5.6.3: Expand the Solution (Expansion Pass)). Jobname.TRI is needed only if the reduced method was used for the modal solution. The output from the expansion pass includes the structural results file, Jobname.RST, containing expanded results.
5.5.5. Review the Results Results consist of displacements, stresses, and reaction forces at each time-point for which the solution was expanded. You can review these results using POST26 or POST1, as explained for the full method (see Section 5.4.11: Review the Results). Note — In the mode superposition or reduced methods, only static force is available with the FORCE command.
5.5.6. Sample Input for a Mode Superposition Transient Dynamic Analysis A sample input listing for a mode superposition transient analysis is shown below: ! Build the Model /FILNAM,... /TITLE,... /PREP7 -----! Generate model --FINISH
! Jobname ! Title ! Enter PREP7
! Obtain the Modal Solution /SOLU ! Enter SOLUTION ANTYPE,MODAL ! Modal analysis MODOPT,REDU ! Reduced method M,... ! Master DOF TOTAL,... D,... ! Constraints SF,... ! Element loads ACEL,... SAVE SOLVE FINISH ! Obtain the Mode Superposition Transient Solution /SOLU ! Reenter SOLUTION ANTYPE,TRANS ! Transient analysis TRNOPT,MSUP,... ! Mode superposition method LVSCALE,... ! Scale factor for element loads F,... ! Nodal Loads MDAMP,... ! Modal damping ratios DELTIM,... ! Integration time step sizes LSWRITE ! Write first load step (Remember: the first load step --! is solved statically at time=0.) -----! Loads, etc. for 2nd load step TIME,... ! Time at end of second load step KBC,... ! Ramped or stepped loads OUTRES,... ! Results-file data controls --LSWRITE ! Write 2nd load step (first transient load step) SAVE
5–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.6: Performing a Reduced Transient Dynamic Analysis LSSOLVE FINISH
! Initiate multiple load step solution
! Review results of the mode superposition solution /POST26 ! Enter POST26 FILE,,RDSP ! Results file is Jobname.RDSP SOLU,... ! Store solution summary data NSOL,... ! Store nodal result as a variable PLVAR,... ! Plot variables PRVAR,... ! List variables FINISH ! Expand the Solution /SOLU ! Reenter SOLUTION EXPASS,ON ! Expansion pass NUMEXP,... ! No. of solutions to expand; time range OUTRES,... ! Results-file data controls SOLVE FINISH ! Review the Results of the Expanded Solution /POST1 SET,... ! Read desired set of results into database PLDISP,... ! Deformed shape PRRSOL,... ! Reaction loads PLNSOL,... ! Contour plot of nodal results PRERR ! Global percent error (a measure of mesh adequacy) -----! Other postprocessing as desired --FINISH
See the ANSYS Commands Reference for discussions of the ANTYPE, MODOPT, M, TOTAL, ACEL, TRNOPT, LVSCALE, MDAMP, DELTIM, TIME, KBC, OUTRES, LSSOLVE, FILE, SOLU, NSOL, PLVAR, PRVAR, EXPASS, NUMEXP, OUTRES, PLDISP, PRRSOL, PLNSOL, and PRERR commands.
5.6. Performing a Reduced Transient Dynamic Analysis The reduced method, as its name implies, uses reduced matrices to calculate the dynamic response. It is available in the ANSYS Multiphysics, ANSYS Mechanical, and ANSYS Structural products. You should consider using this method if you do not want to include nonlinearities (other than simple node-to-node contact) in the analysis. The procedure for a reduced transient dynamic analysis consists of these main steps: 1.
Build the model.
2.
Obtain the reduced solution.
3.
Review the results of the reduced solution.
4.
Expand the solution (expansion pass).
5.
Review the results of the expanded solution.
Of these, the first step is the same as for the full method, except that no nonlinearities are allowed (other than simple node-to-node contact, which is specified in the form of a gap condition instead of an element type). Details of the other steps are explained below.
5.6.1. Obtain the Reduced Solution By reduced solution, we mean the degree of freedom solution calculated at the master DOF. The tasks required to obtain the reduced solution are explained in the following sections. For the following tasks, you need to first enter the SOLUTION processor. Command(s): /SOLU Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–19
Chapter 5: Transient Dynamic Analysis GUI: Main Menu> Solution
5.6.1.1. Define the Analysis Type and Options These are the same as the analysis options that are described for the full method (in Section 5.4.3: Set Solution Controls and Section 5.4.4: Set Additional Solution Options) except for the following differences: •
You cannot use the Solution Controls dialog box to define analysis type and analysis options for a reduced transient dynamic analysis. Instead, you must set them using the standard set of ANSYS solution commands (which are listed in Section 5.4.3: Set Solution Controls and Section 5.4.4: Set Additional Solution Options) and the standard corresponding menu paths.
•
Restarts are not available (ANTYPE).
•
Choose the reduced method of solution (TRNOPT).
•
When you specify a reduced transient analysis, a Solution menu that is appropriate for that specific type of analysis appears. The Solution menu will be either “abridged” or “unabridged,” depending on the actions you took prior to this step in your ANSYS session. The abridged menu contains only those solution options that are valid and/or recommended for reduced transient analyses. If you are on the abridged Solution menu and you want to access other solution options (that is, solution options that are valid for you to use, but their use may not be encouraged for this type of analysis), select the Unabridged Menu option from the Solution menu. For details, see Section 3.11.1: Using Abridged Solution Menus in the ANSYS Basic Analysis Guide.
•
Nonlinear options (NLGEOM, SSTIF, NROPT) are not available.
5.6.1.2. Define Master Degrees of Freedom Master DOF are essential degrees of freedom that characterize the dynamic behavior of the structure. For a reduced transient dynamic analysis, master DOF are also required at locations where you want to define gap conditions, forces, or nonzero displacements. You can list the defined master DOF or delete master DOF as well. See Section 3.14: Matrix Reduction for guidelines to choose master DOF. Command(s): M, MGEN, TOTAL, MLIST, MDELE GUI: Main Menu> Solution> Master DOFs> User Selected> Define Main Menu> Solution> Master DOFs> User Selected> Copy Main Menu> Solution> Master DOFs> Program Selected Main Menu> Solution> Master DOFs> User Selected> List All Main Menu> Solution> Master DOFs> User Selected> Delete
5.6.1.3. Define Gap Conditions Define any gap conditions. Command(s): GP GUI: Main Menu> Solution> Dynamic Gap Cond> Define You can also list the defined gaps and delete gaps. Command(s): GPLIST, GPDELE GUI: Main Menu> Solution> Dynamic Gap Cond> List All Main Menu> Solution> Dynamic Gap Cond> Delete
5.6.1.3.1. Gap Conditions Gap conditions can only be defined between two master degree of freedom (DOF) nodes or between master DOF nodes and ground, as shown in the following figure. 5–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.6: Performing a Reduced Transient Dynamic Analysis
Figure 5.2 Examples of Gap Conditions
Gap conditions are similar to gap elements and are specified between surfaces that are expected to contact (impact) each other during the transient. The ANSYS program accounts for the gap force, which develops when the gap closes, by using an equivalent nodal load vector. Some guidelines to define gap conditions are presented below: •
Use enough gap conditions to obtain a smooth contact stress distribution between the contacting surfaces.
•
Define a reasonable gap stiffness. If the stiffness is too low, the contacting surfaces may overlap too much. If the stiffness is too high, a very small time step will be required during impact. A general recommendation is to specify a gap stiffness that is one or two orders of magnitude higher than the adjacent element stiffness. You can estimate the adjacent element stiffness using AE/L, where A is the contributing area around the gap condition, E is the elastic modulus of the softer material at the interface, and L is the depth of the first layer of elements at the interface.
•
The nonlinear gap damping provided through the DAMP field of the GP command runs faster than a full transient analysis using a gap element COMBIN40. Only TRNOPT = MSUP allows the nonlinear gap damping action. Damping conditions are ignored for the reduced transient analysis method.
5.6.1.4. Apply Initial Conditions to the Model The following loading restrictions apply in a reduced transient dynamic analysis: •
Only displacements, forces, and translational accelerations (such as gravity) are valid. Acceleration loading is not allowed if the model contains any master DOF at any nodes with rotated nodal coordinate systems.
•
Forces and nonzero displacements must be applied only at master DOF.
As mentioned for the full method, multiple load steps are usually required to specify the load history in a transient analysis. The first load step is used to establish initial conditions, and second and subsequent load steps are used for the transient loading, as explained next. •
Establish initial conditions. The only initial condition that may be explicitly established is the initial dis-
u&
&& u
placement (uo); that is, initial velocity and acceleration must be zero ( o = 0, o = 0). Displacements cannot be deleted in subsequent load steps, therefore they cannot be used to specify an initial velocity. In a reduced transient analysis, a static solution is always performed as the first solution, using the loads given, to determine uo. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–21
Chapter 5: Transient Dynamic Analysis •
Specify load step options for the first load step. Valid options appear in Table 5.3: “Options for the First Load Step-Reduced Analysis”.
Table 5.3 Options for the First Load Step-Reduced Analysis Option
Command
GUI Path
Dynamics Options Transient Integration Parameters
TINTP
Main Menu> Solution> Load Step Opts> Time/Frequenc> Time Integration
Damping
ALPHAD, BETAD, MP,DAMP
Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping Main Menu> Solution> Load Step Opts> Other> Change Mat Props> Material Models> Structural> Damping
DELTIM
Main Menu> Solution> Load Step Opts> Time/Frequenc> Time- Time Step
OUTPR
Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout
General Options Integration Time Step Output Control Options Printed Output
5.6.1.4.1. Dynamics Options Dynamic options include the following: •
Transient Integration Parameters (TINTP) Transient integration parameters control the nature of the Newmark time integration technique. The default is to use the constant average acceleration scheme; see the ANSYS, Inc. Theory Reference for further details.
•
Damping Damping in some form is present in most structures and should be included in your analysis. You can specify four forms of damping in a reduced transient dynamic analysis: –
Alpha (mass) damping (ALPHAD)
–
Beta (stiffness) damping (BETAD)
–
Material-dependent beta damping (MP,DAMP)
–
Element damping (COMBIN7, and so on)
See Section 5.10.3: Damping for further details.
5.6.1.4.2. General Options The only valid general option is Integration Time Step (DELTIM). The integration time step is assumed to be constant throughout the transient. Note — If you do issue the TIME command for the first load step, it will be ignored. The first solution is always a static solution at TIME = 0.
5–22
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.6: Performing a Reduced Transient Dynamic Analysis
5.6.1.4.3. Output Control Options Use the Printed Output (OUTPR) option to output the displacement solution at the master DOF.
5.6.1.5. Write the First Load Step to a Load Step File Write the first load step to a load step file (Jobname.S01). Command(s): LSWRITE GUI: Main Menu> Solution> Load Step Opts> Write LS File
5.6.1.6. Specify Loads and Load Step Options Specify loads and load step options for the transient loading portion, writing each load step to a load step file (LSWRITE). The following load step options are valid for the transient load steps: •
•
General Options –
Time (specifies the time at the end of the load step) (TIME)
–
Stepped (KBC,1) or ramped loads (KBC)
Output Controls – Printed output (OUTPR) – Reduced displacement file (OUTRES) The only valid label on these commands is NSOL (nodal solution). The default for OUTRES is to write the solution for every fourth time-point to the reduced displacement file (unless there are gap conditions defined, in which case the default is to write every solution).
5.6.1.7. Obtaining the Solution Solving a reduced transient dynamic analysis involves the same steps as those involved in solving a full transient analysis. See the following sections for a description of those steps: •
Section 5.4.8: Save a Backup Copy of the Database
•
Section 5.4.9: Start the Transient Solution
•
Section 5.4.10: Exit the Solution Processor
5.6.2. Review the Results of the Reduced Solution Results from the reduced transient dynamic solution are written to the reduced displacement file, Jobname.RDSP. They consist of time-varying displacements at the master DOF. You can review the master DOF displacements as a function of time using POST26. (POST1 cannot be used, because the complete solution at all DOF is not available.) The procedure to use POST26 is the same as described for the full method, except for the following differences: •
Before defining the POST26 variables, use the FILE command (Main Menu> TimeHist Postpro> Settings> File) to specify that data are to be read from Jobname.RDSP. For example, if the jobname is TRANS, the
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–23
Chapter 5: Transient Dynamic Analysis FILE command would be: FILE,TRANS,RDSP. (By default, POST26 looks for a results file, which is not written by a reduced transient solution.) •
Only nodal degree of freedom data (at master DOF) are available for processing, so you can use only the NSOL command to define variables.
5.6.3. Expand the Solution (Expansion Pass) The expansion pass starts with the reduced solution and calculates the complete displacement, stress, and force solution at all degrees of freedom. These calculations are done only at time points that you specify. Before you begin the expansion pass, therefore, you should review the results of the reduced solution (using POST26) and identify the critical time points. Note — An expansion pass is not always required. For instance, if you are interested mainly in displacements at specific points on the structure, then the reduced solution could satisfy your requirements. However, if you want to determine displacements at non-master DOF, or if you are interested in the stress or force solution, then you must perform an expansion pass.
5.6.3.1. Points to Remember •
The .RDSP, .EMAT, .ESAV, .DB, and .TRI files from the reduced solution must be available.
•
The database must contain the same model for which the reduced solution was calculated.
The procedure for the expansion pass is explained below.
5.6.3.2. Expanding the Solution 1.
Reenter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution Note — You must explicitly leave SOLUTION (using the FINISH command) and reenter (/SOLU) before performing the expansion pass.
2.
Activate the expansion pass and its options.
Table 5.4 Expansion Pass Options Option Expansion Pass On/Off
Command EXPASS
GUI Path Main Menu> Solution> Analysis Type> ExpansionPass
No. of Solutions to be Expan- NUMEXP ded
Main Menu> Solution> Load Step Opts> ExpansionPass> Range of Solu's
Single Solution to Expand
Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> By Time/Freq
•
EXPSOL
Option: Expansion Pass On/Off (EXPASS) Choose ON.
•
5–24
Option: Number of Solutions to be Expanded (NUMEXP)
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.6: Performing a Reduced Transient Dynamic Analysis Specify the number. This number of evenly spaced solutions will be expanded over the specified time range. The solutions nearest these times will be expanded. Also specify whether to calculate stresses and forces (default is to calculate both). •
Option: Single Solution to Expand (EXPSOL) Use this option to identify a single solution for expansion if you do not need to expand multiple solutions in a range. You can specify it either by load step and substep number or by time. Also specify whether to calculate stresses and forces (default is to calculate both).
3.
Specify load step options. The only options valid for a transient dynamic expansion pass are output controls: •
Output Controls –
Printed Output (OUTPR) Use this option to include any results data on the output file (Jobname.OUT).
–
Database and Results File Output (OUTRES) This option controls the data on the results file (Jobname.RST).
–
Extrapolation of Results (ERESX) Use this option to review element integration point results by copying them to the nodes instead of extrapolating them (default). Note — The FREQ field on OUTPR and OUTRES can only be ALL or NONE. ERESX allows you to review element integration point results by copying them to the nodes instead of extrapolating them (default).
4.
Start expansion pass calculations. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
5.
Repeat steps 2, 3, and 4 for additional solutions to be expanded. Each expansion pass is stored as a separate load step on the results file.
6.
Leave SOLUTION. Command(s): FINISH GUI: Close the Solution window.
5.6.4. Review the Results of the Expanded Solution You review results for an expansion pass in the same way that you review results for most structural analyses. See Section 2.3.6: Review the Results in Chapter 2, “Structural Static Analysis”. You can review these results using POST1. (If you expanded solutions at several time points, you can also use POST26 to obtain graphs of stress versus time, strain versus time, and so on.) The procedure to use POST1 (or POST26) is the same as described for the full method.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–25
Chapter 5: Transient Dynamic Analysis
5.7. Sample Reduced Transient Dynamic Analysis (GUI Method) In this example, you will perform a transient dynamic analysis using the reduced method to determine the transient response to a constant force with a finite rise in time. In this problem, a steel beam supporting a concentrated mass is subjected to a dynamic load.
5.7.1. Problem Description A steel beam of length l and geometric properties shown in Problem Specifications is supporting a concentrated mass, m. The beam is subjected to a dynamic load F(t) with a rise time tr and a maximum value F1. If the weight of the beam is considered to be negligible, determine the time of maximum displacement response tmax and the response ymax. Also determine the maximum bending stress σbend in the beam. The beam is not used in this solution and its area is arbitrarily input as unity. The final time of 0.1 sec allows the mass to reach its largest deflection. One master degree of freedom is selected at the mass in the lateral direction. A static solution is done at the first load step. Symmetry could have been used in this model. The time of maximum response (0.092 sec) is selected for the expansion pass calculation.
5.7.2. Problem Specifications The following material properties are used for this problem: E = 30 x 103 ksi m = 0.0259067 kips-sec2/in The following geometric properties are used for this problem: l = 800.6 in4 h = 18 in l = 20 ft = 240 in. Loading for this problem is: F1 = 20 kips tr = 0.075 sec
5–26
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.7: Sample Reduced Transient Dynamic Analysis (GUI Method)
5.7.3. Problem Sketch Figure 5.3 Model of a Steel Beam Supporting a Concentrated Mass
5.7.3.1. Specify the Title 1.
Choose menu path Utility Menu> File> Change Title.
2.
Enter the text "Transient response to a constant force with a finite rise time."
3.
Click on OK.
5.7.3.2. Define Element Types 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete. The Element Types dialog box appears.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
In the left scroll box, click on "Structural Beam."
4.
In the right scroll box, click on "2D elastic 3," and click on Apply.
5.
In the left scroll box, click on "Structural Mass."
6.
In the right scroll box, click on "3D mass 21," and click on OK.
7.
In the Element Types dialog box, click once on "Type 2," and click on Options.
8.
In the scroll box for Rotary inertia options, scroll to "2D w/o rot iner" and select it.
9.
Click on OK and click on Close in the Element Types dialog box.
5.7.3.3. Define Real Constants 1.
Choose menu path Main Menu> Preprocessor> Real Constants> Add/Edit/Delete. The Real Constants dialog box appears.
2.
Click on Add. The Element Type for Real Constants dialog box appears.
3.
Click on Type1 BEAM3 then Click on OK. The Real Constants for BEAM3 dialog box appears.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–27
Chapter 5: Transient Dynamic Analysis 4.
Enter 1 for Area, 800.6 for IZZ, and 18 for Height.
5.
Click on OK.
6.
In the Real Constants dialog box, click on Add.
7.
Click on Type 2 MASS21 and click on OK. The Real Constant Set Number 2, for MASS21 dialog box appears.
8.
Enter .0259067 in the 2-D mass field and click on OK.
9.
Click on Close in the Real Constants dialog box.
5.7.3.4. Define Material Properties 1.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
2.
In the Material Models Available window, double-click on the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
3.
Enter 30e3 for EX (Young's modulus), enter 0.3 for PRXY, and click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
4.
Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
5.7.3.5. Define Nodes 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Nodes> In Active CS. The Create Nodes in Active Coordinate System dialog box appears.
2.
Enter 1 for node number and click on Apply to define node 1 at 0,0,0.
3.
Enter 3 for node number.
4.
Enter 240,0,0 for X, Y, Z coordinates and click on OK.
5.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Nodes> Fill between Nds. The Fill between Nds picking menu appears.
6.
Click once on nodes 1 and 3 in the ANSYS Graphics window, and click on OK in the picking menu. The Create Nodes Between 2 Nodes dialog box appears.
7.
Click on OK to accept the default settings.
5.7.3.6. Define Elements 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Thru Nodes. The Elements from Nodes picking menu appears.
2.
Click once on nodes 1 and 2, and click on Apply.
3.
Click once on nodes 2 and 3, and click on OK.
4.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes. The Element Attributes dialog box appears.
5.
In the Element type number drop down menu, select “2 MASS21.”
6.
In the Real constant set number drop down menu, select 2 and click OK.
7.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Thru Nodes. The Elements from Nodes picking menu appears.
8.
Click once on node 2 and click OK.
5–28
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.7: Sample Reduced Transient Dynamic Analysis (GUI Method) 9.
Click on SAVE_DB on the ANSYS Toolbar.
5.7.3.7. Define Analysis Type and Analysis Options 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis.
2.
Click on "Transient" to select it, and click on OK. The Transient Analysis dialog box appears.
3.
Click on "Reduced" and click on OK.
4.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Reduced Transient Analysis dialog box appears.
5.
In the drop down menu for Damping effects, select "Ignore."
6.
Click on OK.
5.7.3.8. Define Master Degrees of Freedom 1.
Choose menu path Main Menu> Solution> Master DOFs> User Selected> Define. The Define Master DOFs picking menu appears.
2.
Click on node 2 and click on OK. The Define Master DOFs dialog box appears.
3.
In the drop down menu for 1st degree of freedom, select "UY."
4.
Click on OK.
5.7.3.9. Set Load Step Options 1.
Choose the menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Time-Time Step. The Time and Time Step Options dialog box appears.
2.
Enter .004 for Time step size and click on OK.
5.7.3.10. Apply Loads for the First Load Step 1.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears.
2.
Click on node 1 and click on Apply. The Apply U,ROT on Nodes dialog box appears.
3.
Click on "UY" to select it and click on Apply. The Apply U,ROT on Nodes picking menu appears.
4.
Click on node 3, and click on OK. The Apply U,ROT on Nodes dialog box appears.
5.
Click on "UX" to select it. "UY" should remain selected. Click on OK.
6.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment> On Nodes. The Apply F/M on Nodes picking menu appears.
7.
Click on node 2 and click on OK. The Apply F/M on Nodes dialog box appears.
8.
In the drop down menu for Direction of force/mom, select "FY." Leave the value as blank (zero) for the initial static solution.
9.
Click on OK, and click on SAVE_DB on the ANSYS Toolbar.
5.7.3.11. Specify Output 1.
Choose menu path Main Menu> Solution> Load Step Opts> Output Ctrls> DB/Results File. The Controls for Database and Results File Writing dialog box appears.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–29
Chapter 5: Transient Dynamic Analysis 2.
Click on the "Every substep" radio button and click on OK.
5.7.3.12. Solve the First Load Step 1.
Choose menu path Main Menu> Solution> Solve> Current LS.
2.
Review the information in the status window, and click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to begin the solution.
4.
Click on Close when the Solution is done! window appears.
5.7.3.13. Apply Loads for the Next Load Step 1.
Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc>Time-Time Step. The Time and Time Step Options dialog box appears.
2.
Enter .075 for Time at end of load step and click on OK.
3.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment> On Nodes. The Apply F/M on Nodes picking menu appears.
4.
Click on node 2 and click on OK. The Apply F/M on Nodes dialog box appears.
5.
Enter 20 for Force/moment value and click on OK.
5.7.4. Solve the Next Load Step 1.
Choose menu path Main Menu> Solution> Solve> Current LS.
2.
Review the information in the status window, and click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to begin the solution.
4.
Click on Close when the Solution is done! window appears
5.7.4.1. Set the Next Time Step and Solve 1.
Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Time-Time Step. The Time and Time Step Options dialog box appears.
2.
Enter .1 for Time at end of load step and click on OK.
3.
Choose menu path Main Menu> Solution> Solve> Current LS.
4.
Review the information in the status window, and click on Close.
5.
Click on OK on the Solve Current Load Step dialog box to begin the solution.
6.
Click on Close when the Solution is done! window appears.
7.
Choose menu path Main Menu> Finish.
5.7.4.2. Run the Expansion Pass and Solve 1.
Choose menu path Main Menu> Solution> Analysis Type> ExpansionPass. Set the Expansion pass radio button to On and click on OK.
2.
Choose menu path Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> By Time/Freq. The Expand Single Solution by Time/Frequency dialog box appears.
3.
Enter 0.092 for Time-point/Frequency and click on OK.
4.
Choose menu path Main Menu >Solution> Solve> Current LS.
5–30
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.8: Sample Reduced Transient Dynamic Analysis (Command or Batch Method) 5.
Review the information in the status window, and click on Close.
6.
Click on OK on the Solve Current Load Step dialog box to begin the solution.
7.
Click on Close when the Solution is done! window appears.
5.7.4.3. Review the Results in POST26 1.
Choose menu path Main Menu> TimeHist Postpro> Settings> File. The File Settings dialog box appears.
2.
Click browse and select "file.rdsp" and click on open then OK.
3.
Choose menu path Main Menu> TimeHist Postpro> Define Variables. The Defined Time-History Variables dialog box appears.
4.
Click on Add. The Add Time-History Variable dialog box appears.
5.
Click on OK to accept the default of Nodal DOF result. The Define Nodal Data picking menu appears. Pick node 2 and click OK.
6.
Accept the default of 2 for the reference number of the variable.
7.
Make sure that 2 is entered for node number.
8.
Enter NSOL for user-specified label.
9.
In the right scroll box, click on "Translation UY" to select it.
10. Click on OK, then click on Close in the Defined Time-History Variables dialog box. 11. Choose menu path Main Menu> TimeHist Postpro> Graph Variables. 12. Enter 2 for 1st variable to graph and click on OK. The graph appears in the ANSYS Graphics window. 13. Choose menu path Main Menu> TimeHist Postpro> List Variables. 14. Enter 2 for 1st variable to list and click on OK. 15. Review the information in the status window and click on Close.
5.7.4.4. Review the Results in POST1 1.
Choose menu path Main Menu> General Postproc> Read Results> First Set.
2.
Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears.
3.
Click on "Def + undeformed" and click on OK.
5.7.4.5. Exit ANSYS 1.
Choose QUIT from the ANSYS Toolbar.
2.
Click on the save option you want, and click on OK.
5.8. Sample Reduced Transient Dynamic Analysis (Command or Batch Method) You can perform the example transient dynamic analysis of a bracket using the ANSYS commands shown below instead of GUI choices. Items prefaced with an exclamation point (!) are comments. /PREP7 /TITLE, Transient Response to a Constant Force with a Finite Rise Time ET,1,BEAM3 ! 2-D beam
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–31
Chapter 5: Transient Dynamic Analysis ET,2,MASS21,,,4 R,1,1,800.6,18 R,2,.0259067 MP,EX,1,30e3 N,1 N,3,240 FILL E,1,2! Beam elements EGEN,2,1,1 TYPE,2 REAL,2 E,2 M,2,UY FINISH /SOLU ANTYPE,TRANS TRNOPT,REDUC,,NODAMP DELTIM,.004 D,1,UY D,3,UX,,,,,UY OUTPR,BASIC,1 OUTRES,ALL,1 F,2,FY,0 SOLVE TIME,.075 F,2,FY,20 SOLVE TIME,.1 SOLVE FINISH
! 2-D mass ! Beam area = 1, I = 800.6, h = 18 ! Mass
! Type 2 element with real constant 2 ! Master DOF in Y direction at middle of beam
! Transient dynamic analysis ! Reduced transient analysis, ignore damping ! Integration time step size
! Force = 0 at Time = 0 ! Time at end of load step ! Force is ramped to 20 ! Constant force until time = 0.1
/SOLU ! The following is the expansion pass using BEAM3 and MASS21 elements EXPASS,ON ! Expansion pass on EXPSOL,,,0.092 ! Time of maximum response SOLVE FINISH /POST26 NUMVAR,0 FILE,file,rdsp NSOL,2,2,U,Y,NSOL PLVAR,2 PRVAR,2 FINISH /POST1 SET,FIRST PLDISP,1 FINISH
! Define the variables ! Graph the variables ! List the variables
! Read in results ! Display deformed and undeformed shape
5.9. Performing a Prestressed Transient Dynamic Analysis A prestressed transient dynamic analysis calculates the dynamic response of a prestressed structure, such as a heat-treated part with residual thermal stresses. Prestressed-analysis procedures vary, depending on the type of transient dynamic analysis being performed.
5.9.1. Prestressed Full Transient Dynamic Analysis You can include prestressing effects in a full transient dynamic analysis by applying the prestressing loads in a preliminary static load step. (Do not remove these loads in subsequent load steps.) The procedure consists of two steps: 1.
5–32
Build your model, enter SOLUTION, and define a transient analysis type (ANTYPE,TRANS).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.10: Other Analysis Details •
Apply all prestressing loads.
•
Turn time integration effects off (TIMINT,OFF).
•
Turn stress stiffening effects on (SSTIF,ON).
•
Set time equal to some small dummy value (TIME).
•
Write your first load step to Jobname.S01 (LSWRITE).
If prestressing effects develop because of nonlinear behavior (as in the case of residual thermal stresses in a casting), several load steps might be required to complete the static prestressing phase of your analysis. In the case of geometric nonlinearities (large deformation effects), you can capture the prestressing effect by issuing NLGEOM,ON. 2.
For all subsequent load steps, turn time integration effects on (TIMINT,ON), and proceed using the full transient dynamic analysis procedures described previously. Once all load steps are written to files (LSWRITE), you can initiate the multiple load step solution (LSSOLVE).
Note — The static prestress solution must be done as a separate solution if initial conditions are to be defined with the IC command. (Main Menu> Solution> Define Loads> Apply> Initial Condit'n> Define) The IC command is valid only in the first load step.
5.9.2. Prestressed Mode Superposition Transient Dynamic Analysis In order to include prestress effects in a mode superposition analysis, you must first do a prestressed modal analysis. See Chapter 3, “Modal Analysis” for details. Once prestressed modal analysis results are available, proceed as for any other mode superposition analysis.
5.9.3. Prestressed Reduced Transient Dynamic Analysis The procedure to do a prestressed reduced transient dynamic analysis requires that you first prestress the structure in a separate static analysis, as explained below. It is assumed that the transient (time-varying) stresses (which are superimposed on the prestress) are much smaller than the prestress itself. If they are not, you should use the full transient dynamic analysis. 1.
Build the model and obtain a static solution with prestress effects turned on (PSTRES,ON). The procedure to obtain a static solution is explained in Chapter 2, “Structural Static Analysis”.
2.
Reenter SOLUTION (/SOLU) and obtain the reduced transient solution, also with prestress effects turned on (PSTRES,ON). Files Jobname.DB, Jobname.EMAT, and Jobname.ESAV from the static analysis must be available.
5.10. Other Analysis Details The following sections provide additional details about defining integration time step, automatic time stepping, and damping.
5.10.1. Guidelines for Integration Time Step As mentioned earlier, the accuracy of the transient dynamic solution depends on the integration time step: the smaller the time step, the higher the accuracy. A time step that is too large will introduce error that affects the response of the higher modes (and hence the overall response). A time step that is too small will waste computer resources. To calculate an optimum time step, you should consider the following guidelines: Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–33
Chapter 5: Transient Dynamic Analysis 1.
Resolve the response frequency. The time step should be small enough to resolve the motion (response) of the structure. Since the dynamic response of a structure can be thought of as a combination of modes, the time step should be able to resolve the highest mode that contributes to the response. For the Newmark time integration scheme, it has been found that using approximately twenty points per cycle of the highest frequency of interest results in a reasonably accurate solution. That is, if f is the frequency (in cycles/time), the integration time step (ITS) is given by ITS = 1/20f Smaller ITS values may be required if acceleration results are needed. The following figure shows the effect of ITS on the period elongation of a single-DOF spring-mass system. Notice that 20 or more points per cycle result in a period elongation of less than 1 percent.
Figure 5.4 Effect of Integration Time Step on Period Elongation
For the HHT time integration method, the same guidelines for time step should be applied. Note that if the same time step and time integration parameters are used, the HHT method will be more accurate compared to the Newmark method. 2.
5–34
Resolve the applied load-versus-time curve(s). The time step should be small enough to “follow” the loading function. The response tends to lag the applied loads, especially for stepped loads, as shown in Figure 5.5: “Transient Input vs. Transient Response”. Stepped loads require a small ITS at the time of the step change so that the step change can be closely followed. ITS values as small as 1/180f may be needed to follow stepped loads.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.10: Other Analysis Details
Figure 5.5 Transient Input vs. Transient Response
3.
Resolve the contact frequency. In problems involving contact (impact), the time step should be small enough to capture the momentum transfer between the two contacting surfaces. Otherwise, an apparent energy loss will occur and the impact will not be perfectly elastic. The integration time step can be determined from the contact frequency (fc) as:
ITS =1/Nfc
fc =(1/ 2π) k /m
where k is the gap stiffness, m is the effective mass acting at the gap, and N is the number of points per cycle. To minimize the energy loss, at least thirty points per cycle of (N = 30) are needed. Larger values of N may be required if acceleration results are needed. For the reduced and mode superposition methods, N must be at least 7 to ensure stability. You can use fewer than thirty points per cycle during impact if the contact period and contact mass are much less than the overall transient time and system mass, because the effect of any energy loss on the total response would be small. 4.
Resolve the wave propagation. If you are interested in wave propagation effects, the time step should be small enough to capture the wave as it travels through the elements. See Section 5.4.1: Build the Model for a discussion of element size.
5.
Resolve the nonlinearities. For most nonlinear problems, a time step that satisfies the preceding guidelines is sufficient to resolve the nonlinearities. There are a few exceptions, however: if the structure tends to stiffen under the loading (for example, large deflection problems that change from bending to membrane load-carrying behavior), the higher frequency modes that are excited will have to be resolved.
After calculating the time step using the appropriate guidelines, use the minimum value for your analysis. By using automatic time stepping, you can let the ANSYS program decide when to increase or decrease the time step during the solution. Automatic time stepping is discussed next. Caution: Avoid using exceedingly small time steps, especially when establishing initial conditions. Exceedingly small numbers can cause numerical difficulties. Based on a problem time scale of unity, for example, time steps smaller than 10-10 could cause numerical difficulties.
5.10.2. Automatic Time Stepping Automatic time stepping, also known as time step optimization, attempts to adjust the integration time step during solution based on the response frequency and on the effects of nonlinearities. The main benefit of this feature is that the total number of substeps can be reduced, resulting in computer resource savings. Also, the Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–35
Chapter 5: Transient Dynamic Analysis number of times that you might have to rerun the analysis (adjusting the time step size, nonlinearities, and so on) is greatly reduced. If nonlinearities are present, automatic time stepping gives the added advantage of incrementing the loads appropriately and retreating to the previous converged solution (bisection) if convergence is not obtained. You can activate automatic time stepping with the AUTOTS command. (For more information on automatic time stepping in the context of nonlinearities, see Chapter 8, “Nonlinear Structural Analysis”.) Although it seems like a good idea to activate automatic time stepping for all analyses, there are some cases where it may not be beneficial (and may even be harmful): •
Problems that have only localized dynamic behavior (for example, turbine blade and hub assemblies), where the low-frequency energy content of part of the system may dominate the high-frequency areas
•
Problems that are constantly excited (for example, seismic loading), where the time step tends to change continually as different frequencies are excited
•
Kinematics (rigid-body motion) problems, where the rigid-body contribution to the response frequency term may dominate
5.10.3. Damping Damping is present in most systems and should be specified in a dynamic analysis. The following forms of damping are available in the ANSYS program: •
Alpha and Beta Damping (Rayleigh Damping)
•
Material-Dependent Damping
•
Constant Material Damping Coefficient
•
Constant Damping Ratio
•
Modal Damping
•
Element Damping
Only the constant damping ratio and modal damping are available in the ANSYS Professional program. You can specify more than one form of damping in a model. The program will formulate the damping matrix (C) as the sum of all the specified forms of damping. The constant material damping coefficient is only applicable in full and modal harmonic analyses. Table 5.5: “Damping for Different Analysis Types” shows the types of damping available for different structural analyses.
Table 5.5 Damping for Different Analysis Types Alpha, Beta Damping ALAnalysis Type PHAD, BETAD Static
Material- Dependent Constant Damping Damping Ratio MP,DAMP DMPRAT
Modal Damping MDAMP
Element Constant MaDamping(3) terial Damping COMBIN7, and Coefficient so on MP,DMPR
N/A
N/A
N/A
N/A
N/A
N/A
No(5)
No(5)
No(5)
No
No
No
Yes
Yes
No
No
Yes
No(7)
Full
Yes
Yes
Yes
No
Yes
Yes
Reduced
Yes
Yes
Yes
No
Yes
No
Modal Undamped Damped Harmonic
5–36
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.10: Other Analysis Details
Alpha, Beta Damping ALAnalysis Type PHAD, BETAD Mode Sup
Material- Dependent Constant Damping Damping Ratio MP,DAMP DMPRAT
Modal Damping MDAMP
Element Constant MaDamping(3) terial Damping COMBIN7, and Coefficient so on MP,DMPR
Yes(6)
Yes(4,6)
Yes
Yes
Yes(6)
Yes(7)
Full
Yes
Yes
No
No
Yes
No
Reduced
Yes
Yes
No
No
Yes
No
Mode Sup
Yes(6)
Yes(4,6)
Yes
Yes
Yes(6)
No
SPRS, MPRS(2)
Yes(1)
Yes
Yes
Yes
No
No
DDAM(2)
Yes(1)
Yes
Yes
Yes
No
No
PSD(2)
Yes
No
Yes
Yes
No
No
Buckling
N/A
N/A
N/A
N/A
N/A
N/A
Substructure
Yes
Yes
No
No
Yes
No
Transient
Spectrum
N/A Not applicable 1.
β damping only, no α damping
2.
Damping is used only for mode combination and not for computation of mode coefficients
3.
Includes superelement damping matrix
4.
If converted to modal damping by expansion of modes
5.
If specified, an effective damping ratio is calculated for subsequent spectrum analyses
6.
If you use the QR damped mode-extraction method (MODOPT,QRDAMP), and you specify any kind of damping during preprocessing or in the modal analysis, ANSYS ignores damping specified during the mode superposition analysis
7.
Only the QR damped method supports the constant material damping coefficient application in a downstream mode superposition harmonic analysis
Alpha damping and Beta damping are used to define Rayleigh damping constants α and β. The damping matrix (C) is calculated by using these constants to multiply the mass matrix (M) and stiffness matrix (K): (C) = α(M) + β(K) The ALPHAD and BETAD commands are used to specify α and β, respectively, as decimal numbers. The values of α and β are not generally known directly, but are calculated from modal damping ratios, ξi. ξi is the ratio of actual damping to critical damping for a particular mode of vibration, i. If ωi is the natural circular frequency of mode i, α and β satisfy the relation ξi = α/2ωi + βωi/2 In many practical structural problems, alpha damping (or mass damping) may be ignored (α = 0). In such cases, you can evaluate β from known values of ξi and ωi, as β = 2 ξi/ωi Only one value of β can be input in a load step, so choose the most dominant frequency active in that load step to calculate β. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–37
Chapter 5: Transient Dynamic Analysis To specify both α and β for a given damping ratio ξ, it is commonly assumed that the sum of the α and β terms is nearly constant over a range of frequencies (see Figure 5.6: “Rayleigh Damping”). Therefore, given ξ and a frequency range ωi to ωj, two simultaneous equations can be solved for α and β.
Figure 5.6 Rayleigh Damping
Alpha damping can lead to undesirable results if an artificially large mass has been introduced into the model. One common example is when an artificially large mass is added to the base of a structure to facilitate acceleration spectrum input. (You can use the large mass to convert an acceleration spectrum to a force spectrum.) The alpha damping coefficient, which is multiplied by the mass matrix, will produce artificially large damping forces in such a system, leading to inaccuracies in the spectrum input, as well as in the system response. Beta damping and material damping can lead to undesirable results in a nonlinear analysis. These damping coefficients are multiplied by the stiffness matrix, which is constantly changing in a nonlinear analysis. The resulting change in damping can sometimes be opposite to the actual change in damping that can occur in physical structures. For example, whereas physical systems that experience softening due to plastic response will usually experience a corresponding increase in damping, an ANSYS model that has beta damping will experience a decrease in damping as plastic softening response develops. Material-dependent damping allows you to specify beta damping (β) as a material property (MP,DAMP). Note, however, that MP,DAMP in a spectrum analysis (ANTYPE,SPECTR) specifies a material-dependent damping ratio ξ, not β. Also note that for multi-material elements such as SOLID46, SOLID65, SHELL91, and SHELL99, β can only be specified for the element as a whole, not for each material in the element. In these cases, β is determined from the material pointer for the element (set with the MAT command), rather than the material pointed to by any real constant MAT for the element. MP,DAMP is not assumed to be temperature-dependent, and is always evaluated at T = 0.0. The constant material damping coefficient is available only for full and modal harmonic analyses. The constant damping ratio is the simplest way of specifying damping in the structure. It represents the ratio of actual damping to critical damping, and is specified as a decimal number with the DMPRAT command. DMPRAT is available only for spectrum, harmonic response, and mode superposition transient dynamic analyses. Modal damping gives you the ability to specify different damping ratios for different modes of vibration. It is specified with the MDAMP command and is available only for the spectrum and mode superposition method of solution (transient dynamic and harmonic response analyses). Element damping involves using element types having viscous damping characteristics, such as COMBIN7, COMBIN14, COMBIN37, COMBIN40, and so on.
5–38
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.10: Other Analysis Details If you are running a mode superposition analysis and used the QR damping solution method for the modal solution, alpha (ALPHAD), beta (BETAD), material-dependent, and element damping must be defined in the QR damping modal solution for the damping to be available in a subsequent mode superposition analysis. For more information about damping, see the ANSYS, Inc. Theory Reference. The explicit mathematical expressions that form the damping matrix in different analysis options are shown in Table 5.6: “Damping Matrix Formulation with Different Damping Coefficients”. These expressions define how each of the damping options in Table 5.5: “Damping for Different Analysis Types” is handled in a dynamic analysis.
Table 5.6 Damping Matrix Formulation with Different Damping Coefficients Analysis Type Full Harmonic & Modal Analysis Mode Superposi- Mode Superposi- Spectrum AnaTransient AnaLANB(1) tion Harmonic Ana- tion Transient Ana- lysis(1) (modal lysis lysis(1) lysis(1) damping ratio) Modal Analysis QRDA(1) ALPHAD α
α[M]
No
ΦTα[M]Φ = α
ΦTα[M]Φ = α
No
Φ Tβ[K ]Φ = βω2i
Φ Tβ[K ]Φ = βω2i
βωi 2
α[M] BETAD β
β[K]
No
β[K] MP,DAMP
βm j
No
No
Nm
m ∑ β j [K j ]
No
No
j =1
Nm
m s ∑ βj Ej
j =1 Nm
s ∑ Ej j =1
See Equation 17–104 in the ANSYS, Inc. Theory Reference m ∑ β j [K j ]
Nm Φ T ∑ βm j [K j ]Φ
Nm Φ T ∑ βm j [K j ]Φ
No
No
2ξωi
2ξωi
ξ
Nm
j =1
DMPRAT ξ
Harmonic
j =1
j =1
2ξ [K ] Ω MDAMP
No
No
ξm i
No
2ξm i ωi
2ξm i ωi
ξm i No
Element Damping
No
No
∑ [Ck ]
Φ T ∑ [Ck ]Φ
Φ T ∑ [Ck ]Φ
No
No
No
Ne
∑ [Ck ]
k =1
Ne
k =1
MP,DMPR
βξj
Harmonic Nm
2βξj [K j ]
j =1
Ω
∑
Ne
k =1
No
No
Ne
k =1
No
2βξj [K j ] Φ ∑ Φ Ω j =1 N T m
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–39
Chapter 5: Transient Dynamic Analysis Note — 1.
For modal, mode superposition, and spectrum analyses the boxes are split where applicable with the top indicating the Lanczos method and the bottom indicating the QR damped method.
5.11. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional transient dynamic analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS program. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual includes a variety of transient dynamic analysis test cases: VM9 - Large Lateral Deflection of Unequal Stiffness Springs VM40 - Large Deflection and Rotation of a Beam Pinned at One End VM65 - Transient Response of a Ball Impacting a Flexible Surface VM71 - Transient Response of a Spring, Mass, Damping System VM72 - Logarithmic Decrement VM73 - Free Vibration with Coulomb Damping VM74 - Transient Response to an Impulsive Excitation VM75 - Transient Response to a Step Excitation VM77 - Transient Response to a Constant Force with a Finite Rise Time VM79 - Transient Response of a Bilinear Spring Assembly VM80 - Plastic Response to a Suddenly Applied Constant Force VM81 - Transient Response of a Drop Container VM84 - Displacement Propagation along a Bar with Free Ends VM85 - Transient Displacements in a Suddenly Stopped Moving Bar VM91 - Large Rotation of a Swinging Pendulum VM156 - Natural Frequency of Nonlinear Spring-Mass System VM158 - Motion of a Bobbing Buoy VM179 - Dynamic Double Rotation of a Jointed Beam VM182 - Transient Response of a Spring-Mass System
5–40
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 6: Spectrum Analysis 6.1. Definition of Spectrum Analysis A spectrum analysis is one in which the results of a modal analysis are used with a known spectrum to calculate displacements and stresses in the model. It is mainly used in place of a time-history analysis to determine the response of structures to random or time-dependent loading conditions such as earthquakes, wind loads, ocean wave loads, jet engine thrust, rocket motor vibrations, and so on.
6.2. What is a Spectrum? The spectrum is a graph of spectral value versus frequency that captures the intensity and frequency content of time-history loads. Three types of spectra are available for a spectrum analysis: •
Response Spectrum –
Single-point Response Spectrum (SPRS)
–
Multi-point Response Spectrum (MPRS)
•
Dynamic Design Analysis Method (DDAM)
•
Power Spectral Density (PSD)
The only method available in the ANSYS Professional program is the single-point response spectrum.
6.2.1. Response Spectrum A response spectrum represents the response of single-DOF systems to a time-history loading function. It is a graph of response versus frequency, where the response might be displacement, velocity, acceleration, or force. Two types of response spectrum analysis are possible: single-point response spectrum and multi-point response spectrum.
6.2.1.1. Single-Point Response Spectrum (SPRS) In a single-point response spectrum (SPRS) analysis, you specify one response spectrum curve (or a family of curves) at a set of points in the model, such as at all supports, as shown in Figure 6.1: “Single-Point and Multi-Point Response Spectra” (a).
6.2.1.2. Multi-Point Response Spectrum (MPRS) In a multi-point response spectrum (MPRS) analysis, you specify different spectrum curves at different sets of points, as shown in Figure 6.1: “Single-Point and Multi-Point Response Spectra” (b).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 6: Spectrum Analysis
Figure 6.1 Single-Point and Multi-Point Response Spectra
6.2.2. Dynamic Design Analysis Method (DDAM) The Dynamic Design Analysis Method (DDAM) is a technique used to evaluate the shock resistance of shipboard equipment. The technique is essentially a response spectrum analysis in which the spectrum is obtained from a series of empirical equations and shock design tables provided in the U.S. Naval Research Laboratory Report NRL-1396.
6.2.3. Power Spectral Density Power spectral density (PSD) is a statistical measure defined as the limiting mean-square value of a random variable. It is used in random vibration analyses in which the instantaneous magnitudes of the response can be specified only by probability distribution functions that show the probability of the magnitude taking a particular value. A PSD is a statistical measure of the response of a structure to random dynamic loading conditions. It is a graph of the PSD value versus frequency, where the PSD may be a displacement PSD, velocity PSD, acceleration PSD, or force PSD. Mathematically, the area under a PSD-versus-frequency curve is equal to the variance (square of the standard deviation of the response). Similar to response spectrum analysis, a random vibration analysis may be single-point or multi-point. In a singlepoint random vibration analysis, you specify one PSD spectrum at a set of points in the model. In a multi-point random vibration analysis, you specify different PSD spectra at different points in the model.
6.2.4. Deterministic vs. Probabilistic Analyses Response spectrum and DDAM analyses are deterministic analyses because both the input to the analyses and output from the analyses are actual maximum values. Random vibration analysis, on the other hand, is probabilistic in nature, because both input and output quantities represent only the probability that they take on certain values.
6.3. Steps in a Single-Point Response Spectrum (SPRS) Analysis The procedure for a single-point response spectrum analysis consists of six main steps: 1.
6–2
Build the model.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.3: Steps in a Single-Point Response Spectrum (SPRS) Analysis 2.
Obtain the modal solution.
3.
Obtain the spectrum solution.
4.
Expand the modes.
5.
Combine the modes.
6.
Review the results.
The modal solution is required because the structure's mode shapes and frequencies must be available to calculate the spectrum solution. Also, by performing the spectrum solution ahead of mode expansion, you can expand only the significant modes that contribute to the final solution.
6.3.1. Build the Model See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details, see the ANSYS Modeling and Meshing Guide.
6.3.1.1. Points to Remember •
Only linear behavior is valid in a spectrum analysis. Nonlinear elements, if any, are treated as linear. If you include contact elements, for example, their stiffnesses are calculated based on their initial status and are never changed.
•
Both Young's modulus (EX) (or stiffness in some form) and density (DENS) (or mass in some form) must be defined. Material properties can be linear, isotropic or orthotropic, and constant or temperature-dependent. Nonlinear properties, if any, are ignored.
6.3.2. Obtain the Modal Solution The modal solution - natural frequencies and mode shapes - is needed to calculate the spectrum solution. The procedure to obtain the modal solution is described in Chapter 3, “Modal Analysis”, but you should keep in mind the following additional points: •
Use the Block Lanczos (default), subspace, or reduced method to extract the modes. The other methods - unsymmetric, damped, QR damped, and PowerDynamics - are not valid for subsequent spectrum analysis.
•
The number of modes extracted should be enough to characterize the structure's response in the frequency range of interest.
•
If you are using GUI method, choose NO for mode expansion on the dialog box for the modal analysis options [MODOPT], so that modes are not expanded at this time, but can be expanded selectively in a separate solution pass. (See the use of the SIGNIF field on the MXPAND command.) Otherwise, choose YES to expand all the modes at this phase.
•
If material-dependent damping is to be included in the spectrum analysis, it must be specified in the modal analysis.
•
Be sure to constrain those DOF where you want to apply a base excitation spectrum.
•
At the end of the solution, leave the SOLUTION processor.
6.3.3. Obtain the Spectrum Solution The procedure to obtain the spectrum solution is explained below. The mode file and the full file (jobname.MODE, jobname.FULL) from the modal analysis must be available, and the database must contain the model data.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–3
Chapter 6: Spectrum Analysis 1.
Enter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define the analysis type and analysis options. ANSYS offers the following analysis options for a spectrum analysis. Not all modal analysis options and not all eigenvalue extraction techniques work with all spectrum analysis options.
Table 6.1 Analysis Types and Options Option New Analysis
Command ANTYPE
Analysis Type: Spec- ANTYPE trum
GUI Path Main Menu> Solution> Analysis Type> New Analysis Main Menu> Solution> Analysis Type> New Analysis> Spectrum
SPOPT
Main Menu> Solution> Analysis Type> Analysis Options
No. of Modes to Use SPOPT for Solution
Main Menu> Solution> Analysis Type> Analysis Options
Spectrum Type: SPRS
•
Option: New Analysis [ANTYPE] Choose New Analysis.
•
Option: Analysis Type: Spectrum [ANTYPE] Choose analysis type spectrum.
•
Option: Spectrum Type: Single-point Response Spectrum [SPOPT] Choose Single-point Response Spectrum (SPRS).
•
Option: Number of Modes to Use for Solution [SPOPT] Choose enough modes to cover the frequency range spanned by the spectrum and to characterize the structure's response. The accuracy of the solution depends on the number of modes used: the larger the number, the higher the accuracy. Make sure to choose YES on the SPOPT command if you want to calculate element stresses.
3.
Specify load step options. The following options are available for single-point response spectrum analysis:
Table 6.2 Load Step Options Option
Command
GUI Path
Spectrum Options Type of Response Spectrum
SVTYP
Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Settings
Excitation Direction SED
Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Settings
Spectral-value- vs- FREQ, SV frequency Curve
Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Freq Table or Spectr Values
Damping (Dynamics Options) Beta (Stiffness) Damping
6–4
BETAD
Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.3: Steps in a Single-Point Response Spectrum (SPRS) Analysis Option
Command
GUI Path
Constant Damping DMPRAT Ratio
Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
MDAMP
Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
Modal Damping
•
Spectrum Options These data include the following: –
Type of Response Spectrum [SVTYP] The spectrum type can be displacement, velocity, acceleration, force, or PSD. All except the force spectrum represent seismic spectra; that is, they are assumed to be specified at the base. The force spectrum is specified at non-base nodes with the F or FK command, and the direction is implied by labels FX, FY, FZ. The PSD spectrum [SVTYP,4] is internally converted to a displacement response spectrum and is limited to flat, narrowband spectra; a more robust random vibration analysis procedure is described in Section 6.7: How to Do a Random Vibration (PSD) Analysis.
–
Excitation Direction [SED]
–
Spectral-Value-Versus-Frequency Curve [FREQ, SV] SV and FREQ commands are used to define the spectral curve. You can define a family of spectral curves, each curve for a different damping ratio. Use the STAT command to list current spectrum curve values. Another command, ROCK, allows you to specify a rocking spectrum.
•
Damping (Dynamics Options) If you specify more than one form of damping, the ANSYS program calculates an effective damping ratio at each frequency. The spectral value at this effective damping ratio is then calculated by loglog interpolation of the spectral curves. If no damping is specified, the spectral curve with the lowest damping is used. For further details about the different forms of damping, see Section 5.10.3: Damping in Chapter 5, “Transient Dynamic Analysis”. The following forms of damping are available: –
Beta (stiffness) Damping [BETAD] This option results in a frequency-dependent damping ratio.
–
Constant Damping Ratio [DMPRAT] This option specifies a constant damping ratio to be used at all frequencies.
–
Modal Damping [MDAMP] Note — Material-dependent damping ratio [MP,DAMP] is also available but only if specified in the modal analysis. MP,DAMP also specifies a material-dependent constant damping ratio (and not material-dependent beta damping, as used in other analyses).
4.
Start solution calculations. Command(s): SOLVE Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–5
Chapter 6: Spectrum Analysis GUI: Main Menu> Solution> Solve> Current LS The output from the solution includes the participation factor table. The participation factor table, which is part of the printed output, lists the participation factors, mode coefficients (based on lowest damping ratio), and the mass distribution for each mode. To obtain the maximum response of each mode (modal response), multiply the mode shape by the mode coefficient. You do this by retrieving the mode coefficient with the *GET command and using it as a scale factor in the SET command. 5.
Repeat steps 3 and 4 for additional response spectra, if any. Note that solutions are not written to the file.rst at this time.
6.
Leave the SOLUTION processor. Command(s): FINISH GUI: Close the Solution menu.
6.3.4. Expand the Modes 1.
Click on the expansion pass option button on the Expansion Pass dialog box to signify YES for an expansion pass. Command(s): MXPAND GUI: Main Menu> Solution> Analysis Type> New Analysis> Modal Main Menu> Solution> Analysis Type> Expansion Pass Main Menu> Solution> Load Step Opts> Expansion Pass> Expand Modes
2.
You must expand modes regardless of whether you used the Block Lanczos, subspace, or reduced extraction method. Details of how to expand the modes are explained in Chapter 3, “Modal Analysis” under "Expand the Modes" as a separate solution pass, but you should keep in mind the following points: •
Only significant modes can be selectively expanded. (See the use of the SIGNIF field on the MXPAND command.) If you are using the GUI method and want to selectively expand modes, choose NO for mode expansion on the dialog box for the modal analysis options [MODOPT] in the modal analysis phase. You then perform mode expansion as a separate solution pass after performing the spectrum solution.
•
Only expanded modes are used for the mode combination operation in the subsequent mode combination pass.
•
If you are interested in stresses caused by the spectrum, be sure to request stress calculations here. By default, no stresses are calculated in the expansion pass, which means no stresses are available for the spectrum analysis.
•
If you want to expand all the modes, you can include the mode expansion steps in the modal solution pass by issuing the MXPAND command. If you are using the GUI method and want to expand all the modes, choose YES for mode expansion on the dialog box for the modal analysis options [MODOPT] in the modal solution step. But if you want to expand only the significant modes, you must perform mode expansion as a separate solution pass after performing the spectrum solution.
Note that modal analysis solutions are written to the results file (Jobname.RST) only if the mode expansion is performed.
6.3.5. Combine the Modes Combine the modes in a separate solution phase. The procedure is as follows: 1.
6–6
Enter SOLUTION. Command(s): /SOLU Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.3: Steps in a Single-Point Response Spectrum (SPRS) Analysis GUI: Main Menu> Solution 2.
Define analysis type. Command(s): ANTYPE GUI: Main Menu> Solution> Analysis Type> New Analysis •
Option: New Analysis [ANTYPE] Choose New Analysis.
•
Option: Analysis Type: Spectrum [ANTYPE] Choose analysis type spectrum.
3.
Choose one of the mode combination methods. ANSYS offers five different mode combination methods for the single-point response spectrum analysis: •
Square Root of Sum of Squares (SRSS)
•
Complete Quadratic Combination (CQC)
•
Double Sum (DSUM)
•
Grouping (GRP)
•
Naval Research Laboratory Sum (NRLSUM)
The NRLSUM method is typically used in the context of the Dynamic Design and Analysis Method (DDAM) spectrum analysis. The following commands are used to invoke different methods of mode combinations: Command(s): SRSS, CQC, DSUM, GRP, NRLSUM GUI: Main Menu> Solution> Analysis Type> New Analysis> Spectrum Main Menu> Solution> Analysis Type> Analysis Opts> Single-pt resp Main Menu> Load Step Opts> Spectrum> Spectrum-Single Point-Mode Combine These commands allow computation of three different types of responses: •
Displacement (label = DISP)
Displacement response refers to displacements, stresses, forces, etc. •
Velocity (label = VELO)
Velocity response refers to velocities, "stress velocities," "force velocities," etc. •
Acceleration (label = ACEL)
Acceleration response refers to accelerations, "stress accelerations," "force accelerations," etc. The DSUM method also allows the input of time duration for earthquake or shock spectrum. Note — You must specify damping if you use the Complete Quadratic Combination method of mode combination (CQC). In addition, if you use material-dependent damping [MP,DAMP,...], you must request that element results be calculated in the modal expansion. (Elcalc = YES on the MXPAND command.)
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–7
Chapter 6: Spectrum Analysis 4.
Start solution. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS The mode combination phase writes a file of POST1 commands (Jobname.MCOM). Read in this file in POST1 to do the mode combinations, using the results file (Jobname.RST) from the modal expansion pass. The file Jobname.MCOM contains POST1 commands that combine the maximum modal responses by using the specified mode combination method to calculate the overall response of the structure. The mode combination method determines how the structure's modal responses are to be combined:
5.
•
If you selected displacement as the response type (label = DISP), displacements and stresses are combined for each mode on the mode combination command.
•
If you selected velocity as the response type (label = VELO), velocities and stress velocities are combined for each mode on the mode combination command.
•
If you selected acceleration as the response type (label = ACEL), accelerations and stress accelerations are combined for each mode on the mode combination command.
Leave the SOLUTION processor. Command(s): FINISH GUI: Close the Solution menu. Note — If you want to compute velocity or acceleration in addition to displacement, repeat the mode combination step after postprocessing the displacement solution by using the VELO or ACEL label on the mode combination commands (SRSS, CQC, GRP, DSUM, NRLSUM). Remember that the existing Jobname.MCOM file is overwritten by the additional mode combination step(s).
6.3.6. Review the Results Results from a single-point response spectrum analysis are written to the mode combination file, Jobname.MCOM, in the form of POST1 commands. These commands calculate the overall response of the structure by combining the maximum modal responses in some fashion (specified by one of the mode combination methods). The overall response consists of the overall displacements (or velocities or accelerations) and, if placed on the results file during the expansion pass, the overall stresses (or stress velocities or stress accelerations), strains (or strain velocities or strain accelerations), and reaction forces (or reaction force velocities or reaction force accelerations). You can use POST1, the general postprocessor, to review the results. Note — If you want a direct combination of the derived stresses (S1, S2, S3, SEQV, SI) from the results file, issue the SUMTYPE,PRIN command before reading in the Jobname.MCOM file. With the PRIN option, component stresses are not available. Note that the command default (SUMTYPE,COMP) is to directly operate only on the unaveraged element component stresses and compute the derived quantities from these. Refer to Section 5.5.3: Creating and Combining Load Cases in the ANSYS Basic Analysis Guide. Also, see the ANSYS Commands Reference for a description of the SUMTYPE command. 1.
6–8
Read the commands on Jobname.MCOM. Command(s): /INPUT
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.3: Steps in a Single-Point Response Spectrum (SPRS) Analysis GUI: Utility Menu> File> Read Input From For example, issue /INPUT with the following arguments: /INPUT,FILE,MCOM!Assumes the default jobname FILE
2.
Display results. •
Option: Display Deformed Shape Command(s): PLDISP GUI: Main Menu> General Postproc> Plot Results> Deformed Shape
•
Option: Contour Displays Command(s): PLNSOL or PLESOL GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu Use PLNSOL or PLESOL to contour almost any result item, such as stresses (SX, SY, SZ ...), strains (EPELX, EPELY, EPELZ ...), and displacements (UX, UY, UZ ...). If you previously issued the SUMTYPE command, the results of the PLNSOL or PLESOL command are affected by the particular SUMTYPE command option (SUMTYPE,COMP or SUMTYPE,PRIN) that you selected. Use the PLETAB command to contour element table data and PLLS to contour line element data. Caution: Derived data, such as stresses and strains, are averaged at the nodes by the PLNSOL command. This averaging results in "smeared" values at nodes where elements of different materials, different shell thicknesses, or other discontinuities meet. To avoid the smearing effect, use selecting (described in Chapter 7, “Selecting and Components” in the ANSYS Basic Analysis Guide) to select elements of the same material, same shell thickness, etc. before issuing PLNSOL. You can view correct membrane results for shells (SHELL, MID) by using KEYOPT(8) = 2 (for SHELL181 or SHELL93) or KEYOPT(11) = 2 (SHELL63). These KEYOPTS write the mid-surface node results directly to the results file, and allow the membrane results to be directly operated on during squaring operations. The default method of averaging the TOP and BOTsquared values to obtain a MID value can possibly yield incorrect MID values.
•
Option: Vector Displays Command(s): PLVECT GUI: Main Menu> General Postproc> Plot Results> Vector Plot> Predefined
•
Option: Tabular Listings Command(s): PRNSOL (nodal results) PRESOL (element-by-element results) PRRSOL (reaction data) GUI: Main Menu> General Postproc> List Results> Nodal Solution Main Menu> General Postproc> List Results> Element Solution Main Menu> General Postproc> List Results> Reaction Solution
•
Other Capabilities Many other postprocessing functions, such as mapping results onto a path, transforming results to different coordinate systems, and load case combinations, are available in POST1. See The General Postprocessor (POST1) in the ANSYS Basic Analysis Guide for details.
If you are using batch mode, note the following: Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–9
Chapter 6: Spectrum Analysis •
The modal solution and spectrum solution passes can be combined into a single modal analysis [ANTYPE,MODAL] solution pass, with spectrum loads [SV, SVTYP, SED, FREQ].
•
The mode expansion and mode combination solution passes can be combined into a single modal analysis [ANTYPE,MODAL and EXPASS,ON] solution pass with a mode combination command.
6.4. Sample Spectrum Analysis (GUI Method) In this sample problem, you determine the seismic response of a beam structure.
6.4.1. Problem Description A simply supported beam of length l , mass per unit length m, and section properties shown in Problem Specifications, is subjected to a vertical motion of both supports. The motion is defined in terms of a seismic displacement response spectrum. Determine the nodal displacements, reactions forces, and the element solutions.
6.4.2. Problem Specifications The following material properties are used for this problem: E = 30 x 106 psi m = 0.2 lb-sec2/in2 The following geometric properties are used for this problem: I = (1000/3) in4 A = 273.9726 in2 l = 240 in h = 14 in
6–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.4: Sample Spectrum Analysis (GUI Method)
6.4.3. Problem Sketch Figure 6.2 Simply Supported Beam with Vertical Motion of Both Supports
6.4.4. Procedure 6.4.4.1. Set the Analysis Title 1.
Choose menu path Utility Menu> File> Change Title.
2.
Type the text "Seismic Response of a Beam Structure" and click on OK.
6.4.4.2. Define the Element Type 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete. The Element Types dialog box appears.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
Scroll down the list on the left to "Structural Beam" and select it.
4.
Click on "2D elastic 3" in the list on the right.
5.
Click on OK. The Library of Element Types dialog box closes.
6.
Click on Close in the Element Types dialog box.
6.4.4.3. Define the Real Constants 1.
Choose menu path Main Menu> Preprocessor> Real Constants. The Real Constants dialog box appears.
2.
Click on Add. The Element Type for Real Constants dialog box appears.
3.
Click on OK. The Real Constants for BEAM3 dialog box appears. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–11
Chapter 6: Spectrum Analysis 4.
Enter 273.9726 for cross-sectional area.
5.
Enter (1000/3) for area moment of inertia.
6.
Enter 14 for total beam height and click on OK.
7.
Click on Close to close the Real Constants dialog box.
6.4.4.4. Define Material Properties 1.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
2.
In the Material Models Available window, double-click on the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
3.
Enter 30e3 for EX (Young's modulus), and click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
4.
Double-click on Density. A dialog box appears.
5.
Enter 73E-5 for DENS (density), and click on OK.
6.
Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
6.4.4.5. Define Keypoints and Line 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Keypoints> In Active CS. The Create Keypoints in Active Coordinate System dialog box appears.
2.
Enter 1 for keypoint number.
3.
Click on Apply to accept the default X, Y, Z coordinates of 0,0,0.
4.
Enter 2 for keypoint number.
5.
Enter 240,0,0 for X, Y, and Z coordinates, respectively.
6.
Click on OK.
7.
Choose menu path Utility Menu> PlotCtrls> Numbering. The Plot Numbering Controls dialog box appears.
8.
Click on "keypoint numbers" to turn keypoint numbering on.
9.
Click on OK.
10. Choose menu path Main Menu> Preprocessor> Modeling> Create> Lines> Lines> Straight Line. A picking menu appears. 11. Click on keypoint 1, and then on keypoint 2. A straight line appears between the two keypoints. 12. Click on OK. The picking menu closes.
6.4.4.6. Set Global Element Density and Mesh Line 1.
Choose menu path Main Menu> Preprocessor> Meshing> Size Cntrls> Global> Size. The Global Element Sizes dialog box appears.
2.
Enter 8 for the number of element divisions and click on OK. The Global Element Sizes dialog box closes.
3.
Choose menu path Main Menu> Preprocessor> Meshing> Mesh> Lines. A picking menu appears.
4.
Click on Pick All. The picking menu closes.
6–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.4: Sample Spectrum Analysis (GUI Method)
6.4.4.7. Set Boundary Conditions 1.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. A picking menu appears.
2.
In the graphics window, click once on the node at the left end of the beam.
3.
Click on OK. The Apply U,ROT on Nodes dialog box appears.
4.
In the scroll box of DOFs to be constrained, click once on "UY" to highlight it.
5.
Click on OK.
6.
Repeat steps 1-3 and select the node at the right end of the beam.
7.
In the scroll box of DOFs to be constrained, click once on "UX." Both "UX" and "UY" should be highlighted.
8.
Click on OK. The Apply U,ROT on Nodes dialog box closes.
6.4.4.8. Specify Analysis Type and Options 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis. The New Analysis dialog box appears.
2.
Click on "Modal" to select it and click on OK. The New Analysis dialog box closes.
3.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Modal Analysis dialog box appears.
4.
Click on "Reduced" as the mode extraction method [MODOPT].
5.
Enter 1 for the number of modes to expand.
6.
Click on the Calculate elem. results dialog button [MXPAND] to specify YES.
7.
Click on OK. The Modal Analysis dialog box closes, and the Reduced Modal Analysis dialog box appears.
8.
Enter 3 for the No. of modes to print and click on OK. The Reduced Modal Analysis dialog box closes.
9.
Choose menu path Main Menu> Solution> Master DOFs> User Selected> Define. The picking menu appears.
10. Choose Pick All. The Define Master DOFs dialog box appears. 11. Select UY for the 1st degree of freedom and click on OK. The Define Master DOFs dialog box closes.
6.4.4.9. Solve the Modal Analysis 1.
Choose menu path Main Menu> Solution> Solve> Current LS. The Solve Current Load Step dialog box appears, along with a status window.
2.
Carefully review the information in the status window, and then click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to start the solution.
4.
When the solution is finished, a dialog box stating "Solution is done!" appears. Click on Close.
6.4.4.10. Set Up the Spectrum Analysis 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis. The New Analysis dialog box appears, along with a warning message that states: "Changing the analysis type is only valid within the first load step. Pressing OK will cause you to exit and reenter SOLUTION. This will reset load step count to 1." Click on CLOSE to close the warning message box.
2.
Click on "Spectrum" to select it, and click on OK. The New Analysis dialog box closes. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–13
Chapter 6: Spectrum Analysis 3.
Choose menu path Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Settings. The Settings for Single-point Response Spectrum dialog box appears.
4.
Select "Seismic displac" in the scroll box as the type of response spectrum.
5.
Enter 0,1,0 for excitation direction into the excitation direction input windows and click on OK.
6.4.4.11. Define Spectrum Value vs. Frequency Table 1.
Choose menu path Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Freq Table. The Frequency Table dialog box appears.
2.
Enter 0.1 for FREQ1, enter 10 for FREQ2, and click on OK.
3.
Choose menu path Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Spectr Values. The Spectrum Values - Damping Ratio dialog box appears.
4.
Click on OK to accept the default of no damping. The Spectrum Values dialog box appears.
5.
Enter 0.44 and 0.44 for FREQ1 and FREQ2, respectively.
6.
Click on OK. The Spectrum Values dialog box closes.
6.4.4.12. Solve Spectrum Analysis 1.
Choose menu path Main Menu> Solution> Solve> Current LS. The Solve Current Load Step dialog box appears, along with a status window.
2.
Carefully review the information in the status window, and then click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to start the solution.
4.
When the solution is finished, a dialog box stating "Solution is done!" appears. Click on Close.
6.4.4.13. Set up the Expansion Pass 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis. The New Analysis dialog box appears, along with a warning message that states: "Changing the analysis type is only valid within the first load step. Pressing OK will cause you to exit and reenter SOLUTION. This will reset load step count to 1." Click on CLOSE to close the warning message box.
2.
Click on "Modal" to select it, and click on OK. The New Analysis dialog box closes.
3.
Choose menu path Main Menu> Solution> Analysis Type> Expansion Pass. The Expansion Pass dialog box appears.
4.
Click on the expansion pass dialog button to turn it ON and click on OK. The Expansion Pass dialog box closes.
6.4.4.14. Expand the Modes 1.
Choose menu path Main Menu> Solution> Load Step Opts> ExpansionPass> Expand Modes. The Expand Modes dialog box appears.
2.
Enter 10 for the number of modes to expand and enter 0.005 for the significant threshold.
3.
Click on the calculate element results dialog button to specify YES for element results calculation.
4.
Click on OK. The Expand Modes dialog box closes.
6–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.4: Sample Spectrum Analysis (GUI Method)
6.4.4.15. Start Expansion Pass Calculation 1.
Choose menu path Main Menu> Solution> Solve> Current LS. The Solve Current Load Step dialog box appears, along with a status window.
2.
Carefully review the information in the status window, and then click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to start the solution.
4.
When the solution is finished, a dialog box stating "Solution is done!" appears. Click on Close.
6.4.4.16. Set Up Mode Combination for Spectrum Analysis 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis. The New Analysis dialog box appears, along with a warning message that states: "Changing the analysis type is only valid within the first load step. Pressing OK will cause you to exit and reenter SOLUTION. This will reset load step count to 1." Click on CLOSE to close the warning message box.
2.
Click on "Spectrum" to select it, and click on OK. The New Analysis dialog box closes.
3.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Spectrum Analysis dialog box appears.
4.
Accept the default spectrum type single-point response. Click on OK. The Spectrum Analysis dialog box closes.
6.4.4.17. Select Mode Combination Method 1.
Choose menu path Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Mode Combine. The Mode Combination Methods dialog box appears.
2.
Select SRSS as the mode combination method.
3.
Enter 0.15 for the significant threshold.
4.
Select displacement for the type of output. Click OK. The Mode Combination Methods dialog box closes.
6.4.4.18. Combine the Modes 1.
Choose menu path Main Menu> Solution> Solve> Current LS. The Solve Current Load Step dialog box appears, along with a status window.
2.
Carefully review the information in the status window, and then click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to start the solution.
4.
When the solution is finished, a dialog box stating "Solution is done!" appears. Click on Close.
6.4.4.19. Postprocessing: Print Out Nodal, Element, and Reaction Solutions 1.
Choose menu path Main Menu> General Postproc> List Results> Results Summary. The SET Command listing window appears.
2.
Review the information in the listing window, and click on Close. The SET Command listing window closes.
3.
Choose menu path Utility Menu> File> Read Input From. The Read File dialog box appears.
4.
From the left side of the Read File dialog box, select the directory containing your results from the scroll box.
5.
From the right side of the Read File dialog box, select the jobname.mcom file from the scroll box. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–15
Chapter 6: Spectrum Analysis 6.
Click on OK. The Read File dialog box closes.
7.
Choose menu path Main Menu> General Postproc> List Results> Nodal Solution. The List Nodal Solution dialog box appears.
8.
Click on OK to accept the default settings of "DOF solution" in the scroll box on the left and "All DOFs DOF" in the scroll box on the right. The List Nodal Solution dialog box closes.
9.
The PRNSOL Command listing window appears. Review the results and click on Close to close the PRNSOL Command listing window.
10. Choose menu path Main Menu> General Postproc> List Results> Element Solution. The List Element Solution dialog box appears. 11. Scroll down the list on the left to select "Line Elem results" and select "Structural ELEM" on the scroll box on the right. Click on OK. The List Element Solution dialog box closes. 12. The PRESOL Command listing window appears. Review the results and click on Close to close the PRESOL Command listing window. 13. Choose menu path Main Menu> General Postproc> List Results> Reaction Solu. The List Reaction Solution dialog box appears. 14. Scroll down the list to "All struc forc F" to select it and click on OK. The List Reaction Solution dialog box closes. 15. The PRRSOL Command listing window appears. Review the results in the listing window and click on Close to close the PRRSOL Command listing window.
6.4.4.20. Exit ANSYS 1.
In the ANSYS Toolbar, click on Quit.
2.
Choose the save option you want and click on OK.
You are now finished with this sample problem.
6.5. Sample Spectrum Analysis (Command or Batch Method) You can perform the example spectrum analysis using the ANSYS commands shown below instead of GUI choices. Items prefaced by an exclamation point (!) are comments. /PREP7 /TITLE Seismic Response of a Beam Structure ET,1,BEAM3 R,1,273.9726,(1000/3),14 ! A = 273.9726, I = (1000/3), H = 14 MP,EX,1,30E6 MP,DENS,1,73E-5 K,1 K,2,240 L,1,2 ESIZE,,8 LMESH,1 NSEL,S,LOC,X,0 D,ALL,UY NSEL,S,LOC,X,240 D,ALL,UX,,,,,UY NSEL,ALL FINISH /SOLU ANTYPE,MODAL
6–16
! Mode-frequency analysis
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.6: Where to Find Other Examples MODOPT,REDUC,,,,3 MXPAND,1,,,YES M,ALL,UY OUTPR,BASIC,1 SOLVE FINISH
! Householder, print first 3 reduced mode shapes ! Expand first mode shape, calculate element stresses
/SOLU ANTYPE,SPECTR SPOPT,SPRS SED,,1 SVTYPE,3 FREQ,.1,10 SV,,.44,.44 SOLVE FINISH
! ! ! ! ! !
/SOLU ANTYPE,MODAL EXPASS,ON MXPAND,10,,,YES,0.005
Spectrum analysis Single point spectrum Global Y-axis as spectrum direction Seismic displacement spectrum Frequency points for SV vs. freq. table Spectrum values associated with frequency points
! Mode-frequency analysis ! Expand 10 mode shapes, calculate element stresses ! set signif=0.005
SOLVE FINISH /SOLU ANTYPE,SPECTR SRSS,0.15,DISP
! Square Root of Sum of Squares Mode combination ! with signif=0.15 and displacement solution requested
SOLVE FINISH /POST1 SET,LIST /INP,,mcom PRNSOL,DOF PRESOL,ELEM PRRSOL,F FINISH
! Print nodal solution ! Print element solution in element format ! Print reaction solution
6.6. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional spectrum analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS program. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual includes a variety of spectrum analysis test cases: VM19 - Random Vibration Analysis of a Deep Simply-Supported Beam VM68 - PSD Response of a Two DOF Spring-Mass System VM69 - Seismic Response VM70 - Seismic Response of a Beam Structure VM203 - Dynamic Load Effect on Simply-Supported Thick Square Plate See the ANSYS Commands Reference for a discussion of the ANTYPE, MODOPT, D, EXPASS, MXPAND, SPOPT, SVTYP, SED, FREQ, SV, SRSS, CQC, DSUM, GRP, NRLSUM, and DMPRAT commands.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–17
Chapter 6: Spectrum Analysis
6.7. How to Do a Random Vibration (PSD) Analysis The procedure for a PSD analysis consists of six main steps: 1.
Build the model.
2.
Obtain the modal solution.
3.
Expand the modes.
4.
Obtain the spectrum solution.
5.
Combine the modes.
6.
Review the results.
Of these, the first two steps are the same as described for a single-point response spectrum analysis. The procedure for the remaining four steps is explained below. Random vibration analysis is not available in the ANSYS Professional program. In the GUI method, the dialog box for the modal analysis options [MODOPT] contains an option for mode expansion [MXPAND]. Choose YES for mode expansion. You then follow the instructions in Section 6.7.1: Expand the Modes. The procedures for obtaining the modal solution and expanding the nodes are combined into a single step.
6.7.1. Expand the Modes You must expand modes regardless of whether you used the subspace, Block Lanczos, or reduced extraction method. Details about expanding the modes are explained in Section 3.6: Expand the Modes, but keep in mind the following additional points: •
Only expanded modes are used for the mode combination step.
•
If you are interested in stresses caused by the spectrum, be sure to request stress calculations here. By default, no stresses are calculated in the expansion pass, which means no stresses are available at the end of the spectrum solution.
•
The mode expansion can be performed as a separate step, or can be included in the modal analysis phase.
•
At the end of the expansion pass, leave SOLUTION with the FINISH command. If you want to exit ANSYS after running the modal analysis, you must save the database at this point.
As explained in Chapter 3, “Modal Analysis”, you can combine the modal solution and mode expansion steps by including the MXPAND command in the modal analysis step (GUI and batch modes).
6.7.2. Obtain the Spectrum Solution To obtain the PSD spectrum solution, the database must contain the model data as well as the modal solution data. If you leave ANSYS after running the modal analysis, you must save the database. In addition, the following files from the modal solution must be available: Jobname.MODE, .ESAV, .EMAT, .FULL (only for subspace and Block Lanczos methods), .RST. 1.
Enter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define the analysis type and analysis options:
6–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.7: How to Do a Random Vibration (PSD) Analysis
3.
•
For spectrum type [SPOPT], choose Power Spectral Density (PSD).
•
Specify stress calculations ON [SPOPT] if you are interested in stress results. Stresses caused by the spectrum are calculated only if they were also requested during the modal expansion pass.
Specify load step options. The following options are available for a random vibration analysis: •
Spectrum Data –
Type of PSD Command(s): PSDUNIT GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> Settings The PSD type can be displacement, velocity, force, pressure, or acceleration. Whether it is a base excitation or a nodal excitation is specified in Steps 4 and 5. If a pressure PSD is to be applied, the pressures should be applied in the modal analysis itself.
–
PSD-versus-frequency table Define a piecewise-linear (in log-log scale) PSD versus frequency table. Since a curve-fitting polynomial is used for the closed-form integration of the curve, you should graph the input, which is overlaid with the fitted curve, to ensure a good fit. If the fit is not good, you should add one or more intermediate points to the table until you obtain a good fit. Command(s): PSDFRQ, PSDVAL, PSDGRAPH GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> PSD vs Freq Main Menu> Solution> Load Step Opts> Spectrum> PSD> Graph PSD Tables PSDFRQ and PSDVAL are used to define the PSD-versus-frequency table. Step 6 describes how to apply additional PSD excitations (if any). You can issue STAT to list PSD tables and issue PSDGRAPH to graph them.
•
Damping (Dynamics Options) The following forms of damping are available: ALPHAD, BETAD, and MDAMP result in a frequencydependent damping ratio, whereas DMPRAT specifies a constant damping ratio to be used at all frequencies. If you specify more than one form of damping, ANSYS calculates an effective damping ratio at each frequency. Note — If no damping is specified in a PSD analysis, a default DMPRAT of 1 percent is used. –
Alpha (Mass) Damping Command(s): ALPHAD GUI: Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
–
Beta (Stiffness) Damping Command(s): BETAD GUI: Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
–
Constant Damping Ratio Command(s): DMPRAT GUI: Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
–
Frequency-Dependent Damping Ratio Command(s): MDAMP GUI: Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–19
Chapter 6: Spectrum Analysis
The remaining steps are specific to a random vibration analysis: 4.
Apply the PSD excitation at the desired nodes. Use a value of 1.0 to indicate points where the PSD excitation applies. A value of 0.0 (or blank) can be used to remove a specification. The excitation direction is implied by the UX, UY, UZ labels on the D command (for base excitation), and by FX, FY, FZ on the F command (for nodal excitation). For nodal excitation, values other than 1.0 can be used to scale the participation factors. For pressure PSD, bring in the load vector from the modal analysis (LVSCALE). You can use the scale factor. Note — You can apply base excitations only at nodes that were constrained in the modal analysis. Command(s): D (or DK, DL, or DA) for base excitation F (or FK) for nodal excitation LVSCALE for pressure PSD GUI: Main Menu> Solution> Define Loads> Apply> Structural> Spectrum> Base PSD Excit> On Nodes
5.
Begin participation factor calculations for the above PSD excitation. Use the TBLNO field to indicate which PSD table to use, and Excit to specify whether the calculations are for a base or nodal excitation. Command(s): PFACT GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> Calculate PF
6.
If you need to apply multiple PSD excitations on the same model, repeat steps 3, 4, and 5 for each additional PSD table. Then define, as necessary, the degree of correlation between the excitations, using any of the following commands: Command(s): COVAL for cospectral values QDVAL for quadspectral values PSDSPL for a spatial relationship PSDWAV for a wave propagation relationship PSDGRAPH to graph the data overlaid with the fitted curve GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> Correlation Main Menu> Solution> Load Step Opts> Spectrum> PSD> Graph Tables When you use the PSDSPL or PSDWAV command, you must use SPATIAL or WAVE, respectively, for Parcor on the PFACT command. PSDSPL and PSDWAV relationships might be quite CPU intensive for multi-point base excitations. Nodal excitation and base excitation input must be consistent when using PSDWAV and PSDSPL (for example, FY cannot be applied to one node and FZ be applied to another). The PSDSPL and PSDWAV commands are not available for a pressure PSD analysis.
7.
Specify the output controls. The only valid output control command for this analysis is PSDRES, which specifies the amount and form of output written to the results file. Up to three sets of solution quantities can be calculated: displacement solution, velocity solution, or acceleration solution. Each of these can be relative to the base or absolute. Command(s): PSDRES GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> Calc Controls Table 6.3: “Solution Items Available in a PSD Analysis” shows a summary of the possible solution sets. To limit the amount of data written to the results file, use OUTRES at the mode expansion step. Using OUTPR,NSOL,ALL provides a summary table of the significant modal covariance terms.
6–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.7: How to Do a Random Vibration (PSD) Analysis
Table 6.3 Solution Items Available in a PSD Analysis Solution
Items
Displacement Solution (label DISP Displacements, stresses, strains, forces on PSDRES) Velocity Solution (label VELO on PSDRES)
Form Relative, absolute, or neither
Velocities, stress velocities, force Relative, absolute, or neither velocities, etc.
Acceleration Solution (label ACEL Accelerations, stress accl's, force accl's, etc. on PSDRES)
8.
Start solution calculations. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
9.
Leave the SOLUTION processor. Command(s): FINISH GUI: Close the Solution menu.
Relative, absolute, or neither
6.7.3. Combine the Modes The modes can be combined in a separate solution phase. The procedure is as follows: 1.
Enter Solution. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define analysis type. •
Option: New Analysis [ANTYPE] Choose New Analysis.
•
Option: Analysis Type: Spectrum [ANTYPE] Choose analysis type spectrum.
3.
Only the PSD mode combination method is valid in a random vibration analysis. This method triggers calculation of the one-sigma displacements, stresses, etc., in the structure. If you do not issue the PSDCOM command, the program does not calculate the one-sigma response of the structure. Command(s): PSDCOM GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> Mode Combin The SIGNIF and COMODE fields on the PSD mode combination method [PSDCOM] offer options to reduce the number of modes to be combined (see the description of PSDCOM command). If you want to exercise these options, it is prudent to print the modal covariance matrices in Section 6.7.2: Obtain the Spectrum Solution to first investigate the relative contributions of the modes toward the final solution.
4.
Start the solution. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
5.
Leave the SOLUTION processor. Command(s): FINISH GUI: Close the Solution menu.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–21
Chapter 6: Spectrum Analysis
6.7.4. Review the Results Results from a random vibration analysis are written to the structural results file, Jobname.RST. They consist of the following quantities: 1.
Expanded mode shapes from the modal analysis
2.
Static solution for base excitation [PFACT,,BASE]
3.
The following output, if mode combinations are requested [PSDCOM] and based on the PSDRES setting: •
1 σ displacement solution (displacements, stresses, strains, and forces)
•
1 σ velocity solution (velocities, stress velocities, strain velocities, and force velocities)
•
1 σ acceleration solution (accelerations, stress accelerations, strain accelerations, and force accelerations)
You can review these results in POST1, the general postprocessor, and then calculate response PSDs in POST26, the time-history postprocessor.
6.7.4.1. Reviewing the Results in POST1 To review results in POST1, you first need to understand how the results data are organized on the results file. Table 6.4: “Organization of Results Data from a PSD Analysis” shows the organization. Note — Load step 2 is left blank if you specify only nodal PSD excitation. Also, if you suppress the displacement, velocity, or acceleration solution using the PSDRES command, the corresponding load step is left blank. Also, the superelement displacement file (.DSUB) is not written for load steps 3, 4, or 5 in a PSD analysis.
Table 6.4 Organization of Results Data from a PSD Analysis Load Step
Substep
1
1
Expanded modal solution for 1st mode
2
Expanded modal solution for 2nd mode
3
Expanded modal solution for 3rd mode
Etc. 2 (Base excit. only)
Contents
Etc.
1
Unit static solution for PSD table 1
2
Unit static solution for PSD table 2
Etc.
Etc.
3
1
1 sigma displacement solution
4
1
1 sigma velocity solution (if requested)
5
1
1 sigma acceleration solution (if requested)
6.7.4.1.1. Read the Desired Set of Results into the Database For example, to read in the 1 σ displacement solution, issue the command: SET,3,1
Command(s): SET GUI: Main Menu> General Postproc> Read Results> First Set 6–22
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.7: How to Do a Random Vibration (PSD) Analysis
6.7.4.1.2. Display the Results Use the same options available for the SPRS analysis. Note — Nodal stress averaging performed by the PLNSOL command may not be appropriate in a random vibration analysis because the "stresses" are not actual stresses but stress statistics.
6.7.4.2. Calculating Response PSDs in POST26 You can calculate and display response PSDs for any results quantity available on the results file (displacements, velocities, and/or accelerations) if the Jobname.RST and Jobname.PSD files are available. The procedure to calculate the response PSD is as follows: 1.
Enter POST26, the time-history postprocessor. Command(s): /POST26 GUI: Main Menu> TimeHist PostPro
2.
Store the frequency vector. NPTS is the number of frequency points to be added on either side of natural frequencies in order to "smooth" the frequency vector (defaults to 5). The frequency vector is stored as variable 1. Command(s): STORE,PSD,NPTS GUI: Main Menu> TimeHist Postpro> Store Data
3.
Define the variables in which the result items of interest (displacements, stresses, reaction forces, etc.) are to be stored. Command(s): NSOL, ESOL, and/or RFORCE GUI: Main Menu> TimeHist Postpro> Define Variables
4.
Calculate the response PSD and store it in the desired variable. The PLVAR command can then be used to plot the response PSD. Command(s): RPSD GUI: Main Menu> TimeHist Postpro> Calc Resp PSD
6.7.4.3. Calculating Covariance in POST26 You can compute the covariance between two quantities available on the results file (displacements, velocities, and/or accelerations), if the Jobname.RST and Jobname.PSD files are available. The procedure to calculate the covariance between two quantities is as follows: 1.
Enter POST26, the time-history postprocessor. Command(s): /POST26 GUI: Main Menu> TimeHist PostPro
2.
Define the variables in which the result items of interest (displacements, stresses, reaction forces, etc.) are to be stored. Command(s): NSOL, ESOL, and/or RFORCE GUI: Main Menu> TimeHist Postpro> Define Variables
3.
Calculate the contributions of each response component (relative or absolute response) and store them in the desired variable. The PLVAR command can then be used to plot the modal contributions (relative response) followed by the contributions of pseudo-static and mixed part responses to the total covariance. Command(s): CVAR GUI: Main Menu> TimeHist Postpro> Calc Covariance
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–23
Chapter 6: Spectrum Analysis 4.
Obtain the covariance. Command(s): *GET,NameVARI,n,EXTREM,CVAR GUI: Utility Menu> Parameters> Get Scalar Data
6.7.5. Sample Input A sample input listing for a random vibration (PSD) analysis is shown below: ! Build the Model /FILNAM, /TITLE, /PREP7 ... ... ... FINISH ! ! Obtain the Modal Solution /SOLU ANTYPE,MODAL MODOPT,REDU M, ... TOTAL, ... D, ... SAVE SOLVE FINISH ! Expand the Modes /SOLU EXPASS,ON MXPAND, ... SOLVE FINISH ! ! Obtain the Spectrum Solution /SOLU! Reenter SOLUTION ANTYPE,SPECTR SPOPT,PSD, ... PSDUNIT, ... PSDFRQ, ...
! Jobname ! Title ! Enter PREP7 ! Generate model
! ! ! !
Enter SOLUTION Modal analysis Reduced method Master DOF
! Constraints ! Initiates solution
! Reenter SOLUTION ! Expansion pass ! Number of modes to expand
! ! ! ! ! ! ! ! ! ! !
Spectrum analysis Power Spectral Density; No. of modes; Stress calcs. on/off Type of spectrum Frequency pts. (for spectrum values vs. frequency tables) Spectrum values Damping ratio Base excitation Calculate participation factors Output controls
PSDVAL, ... DMPRAT, ... D,0 PFACT, ... PSDRES, ... SAVE SOLVE FINISH ! ! Combine modes using PSD method /SOLU ! Re-enter SOLUTION ANTYPE,SPECTR ! Spectrum analysis PSDCOM,SIGNIF,COMODE ! PSD mode combinations with significance factor and ! option for selecting a subset of modes for ! combination SOLVE FINISH ! ! Review the Results /POST1 ! Enter POST1 SET, ... ! Read results from appropriate load step, substep ...! Postprocess as desired ...! (PLDISP; PLNSOL; NSORT; PRNSOL; etc.) ... FINISH ! ! Calculate Response PSD /POST26 ! Enter POST26
6–24
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.9: How to Do Multi-Point Response Spectrum (MPRS) Analysis STORE,PSD NSOL,2,... RPSD,3,2,,... PLVAR,3 ... ! Calculate Covariance RESET NSOL,2 NSOL,3 CVAR,4,2,3,1,1
! ! ! !
! ! ! ! ! *GET,CVAR23U,VARI,4,EXREME,CVAR ! FINISH
Store frequency vector (variable 1) Define variable 2 (nodal data) Calculate response PSD (variable 3) Plot the response PSD
Reset all POST26 specifications to initial defaults. Define variable 2 (nodal data). Define variable 3 (nodal data). Calculate covariance between displacement at nodes 2 and 3. Obtain covariance.
See the ANSYS Commands Reference for a discussion of the ANTYPE, MODOPT, M, TOTAL, D, EXPASS, MXPAND, SPOPT, PSDUNIT, PSDFRQ, PSDVAL, DMPRAT, PFACT, PSDCOM, SUMTYPE, and PSDRES commands.
6.8. How to Do DDAM Spectrum Analysis The procedure for a DDAM spectrum analysis is the same as that for a single-point response spectrum (SPRS) analysis (including file requirements), with the following exceptions: •
Use the British system of units [inches (not feet), pounds, etc.] for all input data - model geometry, material properties, element real constants, etc.
•
Choose DDAM instead of SPRS as the spectrum type [SPOPT command].
•
Use the ADDAM and VDDAM commands instead of SVTYP, SV, and FREQ to specify the spectrum values and types. Specify the global direction of excitation using the SED command. Based on the coefficients specified in the ADDAM and VDDAM commands, the program computes the mode coefficients according to the empirical equations given in the ANSYS, Inc. Theory Reference.
•
The most applicable mode combination method is the NRL sum method [NRLSUM]. Mode combinations are done in the same manner as for a single-point response spectrum. Mode combinations require damping.
•
No damping needs to be specified for solution because it is implied by the ADDAM and VDDAM commands. If damping is specified, it is used for mode combinations but ignored for solution. Note — As in the Single-point Response Spectrum analysis, DDAM spectrum analysis requires six steps to systematically perform the analysis.
If you are using batch mode, note the following: •
The modal solution and DDAM spectrum solution passes can be combined into a single modal analysis [ANTYPE,MODAL] solution pass with DDAM spectrum loads [ADDAM, VDDAM, SED].
•
The mode expansion and mode combination solution passes can be combined into a single modal analysis [ANTYPE,MODAL and EXPASS,ON] solution pass with a mode combination command.
DDAM spectrum analysis is not available in the ANSYS Professional program.
6.9. How to Do Multi-Point Response Spectrum (MPRS) Analysis The procedure for a multi-point response spectrum analysis is the same as that for random vibration (PSD) analysis (including file requirements), with the following exceptions: •
Choose MPRS instead of PSD as the type of spectrum [SPOPT command].
•
The "PSD-versus-frequency" tables now represent spectral values versus frequency. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–25
Chapter 6: Spectrum Analysis •
You cannot specify any degree of correlation between the spectra (i.e., they are assumed to be uncorrelated).
•
Only relative results (relative to the base excitation) not absolute values, are calculated.
•
All mode combination methods are available except PSDCOM.
•
Results from a multi-point response spectrum analysis are written to the mode combination file, Jobname.MCOM, in the form of POST1 commands. The commands calculate the overall response of the structure by combining the maximum modal responses in some fashion (specified by the mode combination command in SOLUTION). The overall response consists of the overall displacements and, if placed on the results file during the modal expansion pass, the overall stresses, strains, and reaction forces. If Label = VELO or ACEL on the mode combination command (SRSS, CQC, GRP, DSUM, or NRLSUM) during SOLUTION, the corresponding velocity or acceleration responses are written to the mode combination file.
Multi-point response spectrum analysis is not available in the ANSYS Professional program.
6–26
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 7: Buckling Analysis 7.1. Definition of Buckling Analysis Buckling analysis is a technique used to determine buckling loads - critical loads at which a structure becomes unstable - and buckled mode shapes - the characteristic shape associated with a structure's buckled response.
7.2. Types of Buckling Analyses Two techniques are available in the ANSYS Multiphysics, ANSYS Mechanical, ANSYS Structural, and ANSYS Professional programs for predicting the buckling load and buckling mode shape of a structure: nonlinear buckling analysis, and eigenvalue (or linear) buckling analysis. Since these two methods frequently yield quite different results, let's examine the differences between them before discussing the details of their implementation.
7.2.1. Nonlinear Buckling Analysis Nonlinear buckling analysis is usually the more accurate approach and is therefore recommended for design or evaluation of actual structures. This technique employs a nonlinear static analysis with gradually increasing loads to seek the load level at which your structure becomes unstable, as depicted in Figure 7.1: “Buckling Curves” (a). Using the nonlinear technique, your model can include features such as initial imperfections, plastic behavior, gaps, and large-deflection response. In addition, using deflection-controlled loading, you can even track the post-buckled performance of your structure (which can be useful in cases where the structure buckles into a stable configuration, such as "snap-through" buckling of a shallow dome).
7.2.2. Eigenvalue Buckling Analysis Eigenvalue buckling analysis predicts the theoretical buckling strength (the bifurcation point) of an ideal linear elastic structure. (See Figure 7.1: “Buckling Curves” (b).) This method corresponds to the textbook approach to elastic buckling analysis: for instance, an eigenvalue buckling analysis of a column will match the classical Euler solution. However, imperfections and nonlinearities prevent most real-world structures from achieving their theoretical elastic buckling strength. Thus, eigenvalue buckling analysis often yields unconservative results, and should generally not be used in actual day-to-day engineering analyses.
Figure 7.1 Buckling Curves
(a) Nonlinear load-deflection curve, (b) Linear (Eigenvalue) buckling curve Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 7: Buckling Analysis
7.3. Commands Used in a Buckling Analysis You use the same set of commands to build a model and perform a buckling analysis that you use to do any other type of finite element analysis. Likewise, you choose similar options from the graphical user interface (GUI) to build and solve models no matter what type of analysis you are doing. Section 7.6: Sample Buckling Analysis (GUI Method) and Section 7.7: Sample Buckling Analysis (Command or Batch Method) show you how to perform an example eigenvalue buckling analysis via the GUI or via commands, respectively. For detailed, alphabetized descriptions of the ANSYS commands, see the ANSYS Commands Reference.
7.4. Procedure for Nonlinear Buckling Analysis A nonlinear buckling analysis is a static analysis with large deflections turned on [NLGEOM,ON], extended to a point where the structure reaches its limit load or maximum load. Other nonlinearities such as plasticity may be included in the analysis. The procedure for a static analysis is described in Chapter 2, “Structural Static Analysis”, and nonlinearities are described in Chapter 8, “Nonlinear Structural Analysis”.
7.4.1. Applying Load Increments The basic approach in a nonlinear buckling analysis is to constantly increment the applied loads until the solution begins to diverge. Be sure to use a sufficiently fine load increment as your loads approach the expected critical buckling load. If the load increment is too coarse, the buckling load predicted may not be accurate. Turn on bisection and automatic time stepping [AUTOTS,ON] to help avoid this problem.
7.4.2. Automatic Time Stepping With automatic time stepping on, the program automatically seeks out the buckling load. If automatic time stepping is ON in a static analysis having ramped loading and the solution does not converge at a given load, the program bisects the load step increment and attempts a new solution at a smaller load. In a buckling analysis, each such convergence failure is typically accompanied by a "negative pivot" message indicating that the attempted load equals or exceeds the buckling load. You can usually ignore these messages if the program successfully obtains a converged solution at the next, reduced load. If stress stiffness is active [SSTIF,ON], you should run without adaptive descent active [NROPT,FULL,,OFF] to ensure that a lower bound to the buckling load is attained. The program normally converges to the limiting load as the process of bisection and resolution continues to the point at which the minimum time step increment (specified by DELTIM or NSUBST) is achieved. The minimum time step will directly affect the precision of your results.
7.4.3. Important Remember that an unconverged solution does not necessarily mean that the structure has reached its maximum load. It could also be caused by numerical instability, which might be corrected by refining your modeling technique. Track the load-deflection history of your structure's response to decide whether an unconverged load step represents actual structural buckling, or whether it reflects some other problem. Perform a preliminary analysis using the arc-length method [ARCLEN] to predict an approximate value of buckling load. Compare this approximate value to the more precise value calculated using bisection to help determine if the structure has indeed reached its maximum load. You can also use the arc-length method itself to obtain a precise buckling load, but this method requires you to adjust the arc-length radius by trial-and-error in a series of manually directed reanalyses.
7–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 7.5: Procedure for Eigenvalue Buckling Analysis
7.4.4. Points to Remember •
If the loading on the structure is perfectly in-plane (that is, membrane or axial stresses only), the out-ofplane deflections necessary to initiate buckling will not develop, and the analysis will fail to predict buckling behavior. To overcome this problem, apply a small out-of-plane perturbation, such as a modest temporary force or specified displacement, to begin the buckling response. (A preliminary eigenvalue buckling analysis of your structure may be useful as a predictor of the buckling mode shape, allowing you to choose appropriate locations for applying perturbations to stimulate the desired buckling response.) The imperfection (perturbation) induced should match the location and size of that in the real structure. The failure load is very sensitive to these parameters.
•
In a large-deflection analysis, forces (and displacements) will maintain their original orientation, but surface loads will "follow" the changing geometry of the structure as it deflects. Therefore, be sure to apply the proper type of loads.
•
You should carry your stability analysis through to the point of identifying the critical load in order to calculate the structure's factor of safety with respect to nonlinear buckling. (Merely establishing the fact that a structure is stable at a given load level is generally insufficient for most design practice; you will usually be required to provide a specified safety factor, which can only be determined by establishing the actual limit load.)
•
You can extend your analysis into the post-buckled range by activating the arc-length method [ARCLEN]. Use this feature to trace the load-deflection curve through regions of "snap-through" and "snap-back" response.
•
For those elements that support the consistent tangent stiffness matrix (BEAM4, SHELL63, and SHELL143), activate the consistent tangent stiffness matrix (KEYOPT(2) = 1 and NLGEOM,ON) to enhance the convergence behavior of your nonlinear buckling analyses and improve the accuracy of your results. This element KEYOPT must be defined before the first load step of the solution and cannot be changed once the solution has started.
•
Many other elements (such as BEAM188, BEAM189, and SHELL181) will provide consistent tangent stiffness matrix with NLGEOM,ON.
7.5. Procedure for Eigenvalue Buckling Analysis Again, remember that eigenvalue buckling analysis generally yields unconservative results, and should usually not be used for design of actual structures. If you decide that eigenvalue buckling analysis is appropriate for your application, follow this procedure: 1.
Build the model.
2.
Obtain the static solution.
3.
Obtain the eigenvalue buckling solution.
4.
Expand the solution.
5.
Review the results.
7.5.1. Build the Model See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details, see the ANSYS Modeling and Meshing Guide.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
7–3
Chapter 7: Buckling Analysis
7.5.1.1. Points to Remember •
Only linear behavior is valid. Nonlinear elements, if any, are treated as linear. If you include contact elements, for example, their stiffnesses are calculated based on their status after the static prestress run and are never changed.
•
Young's modulus (EX) (or stiffness in some form) must be defined. Material properties may be linear, isotropic or orthotropic, and constant or temperature-dependent. Nonlinear properties, if any, are ignored.
7.5.2. Obtain the Static Solution The procedure to obtain a static solution is the same as described in Chapter 2, “Structural Static Analysis”, with the following exceptions: •
Prestress effects [PSTRES] must be activated. Eigenvalue buckling analysis requires the stress stiffness matrix to be calculated.
•
Unit loads are usually sufficient (that is, actual load values need not be specified). The eigenvalues calculated by the buckling analysis represent buckling load factors. Therefore, if a unit load is specified, the load factors represent the buckling loads. All loads are scaled. (Also, the maximum permissible eigenvalue is 1,000,000 - you must use larger applied loads if your eigenvalue exceeds this limit.)
•
Note that eigenvalues represent scaling factors for all loads. If certain loads are constant (for example, self-weight gravity loads) while other loads are variable (for example, externally applied loads), you need to ensure that the stress stiffness matrix from the constant loads is not factored by the eigenvalue solution. One strategy that you can use to achieve this end is to iterate on the eigensolution, adjusting the variable loads until the eigenvalue becomes 1.0 (or nearly 1.0, within some convergence tolerance). Design optimization could be useful in driving this iterative procedure to a final answer. Consider, for example, a pole having a self-weight W0, which supports an externally-applied load, A. To determine the limiting value of A in an eigenvalue buckling solution, you could solve repetitively, using different values of A, until by iteration you find an eigenvalue acceptably close to 1.0.
Figure 7.2 Adjusting Variable Loads to Find an Eigenvalue of 1.0
•
You can apply a nonzero constraint in the prestressing pass as the static load. The eigenvalues found in the buckling solution will be the load factors applied to these nonzero constraint values. However, the mode shapes will have a zero value at these degrees of freedom (and not the nonzero value specified).
•
At the end of the solution, leave SOLUTION [FINISH].
7–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 7.5: Procedure for Eigenvalue Buckling Analysis
7.5.3. Obtain the Eigenvalue Buckling Solution This step requires files Jobname.EMAT and Jobname.ESAV from the static analysis. Also, the database must contain the model data (issue RESUME if necessary). Follow the steps below to obtain the eigenvalue buckling solution. 1.
Enter the ANSYS solution processor. Command(s): /SOLU GUI: Main Menu> Solution
2.
Specify the analysis type. Command(s): ANTYPE,BUCKLE GUI: Main Menu> Solution> Analysis Type> New Analysis Note — Restarts are not valid in an eigenvalue buckling analysis. Note — When you specify an eigenvalue buckling analysis, a Solution menu that is appropriate for buckling analyses appears. The Solution menu will be either "abridged" or "unabridged", depending on the actions you took prior to this step in your ANSYS session. The abridged menu contains only those solution options that are valid and/or recommended for buckling analyses. If you are on the abridged Solution menu and you want to access other solution options (that is, solution options that are valid for you to use, but their use may not be encouraged for this type of analysis), select the Unabridged Menu option from the Solution menu. For details, see Section 3.11.1: Using Abridged Solution Menus in the ANSYS Basic Analysis Guide.
3.
Specify analysis options. Command(s): BUCOPT, Method, NMODE, SHIFT GUI: Main Menu> Solution> Analysis Type> Analysis Options Regardless of whether you use the command or GUI method, you can specify values for these options:
4.
•
For Method, specify the eigenvalue extraction method. You can choose subspace iteration or Block Lanczos. The Block Lanczos and subspace iteration methods use the full system matrices. See Section 3.5.2.3: Option: Mode-Extraction Method [MODOPT] in this manual for more information about these solution methods.
•
For NMODE, specify the number of eigenvalues to be extracted. This argument defaults to one, which is usually sufficient for eigenvalue buckling.
•
For SHIFT, specify the point (load factor) about which eigenvalues are calculated. The shift point is helpful when numerical problems are encountered (due to negative eigenvalues, for example). Defaults to 0.0.
Specify load step options. The only load step options valid for eigenvalue buckling are output controls and expansion pass options. Command(s): OUTPR,NSOL,ALL GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout You can make the expansion pass a part of the eigenvalue buckling solution or perform it as a separate step. In this document, we treat the expansion pass as a separate step. See Section 7.5.4: Expand the Solution for details.
5.
Save a backup copy of the database to a named file. Command(s): SAVE Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
7–5
Chapter 7: Buckling Analysis GUI: Utility Menu> File> Save As 6.
Start solution calculations. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS The output from the solution mainly consists of the eigenvalues, which are printed as part of the printed output (Jobname.OUT). The eigenvalues represent the buckling load factors; if unit loads were applied in the static analysis, they are the buckling loads. No buckling mode shapes are written to the database or the results file, so you cannot postprocess the results yet. To do this, you need to expand the solution (explained next). Sometimes you may see both positive and negative eigenvalues calculated. Negative eigenvalues indicate that buckling occurs when the loads are applied in an opposite sense.
7.
Exit the SOLUTION processor. Command(s): FINISH GUI: Close the Solution menu.
7.5.4. Expand the Solution If you want to review the buckled mode shape(s), you must expand the solution regardless of which eigenvalue extraction method is used. In the case of the subspace iteration method, which uses full system matrices, you may think of "expansion" to simply mean writing buckled mode shapes to the results file.
7.5.4.1. Points to Remember •
The mode shape file (Jobname.MODE) from the eigenvalue buckling solution must be available.
•
The database must contain the same model for which the solution was calculated.
7.5.4.2. Expanding the Solution The procedure to expand the mode shapes is explained below. 1.
Reenter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution Note — You must explicitly leave SOLUTION (using the FINISH command) and reenter (/SOLU) before performing the expansion pass.
2.
Specify that this is an expansion pass. Command(s): EXPASS,ON GUI: Main Menu> Solution> Analysis Type> ExpansionPass
3.
Specify expansion pass options. Command(s): MXPAND, NMODE, , , Elcalc GUI: Main Menu> Solution> Load Step Opts> ExpansionPass> Expand Modes Regardless of whether you use the command or GUI method, the following options are required for the expansion pass: •
7–6
For NMODE, specify the number of modes to expand. This argument defaults to the total number of modes that were extracted. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 7.5: Procedure for Eigenvalue Buckling Analysis •
4.
For Elcalc, indicate whether you want ANSYS to calculate stresses. "Stresses" in an eigenvalue analysis do not represent actual stresses, but give you an idea of the relative stress or force distribution for each mode. By default, no stresses are calculated.
Specify load step options. The only options valid in a buckling expansion pass are the following output controls: •
Printed Output Use this option to include any results data on the output file (Jobname.OUT). Command(s): OUTPR GUI: Main Menu> Solution> Load Step Opts> Output Ctrl> Solu Printout
•
Database and Results File Output This option controls the data on the results file (Jobname.RST). Command(s): OUTRES GUI: Main Menu> Solution> Load Step Opts> Output Ctrl> DB/Results File Note — The FREQ field on OUTPR and OUTRES can only be ALL or NONE, that is, the data can be requested for all modes or no modes - you cannot write information for every other mode, for instance.
5.
Start expansion pass calculations. The output consists of expanded mode shapes and, if requested, relative stress distributions for each mode. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
6.
Leave the SOLUTION processor. You can now review results in the postprocessor. Command(s): FINISH GUI: Close the Solution menu. Note — The expansion pass has been presented here as a separate step. You can make it part of the eigenvalue buckling solution by including the MXPAND command (Main Menu> Solution> Load Step Opts> ExpansionPass> Expand Modes) as one of the analysis options.
7.5.5. Review the Results Results from a buckling expansion pass are written to the structural results file, Jobname.RST. They consist of buckling load factors, buckling mode shapes, and relative stress distributions. You can review them in POST1, the general postprocessor. Note — To review results in POST1, the database must contain the same model for which the buckling solution was calculated (issue RESUME if necessary). Also, the results file (Jobname.RST) from the expansion pass must be available. 1.
List all buckling load factors. Command(s): SET,LIST GUI: Main Menu> General Postproc> Results Summary Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
7–7
Chapter 7: Buckling Analysis 2.
Read in data for the desired mode to display buckling mode shapes. (Each mode is stored on the results file as a separate substep.) Command(s): SET,SBSTEP GUI: Main Menu> General Postproc> Read Results> load step
3.
Display the mode shape. Command(s): PLDISP GUI: Main Menu> General Postproc> Plot Results> Deformed Shape
4.
Contour the relative stress distributions. Command(s): PLNSOL or PLESOL GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solution Main Menu> General Postproc> Plot Results> Contour Plot> Element Solution
See the ANSYS Commands Reference for a discussion of the ANTYPE, PSTRES, D, F, SF, BUCOPT, EXPASS, MXPAND, OUTRES, SET, PLDISP, and PLNSOL commands.
7.6. Sample Buckling Analysis (GUI Method) In this sample problem, you will analyze the buckling of a bar with hinged ends.
7.6.1. Problem Description Determine the critical buckling load of an axially loaded long slender bar of length l with hinged ends. The bar has a cross-sectional height h, and area A. Only the upper half of the bar is modeled because of symmetry. The boundary conditions become free-fixed for the half-symmetry model. The moment of inertia of the bar is calculated as I = Ah2/12 = 0.0052083 in4.
7.6.2. Problem Specifications The following material properties are used for this problem: E = 30 x 106 psi The following geometric properties are used for this problem: l = 200 in A = 0.25 in2 h = 0.5 in Loading for this problem is: F = 1 lb.
7–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 7.6: Sample Buckling Analysis (GUI Method)
7.6.3. Problem Sketch Figure 7.3 Bar with Hinged Ends
7.6.3.1. Set the Analysis Title After you enter the ANSYS program, follow these steps to set the title. 1.
Choose menu path Utility Menu> File> Change Title.
2.
Enter the text "Buckling of a Bar with Hinged Ends" and click on OK.
7.6.3.2. Define the Element Type In this step, you define BEAM3 as the element type. 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete. The Element Types dialog box appears.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
In the scroll box on the left, click on "Structural Beam" to select it.
4.
In the scroll box on the right, click on "2D elastic 3" to select it.
5.
Click on OK, and then click on Close in the Element Types dialog box.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
7–9
Chapter 7: Buckling Analysis
7.6.3.3. Define the Real Constants and Material Properties 1.
Choose menu path Main Menu> Preprocessor> Real Constants> Add/Edit/Delete. The Real Constants dialog box appears.
2.
Click on Add. The Element Type for Real Constants dialog box appears.
3.
Click on OK. The Real Constants for BEAM3 dialog box appears.
4.
Enter .25 for area, 52083e-7 for IZZ, and .5 for height.
5.
Click on OK.
6.
Click on Close in the Real Constants dialog box.
7.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
8.
In the Material Models Available window, double-click on the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
9.
Enter 30e6 for EX (Young's modulus), and click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
10. Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
7.6.3.4. Define Nodes and Elements 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Nodes> In Active CS. The Create Nodes in Active Coordinate System dialog box appears.
2.
Enter 1 for node number.
3.
Click on Apply. Node location defaults to 0,0,0.
4.
Enter 11 for node number.
5.
Enter 0,100,0 for the X, Y, Z coordinates.
6.
Click on OK. The two nodes appear in the ANSYS Graphics window. Note — The triad, by default, hides the node number for node 1. To turn the triad off, choose menu path Utility Menu> PlotCtrls> Window Controls> Window Options and select the "Not Shown" option for Location of triad. Then click OK to close the dialog box.
7.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Nodes> Fill between Nds. The Fill between Nds picking menu appears.
8.
Click on node 1, then 11, and click on OK. The Create Nodes Between 2 Nodes dialog box appears.
9.
Click on OK to accept the settings (fill between nodes 1 and 11, and number of nodes to fill 9).
10. Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Thru Nodes. The Elements from Nodes picking menu appears. 11. Click on nodes 1 and 2, then click on OK. 12. Choose menu path Main Menu> Preprocessor> Modeling> Copy> Elements> Auto Numbered. The Copy Elems Auto-Num picking menu appears. 13. Click on Pick All. The Copy Elements (Automatically-Numbered) dialog box appears. 14. Enter 10 for total number of copies and enter 1 for node number increment. 15. Click on OK. The remaining elements appear in the ANSYS Graphics window. 7–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 7.6: Sample Buckling Analysis (GUI Method)
7.6.3.5. Define the Boundary Conditions 1.
Choose menu path Main Menu> Solution> Unabridged Menu> Analysis Type> New Analysis. The New Analysis dialog box appears.
2.
Click OK to accept the default of "Static."
3.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Static or SteadyState Analysis dialog box appears.
4.
In the scroll box for stress stiffness or prestress, scroll to "Prestress ON" to select it.
5.
Click on OK.
6.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears.
7.
Click on node 1 in the ANSYS Graphics window, then click on OK in the picking menu. The Apply U,ROT on Nodes dialog box appears.
8.
Click on "All DOF" to select it, and click on OK.
9.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment> On Nodes. The Apply F/M on Nodes picking menu appears.
10. Click on node 11, then click OK. The Apply F/M on Nodes dialog box appears. 11. In the scroll box for Direction of force/mom, scroll to "FY" to select it. 12. Enter -1 for the force/moment value, and click on OK. The force symbol appears in the ANSYS Graphics window.
7.6.3.6. Solve the Static Analysis 1.
Choose menu path Main Menu> Solution> Solve> Current LS.
2.
Carefully review the information in the status window, and click on Close.
3.
Click on OK in the Solve Current Load Step dialog box to begin the solution.
4.
Click on Close in the Information window when the solution is finished.
7.6.3.7. Solve the Buckling Analysis 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis. Note — Click on Close in the Warning window if the following warning appears: Changing the analysis type is only valid within the first load step. Pressing OK will cause you to exit and reenter SOLUTION. This will reset the load step count to 1.
2.
In the New Analysis dialog box, click the "Eigen Buckling" option on, then click on OK.
3.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Eigenvalue Buckling Options dialog box appears.
4.
Click on the "Block Lanczos" option, and enter 1 for number of modes to extract.
5.
Click on OK.
6.
Choose menu path Main Menu> Solution> Load Step Opts> ExpansionPass> Expand Modes.
7.
Enter 1 for number of modes to expand, and click on OK.
8.
Choose menu path Main Menu> Solution> Solve> Current LS. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
7–11
Chapter 7: Buckling Analysis 9.
Carefully review the information in the status window, and click on Close.
10. Click on OK in the Solve Current Load Step dialog box to begin the solution. 11. Click on Close in the Information window when the solution is finished.
7.6.3.8. Review the Results 1.
Choose menu path Main Menu> General Postproc> Read Results> First Set.
2.
Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears.
3.
Click the "Def + undeformed" option on. Click on OK. The deformed and undeformed shapes appear in the ANSYS graphics window.
7.6.3.9. Exit ANSYS 1.
In the ANSYS Toolbar, click on Quit.
2.
Choose the save option you want and click on OK.
7.7. Sample Buckling Analysis (Command or Batch Method) You can perform the example buckling analysis of a bar with hinged ends using the ANSYS commands shown below instead of GUI choices. Items prefaced by an exclamation point (!) are comments. /PREP7 /TITLE, BUCKLING OF A BAR WITH HINGED SOLVES ET,1,BEAM3 ! Beam element R,1,.25,52083E-7,.5 ! Area,IZZ, height MP,EX,1,30E6 ! Define material properties N,1 N,11,,100 FILL E,1,2 EGEN,10,1,1 FINISH /SOLU ANTYPE,STATIC PSTRES,ON D,1,ALL F,11,FY,-1 SOLVE FINISH /SOLU ANTYPE,BUCKLE BUCOPT,LANB,1 MXPAND,1 SOLVE FINISH /POST1 SET,FIRST PLDISP,1 FINISH
! ! ! !
Static analysis Calculate prestress effects Fix symmetry ends Unit load at free end
! Buckling analysis ! Use Block Lanczos solution method, extract 1 mode ! Expand 1 mode shape
7.8. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional buckling analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS program. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification 7–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 7.8: Where to Find Other Examples Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual contains a variety of buckling analysis test cases: VM17 - Snap-Through Buckling of a Hinged Shell VM127 - Buckling of a Bar with Hinged Ends (Line Elements) VM128 - Buckling of a Bar with Hinged Ends (Area Elements)
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
7–13
7–14
Chapter 8: Nonlinear Structural Analysis 8.1. What is Structural Nonlinearity? You encounter structural nonlinearities on a routine basis. For instance, whenever you staple two pieces of paper together, the metal staples are permanently bent into a different shape. (See Figure 8.1: “Common Examples of Nonlinear Structural Behavior” (a).) If you heavily load a wooden shelf, it will sag more and more as time passes. (See Figure (b).) As weight is added to a car or truck, the contact surfaces between its pneumatic tires and the underlying pavement change in response to the added load. (See Figure (c).) If you were to plot the load-deflection curve for each of these examples, you would discover that they all exhibit the fundamental characteristic of nonlinear structural behavior - a changing structural stiffness.
Figure 8.1 Common Examples of Nonlinear Structural Behavior
8.1.1. Causes of Nonlinear Behavior Nonlinear structural behavior arises from a number of causes, which can be grouped into these principal categories: •
Changing status
•
Geometric nonlinearities
•
Material nonlinearities
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 8: Nonlinear Structural Analysis
8.1.1.1. Changing Status (Including Contact) Many common structural features exhibit nonlinear behavior that is status-dependent. For example, a tensiononly cable is either slack or taut; a roller support is either in contact or not in contact. Status changes might be directly related to load (as in the case of the cable), or they might be determined by some external cause. Situations in which contact occurs are common to many different nonlinear applications. Contact forms a distinctive and important subset to the category of changing-status nonlinearities. See Chapter 11, “Contact” for detailed information on performing contact analyses using ANSYS.
8.1.1.2. Geometric Nonlinearities If a structure experiences large deformations, its changing geometric configuration can cause the structure to respond nonlinearly. An example would be the fishing rod shown in Figure 8.2: “A Fishing Rod Demonstrates Geometric Nonlinearity”. Geometric nonlinearity is characterized by "large" displacements and/or rotations.
Figure 8.2 A Fishing Rod Demonstrates Geometric Nonlinearity
8.1.1.3. Material Nonlinearities Nonlinear stress-strain relationships are a common cause of nonlinear structural behavior. Many factors can influence a material's stress-strain properties, including load history (as in elastoplastic response), environmental conditions (such as temperature), and the amount of time that a load is applied (as in creep response).
8.1.2. Basic Information About Nonlinear Analyses ANSYS employs the "Newton-Raphson" approach to solve nonlinear problems. In this approach, the load is subdivided into a series of load increments. The load increments can be applied over several load steps. Figure 8.3: “Newton-Raphson Approach” illustrates the use of Newton-Raphson equilibrium iterations in a single DOF nonlinear analysis.
8–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.1: What is Structural Nonlinearity?
Figure 8.3 Newton-Raphson Approach
Before each solution, the Newton-Raphson method evaluates the out-of-balance load vector, which is the difference between the restoring forces (the loads corresponding to the element stresses) and the applied loads. The program then performs a linear solution, using the out-of-balance loads, and checks for convergence. If convergence criteria are not satisfied, the out-of-balance load vector is reevaluated, the stiffness matrix is updated, and a new solution is obtained. This iterative procedure continues until the problem converges. A number of convergence-enhancement and recovery features, such as line search, automatic load stepping, and bisection, can be activated to help the problem to converge. If convergence cannot be achieved, then the program attempts to solve with a smaller load increment. In some nonlinear static analyses, if you use the Newton-Raphson method alone, the tangent stiffness matrix may become singular (or non-unique), causing severe convergence difficulties. Such occurrences include nonlinear buckling analyses in which the structure either collapses completely or "snaps through" to another stable configuration. For such situations, you can activate an alternative iteration scheme, the arc-length method, to help avoid bifurcation points and track unloading. The arc-length method causes the Newton-Raphson equilibrium iterations to converge along an arc, thereby often preventing divergence, even when the slope of the load vs. deflection curve becomes zero or negative. This iteration method is represented schematically in Figure 8.4: “Traditional Newton-Raphson Method vs. ArcLength Method”.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–3
Chapter 8: Nonlinear Structural Analysis
Figure 8.4 Traditional Newton-Raphson Method vs. Arc-Length Method
To summarize, a nonlinear analysis is organized into three levels of operation: •
The "top" level consists of the load steps that you define explicitly over a "time" span (see the discussion of "time" in Chapter 2, “Loading” in the ANSYS Basic Analysis Guide). Loads are assumed to vary linearly within load steps (for static analyses).
•
Within each load step, you can direct the program to perform several solutions (substeps or time steps) to apply the load gradually.
•
At each substep, the program will perform a number of equilibrium iterations to obtain a converged solution.
Figure 8.5: “Load Steps, Substeps, and Time” illustrates a typical load history for a nonlinear analysis. Also see the discussion of load steps, substeps, and equilibrium iterations in Chapter 2, “Loading” in the ANSYS Basic Analysis Guide.
Figure 8.5 Load Steps, Substeps, and Time
8–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.1: What is Structural Nonlinearity? The ANSYS program gives you a number of choices when you designate convergence criteria: you can base convergence checking on forces, moments, displacements, or rotations, or on any combination of these items. Additionally, each item can have a different convergence tolerance value. For multiple-degree-of-freedom problems, you also have a choice of convergence norms. You should almost always employ a force-based (and, when applicable, moment-based) convergence tolerance. Displacement-based (and, when applicable, rotation-based) convergence checking can be added, if desired, but should usually not be used alone.
8.1.2.1. Conservative versus Nonconservative Behavior; Path Dependency If all energy put into a system by external loads is recovered when the loads are removed, the system is said to be conservative. If energy is dissipated by the system (such as by plastic deformation or sliding friction), the system is said to be nonconservative. An example of a nonconservative system is shown in Figure 8.6: “Nonconservative (Path-Dependent) Behavior”. An analysis of a conservative system is path independent: loads can usually be applied in any order and in any number of increments without affecting the end results. Conversely, an analysis of a nonconservative system is path dependent: the actual load-response history of the system must be followed closely to obtain accurate results. An analysis can also be path dependent if more than one solution could be valid for a given load level (as in a snap-through analysis). Path dependent problems usually require that loads be applied slowly (that is, using many substeps) to the final load value.
Figure 8.6 Nonconservative (Path-Dependent) Behavior
8.1.2.2. Substeps When using multiple substeps, you need to achieve a balance between accuracy and economy: more substeps (that is, small time step sizes) usually result in better accuracy, but at a cost of increased run times. ANSYS provides automatic time stepping that is designed for this purpose. Automatic time stepping adjusts the time step size as needed, gaining a better balance between accuracy and economy. Automatic time stepping activates the ANSYS program's bisection feature. Bisection provides a means of automatically recovering from a convergence failure. This feature will cut a time step size in half whenever equilibrium iterations fail to converge and automatically restart from the last converged
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–5
Chapter 8: Nonlinear Structural Analysis substep. If the halved time step again fails to converge, bisection will again cut the time step size and restart, continuing the process until convergence is achieved or until the minimum time step size (specified by you) is reached.
8.1.2.3. Load Direction in a Large-Deflection Analysis Consider what happens to loads when your structure experiences large deflections. In many instances, the loads applied to your system maintain constant direction no matter how the structure deflects. In other cases, forces will change direction, "following" the elements as they undergo large rotations. The ANSYS program can model both situations, depending on the type of load applied. Accelerations and concentrated forces maintain their original orientation, regardless of the element orientation. Pressure loads always act normal to the deflected element surface, and can be used to model "following" forces. Figure 8.7: “Load Directions Before and After Deflection” illustrates constant-direction and following forces. Note — Nodal coordinate system orientations are not updated in a large deflection analysis. Calculated displacements are therefore output in the original directions.
Figure 8.7 Load Directions Before and After Deflection
8.1.2.4. Nonlinear Transient Analyses The procedure for analyzing nonlinear transient behavior is similar to that used for nonlinear static behavior: you apply the load in incremental steps, and the program performs equilibrium iterations at each step. The main difference between the static and transient procedures is that time-integration effects can be activated in the transient analysis. Thus, "time" always represents actual chronology in a transient analysis. The automatic time stepping and bisection feature is also applicable for transient analyses.
8.2. Using Geometric Nonlinearities Small deflection and small strain analyses assume that displacements are small enough that the resulting stiffness changes are insignificant.
8–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.2: Using Geometric Nonlinearities In contrast, large strain analyses account for the stiffness changes that result from changes in an element's shape and orientation. By issuing NLGEOM,ON (GUI path Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) or Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options), you activate large strain effects in those element types that support this feature. The large strain feature is available in most of the solid elements (including all of the large strain and hyperelastic elements), as well as in most of the shell and beam elements. Large strain effects are not available in the ANSYS Professional program. The large strain procedure places no theoretical limit on the total rotation or strain experienced by an element. (Certain ANSYS element types will be subject to practical limitations on total strain - see below.) However, the procedure requires that strain increments must be restricted to maintain accuracy. Thus, the total load should be broken into smaller steps.
8.2.1. Stress-Strain In large strain solutions, all stress-strain input and results will be in terms of true stress and true (or logarithmic) strain. (In one dimension, true strain would be expressed as ε = ln ( l / l 0). For small-strain regions of response, true strain and engineering strain are essentially identical.) To convert strain from small (engineering) strain to logarithmic strain, use εln = ln (1 + εeng). To convert from engineering stress to true stress, use σtrue = σeng (1 + εeng). (This stress conversion is valid only for incompressible plasticity stress-strain data.)
8.2.1.1. Large Deflections with Small Strain This feature is available in all beam and most shell elements, as well as in a number of the nonlinear elements. Issue NLGEOM,ON (Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) or Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options) to activate large deflection effects for those elements that are designed for small strain analysis types that support this feature.
8.2.2. Stress Stiffening The out-of-plane stiffness of a structure can be significantly affected by the state of in-plane stress in that structure. This coupling between in-plane stress and transverse stiffness, known as stress stiffening, is most pronounced in thin, highly stressed structures, such as cables or membranes. A drumhead, which gains lateral stiffness as it is tightened, would be a common example of a stress-stiffened structure. Even though stress stiffening theory assumes that an element's rotations and strains are small, in some structural systems (such as in Figure 8.8: “Stress-Stiffened Beams” (a)), the stiffening stress is only obtainable by performing a large deflection analysis. In other systems (such as in Figure 8.8: “Stress-Stiffened Beams” (b)), the stiffening stress is obtainable using small deflection, or linear, theory.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–7
Chapter 8: Nonlinear Structural Analysis
Figure 8.8 Stress-Stiffened Beams
To use stress stiffening in the second category of systems, you must issue PSTRES,ON (GUI path Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options) in your first load step. Large strain and large deflection procedures include initial stress effects as a subset of their theory. For most elements, initial stiffness effects are automatically included when large deformation effects are activated [NLGEOM,ON] (GUI path Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) or Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options).
8.2.3. Spin Softening Spin softening adjusts (softens) the stiffness matrix of a rotating body for dynamic mass effects. The adjustment approximates the effects of geometry changes due to large deflection circumferential motion in a small deflection analysis. It is usually used in conjunction with prestressing [PSTRES] (GUI path Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options), which is caused by centrifugal force in the rotating body. It should not be used with the other deformation nonlinearities, large deflection, or large strain. Spin softening is activated by the KSPIN field on the OMEGA and CMOMEGA commands (GUI path Main Menu> Preprocessor> Loads> Define Loads> Apply> Structural> Inertiav Angular Velocity).
8.3. Modeling Material Nonlinearities A number of material-related factors can cause your structure's stiffness to change during the course of an analysis. Nonlinear stress-strain relationships of plastic, multilinear elastic, and hyperelastic materials will cause a structure's stiffness to change at different load levels (and, typically, at different temperatures). Creep, viscoplasticity, and viscoelasticity will give rise to nonlinearities that can be time-, rate-, temperature-, and stress-related. Swelling will induce strains that can be a function of temperature, time, neutron flux level (or some analogous quantity), and stress. Any of these kinds of material properties can be incorporated into an ANSYS analysis if you use appropriate element types.
8.3.1. Nonlinear Materials If a material displays nonlinear or rate-dependent stress-strain behavior, then you must use the TB family of commands [TB, TBTEMP, TBDATA, TBPT, TBCOPY, TBLIST, TBPLOT, TBDELE] (GUI path Main Menu> Preprocessor> Material Props> Material Models> Structural> Nonlinear) to define the nonlinear material property relationships in terms of a data table. The exact form of these commands varies depending on the type of non8–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities linear material behavior being defined. The different material behavior options are described briefly below. See Data Tables - Implicit Analysis in the ANSYS Elements Reference for specific details for each material behavior type.
8.3.1.1. Plasticity Most common engineering materials exhibit a linear stress-strain relationship up to a stress level known as the proportional limit. Beyond this limit, the stress-strain relationship will become nonlinear, but will not necessarily become inelastic. Plastic behavior, characterized by nonrecoverable strain, begins when stresses exceed the material's yield point. Because there is usually little difference between the yield point and the proportional limit, the ANSYS program assumes that these two points are coincident in plasticity analyses (see Figure 8.9: “Elastoplastic Stress-Strain Curve”). Plasticity is a nonconservative, path-dependent phenomenon. In other words, the sequence in which loads are applied and in which plastic responses occur affects the final solution results. If you anticipate plastic response in your analysis, you should apply loads as a series of small incremental load steps or time steps, so that your model will follow the load-response path as closely as possible. The maximum plastic strain is printed with the substep summary information in your output (Jobname.OUT).
Figure 8.9 Elastoplastic Stress-Strain Curve
The automatic time stepping feature [AUTOTS] (GUI path Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) or Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc>Time and Substps) will respond to plasticity after the fact, by reducing the load step size after a load step in which a large number of equilibrium iterations was performed or in which a plastic strain increment greater than 15% was encountered. If too large a step was taken, the program will bisect and resolve using a smaller step size. Other kinds of nonlinear behavior might also occur along with plasticity. In particular, large deflection and large strain geometric nonlinearities will often be associated with plastic material response. If you expect large deformations in your structure, you must activate these effects in your analysis with the NLGEOM command (GUI path Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) or Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options). For large strain analyses, material stress-strain properties must be input in terms of true stress and logarithmic strain.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–9
Chapter 8: Nonlinear Structural Analysis
8.3.1.1.1. Plastic Material Options Several options are available for describing plasticity behavior. You may incorporate other options into the program by using User Programmable Features (see the Guide to ANSYS User Programmable Features). The Bilinear Kinematic Hardening (BKIN) option assumes the total stress range is equal to twice the yield stress, so that the Bauschinger effect is included (see Figure 8.11: “Bauschinger Effect”). This option is recommended for general small-strain use for materials that obey von Mises yield criteria (which includes most metals). It is not recommended for large-strain applications. You can combine the BKIN option with creep and Hill anisotropy options to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. Stress-strain-temperature data are demonstrated in the following example. Figure 8.10: “Kinematic Hardening”(a) illustrates a typical display [TBPLOT] of bilinear kinematic hardening properties. MPTEMP,1,0,500 MP,EX,1,12E6,-8E3 TB,BKIN,1,2 TBTEMP,0.0 TBDATA,1,44E3,1.2E6 TBTEMP,500 TBDATA,1,29.33E3,0.8E6 TBLIST,BKIN,1 /XRANGE,0,0.01 TBPLOT,BKIN,1
! ! ! ! ! ! ! ! ! !
Define temperatures for Young's modulus C0 and C1 terms for Young's modulus Activate a data table Temperature = 0.0 Yield = 44,000; Tangent modulus = 1.2E6 Temperature = 500 Yield = 29,330; Tangent modulus = 0.8E6 List the data table X-axis of TBPLOT to extend from varepsilon=0 to 0.01 Display the data table
See the MPTEMP, MP, TB, TBTEMP, TBDATA, TBLIST, /XRANGE, and TBPLOT command descriptions for more information.
Figure 8.10 Kinematic Hardening
(a) Bilinear kinematic hardening, (b) Multilinear kinematic hardening
8–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
Figure 8.11 Bauschinger Effect
The Multilinear Kinematic Hardening (KINH and MKIN) options use the Besseling model, also called the sublayer or overlay model, so that the Bauschinger effect is included. KINH is preferred for use over MKIN because it uses Rice's model where the total plastic strains remain constant by scaling the sublayers. KINH allows you to define more stress-strain curves (40 vs. 5), and more points per curve (20 vs. 5). Also, when KINH is used with LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189, you can use TBOPT = 4 (or PLASTIC) to define the stress vs. plastic strain curve. For either option, if you define more than one stressstrain curve for temperature dependent properties, then each curve should contain the same number of points. The assumption is that the corresponding points on the different stress-strain curves represent the temperature dependent yield behavior of a particular sublayer. These options are not recommended for large-strain analyses. You can combine either of these options with the Hill anisotropy option to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. Figure 8.10: “Kinematic Hardening”(b) illustrates typical stress-strain curves for the MKIN option. A typical stress-strain temperature data input using KINH is demonstrated by this example. TB,KINH,1,2,3 TBTEMP,20.0 TBPT,,0.001,1.0 TBPT,,0.1012,1.2 TBPT,,0.2013,1.3 TBTEMP,40.0 TBPT,,0.008,0.9 TBPT,,0.09088,1.0 TBPT,,0.12926,1.05
! ! ! ! ! ! ! ! !
Activate a data table Temperature = 20.0 Strain = 0.001, Stress = 1.0 Strain = 0.1012, Stress = 1.2 Strain = 0.2013, Stress = 1.3 Temperature = 40.0 Strain = 0.008, Stress = 0.9 Strain = 0.09088, Stress = 1.0 Strain = 0.12926, Stress = 1.05
In this example, the third point in the two stress-strain curves defines the temperature-dependent yield behavior of the third sublayer. A typical stress- plastic strain temperature data input using KINH is demonstrated by this example. TB,KINH,1,2,3,PLASTIC TBTEMP,20.0 TBPT,,0.000,1.0 TBPT,,0.1012,1.2 TBPT,,0.2013,1.3 TBTEMP,40.0 TBPT,,0.008,0.9 TBPT,,0.09088,1.0 TBPT,,0.12926,1.05
! Activate a data table ! Temperature = 20.0 ! Plastic Strain = 0.0000, ! Plastic Strain = 0.1000, ! Plastic Strain = 0.2000, ! Temperature = 40.0 ! Plastic Strain = 0.0000, ! Plastic Strain = 0.0900, ! Plastic Strain = 0.1290,
Stress = 1.0 Stress = 1.2 Stress = 1.3 Stress = 0.9 Stress = 1.0 Stress = 1.05
In this example, the stress - strain behavior is the same as the previous sample, except now the strain value is the plastic strain. The plastic strain can be converted from total strain as follows:
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–11
Chapter 8: Nonlinear Structural Analysis Plastic Stain = (total strain - stress)/Young's Modulus. A typical stress-strain temperature data input using MKIN is demonstrated by this example. MPTEMP,1,0,500 ! Define temperature-dependent EX, MP,EX,1,12E6,-8E3 ! as in BKIN example TB,MKIN,1,2 ! Activate a data table TBTEMP,,STRAIN ! Next TBDATA values are strains TBDATA,1,3.67E-3,5E-3,7E-3,10E-3,15E-3 ! Strains for all temps TBTEMP,0.0 ! Temperature = 0.0 TBDATA,1,44E3,50E3,55E3,60E3,65E3 ! Stresses at temperature = 0.0 TBTEMP,500 ! Temperature = 500 TBDATA,1,29.33E3,37E3,40.3E3,43.7E3,47E3 ! Stresses at temperature = 500 /XRANGE,0,0.02 TBPLOT,MKIN,1
Please see the MPTEMP, MP, TB, TBPT, TBTEMP, TBDATA, /XRANGE, and TBPLOT command descriptions for more information. The Nonlinear Kinematic Hardening (CHABOCHE) option uses the Chaboche model, which is a multi-component nonlinear kinematic hardening model that allows you to superpose several kinematic models. See the ANSYS, Inc. Theory Reference for details. Like the BKIN and MKIN options, you can use the CHABOCHE option to simulate monotonic hardening and the Bauschinger effect. This option also allows you to simulate the ratcheting and shakedown effect of materials. By combining the CHABOCHE option with isotropic hardening model options BISO, MISO, and NLISO, you have the further capability of simulating cyclic hardening or softening. You can also combine this option with the Hill anisotropy option to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. The model has 1 + 2 x n constants, where n is the number of kinematic models, and is defined by NPTS in the TB command. See the ANSYS, Inc. Theory Reference for details. You define the material constants using the TBTEMP and TBDATA commands. This model is suitable for large strain analysis. The following example is a typical data table with no temperature dependency and one kinematic model: TB,CHABOCHE,1 TBDATA,1,C1,C2,C3
! Activate CHABOCHE data table ! Values for constants C1, C2, and C3
The following example illustrates a data table of temperature dependent constants with two kinematic models at two temperature points: TB,CHABOCHE,1,2,2 TBTEMP,100 TBDATA,1,C11,C12,C13,C14,C15 TBTEMP,200 TBDATA,1,C21,C22,C23,C24,C25
! ! ! ! ! ! !
Activate CHABOCHE data table Define first temperature Values for constants C11, C12, C13, C14, and C15 at first temperature Define second temperature Values for constants C21, C22, C23, C24, and C25 at second temperature
Please see the TB, TBTEMP, and TBDATA command descriptions for more information. The Bilinear Isotropic Hardening (BISO) option uses the von Mises yield criteria coupled with an isotropic work hardening assumption. This option is often preferred for large strain analyses. You can combine BISO with Chaboche, creep, viscoplastic, and Hill anisotropy options to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. The Multilinear Isotropic Hardening (MISO) option is like the bilinear isotropic hardening option, except that a multilinear curve is used instead of a bilinear curve. This option is not recommended for cyclic or highly nonproportional load histories in small-strain analyses. It is, however, recommended for large strain analyses. The MISO option can contain up to 20 different temperature curves, with up to 100 different stress-strain points allowed 8–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities per curve. Strain points can differ from curve to curve. You can combine this option with nonlinear kinematic hardening (CHABOCHE) for simulating cyclic hardening or softening. You can also combine the MISO option with creep, viscoplastic, and Hill anisotropy options to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. The stress-straintemperature curves from the MKIN example would be input for a multilinear isotropic hardening material as follows: /prep7 MPTEMP,1,0,500 ! Define temperature-dependent EX, MPDATA,EX,1,,14.665E6,12.423e6 MPDATA,PRXY,1,,0.3 TB,MISO,1,2,5 TBTEMP,0.0 TBPT,DEFI,2E-3,29.33E3 TBPT,DEFI,5E-3,50E3 TBPT,DEFI,7E-3,55E3 TBPT,DEFI,10E-3,60E3 TBPT,DEFI,15E-3,65E3 TBTEMP,500 TBPT,DEFI,2.2E-3,27.33E3 TBPT,DEFI,5E-3,37E3 TBPT,DEFI,7E-3,40.3E3 TBPT,DEFI,10E-3,43.7E3 TBPT,DEFI,15E-3,47E3 /XRANGE,0,0.02 TBPLOT,MISO,1
! Activate a data table ! Temperature = 0.0 ! Strain, stress at temperature = 0
! Temperature = 500 ! Strain, stress at temperature = 500
See the MPTEMP, MP, TB, TBTEMP, TBPT, /XRANGE, and TBPLOT command descriptions for more information. The Nonlinear Isotropic Hardening (NLISO) option is based on the Voce hardening law (see the ANSYS, Inc. Theory Reference for details). The NLISO option is a variation of BISO where an exponential saturation hardening term is appended to the linear term (see Figure 8.12: “NLISO Stress-Strain Curve”).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–13
Chapter 8: Nonlinear Structural Analysis
Figure 8.12 NLISO Stress-Strain Curve
The advantage of this model is that the material behavior is defined as a specified function which has four material constants that you define through the TBDATA command. You can obtain the material constants by fitting material tension stress-strain curves. Unlike MISO, there is no need to be concerned about how to appropriately define the pairs of the material stress-strain points. However, this model is only applicable to the tensile curve like the one shown in Figure 8.12: “NLISO Stress-Strain Curve”. This option is suitable for large strain analyses. You can combine NLISO with Chaboche, creep, viscoplastic, and Hill anisotropy options to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. The following example illustrates a data table of temperature dependent constants at two temperature points: TB,NLISO,1 TBTEMP,100 TBDATA,1,C11,C12,C13,C14 TBTEMP,200 TBDATA,1,C21,C22,C23,C24
! ! ! ! ! ! !
Activate NLISO data table Define first temperature Values for constants C11, C12, C13, C14 at first temperature Define second temperature Values for constants C21, C22, C23, C24 at second temperature
Please see the TB, TBTEMP, and TBDATA command descriptions for more information. The Anisotropic (ANISO) option allows for different bilinear stress-strain behavior in the material x, y, and z directions as well as different behavior in tension, compression, and shear. This option is applicable to metals that have undergone some previous deformation (such as rolling). It is not recommended for cyclic or highly nonproportional load histories since work hardening is assumed. The yield stresses and slopes are not totally independent (see the ANSYS, Inc. Theory Reference for details).
8–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities To define anisotropic material plasticity, use MP commands (Main Menu> Solution> Load Step Opts> Other> Change Mat Props) to define the elastic moduli (EX, EY, EZ, NUXY, NUYZ, and NUXZ). Then, issue the TB command [TB,ANISO] followed by TBDATA commands to define the yield points and tangent moduli. (See Nonlinear StressStrain Materials in the ANSYS Elements Reference for more information.) The Hill Anisotropy (HILL) option, when combined with other material options simulates plasticity, viscoplasticity, and creep - all using the Hill potential. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. The Hill potential may only be used with the following elements: PLANE42, SOLID45, PLANE82, SOLID92, SOLID95, LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189. The Drucker-Prager (DP) option is applicable to granular (frictional) material such as soils, rock, and concrete, and uses the outer cone approximation to the Mohr-Coulomb law. MP,EX,1,5000 MP,NUXY,1,0.27 TB,DP,1 TBDATA,1,2.9,32,0
! Cohesion = 2.9 (use consistent units), ! Angle of internal friction = 32 degrees, ! Dilatancy angle = 0 degrees
See the MP, TB, and TBDATA command descriptions for more information. The Cast Iron (CAST, UNIAXIAL) option assumes a modified von Mises yield surface, which consists of the von Mises cylinder in compression and a Rankine cube in tension. It has different yield strengths, flows, and hardenings in tension and compression. Elastic behavior is isotropic, and is the same in tension and compression. The TB,CAST command is used to input the plastic Poisson's ration in tension, which can be temperature dependent. Use the TB,UNIAXIAL command to enter the yield and hardening in tension and compression. Note — Cast Iron is intended for monotonic loading only and cannot be used with any other material model. TB,CAST,1,,,ISOTROPIC TBDATA,1,0.04 TB,UNIAXIAL,1,1,5,TENSION TBTEMP,10 TBPT,,0.550E-03,0.813E+04 TBPT,,0.100E-02,0.131E+05 TBPT,,0.250E-02,0.241E+05 TBPT,,0.350E-02,0.288E+05 TBPT,,0.450E-02,0.322E+05 TB,UNIAXIAL,1,1,5,COMPRESSION TBTEMP,10 TBPT,,0.203E-02,0.300E+05 TBPT,,0.500E-02,0.500E+05 TBPT,,0.800E-02,0.581E+05 TBPT,,0.110E-01,0.656E+05 TBPT,,0.140E-01,0.700E+05
Figure 8.13: “Cast Iron Plasticity” illustrates the idealized response of gray cast iron in tension and compression.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–15
Chapter 8: Nonlinear Structural Analysis
Figure 8.13 Cast Iron Plasticity Compression
σc
σt
Tension ε
See the TB and TBPT command descriptions for more information.
8.3.1.2. Multilinear Elasticity The Multilinear Elastic (MELAS) material behavior option describes a conservative (path-independent) response in which unloading follows the same stress-strain path as loading. Thus, relatively large load steps might be appropriate for models that incorporate this type of material nonlinearity. Input format is similar to that required for the multilinear isotropic hardening option, except that the TB command now uses the label MELAS.
8.3.1.3. User Defined Material The User Defined (USER) material option describes input parameters for defining a material model based on either of two subroutines, which are ANSYS user-programmable features (see the Guide to ANSYS User Programmable Features). The choice of which subroutine to use is based on which element you are using. The USER option works with the USERMAT subroutine in defining any material model (except incompressible materials), when you use any of the following elements: LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189. The USER option works with the USERPL subroutine in defining plasticity or viscoplasticity material models, when you use any of the following elements: LINK1, PLANE2, LINK8, PIPE20, BEAM23, BEAM24, PLANE42, SHELL43, SOLID45, SHELL51, PIPE60, SOLID62, SOLID65, PLANE82, SHELL91, SOLID92, SHELL93, SOLID95. To access the user material option, issue the TB,USER command to define the material number, the number of temperatures, and the number of data points. Then define the temperatures and material constants using the TBTEMP and TBDATA commands. The following example illustrates defining a material with two temperatures and four data points: TB,USER,1,2,4
TBTEMP,1.0 TBDATA,1,19e5,0.3,1e3,100, TBTEMP,2.0
8–16
! ! ! ! ! ! ! ! !
Define material 1 as user material with 2 temperatures and 4 data points at each temperature point. First temperature. 4 material constants for first temperature. Second temperature.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities TBDATA,1,21e5,0.3,2e3,100,
! 4 material constants for ! second temperature.
If you use state variables in the USERMAT subroutine, you must first define the number of state variables using the TB,STATE command. You then use the TBDATA command to initialize the value of the state variables, as shown in the following example: TB,STATE,1,,4, TBDATA,1,C1,C2,C3,C4,
! Define material 1, which ! has 4 state variables. ! Initialize the 4 state variables.
You cannot use TB,STATE in the USERPL subroutine. See the TB, and TBDATA command descriptions for more information.
8.3.1.4. Hyperelasticity A material is said to be hyperelastic if there exists an elastic potential function (or strain energy density function), which is a scalar function of one of the strain or deformation tensors, whose derivative with respect to a strain component determines the corresponding stress component. Hyperelasticity can be used to analyze rubber-like materials (elastomers) that undergo large strains and displacements with small volume changes (nearly incompressible materials). Large strain theory is required [NLGEOM,ON]. A representative hyperelastic structure (a balloon seal) is shown in Figure 8.14: “Hyperelastic Structure”.
Figure 8.14 Hyperelastic Structure
There are two types of elements suitable for simulating hyperelastic materials: the hyperelastic elements (HYPER56, HYPER58, HYPER74, HYPER158), and all of the 18x family of elements except the link and beam elements (SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, and SOLID187). For further details on the use of hyperelastic elements, and on mixed formulation of the 18x solid elements, see Mixed u-P Formulation Elements in the ANSYS Elements Reference. The material response in ANSYS hyperelastic models is always assumed to be isotropic and isothermal. Because of this assumption, the strain energy potentials are expressed in terms of strain invariants. Unless indicated otherwise, the hyperelastic materials are also assumed to be nearly or purely incompressible. Material thermal expansion is also assumed to be isotropic.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–17
Chapter 8: Nonlinear Structural Analysis ANSYS supports several options of strain energy potentials for the simulation of incompressible or nearly incompressible hyperelastic materials. All options are applicable to elements SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, and SOLID187. Access these options through the TBOPT argument of TB,HYPER. One of the options, the Mooney-Rivlin option, is also applicable to elements HYPER56, HYPER58, HYPER74, HYPER158, and explicit dynamics elements PLANE162, SHELL163, SOLID164, and SOLID168. To access the MooneyRivlin option for these elements, use TB,MOONEY. ANSYS provides tools to help you determine the coefficients for all of the hyperelastic options defined by TB,HYPER. The TBFT command allows you to compare your experimental data with existing material data curves and visually “fit” your curve for use in the TB command. All of the TBFT command capability is available via either batch or interactive (GUI) mode. See Material Curve Fitting (also in this manual) for more information. Each of the hyperelastic options is presented in the following sections.
8.3.1.4.1. Mooney-Rivlin Hyperelastic Option (TB,HYPER) Note that this section applies to using the Mooney-Rivlin option with elements SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, and SOLID187. If you want to use the Mooney-Rivlin option with elements HYPER56, HYPER58, HYPER74, HYPER158, PLANE162, SHELL163, SOLID164, or SOLID168, see Section 8.3.1.4.11: Mooney-Rivlin Hyperelastic Option (TB,MOONEY). The Mooney-Rivlin option (TB,HYPER,,,,MOONEY), which is the default, allows you to define 2, 3, 5, or 9 parameters through the NPTS argument of the TB command. For example, to define a 5 parameter model you would issue TB,HYPER,1,,5,MOONEY. The 2 parameter Mooney-Rivlin option has an applicable strain of about 100% in tension and 30% in compression. Compared to the other options, higher orders of the Mooney-Rivlin option may provide better approximation to a solution at higher strain. The following example input listing shows a typical use of the Mooney-Rivlin option with 3 parameters: TB,HYPER,1,,3,MOONEY TBDATA,1,0.163498 TBDATA,2,0.125076 TBDATA,3,0.014719 TBDATA,4,6.93063E-5
!Activate 3 parameter Mooney-Rivlin data table !Define c10 !Define c01 !Define c11 !Define incompressibility parameter !(as 2/K, K is the bulk modulus)
Refer to Mooney-Rivlin Hyperelastic Material (TB,HYPER) in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.2. Ogden Hyperelastic Option The Ogden option (TB,HYPER,,,,OGDEN) allows you to define an unlimited number of parameters through the NPTS argument of the TB command. For example, to define a 3 parameter model, use TB,HYPER,1,,3,OGDEN. Compared to the other options, the Ogden option usually provides the best approximation to a solution at larger strain levels. The applicable strain level can be up to 700%. A higher parameter value can provide a better fit to the exact solution. It may however cause numerical difficulties in fitting the material constants, and it requires enough data to cover the whole range of deformation for which you may be interested. For these reasons, a high parameter value is not recommended. The following example input listing shows a typical use of the Ogden option with 2 parameters:
8–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities TB,HYPER,1,,2,OGDEN TBDATA,1,0.326996 TBDATA,2,2 TBDATA,3,-0.250152 TBDATA,4,-2 TBDATA,5,6.93063E-5
!Activate 2 parameter Ogden data table !Define µ1 !Define 1 !Define µ2 !Define 2 !Define incompressibility parameter !(as 2/K, K is the bulk modulus) !(Second incompressibility parameter d2 is zero)
Refer to Ogden Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.3. Neo-Hookean Hyperelastic Option The Neo-Hookean option (TB,HYPER,,,,NEO) represents the simplest form of strain energy potential, and has an applicable strain range of 20-30%. An example input listing showing a typical use of the Neo-Hookean option is presented below. TB,HYPER,1,,,NEO TBDATA,1,0.577148 TBDATA,2,7.0e-5
!Activate Neo-Hookean data table !Define mu shear modulus !Define incompressibility parameter !(as 2/K, K is the bulk modulus)
Refer to Neo-Hookean Hyperelastic Material in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.4. Polynomial Form Hyperelastic Option The polynomial form option (TB,HYPER,,,,POLY) allows you to define an unlimited number of parameters through the NPTS argument of the TB command. For example, to define a 3 parameter model you would issue TB,HYPER,1,,3,POLY. Similar to the higher order Mooney-Rivlin options, the polynomial form option may provide a better approximation to a solution at higher strain. For NPTS = 1 and constant c01 = 0, the polynomial form option is equivalent to the Neo-Hookean option (see Section 8.3.1.4.3: Neo-Hookean Hyperelastic Option for a sample input listing). Also, for NPTS = 1, it is equivalent to the 2 parameter Mooney-Rivlin option. For NPTS = 2, it is equivalent to the 5 parameter Mooney-Rivlin option, and for NPTS = 3, it is equivalent to the 9 parameter Mooney-Rivlin option (see Section 8.3.1.4.1: Mooney-Rivlin Hyperelastic Option (TB,HYPER) for a sample input listing). Refer to Polynomial Form Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.5. Arruda-Boyce Hyperelastic Option The Arruda-Boyce option (TB,HYPER,,,,BOYCE) has an applicable strain level of up to 300%. An example input listing showing a typical use of the Arruda-Boyce option is presented below. TB,HYPER,1,,,BOYCE TBDATA,1,200.0 TBDATA,2,5.0 TBDATA,3,0.001
!Activate Arruda-Boyce data table !Define initial shear modulus !Define limiting network stretch !Define incompressibility parameter !(as 2/K, K is the bulk modulus)
Refer to Arruda-Boyce Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–19
Chapter 8: Nonlinear Structural Analysis
8.3.1.4.6. Gent Hyperelastic Option The Gent option (TB,HYPER,,,,GENT) has an applicable strain level of up to 300%. An example input listing showing a typical use of the Gent option is presented below. TB,HYPER,1,,,GENT TBDATA,1,3.0 TBDATA,2,42.0 TBDATA,3,0.001
!Activate Gent data table !Define initial shear modulus !Define limiting I1 - 3 !Define incompressibility parameter !(as 2/K, K is the bulk modulus)
Refer to Gent Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.7. Yeoh Hyperelastic Option The Yeoh option (TB,HYPER,,,,YEOH) is a reduced polynomial form of the hyperelasticity option TB,HYPER,,,,POLY. An example of a 2 term Yeoh model is TB,HYPER,1,,2,YEOH. Similar to the polynomial form option, the higher order terms may provide a better approximation to a solution at higher strain. For NPTS = 1, the Yeoh form option is equivalent to the Neo-Hookean option (see Section 8.3.1.4.3: Neo-Hookean Hyperelastic Option for a sample input listing). The following example input listing shows a typical use of the Yeoh option with 2 terms and 1 incompressibility term: TB,HYPER,1,,2,YEOH TBDATA,1,0.163498 TBDATA,2,0.125076 TBDATA,3,6.93063E-5
!Activate 2 term Yeoh data table !Define C1 !Define C2 !Define first incompressibility parameter
Refer to Yeoh Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.8. Blatz-Ko Foam Hyperelastic Option The Blatz-Ko option (TB,HYPER,,,,BLATZ) is the simplest option for simulating the compressible foam type of elastomer. This option is analogous to the Neo-Hookean option of incompressible hyperelastic materials. An example input listing showing a typical use of the Blatz-Ko option is presented below. TB,HYPER,1,,,BLATZ TBDATA,1,5.0
!Activate Blatz-Ko data table !Define initial shear modulus
Refer to Blatz-Ko Foam Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.9. Ogden Compressible Foam Hyperelastic Option The Ogden compressible foam option (TB,HYPER,,,,FOAM) simulates highly compressible foam material. An example of a 3 parameter model is TB,HYPER,1,,3,FOAM. Compared to the Blatz-Ko option, the Ogden foam option usually provides the best approximation to a solution at larger strain levels. The higher the number of parameters, the better the fit to the experimental data. It may however cause numerical difficulties in fitting the material constants, and it requires sufficient data to cover the whole range of deformation for which you may be interested. For these reasons, a high parameter value is not recommended. 8–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities The following example input listing shows a typical use of the Ogden foam option with 2 parameters: TB,HYPER,1,,2,FOAM TBDATA,1,1.85 TBDATA,2,4.5 TBDATA,3,-9.20 TBDATA,4,-4.5 TBDATA,5,0.92 TBDATA,6,0.92
!Activate 2 parameter Ogden foam data table !Define µ1 !Define 1 !Define µ2 !Define 2 !Define first compressibility parameter !Define second compressibility parameter
Refer to Ogden Compressible Foam Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.10. User-Defined Hyperelastic Option The User option (TB,HYPER,,,,USER) allows you to use the subroutine USERHYPER to define the derivatives of the strain energy potential with respect to the strain invariants. Refer to the Guide to ANSYS User Programmable Features for a detailed description on writing a user hyperelasticity subroutine.
8.3.1.4.11. Mooney-Rivlin Hyperelastic Option (TB,MOONEY) Note that this section applies to using the Mooney-Rivlin option with elements HYPER56, HYPER58, HYPER74, HYPER158, PLANE162, SHELL163, SOLID164, or SOLID168. If you want to use the Mooney-Rivlin option with elements SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, and SOLID187, see Section 8.3.1.4.1: Mooney-Rivlin Hyperelastic Option (TB,HYPER). ANSYS element types HYPER56, HYPER58, HYPER74, and HYPER158 use up to a nine-term Mooney-Rivlin elastic potential function. If you already know the values for two-term, three-term, five-term, or nine-term MooneyRivlin constants, you can enter them directly with the TB family of commands. (See the ANSYS, Inc. Theory Reference for information on the Mooney-Rivlin function.) For these element types, you can also specify the material function as a User Programmable Feature (see the Guide to ANSYS User Programmable Features). An example input listing showing a typical use of the Mooney-Rivlin for these elements is presented below : MP,NUXY,1,0.49999 ! NUXY should be almost equal to, but less than 0.5 TB,MOONEY,1,1 TBDATA,1,0.163498 TBDATA,2,0.125076 TBDATA,3,-0.0047583 TBDATA,4,0.014719 TBDATA,6,0.0003882 ! (Constants 5, 7, 8, and 9 default to 0.0 in this example)
Refer to Mooney-Rivlin Hyperelastic Material Constants (TB,MOONEY) in the ANSYS Elements Reference for a description of the constants required as input for this option. The Mooney-Rivlin constants for any given hyperelastic material are not generally available in the open literature. Consequently, you can use the *MOONEY command to automatically determine a set of Mooney-Rivlin constants from a set of known experimental test data. Sometimes the manufacturer of the material will be able to supply some or all of the needed test data, but you might find that you need to obtain more data from a testing laboratory. Hyperelastic material behavior is much more complicated than typical metallic material behavior. Hyperelastic stress-strain relationships usually differ significantly for tension, compression, and shear modes of deformation. Therefore, using *MOONEY to generate a generally applicable hyperelastic material model will require test data that encompasses all possible modes of deformation: tension, compression, and shear. See the ANSYS, Inc. Theory Reference for a discussion of hyperelastic test methods and equivalent deformation modes. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–21
Chapter 8: Nonlinear Structural Analysis If an incomplete set of data is provided (for instance, if only uniaxial tension data are available), the program can still determine usable hyperelastic material properties. However, in such cases the deformations experienced in the model should be limited to be of the same nature as those experienced in the tests. In other words, the test data should represent all modes of deformation and ranges of response (strain) that will be experienced in the model. This advice is simply common sense - if you do not know how the material behaves in a certain mode of deformation or range of strain, you cannot accurately predict the behavior of a part that experiences such deformations or strains. For example, if all you have is uniaxial tension data, do not model a part that experiences significant shear deformations. If your test data extend only from 0% to 100% strain, do not model a part that experiences 150% strain. If, after reviewing your analysis, you discover that the available test data do not adequately characterize the model's response, get more test data! You can use the *MOONEY command to automatically determine a set of Mooney-Rivlin constants from experimental test data. ANSYS determines the constants and stores them in the database, and in an array parameter. Additionally, it writes an ASCII file (Jobname.TB) that records the Mooney-Rivlin constants in the form of a series of TB and TBDATA commands. Once such a file exists, you can use it in future analyses to define that same material's Mooney-Rivlin constants - you do not need to use the *MOONEY command every time to regenerate these constants. Determining and Applying Mooney-Rivlin Constants The procedure for determining and applying Mooney-Rivlin constants consists of five main steps: 1.
Dimension all arrays that will be used for data input, Mooney-Rivlin constant storage, and calculated stress-strain evaluation.
2.
Fill the input-data arrays with engineering stress and strain test data.
3.
Determine the Mooney-Rivlin constants automatically.
4.
Evaluate the quality of the automatically determined Mooney-Rivlin constants.
5.
Apply the Mooney-Rivlin constants in your analysis.
Step 1: Dimension the Arrays Command(s): *DIM GUI: Utility Menu> Parameters> Array Parameters> Define/Edit You must dimension arrays before using the *MOONEY command. In most cases, you will need to dimension at least six different arrays. (You can give these arrays any valid parameter names, but for convenience, we will use specific array names, such as STRAIN, STRESS, and so on, in our discussion. You can substitute any other valid parameter names that you like.) The arrays are STRAIN, STRESS, CONST, CALC, SORTSN, and SORTSS. STRAIN Array: An array of engineering strain data from mechanical material tests, arranged in three columns: •
Column 1: uniaxial tension and/or compression data
•
Column 2: equibiaxial tension and/or compression data
•
Column 3: shear data (planar tension and/or compression)
This array has the dimensions N x 3, where N equals the maximum number of data points in any one of the three columns. For example, if you have 20 data points from uniaxial tension/compression tests and 10 data points from shear tests, N = 20. This array must always be N x 3, even if fewer than three types of test data are available. Although it might be preferable to input the data points in order of ascending strain values, it is not necessary to do so.
8–22
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities STRESS Array: An array of engineering stress data from mechanical material tests input stress-data array, also of dimension N x 3. You must input stress data points in the same order as the corresponding strain-data input. CONST Array: A Mooney-Rivlin constant array of dimension M x 1, where M equals the desired number of Mooney-Rivlin constants. (M must be either 2, 5, or 9; any other value will produce an error message when *MOONEY is invoked.) You actually tell the program in this dimensioning operation how many Mooney-Rivlin constants you want. The *MOONEY command later reads the dimensions of this array to determine how many Mooney-Rivlin constants to generate, and then writes the values of those constants to this array. How many Mooney-Rivlin constants should you use? As a rule of thumb, you should have at least twice as many data points (N, as defined above) as the desired number of Mooney-Rivlin constants. Using more terms will usually improve the statistical quality of your curve fit (that is, it will probably be more tightly fitted through the data points), but the overall shape of the curve might be worse than that obtained with fewer terms. As a practical matter, you should probably try two-term, five-term, and nine-term functions in sequence, and examine the resulting stress-strain curves to decide which function gives you the best combination of tight fit and satisfactory curve shape.
Table 8.1 Suggested Mooney-Rivlin Constants Number of Points in the Stress-strain Curve
Suggested Mooney-Rivlin Function
No inflection points (that is, single curvature)
Two-term
One inflection point (that is, double curvature)
Five-term
Two inflection points
Nine-term
Figure 8.15 Typical Hyperelastic Stress-Strain Curves
CALC Array: An output stress-data array of dimension N x 3 (where N is as described above), in which sorted calculated stress values are stored. These stress values will be sorted into the same order as their corresponding sorted strain values (which will be sorted into ascending order). SORTSN Array: An array of dimension N x 3 in which sorted input strain data are stored. SORTSS Array: An array of dimension N x 3 in which sorted input stress data are stored. For example, if your test data contained up to 20 data points for any one test type, and if you wanted to generate a five-term set of Mooney-Rivlin constants, you might issue the following commands to dimension the necessary arrays (remember that you can substitute any valid parameter names for the ones shown here): *DIM,STRAIN,,20,3 *DIM,STRESS,,20,3 *DIM,CONST,,5,1 *DIM,CALC,,20,3 *DIM,SORTSN,,20,3 *DIM,SORTSS,,20,3
! ! ! ! ! !
Dim. Dim. Dim. Dim. Dim. Dim.
array array array array array array
(STRAIN) for 20 input strain-data points (STRESS) for input stress data (20 pts.) (CONST) for 5-term M-R constants (CALC) for sorted calculated stresses (SORTSN) for sorted input strain data (SORTSS) for sorted input stress data
See the *DIM command description for more information.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–23
Chapter 8: Nonlinear Structural Analysis Step 2: Fill the Input-Data Arrays Once you have dimensioned your arrays, you can then fill the STRAIN and STRESS arrays with test data using the *SET command (GUI path Utility Menu> Parameters> Scalar Parameters). (Again, remember that you can give these arrays any valid parameter names; particular array names are used here only for the convenience of this discussion.) Note — The *MOONEY command interprets all input stress and strain data as engineering stress and engineering strain. These arrays are of dimension N x 3, with each column of the arrays containing data from one type of test, in this order: •
First column: Uniaxial tension and/or uniaxial compression
•
Second column: Equibiaxial tension and/or equibiaxial compression
•
Third column: Shear (planar tension or compression)
Note that these do not have a 1:1 relationship with the modes of deformation and their equivalencies. The first mode of deformation, uniaxial tension, has equibiaxial compression as its equivalency, but the first column of the array contains data from uniaxial tension and/or uniaxial compression. Likewise, the second mode of deformation, equibiaxial tension, has uniaxial compression as its equivalency, but the second column of the array contains data from equibiaxial tension and/or equibiaxial compression.
Table 8.2 Data Locations in Stress and Strain Input Arrays Mode of Deformation
Equivalent Test Types
Array Location for Test Data
Uniaxial tension
Uniaxial tension Equibiaxial compression
Column one Column two
Equibiaxial tension
Equibiaxial tension Uniaxial compression
Column two Column one
Shear
Planar tension Planar compression
Column three Column three
If fewer than three types of tests are used, you must leave the missing columns blank. Schematically, data input might be represented as shown in Figure 8.16: “Data Locations in Stress and Strain Input Arrays”.
8–24
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
Figure 8.16 Data Locations in Stress and Strain Input Arrays
Consider a case in which data from uniaxial tension and shear tests are available. The commands to store the strain and stress data in the input-data arrays could look something like this (of course, the arrays can have any valid array names, and the number of data points represented by N1 and N2 in this example can be any integral numbers): ! Uniaxial Tension Data *SET,STRAIN(1,1), ... ! *SET,STRAIN(11,1),... ! *SET,STRESS(1,1), ... ! *SET,STRESS(11,1),... ! ! Shear Data *SET,STRAIN(1,3), ... ! *SET,STRESS(1,3), ... !
First 10 strain data points Strain data points 11 through N1 (if N1<21) First 10 stress data points Stress data points 11 through N1 Strain data points 1 through N2 (if N2<11) Stress data points 1 through N2
See the *SET command description for more information. Step 3: Determine the Mooney-Rivlin Constants To generate Mooney-Rivlin constants automatically, first use the TB command, with Lab = MOONEY and TBOPT = 1. Next, issue the *MOONEY command, inserting the appropriate names of arrays that you have already dimensioned (particular names have been used in this example for convenience of discussion only; you can use any valid parameter names): TB,MOONEY,MAT,NTEMP,,1 *MOONEY,STRAIN(1,1),STRESS(1,1),,CONST(1),CALC(1),SORTSN(1), SORTSS(1),Fname,Ext
The program automatically determines the Mooney-Rivlin constants, stores them in the database and in the CONST array (which can have any valid parameter name), and writes a series of TB and TBDATA commands in the ASCII file Fname.Ext (default file name = Jobname.TB). Uniaxial equations will be used for the data in column 1, equibiaxial equations for the data in column 2, and planar (pure shear) equations for the data in column 3. Note — All the laboratory test data entered in the STRAIN and STRESS arrays will be used to determine the Mooney-Rivlin hyperelastic material constants. Step 4: Evaluate the Quality of the Mooney-Rivlin Constants Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–25
Chapter 8: Nonlinear Structural Analysis In your printout (file Jobname.OUT), examine the "ROOT-MEAN-SQUARE ERROR (PERCENTAGE)" and the "COEFFICIENT OF DETERMINATION." These two values give you a statistical measure of how well your calculated stress-strain curve fits the experimental data points. The root-mean-square error, which is expressed as a percentage (that is, a value of 2.5 means 2.5 %), should be "close" to zero. The coefficient of determination will be less than 1.0, but should be "close" to 1.0 (that is, typically 0.99 or better). In addition, you should use the *EVAL and *VPLOT commands (GUI paths Main Menu> Preprocessor> Material Props> Mooney-Rivlin> Evaluate Const and Utility Menu> Plot> Array Parameters) to graph the input and calculated stress-strain curves, in order to obtain a visual check on how well the calculated curve matches the experimental data. In comparing these curves, you should compare calculated values against test data that represent the same mode of deformation. That is, you should compare the shape of the calculated uniaxial tension curve (EVPARM = 1 in the *EVAL command) against uniaxial tension data only (column 1 of the sorted STRAIN and STRESS arrays). Similarly, you should compare the calculated uniaxial compression curve against the uniaxial compression data only, and the calculated shear curve against the shear data only. When you graph your calculated stress-strain curves, you can extend the displayed curve into regions that were not defined by the experimental data. Graphing your curves over such an extended range can help you qualitatively understand your model's behavior if its response ever happens to exceed the range of experimental strain. However, realize that if you extend a displayed curve into a region that represents a different mode of deformation, then that portion of the display will be meaningless. For instance, you should graph a uniaxial tension curve only in regions of positive strain, and a uniaxial compression curve only in regions of compressive strain. Remember that good practice usually requires that the test data should represent all modes of deformation and ranges of response (strain) experienced by your model. The *MOONEY command automatically writes the Mooney-Rivlin constants to the CONST array. Because *EVAL reads these same constants from this CONST array, you can readily do a *EVAL following a *MOONEY operation in the same ANSYS session. If you already have the Mooney-Rivlin constants (and thus will not be doing a *MOONEY calculation), you must first dimension [*DIM]and fill the CONST array with the Mooney-Rivlin constants before you can evaluate the curves [*EVAL]. You can fill this array fairly easily, given that the CONST array is either 1 x 2, 1 x 5, or 1 x 9 at most. You could also add the *DIM and array-filling commands to your archived Jobname.TB file to make this operation more convenient. To check your curve's shape, you must dimension [*DIM] two more table array vectors (identified as XVAL and ECALC in the *EVAL command description; any valid parameter names may be used). Each of these table array vectors should have dimension P, where P is the number of points you want to use to plot your curve. (Typically, you will want to make P fairly large in order to generate a very smooth curve.) Next, specify the mode of deformation, define an extended range of strain, and fill the arrays with engineering strain and calculated engineering stress data, using the *EVAL command. Finally, graph [*VPLOT] the calculated stress-strain curve. The following example demonstrates how to graph a calculated curve for the uniaxial compression deformation mode: ! Dimension strain and stress arrays for the calculated curve: ! (Any valid parameter names can be used) *DIM,XVAL,TABLE,1000 *DIM,ECALC,TABLE,1000 ! Specify the mode of deformation (EVPARM), define the strain range ! (XMIN,XMAX), and use the M-R constants (CONST) to fill the strain (XVAL) ! and stress (ECALC) arrays with calculated data: *EVAL,1,2,CONST(1),XMIN,XMAX,XVAL(1),ECALC(1) ! Label the graph axes: /AXLAB,X,Engineering Strain /AXLAB,Y,Engineering Stress ! Plot the calculated uniaxial compression curve: *VPLOT,XVAL(1),ECALC(1)
See the *DIM, *EVAL, /AXLAB, and *VPLOT command descriptions for more information.
8–26
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
Figure 8.17 Typical Evaluated Hyperelastic Stress-Strain Curve
Step 5: Using the Mooney-Rivlin Constants If the curve-fit statistics and the overall curve shape are satisfactory, then you can proceed to use the generated Mooney-Rivlin material properties in your analysis. (The *MOONEY command will have stored these constants in the database.) In future analyses using the same material model, you can simply read in [/INPUT] the file Jobname.TB to load the constants into your new database. However, do not forget to define a value for Poisson's ratio [MP,NUXY,...]. Always remember to examine your analysis results carefully to determine whether or not your model's modes of deformation and values of maximum strain were properly represented by the original test data. Analyses involving hyperelastic elements are sometimes very sensitive to material property specification and load application. Some values of Mooney-Rivlin constants result in very stable stiffness matrices whereas others do not. Therefore, choose constants with caution and experiment with slightly different values. ANSYS provides internal stability checks for hyperelastic materials based on the Mooney-Rivlin constants that you enter. These checks occur at two levels: •
The first stability check occurs before the analysis. The check is for six typical stress paths (uniaxial tension and compression, equibiaxial tension and compression, and planar tension and compression), and covers a stretch ratio ranging from 0.1 to 10. If the material is not stable over the range, a message appears that states the critical values of the nominal strains where the material first becomes unstable, and lists the Mooney-Rivlin constants that you entered. If the material is stable over the range, you will not see any message or indication. The sample warning message below lists the nominal strains where Material 1 loses stability, then lists the constants that were entered for this example:
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–27
Chapter 8: Nonlinear Structural Analysis *** WARNING *** CP= 1.110 TIME= 16:59:52 Material 1 can become unstable under certain loading. The strain (nominal) limits where the material becomes unstable are: UNIAXIAL TENSION UNIAXIAL COMPRESSION EQUIBIAXIAL TENSION EQUIBIAXIAL COMPRESSION PLANAR TENSION PLANAR COMPRESSION
0.645E+00 -0.565E+00 0.516E+00 -0.220E+00 0.585E+00 -0.369E+00
Mooney-Rivlin constants of the hyperelastic material are: 0.170E+02, 0.000E+00, 0.000E+00,
•
0.000E+00, 0.000E+00, 0.000E+00,
0.150E+03 0.000E+00 0.000E+00
For the hyperelastic elements with mixed u-P formulation (HYPER56, HYPER58, HYPER74, and HYPER158), you can also have ANSYS perform a stability check during an analysis by setting KEYOPT(8) = 1. For each equilibrium iteration, the program checks every Gauss point in the problem for stability violations. If the problem fails the stability check, you will see a message in the solution history section of the ANSYS Output window reporting the total number of Gauss points that were unstable for that iteration. You will not see any messages if the problem passes the check. The sample message below shows that, during an analysis, ANSYS detected 3 Gauss points that exceeded the material stability limit: DISP CONVERGENCE VALUE = 22.81 CRITERION= 0.5000 EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 10.00 FORCE CONVERGENCE VALUE = 0.5018E+07 CRITERION= 0.1917E+05 >>> 3 Gauss points have exceeded the material stability limit
For elements that contain at least one unstable Gauss point, the instability indicator is set to 1 and stored in the result file as an item in the SMISC record. You can plot the region of instability in POST1 by plotting this SMISC record identified as STFLAG for the element. The SMISC number for STFLAG differs for some of the elements. See the appropriate table for the SMISC item that corresponds to instability indicator STFLAG, for the particular element of interest: HYPER56 Item and Sequence Numbers for ETABLE and ESOL Commands, HYPER58 Item and Sequence Numbers for ETABLE and ESOL Commands, HYPER74 Item and Sequence Numbers for ETABLE and ESOL Commands, HYPER158 Item and Sequence Numbers for ETABLE and ESOL Commands. You should be aware that even though a material failing a stability check is often an indication of convergence difficulty, it does not necessarily mean that your solution is invalid once the material enters the unstable region. The material stability check is simply a tool to help you diagnose the problem when the solution fails to converge. For nearly incompressible materials with Poisson's ratio greater than 0.49, we recommend that you use the hyperelastic elements with mixed u-P formulation (HYPER56, HYPER58, HYPER74, and HYPER158). Note — The element types HYPER84 and HYPER86 are intended primarily for modeling compressible, foam-like elastomers, using a Blatz-Ko function to describe the material properties. Select the Blatz-Ko option by setting KEYOPT(2) = 1 for these elements, then use MP commands to enter appropriate values for EX and NUXY to define the initial material shear modulus. An incompressible hyperelastic material option is also available for HYPER84 and HYPER86, but it is limited to two-term Mooney-Rivlin only. In general, it is recommended that you use HYPER56, HYPER58, HYPER74, or HYPER158 (not HYPER84 or HYPER86) for all incompressible hyperelastic materials. Problems using hyperelastic elements can be sensitive to the rate of load application. In most instances, load application should be slow so as not to over-distort elements in the converging sequence. Each problem may be unique and require special consideration. Bifurcation of the solution, indicating that two or more different geometric configurations have the same minimum potential energy, may occur at various times during the
8–28
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities loading history. Automatic time stepping with bisection [AUTOTS,ON] is often effective in overcoming these difficulties.
8.3.1.5. Creep Creep is a rate dependent material nonlinearity in which the material continues to deform under a constant load. Conversely, if a displacement is imposed, the reaction force (and stresses) will diminish over time (stress relaxation; see Figure 8.18: “Stress Relaxation and Creep”(a)). The three stages of creep are shown in Figure 8.18: “Stress Relaxation and Creep”(b). The ANSYS program has the capability of modeling the first two stages (primary and secondary). The tertiary stage is usually not analyzed since it implies impending failure.
Figure 8.18 Stress Relaxation and Creep
Creep is important in high temperature stress analyses, such as for nuclear reactors. For example, suppose you apply a preload to some part in a nuclear reactor to keep adjacent parts from moving. Over a period of time at high temperature, the preload would decrease (stress relaxation) and potentially let the adjacent parts move. Creep can also be significant for some materials such as prestressed concrete. Typically, the creep deformation is permanent. ANSYS analyzes creep using two time integration methods. Both are applicable to static or transient analyses.The implicit creep method is robust, fast, accurate, and recommended for general use. It can handle temperature dependent creep constants, as well as simultaneous coupling with isotropic hardening plasticity models. The explicit creep method is useful for cases where very small time steps are required. Creep constants cannot be dependent on temperature. Coupling with other plastic models is available by superposition only. Note — The terms “implicit” and “explicit” as applied to creep, have no relationship to “explicit dynamics,” or any elements referred to as “explicit elements.” The implicit creep method supports the following elements: PLANE42, SOLID45, PLANE82, SOLID92, SOLID95, LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189. The explicit creep method supports the following elements: LINK1, PLANE2, LINK8, PIPE20, BEAM23, BEAM24, PLANE42, SHELL43, SOLID45, SHELL51, PIPE60, SOLID62, SOLID65, PLANE82, SOLID92, and SOLID95. The creep strain rate may be a function of stress, strain, temperature, and neutron flux level. Libraries of creep strain rate equations are built into the ANSYS program for primary, secondary, and irradiation induced creep. (See Creep Equations in the ANSYS Elements Reference for discussions of, and input procedures for, these various creep equations.) Some equations require specific units. In particular, for the explicit creep option, temperatures used in the creep equations should be based on an absolute scale.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–29
Chapter 8: Nonlinear Structural Analysis
8.3.1.5.1. Implicit Creep Procedure The basic procedure for using the implicit creep method involves issuing the TB command with Lab = CREEP, and choosing a creep equation by specifying a value for TBOPT. The following example input shows the use of the implicit creep method. TBOPT = 2 specifies that the primary creep equation for model 2 will be used. Temperature dependency is specified using the TBTEMP command, and the four constants associated with this equation are specified as arguments with the TBDATA command. TB,CREEP,1,1,4,2 TBTEMP,100 TBDATA,1,C1,C2,C3,C4
You can input other creep expressions using the user programmable feature and setting TBOPT = 100. You can define the number of state variables using the TB command with Lab = STATE. The following example shows how five state variables are defined. TB,STATE,1,,5
You can simultaneously model creep [TB,CREEP] and isotropic, bilinear kinematic, and Hill anisotropy options to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. To perform an implicit creep analysis, you must also issue the solution RATE command, with Option = ON (or 1). The following example shows a procedure for a time hardening creep analysis (See Figure 8.19: “Time Hardening Creep Analysis”).
Figure 8.19 Time Hardening Creep Analysis
The user applied mechanical loading in the first load step, and turned the RATE command OFF to bypass the creep strain effect. Since the time period in this load step will affect the total time thereafter, the time period for this load step should be small. For this example, the user specified a value of 1.0E-8 seconds. The second load step is a creep analysis. The RATE command must be turned ON. Here the mechanical loading was kept constant, and the material creeps as time increases. /SOLU RATE,OFF TIME,1.0E-8
8–30
!First load step, apply mechanical loading !Creep analysis turned off !Time period set to a very small value
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities ... SOLV RATE,ON TIME,100 ... SOLV
!Solve this load step !Second load step, no further mechanical load !Creep analysis turned on !Time period set to desired value !Solve this load step
The RATE command works only when modeling implicit creep with either von Mises or Hill potentials. When modeling implicit creep with von Mises potential, you can use the RATE command with the following elements: LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189. When modeling anisotropic creep (TB,CREEP with TB,HILL), you can use the RATE command with the following elements: PLANE42, SOLID45, PLANE82, SOLID92, SOLID95, LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189. For most materials, the creep strain rate changes significantly at an early stage. Because of this, a general recommendation is to use a small initial incremental time step, then specify a large maximum incremental time step by using solution command DELTIM or NSUBST. For implicit creep, you may need to examine the effect of the time increment on the results carefully because ANSYS does not enforce any creep ratio control by default. You can always enforce a creep limit ratio using the creep ratio control option in commands CRPLIM or CUTCONTROL,CRPLIMIT. A recommended value for a creep limit ratio ranges from 1 to 10. The ratio may vary with materials so your decision on the best value to use should be based on your own experimentation to gain the required performance and accuracy. For larger analyses, a suggestion is to first perform a time increment convergence analysis on a simple small size test. ANSYS provides tools to help you determine the coefficients for all of the implicit creep options defined in TB,CREEP. The TBFT command allows you to compare your experimental data with existing material data curves and visually “fit” your curve for use in the TB command. All of the TBFT command capability is available via either batch or interactive (GUI) mode. See Material Curve Fitting (also in this manual) for more information.
8.3.1.5.2. Explicit Creep Procedure The basic procedure for using the explicit creep method involves issuing the TB command with Lab = CREEP and choosing a creep equation by adding the appropriate constant as an argument with the TBDATA command. TBOPT is either left blank or = 0. The following example input uses the explicit creep method. Note that all constants are included as arguments with the TBDATA command, and that there is no temperature dependency. TB,CREEP,1 TBDATA,1,C1,C2,C3,C4, ,C6
For the explicit creep method, you can incorporate other creep expressions into the program by using User Programmable Features (see the Guide to ANSYS User Programmable Features). For highly nonlinear creep strain vs. time curves, a small time step must be used with the explicit creep method. Creep strains are not computed if the time step is less than 1.0e-6. A creep time step optimization procedure is available [AUTOTS and CRPLIM] for automatically adjusting the time step as appropriate.
8.3.1.6. Shape Memory Alloy The Shape Memory Alloy (SMA) material behavior option describes the super-elastic behavior of nitinol alloy. Nitinol is a flexible metal alloy that can undergo very large deformations in loading-unloading cycles without permanent deformation. As illustrated in Figure 8.20: “Shape Memory Alloy Phases”, the material behavior has three distinct phases: an austenite phase (linear elastic), a martensite phase (also linear elastic), and the transition phase between these two.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–31
Chapter 8: Nonlinear Structural Analysis
Figure 8.20 Shape Memory Alloy Phases σ
σ
ε
∫
σ
σ σ
∫
ε
Use the MP command to input the linear elastic behavior of the austenite phase, and the TB,SMA command to input the behavior of the transition and martensite phases. Use the TBDATA command to enter the specifics (data sets) of the alloy material. You can enter up to six sets of data. SMAs can be specified for the following elements: PLANE182, PLANE183, SOLID185, SOLID186, SOLID187. A typical ANSYS input listing (fragment) will look similar to this: MP,EX,1,60.0E3 MP,NUXY,1.0.3
! Define austenite elastic properties !
TB,SMA,1,2 TBTEMP,10 TBDATA,1,520.0,600.0,300.0,200.0,0.07,0.12 TBDATA,7,5.0E4 TBTEMP,20 TBDATA,1,420.0,540.0,300.0,200.0,0.10,0.15 TBDATA,7,4.0E3
! ! ! ! ! ! ! ! !
Define material 1 as SMA, with two temperatures Define first starting temp Define SMA parameters
Define second starting temp Define SMA parameters
See TB, and TBDATA for more information.
8.3.1.7. Viscoplasticity Viscoplasticity is a time-dependent plasticity phenomenon, where the development of the plastic strains are dependent on the rate of loading. The primary applications are high-temperature metal forming processes such as rolling and deep drawing, which involve large plastic strains and displacements with small elastic strains (see Figure 8.21: “Viscoplastic Behavior in a Rolling Operation”). The plastic strains are typically very large (for example, 50% or greater), requiring large strain theory [NLGEOM,ON]. 8–32
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities Viscoplasticity is modeled with element types VISCO106, VISCO107, and VISCO108, using Anand's model for material properties as described in Nonlinear Stress-Strain Materials in the ANSYS Elements Reference.
Figure 8.21 Viscoplastic Behavior in a Rolling Operation
Viscoplasticity is defined by unifying plasticity and creep via a set of flow and evolutionary equations. A constraint equation is used to preserve volume in the plastic region. The Rate-Dependent Plasticity (Viscoplasticity) or TB,RATE option allows you to introduce the strain rate effect in material models to simulate the time-dependent response of materials. Two material options are available, the Perzyna model and the Peirce model (see the ANSYS, Inc. Theory Reference for details). In contrast to other rate-dependent material options in ANSYS such as Creep or Anand's model, the Perzyna and Peirce models also include a yield surface. The plasticity and thus the strain rate hardening effect are active only after plastic yielding. You must use the models in combination with the BISO, MISO, or NLISO material options to simulate viscoplasticity. Further, you can simulate anisotropic viscoplasticity by also combining the HILL option. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. For isotropic hardening, the intent is for simulating the strain rate hardening of materials rather than softening. This option is also suitable for large strain analysis, and is applicable to the following elements: PLANE42, SOLID45, PLANE82, SOLID92, SOLID95, LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189. Some typical applications of these material options are metal forming and micro-electromechanical systems (MEMS).
8.3.1.8. Viscoelasticity Viscoelasticity is similar to creep, but part of the deformation is removed when the loading is taken off. A common viscoelastic material is glass. Some plastics are also considered to be viscoelastic. One type of viscoelastic response is illustrated in Figure 8.22: “Viscoelastic Behavior (Maxwell Model)”.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–33
Chapter 8: Nonlinear Structural Analysis
Figure 8.22 Viscoelastic Behavior (Maxwell Model)
Viscoelasticity is modeled with element types VISCO88 and VISCO89 for small deformation viscoelasticity and LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189 for small and large deformation viscoelasticity. You must input material properties using the TB family of commands. For SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, and SOLID187 the underlying elasticity is specified by either the MP command (hypoelasticity) or by the TB,HYPER command (hyperelasticity). For LINK180, BEAM188, and BEAM189, the underlying elasticity is specified using the MP command (hypoelasticity) only. The elasticity constants correspond to those of the fast load limit. Use the TB,PRONY and TB,SHIFT commands to input the relaxation property (see the TB command description for more information). !Small Strain Viscoelasticity mp,ex,1,20.0E5 !elastic properties mp,nuxy,1,0.3 tb,prony,1,,2,shear !define viscosity parameters (shear) tbdata,1,0.5,2.0,0.25,4.0 tb,prony,1,,2,bulk !define viscosity parameters (bulk) tbdata,1,0.5,2.0,0.25,4.0 !Large Strain Viscoelasticity tb,hyper,1,,,moon !elastic properties tbdata,1,38.462E4,,1.2E-6 tb,prony,1,,1,shear !define viscosity parameters tbdata,1,0.5,2.0 tb,prony,1,,1,bulk !define viscosity parameters tbdata,1,0.5,2.0
See Viscoelastic Material Constants in the ANSYS Elements Reference and the ANSYS, Inc. Theory Reference for details about how to input viscoelastic material properties using the TB family of commands. ANSYS provides tools to help you determine the coefficients for all of the viscoelastic options defined by TB,PRONY. The TBFT command allows you to compare your experimental data with existing material data curves and visually “fit” your curve for use in the TB command. All of the TBFT command capability is available via either batch or interactive (GUI) mode. See Material Curve Fitting (also in this manual) for more information.
8.3.1.9. Swelling Certain materials respond to neutron flux by enlarging volumetrically, or swelling. In order to include swelling effects, you must write your own swelling subroutine, USERSW. (See the Guide to ANSYS User Programmable Features for a discussion of User-Programmable Features.) Swelling Equations in the ANSYS Elements Reference discusses how to use the TB family of commands to input constants for the swelling equations. Swelling can also be related to other phenomena, such as moisture content. The ANSYS commands for nuclear swelling can be used analogously to define swelling due to other causes.
8–34
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
8.3.2. Material Model Combinations You can combine several material model options discussed in this chapter to simulate complex material behaviors. Material Model Combinations in the ANSYS Elements Reference presents the model options you can combine along with the associated TB command labels and links to sample input listings. These sample input listings are presented below in sections identified by the TB command labels.
8.3.2.1. BISO and CHAB Example This input listing illustrates an example of combining bilinear isotropic hardening plasticity with Chaboche nonlinear kinematic hardening plasticity. MP,EX,1,185.0E3 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,CHAB,1 TBDATA,1,180,100,3
! CHABOCHE TABLE
TB,BISO,1 TBDATA,1,180,200
! BISO TABLE
For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.2. MISO and CHAB Example This input listing illustrates an example of combining multilinear isotropic hardening plasticity with Chaboche nonlinear kinematic hardening plasticity. MP,EX,1,185E3 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,CHAB,1 TBDATA,1,180,100,3
! CHABOCHE TABLE ! THIS EXAMPLE ISOTHERMAL
TB,MISO,1 TBPT,,9.7E-4,180 TBPT,,1.0,380
! MISO TABLE
For information on the MISO option, see Multilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.3. NLISO and CHAB Example This input listing illustrates an example of combining nonlinear isotropic hardening plasticity with Chaboche nonlinear kinematic hardening plasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,CHAB,1,3,5 ! CHABOCHE TABLE TBTEMP,20,1 ! THIS EXAMPLE TEMPERATURE DEPENDENT TBDATA,1,500,20000,100,40000,200,10000 TBDATA,7,1000,200,100,100,0 TBTEMP,40,2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–35
Chapter 8: Nonlinear Structural Analysis TBDATA,1,880,204000,200,43800,500,10200 TBDATA,7,1000,2600,2000,500,0 TBTEMP,60,3 TBDATA,1,1080,244000,400,45800,700,12200 TBDATA,7,1400,3000,2800,900,0 TB,NLISO,1,2 TBTEMP,40,1 TBDATA,1,880,0.0,80.0,3 TBTEMP,60,2 TBDATA,1,1080,0.0,120.0,7
! NLISO TABLE
For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.4. BISO and RATE Example This input listing illustrates an example of combining bilinear isotropic hardening plasticity with the TB,RATE command to model viscoplasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,BISO,1 TBDATA,1,9000,10000
! BISO TABLE
TB,RATE,1,,,PERZYNA TBDATA,1,0.5,1
! RATE TABLE
For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the RATE option, see Rate-Dependent Viscoplastic Materials in the ANSYS Elements Reference, and Section 8.3.1.7: Viscoplasticity in this chapter.
8.3.2.5. MISO and RATE Example This input listing illustrates an example of combining multilinear isotropic hardening plasticity with the TB,RATE command to model viscoplasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,MISO,1 TBPT,,0.015,30000 TBPT,,0.020,32000 TBPT,,0.025,33800 TBPT,,0.030,35000 TBPT,,0.040,36500 TBPT,,0.050,38000 TBPT,,0.060,39000
! MISO TABLE
TB,RATE,1,,,PERZYNA TBDATA,1,0.5,1
! RATE TABLE
For information on the MISO option, see Multilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the RATE option, see Rate-Dependent Viscoplastic Materials in the ANSYS Elements Reference, and Section 8.3.1.7: Viscoplasticity in this chapter. 8–36
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
8.3.2.6. NLISO and RATE Example This input listing illustrates an example of combining nonlinear isotropic hardening plasticity with the TB,RATE command to model viscoplasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,NLISO,1 TBDATA,1,30000,100000,5200,172
! NLISO TABLE
TB,RATE,1,,,PERZYNA TBDATA,1,0.5,1
! RATE TABLE
For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the RATE option, see Rate-Dependent Viscoplastic Materials in the ANSYS Elements Reference, and Section 8.3.1.7: Viscoplasticity in this chapter.
8.3.2.7. BISO and CREEP Example This input listing illustrates an example of combining bilinear isotropic hardening plasticity with implicit creep. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,BISO,1 TBDATA,1,9000,10000
! BISO TABLE
TB,CREEP,1,,,2 ! CREEP TABLE TBDATA,1,1.5625E-14,5.0,-0.5,0.0
For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter.
8.3.2.8. MISO and CREEP Example This input listing illustrates an example of combining multilinear isotropic hardening plasticity with implicit creep. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,MISO,1 TBPT,,0.015,30000 TBPT,,0.020,32000 TBPT,,0.025,33800 TBPT,,0.030,35000 TBPT,,0.040,36500 TBPT,,0.050,38000 TBPT,,0.060,39000
! MISO TABLE
TB,CREEP,1,,,2 ! CREEP TABLE TBDATA,1,1.5625E-14,5.0,-0.5,0.0
For information on the MISO option, see Multilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–37
Chapter 8: Nonlinear Structural Analysis For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter.
8.3.2.9. NLISO and CREEP Example This input listing illustrates an example of combining nonlinear isotropic hardening plasticity with implicit creep. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,NLISO,1 TBDATA,1,30000,100000,5200,172
! NLISO TABLE
TB,CREEP,1,,,2 ! CREEP TABLE TBDATA,1,1.5625E-14,5.0,-0.5,0.0
For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter.
8.3.2.10. BKIN and CREEP Example This input listing illustrates an example of combining bilinear kinematic hardening plasticity with implicit creep. MP,EX,1,1e7 MP,NUXY,1,0.32
! ELASTIC CONSTANTS
TB,BKIN,1, TBDATA,1,42000,1000
! BKIN TABLE
TB,CREEP,1,,,6 TBDATA,1,7.4e-21,3.5,0,0,0,0
! CREEP TABLE
For information on the BKIN option, see Bilinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter.
8.3.2.11. HILL and BISO Example This input listing illustrates an example of modeling anisotropic plasticity with bilinear isotropic hardening. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,HILL,1,2 ! HILL TABLE TBTEMP,100 TBDATA,1,1,1.0402,1.24897,1.07895,1,1 TBTEMP,200 TBDATA,1,0.9,0.94,1.124,0.97,0.9,0.9 TB,BISO,1,2 TBTEMP,100 TBDATA,1,461.0,374.586 TBTEMP,200 TBDATA,1,400.0,325.0
! BISO TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8–38
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.12. HILL and MISO Example This input listing illustrates an example of modeling anisotropic plasticity with multilinear isotropic hardening. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,MISO,1 TBPT,,0.015,30000 TBPT,,0.020,32000 TBPT,,0.025,33800 TBPT,,0.030,35000 TBPT,,0.040,36500 TBPT,,0.050,38000 TBPT,,0.060,39000
! MISO TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the MISO option, see Multilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.13. HILL and NLISO Example This input listing illustrates an example of modeling anisotropic plasticity with nonlinear isotropic hardening. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,NLISO,1 TBDATA,1,30000,100000,5200,172
! NLISO TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.14. HILL and BKIN Example This input listing illustrates an example of modeling anisotropic plasticity with bilinear kinematic hardening. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,BKIN,1 TBDATA,1,9000,10000
! BKIN TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–39
Chapter 8: Nonlinear Structural Analysis For information on the BKIN option, see Bilinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.15. HILL and MKIN Example This input listing illustrates an example of modeling anisotropic plasticity with multilinear kinematic hardening. MPTEMP,1,20,400,650,800,950
! ELASTIC CONSTANTS
MPDATA,EX,1,1,30.00E6,27.36E6,25.20E6,23.11E6,20.76E6 MPDATA,EY,1,1,30.00E6,27.36E6,25.20E6,23.11E6,20.76E6 MPDATA,EZ,1,1,30.00E6,27.36E6,25.20E6,23.11E6,20.76E6 MPDATA,PRXY,1,1,0.351,0.359,0.368,0.375,0.377 MPDATA,PRYZ,1,1,0.351,0.359,0.368,0.375,0.377 MPDATA,PRXZ,1,1,0.351,0.359,0.368,0.375,0.377 MPDATA,GXY,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4 MPDATA,GYZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4 MPDATA,GXZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4
TB,MKIN,1,5,5 ! MKIN TABLE TBTEMP,,strain TBDATA,1,0.0015,0.006,0.04,0.08,0.1 TBTEMP,20 TBDATA,1,45000,60000,90000,115000,120000 TBTEMP,400 TBDATA,1,41040,54720,82080,104880,109440 TBTEMP,650 TBDATA,1,37800,50400,75600,96600,100800 TBTEMP,800 TBDATA,1,34665,46220,69330,88588,92440 TBTEMP,950 TBDATA,1,31140,41520,62280,79580,83040
TB,HILL,1,5 ! HILL TABLE TBTEMP,20.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,400.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,650.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,800.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00 TBTEMP,950.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the MKIN option, see Multilinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.16. HILL and KINH Example This input listing illustrates an example of modeling anisotropic plasticity with multilinear kinematic hardening. MP,EX,1,20E6 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,KINH,1,,3 TBPT,,5E-5,1E3 TBPT,,0.01,2E3 TBPT,,0.60,6E4
! KINH TABLE
8–40
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities TB,HILL,1 TBDATA,1,1.0,1.1,0.9,0.85,0.90,0.95
! HILL TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the KINH option, see Multilinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.17. HILL and CHAB Example This input listing illustrates an example of modeling anisotropic plasticity with Chaboche nonlinear kinematic hardening. MP,EX,1,185E3 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,CHAB,1 TBDATA,1,180,400,3,0
! CHABOCHE TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.18. HILL and BISO and CHAB Example This input listing illustrates an example of modeling anisotropic plasticity with bilinear isotropic hardening and Chaboche nonlinear kinematic hardening. MP,EX,1,185E3 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,CHAB,1 TBDATA,1,180,100,3
! CHABOCHE TABLE
TB,BISO,1 TBDATA,1,180,200
! BISO TABLE
TB,HILL,1 TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80
! HILL TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.19. HILL and MISO and CHAB Example This input listing illustrates an example of modeling anisotropic plasticity with multilinear isotropic hardening and Chaboche nonlinear kinematic hardening.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–41
Chapter 8: Nonlinear Structural Analysis MP,EX,1,185E3 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,CHAB,1 TBDATA,1,185,100,3
! CHABOCHE TABLE
TB,MISO,1 TBPT,,0.001,185 TBPT,,1.0,380
! MISO TABLE
TB,HILL,1 TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80
! HILL TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the MISO option, see Multilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.20. HILL and NLISO and CHAB Example This input listing illustrates an example of combining anisotropic plasticity with nonlinear isotropic hardening and Chaboche nonlinear kinematic hardening. MPTEMP,1,20,200,400,550,600,650 ! ELASTIC CONSTANTS MPTEMP,,700,750,800,850,900,950 ! MPDATA,EX,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EX,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,EY,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EY,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,EZ,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EZ,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,PRXY,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRXY,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,PRYZ,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRYZ,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,PRXZ,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRXZ,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,GXY,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GXY,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4 ! MPDATA,GYZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GYZ,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4 ! MPDATA,GXZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GXZ,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4
TB,NLISO,1 TBDATA,1,180,0.0,100.0,5
! NLISO TABLE
! TB,CHAB,1 TBDATA,1,180,100,3
8–42
! CHABOCHE TABLE
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
TB,HILL,1,5 TBTEMP,750.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,800.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,850.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,900.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00 TBTEMP,950.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00
! HILL TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.21. HILL and RATE and BISO Example This input listing illustrates an example of modeling anisotropic viscoplasticity with bilinear isotropic hardening plasticity. MPTEMP,1,20,400,650,800,950 ! ELASTIC CONSTANTS ! MPDATA,EX,1,1,30.00E6,27.36E6,25.20E6,23.11E6,20.76E6 ! MPDATA,EY,1,1,30.00E6,27.36E6,25.20E6,23.11E6,20.76E6 ! MPDATA,EZ,1,1,30.00E6,27.36E6,25.20E6,23.11E6,20.76E6 ! MPDATA,PRXY,1,1,0.351,0.359,0.368,0.375,0.377 ! MPDATA,PRYZ,1,1,0.351,0.359,0.368,0.375,0.377 ! MPDATA,PRXZ,1,1,0.351,0.359,0.368,0.375,0.377 ! MPDATA,GXY,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4 ! MPDATA,GYZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4 ! MPDATA,GXZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4
TB,BISO,1, TBDATA,1,45000,760000
! BISO TABLE
TB,RATE,1,2,,PERZYNA TBTEMP,20 TBDATA,1,0.1,0.3 TBTEMP,950 TBDATA,1,0.3,0.5
! RATE TABLE
TB,HILL,1,5 ! HILL TABLE TBTEMP,750.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,800.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,850.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,900.0
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–43
Chapter 8: Nonlinear Structural Analysis TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00 TBTEMP,950.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the RATE option, see Rate-Dependent Viscoplastic Materials in the ANSYS Elements Reference, and Section 8.3.1.7: Viscoplasticity in this chapter. For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.22. HILL and RATE and MISO Example This input listing illustrates an example of modeling anisotropic viscoplasticity with multilinear isotropic hardening plasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,MISO,1 TBPT,,0.015,30000 TBPT,,0.020,32000 TBPT,,0.025,33800 TBPT,,0.030,35000 TBPT,,0.040,36500 TBPT,,0.050,38000 TBPT,,0.060,39000
! MISO TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80 TB,RATE,1,,,PERZYNA TBDATA,1,0.5,1
! RATE TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the RATE option, see Rate-Dependent Viscoplastic Materials in the ANSYS Elements Reference, and Section 8.3.1.7: Viscoplasticity in this chapter. For information on the MISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.23. HILL and RATE and NLISO Example This input listing illustrates an example of modeling anisotropic viscoplasticity with nonlinear isotropic hardening plasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,NLISO,1 TBDATA,1,30000,100000,5200,172
! NLISO TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80 TB,RATE,1,,,PERZYNA TBDATA,1,0.5,1
8–44
! RATE TABLE
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the RATE option, see Rate-Dependent Viscoplastic Materials in the ANSYS Elements Reference, and Section 8.3.1.7: Viscoplasticity in this chapter. For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.24. HILL and CREEP Example This input listing illustrates an example of modeling anisotropic implicit creep. MPTEMP,1,20,200,400,550,600,650 ! ELASTIC CONSTANTS MPTEMP,,700,750,800,850,900,950 ! MPDATA,EX,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EX,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,EY,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EY,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,EZ,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EZ,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,PRXY,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRXY,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,PRYZ,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRYZ,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,PRXZ,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRXZ,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,GXY,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GXY,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4 ! MPDATA,GYZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GYZ,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4 ! MPDATA,GXZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GXZ,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4
TB,CREEP,1,,,2 TBDATA,1,5.911E-34,6.25,-0.25
! CREEP TABLE
TB,HILL,1,5 TBTEMP,750.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,800.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,850.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,900.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00 TBTEMP,950.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00
! HILL TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–45
Chapter 8: Nonlinear Structural Analysis
8.3.2.25. HILL and CREEP and BISO Example This input listing illustrates an example of modeling anisotropic implicit creep with bilinear isotropic hardening plasticity. MPTEMP,1,20,200,400,550,600,650 ! ELASTIC CONSTANTS MPTEMP,,700,750,800,850,900,950 ! MPDATA,EX,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EX,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,EY,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EY,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,EZ,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EZ,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,PRXY,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRXY,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,PRYZ,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRYZ,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,PRXZ,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRXZ,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,GXY,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GXY,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4 ! MPDATA,GYZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GYZ,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4 ! MPDATA,GXZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GXZ,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4
TB,BISO,1 TBDATA,1,180,200
! BISO TABLE
TB,CREEP,1,,,2 TBDATA,1,5.911E-34,6.25,-0.25
! CREEP TABLE
TB,HILL,1,5 TBTEMP,750.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,800.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,850.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,900.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00 TBTEMP,950.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00
! HILL TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter. For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8–46
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
8.3.2.26. HILL and CREEP and MISO Example This input listing illustrates an example of modeling anisotropic implicit creep with multilinear isotropic hardening plasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,MISO,1 TBPT,,0.015,30000 TBPT,,0.020,32000 TBPT,,0.025,33800 TBPT,,0.030,35000 TBPT,,0.040,36500 TBPT,,0.050,38000 TBPT,,0.060,39000
! MISO TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80 TB,CREEP,1,,,2 ! CREEP TABLE TBDATA,1,1.5625E-14,5.0,-0.5,0.0
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter. For information on the MISO option, see Multilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.27. HILL and CREEP and NLISO Example This input listing illustrates an example of modeling anisotropic implicit creep with nonlinear isotropic hardening plasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,NLISO,1 TBDATA,1,30000,100000,5200,172
! NLISO TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80 TB,CREEP,1,,,2 ! CREEP TABLE TBDATA,1,1.5625E-14,5.0,-0.5,0.0
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter. For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.28. HILL and CREEP and BKIN Example This input listing illustrates an example of modeling anisotropic implicit creep with bilinear kinematic hardening plasticity. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–47
Chapter 8: Nonlinear Structural Analysis MP,EX,1,1e7 MP,NUXY,1,0.32
! ELASTIC CONSTANTS
TB,BKIN,1 TBDATA,1,42000,1000
! BKIN TABLE
TB,CREEP,1,,,6 TBDATA,1,7.4e-21,3.5,0,0,0,0
! CREEP TABLES
TB,HILL,1 ! HILL TABLE TBDATA,1,1.15,1.05,1.0,1.0,1.0,1.0
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter. For information on the BKIN option, see Bilinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.4. Running a Nonlinear Analysis in ANSYS ANSYS employs an automatic solution control method that, based on the physics of your problem, sets various nonlinear analysis controls to the appropriate values. If you are not satisfied with the results obtained with these values, you can manually override the settings. The following commands are set to optimal defaults: AUTOTS
PRED
MONITOR
DELTIM
NROPT
NEQIT
NSUBST
TINTP
SSTIF
CNVTOL
CUTCONTROL
KBC
LNSRCH
OPNCONTROL
EQSLV
ARCLEN
CDWRITE
LSWRITE
These commands and the settings they control are discussed in later sections. You can also refer to the individual command descriptions in the ANSYS Commands Reference. If you do choose to override the ANSYS-specified settings, or if you wish to use an input list from a previous release of ANSYS, issue SOLCONTROL,OFF in the /SOLU phase. See the SOLCONTROL command description for more details. ANSYS' automatic solution control is active for the following analyses: •
Single-field nonlinear or transient structural and solid mechanics analysis where the solution DOFs are combinations of UX, UY, UZ, ROTX, ROTY, and ROTZ.
•
Single-field nonlinear or transient thermal analysis where the solution DOF is TEMP. Note — The Solution Controls dialog box, which is described later in this chapter, cannot be used to set solution controls for a thermal analysis. Instead, you must use the standard set of ANSYS solution commands and the standard corresponding menu paths.
8.5. Performing a Nonlinear Static Analysis The procedure for performing a nonlinear static analysis consists of these tasks:
8–48
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.5: Performing a Nonlinear Static Analysis •
Section 8.5.1: Build the Model
•
Section 8.5.2: Set Solution Controls
•
Section 8.5.3: Set Additional Solution Options
•
Section 8.5.4: Apply the Loads
•
Section 8.5.5: Solve the Analysis
•
Section 8.5.6: Review the Results
8.5.1. Build the Model This step is essentially the same for both linear and nonlinear analyses, although a nonlinear analysis might include special elements or nonlinear material properties. See Section 8.9: Using Nonlinear (Changing-Status) Elements, and Section 8.3: Modeling Material Nonlinearities, for more details. If your analysis includes large-strain effects, your stress-strain data must be expressed in terms of true stress and true (or logarithmic) strain. For more information on building models in ANSYS, see the ANSYS Modeling and Meshing Guide. After you have created a model in ANSYS, you set solution controls (analysis type, analysis options, load step options, and so on), apply loads, and solve. A nonlinear solution will differ from a linear solution in that it often requires multiple load increments, and always requires equilibrium iterations. The general procedure for performing these tasks follows. See Section 8.11: Sample Nonlinear Analysis (GUI Method) for a sample problem that walks you through a specific nonlinear analysis.
8.5.2. Set Solution Controls Setting solution controls for a nonlinear analysis involves the same options and method of access (the Solution Controls dialog box) as those used for a linear structural static analysis. For a nonlinear analysis, the default settings in the Solution Controls dialog box are essentially the same settings employed by the automatic solution control method described in Section 8.4: Running a Nonlinear Analysis in ANSYS. See the following sections in Chapter 2, “Structural Static Analysis”, with exceptions noted: •
Section 2.3.2: Set Solution Controls
•
Section 2.3.2.1: Access the Solution Controls Dialog Box
•
Section 2.3.2.2: Using the Basic Tab
•
Section 2.3.2.3: The Transient Tab
•
Section 2.3.2.4: Using the Sol'n Options Tab
•
Section 2.3.2.5: Using the Nonlinear Tab
•
Section 2.3.2.6: Using the Advanced NL Tab
8.5.2.1. Using the Basic Tab: Special Considerations Special considerations for setting these options in a nonlinear structural static analysis include: •
When setting ANTYPE and NLGEOM, choose Large Displacement Static if you are performing a new analysis. (But, keep in mind that not all nonlinear analyses will produce large deformations. See Section 8.2: Using Geometric Nonlinearities for further discussion of large deformations.) Choose Restart Current Analysis if you want to restart a failed nonlinear analysis. You cannot change this setting after the first load step (that is, after you issue your first SOLVE command). You will usually choose to do a new analysis, rather than a restart. Restarts are discussed in the ANSYS Basic Analysis Guide.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–49
Chapter 8: Nonlinear Structural Analysis •
When working with time settings, remember that these options can be changed at any load step. See Chapter 2, “Loading” in the ANSYS Basic Analysis Guide for more information on these options. Advanced time/frequency options, in addition to those available on the Solution Controls dialog box, are discussed in Section 8.5.2.3: Advanced Load Step Options You Can Set on the Solution Controls Dialog Box. A nonlinear analysis requires multiple substeps (or time steps; the two terms are equivalent) within each load step so that ANSYS can apply the specified loads gradually and obtain an accurate solution. The NSUBST and DELTIM commands both achieve the same effect (establishing a load step's starting, minimum, and maximum step size), but by reciprocal means. NSUBST defines the number of substeps to be taken within a load step, whereas DELTIM defines the time step size explicitly. If automatic time stepping is off [AUTOTS], then the starting substep size is used throughout the load step.
•
OUTRES controls the data on the results file (Jobname.RST). By default, only the last substep is written to the results file in a nonlinear analysis. Only 1000 results sets (substeps) can be written to the results file, but you can use the command /CONFIG,NRES to increase the limit (see the ANSYS Basic Analysis Guide).
8.5.2.2. Advanced Analysis Options You Can Set on the Solution Controls Dialog Box The following sections provide more detail about some of the advanced analysis options that you can set on the Solution Controls dialog box.
8.5.2.2.1. Equation Solver ANSYS' automatic solution control activates the sparse direct solver (EQSLV,SPARSE) for most cases. The sparse direct solver is the default, except for the generation pass of a substructure analysis (which uses the frontal direct solver). Other choices include the frontal direct and PCG solvers. For applications using solid elements (for example, SOLID92 or SOLID45), the PCG solver may be faster, especially when doing 3-D modeling. If you are using the PCG solver, you may be able to considerably reduce your memory usage with the MSAVE command. The MSAVE command triggers an element-by-element approach for the parts of the model that use SOLID92, SOLID95, SOLID186, and/or SOLID187 elements with linear material properties. To use this command, you must be doing a static analysis or a modal analysis with the PowerDynamics method. If using SOLID186 and/or SOLID187 elements, it must be a small strain (NLGEOM,OFF) analysis. Other parts of the model that do not meet the above criteria will be solved using global assembly for the stiffness matrix. MSAVE,ON can result in a memory savings of up to 70% for the part of the model that meets the criteria, although the solution time may increase depending on the manufacturer of your computer and the speed of your processor, as well as the chosen element options (for example, 2 x 2 x 2 integration for SOLID95). The sparse direct solver, in sharp contrast to the iterative solvers included in ANSYS, is a robust solver. Although the PCG solver can solve indefinite matrix equations, when the PCG solver encounters an ill-conditioned matrix, the solver will iterate to the specified number of iterations and stop if it fails to converge. When this happens, it triggers bisection. After completing the bisection, the solver continues the solution if the resulting matrix is wellconditioned. Eventually, the entire nonlinear load step can be solved. Use the following guidelines for selecting either the sparse or the PCG solver for nonlinear structural analysis: •
If it is a beam/shell or beam/shell and solid structure, choose the sparse direct solver.
•
If it is a 3-D solid structure and the number of DOF is relatively large (that is, 200,000 or more DOF), choose the PCG solver.
8–50
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.5: Performing a Nonlinear Static Analysis •
If the problem is ill-conditioned (triggered by poor element shapes), or has a big difference in material properties in different regions of the model, or has insufficient displacement boundary constraints, choose the sparse direct solver.
8.5.2.3. Advanced Load Step Options You Can Set on the Solution Controls Dialog Box The following sections provide more detail about some of the advanced load step options that you can set on the Solution Controls dialog box.
8.5.2.3.1. Automatic Time Stepping ANSYS' automatic solution control turns automatic time stepping on [AUTOTS,ON]. An internal auto-time step scheme ensures that the time step variation is neither too aggressive (resulting in many bisection/cutbacks) nor too conservative (time step size is too small). At the end of a time step, the size of the next time step is predicted based on four factors: •
Number of equilibrium iterations used in the last time step (more iterations cause the time step size to be reduced)
•
Predictions for nonlinear element status change (time step sizes are decreased when a status change is imminent)
•
Size of the plastic strain increment
•
Size of the creep strain increment
8.5.2.3.2. Convergence Criteria The program will continue to do equilibrium iterations until the convergence criteria [CNVTOL] are satisfied (or until the maximum number of equilibrium equations is reached [NEQIT]). You can define custom criteria if the default settings are not suitable. ANSYS' automatic solution control uses L2-norm of force (and moment) tolerance (TOLER) equal to 0.5%, a setting that is appropriate for most cases. In most cases, an L2-norm check on displacement with TOLER equal to 5% is also used in addition to the force norm check. The check that the displacements are loosely set serves as a doublecheck on convergence. By default, the program will check for force (and, when rotational degrees of freedom are active, moment) convergence by comparing the square root sum of the squares (SRSS) of the force imbalances against the product of VALUE*TOLER. The default value of VALUE is the SRSS of the applied loads (or, for applied displacements, of the Newton-Raphson restoring forces), or MINREF (which defaults to 0.01), whichever is greater. The default value of TOLER is 0.005. If SOLCONTROL,OFF, TOLER defaults to 0.001 and MINREF defaults to 1.0 for force convergence. You should almost always use force convergence checking. You can also add displacement (and, when applicable, rotation) convergence checking. For displacements, the program bases convergence checking on the change in deflections (∆u) between the current (i) and the previous (i-1) iterations: ∆u=ui-ui-1. Note — If you explicitly define any custom convergence criteria [CNVTOL], the entire default criteria will be overwritten. Thus, if you define displacement convergence checking, you will have to redefine force convergence checking. (Use multiple CNVTOL commands to define multiple convergence criteria.) Using tighter convergence criteria will improve the accuracy of your results, but at the cost of more equilibrium iterations. If you want to tighten (or loosen, which is not recommended) your criteria, you should change TOLER Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–51
Chapter 8: Nonlinear Structural Analysis by one or two orders of magnitude. In general, you should continue to use the default value of VALUE; that is, change the convergence criteria by adjusting TOLER, not VALUE. You should make certain that the default value of MINREF = 0.001 makes sense in the context of your analysis. If your analysis uses certain sets of units or has very low load levels, you might want to specify a smaller value for MINREF. Also, we do not recommend putting two or more disjointed structures into one model for a nonlinear analysis because the convergence check tries to relate these disjointed structures, often producing some unwanted residual force. Checking Convergence in a Single and Multi-DOF System To check convergence in a single degree of freedom (DOF) system, you compute the force (and moment) imbalance for the one DOF, and compare this value against the established convergence criteria (VALUE*TOLER). (You can also perform a similar check for displacement (and rotation) convergence for your single DOF.) However, in a multi-DOF system, you might want to use a different method of comparison. The ANSYS program provides three different vector norms to use for convergence checking: •
The infinite norm repeats the single-DOF check at each DOF in your model.
•
The L1 norm compares the convergence criterion against the sum of the absolute values of force (and moment) imbalance for all DOFs.
•
The L2 norm performs the convergence check using the square root sum of the squares of the force (and moment) imbalances for all DOFs. (Of course, additional L1 or L2 checking can be performed for a displacement convergence check.)
Example For the following example, the substep will be considered to be converged if the out-of-balance force (checked at each DOF separately) is less than or equal to 5000*0.0005 (that is, 2.5), and if the change in displacements (checked as the square root sum of the squares) is less than or equal to 10*0.001 (that is, 0.01). CNVTOL,F,5000,0.0005,0 CNVTOL,U,10,0.001,2
8.5.2.3.3. Maximum Number of Equilibrium Iterations ANSYS' automatic solution control sets the value of NEQIT to between 15 and 26 iterations, depending upon the physics of the problem. The idea is to employ a small time step with fewer quadratically converging iterations. This option limits the maximum number of equilibrium iterations to be performed at each substep (default = 25 if solution control is off). If the convergence criteria have not been satisfied within this number of equilibrium iterations, and if auto time stepping is on [AUTOTS], the analysis will attempt to bisect. If bisection is not possible, then the analysis will either terminate or move on to the next load step, according to the instructions you issue in the NCNV command.
8.5.2.3.4. Predictor-Corrector Option ANSYS' automatic solution control will set PRED,ON if there are no beam or shell elements present. If the time step size is reduced greatly in the current substep, PRED is turned off. For transient analysis, the predictor is also turned off. You can activate a predictor on the DOF solution for the first equilibrium iteration of each substep. This feature accelerates convergence and is particularly useful if nonlinear response is relatively smooth. It is not so helpful
8–52
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.5: Performing a Nonlinear Static Analysis in analyses that incorporate large rotations or viscoelasticity. Using the predictor for large rotations can cause divergence and thus is not recommended for problems with large rotations.
8.5.2.3.5. Line Search Option ANSYS' automatic solution control will toggle line search on and off as needed. For most contact problems, LNSRCH is toggled on. For most non-contact problems, LNSRCH is toggled off. This convergence-enhancement tool multiplies the calculated displacement increment by a program-calculated scale factor (having a value between 0 and 1), whenever a stiffening response is detected. Because the line search algorithm is intended to be an alternative to the adaptive descent option [NROPT], adaptive descent is not automatically activated if the line search option is on. We do not recommend activating both line search and adaptive descent simultaneously. When an imposed displacement exists, a run cannot converge until at least one of the iterations has a line search value of 1. ANSYS scales the entire ∆U vector, including the imposed displacement value; otherwise, a "small" displacement would occur everywhere except at the imposed DOF. Until one of the iterations has a line search value of 1, ANSYS does not impose the full value of the displacement.
8.5.2.3.6. Cutback Criteria For finer control over bisections and cutback in time step size, use [CUTCONTROL, Lab, VALUE, Option]. By default, for Lab = PLSLIMIT (maximum plastic strain increment limit), VALUE is set to 15%. This field is set to such a large value for avoiding unnecessary bisections caused by high plastic strain due to a local singularity which is not normally of interest to the user. For explicit creep (Option = 0), Lab = CRPLIM (creep increment limit) and VALUE is set to 10%. This is a reasonable limit for creep analysis. For implicit creep (Option = 1), there is no maximum creep criteria by default. You can however, specify any creep ratio control. The number of points per cycle for second order dynamic equations (Lab = NPOINT) is set to VALUE = 13 by default to gain efficiency at little cost to accuracy.
8.5.3. Set Additional Solution Options This section discusses additional options that you can set for the solution. These options do not appear on the Solution Controls dialog box because they are used infrequently, and their default settings rarely need to be changed. ANSYS menu paths are provided in this section to help you access these options for those cases in which you choose to override the ANSYS-assigned defaults.
8.5.3.1. Advanced Analysis Options You Cannot Set on the Solution Controls Dialog Box The following sections describe some advanced analysis options that you can set for your analysis. As noted above in Section 8.5.3: Set Additional Solution Options, you cannot use the Solution Controls dialog box to set the options described below. Instead, you must set them using the standard set of ANSYS solution commands and the standard corresponding menu paths.
8.5.3.1.1. Stress Stiffness To account for buckling, bifurcation behavior, ANSYS includes stress stiffness in all geometrically nonlinear analyses. If you are confident of ignoring such effects, you can turn stress stiffening off (SSTIF,OFF). This command has no effect when used with several ANSYS elements; see the ANSYS Elements Reference for the description of the specific elements you are using. Command(s): SSTIF GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–53
Chapter 8: Nonlinear Structural Analysis
8.5.3.1.2. Newton-Raphson Option ANSYS' automatic solution control will use the FULL Newton-Raphson option with adaptive descent off if there is a nonlinearity present. However, when node-to-node, node-to-surface contact elements are used for contact analysis with friction, then adaptive descent is automatically turned on (for example, PIPE20, BEAM23, BEAM24, and PIPE60). The underlying contact elements require adaptive descent for convergence. Command(s): NROPT GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options Use this option only in a nonlinear analysis. This option specifies how often the tangent matrix is updated during solution. If you choose to override the default, you can specify one of these values: •
Program-chosen (NROPT,AUTO): The program chooses which of the options to use, based on the kinds of nonlinearities present in your model. Adaptive descent will be automatically activated, when appropriate.
•
Full (NROPT,FULL): The program uses the full Newton-Raphson procedure, in which the stiffness matrix is updated at every equilibrium iteration. If adaptive descent is on (optional), the program will use the tangent stiffness matrix only as long as the iterations remain stable (that is, as long as the residual decreases, and no negative main diagonal pivot occurs). If divergent trends are detected on an iteration, the program discards the divergent iteration and restarts the solution, using a weighted combination of the secant and tangent stiffness matrices. When the iterations return to a convergent pattern, the program will resume using the tangent stiffness matrix. Activating adaptive descent will usually enhance the program's ability to obtain converged solutions for complicated nonlinear problems but is supported only for elements indicated under "Special Features" in the Input Summary table (Table 4.n.1 for an element, where n is the element number) in the ANSYS Elements Reference.
•
Modified (NROPT,MODI): The program uses the modified Newton-Raphson technique, in which the tangent stiffness matrix is updated at each substep. The matrix is not changed during equilibrium iterations at a substep. This option is not applicable to large deformation analyses. Adaptive descent is not available.
•
Initial Stiffness (NROPT,INIT): The program uses the initial stiffness matrix in every equilibrium iteration. This option can be less likely to diverge than the full option, but it often requires more iterations to achieve convergence. It is not applicable to large deformation analyses. Adaptive descent is not available.
•
Full with unsymmetric matrix (NROPT,UNSYM): The program uses the full Newton-Raphson procedure, in which the stiffness matrix is updated at every equilibrium iteration. In addition, it generates and uses unsymmetric matrices that you can use for any of the following: –
If you are running a pressure-driven collapse analysis, an unsymmetric pressure load stiffness might be helpful in obtaining convergence. You can include pressure load stiffness using SOLCONTROL,INCP.
–
If you are defining an unsymmetric material model using TB,USER, you would need NROPT,UNSYM to fully use the property you defined.
–
If you are running a contact analysis, an unsymmetric contact stiffness matrix would fully couple the sliding and the normal stiffnesses. See Section 11.4.8.4: Determining Contact Stiffness and Allowable Penetration in this manual for details.
You should first try NROPT,FULL; then try NROPT,UNSYM if you experience convergence difficulties. Note that using an unsymmetric solver requires more computer time to obtain a solution, than if you use a symmetric solver. •
8–54
If a multistatus element is in the model, however, it would be updated at the iteration in which it changes status, irrespective of the Newton-Raphson option.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.5: Performing a Nonlinear Static Analysis
8.5.3.2. Advanced Load Step Options You Cannot Set on the Solution Controls Dialog Box The following sections describe some advanced load step options that you can set for your analysis. As noted above in Section 8.5.3: Set Additional Solution Options, you cannot use the Solution Controls dialog box to set the options described below. Instead, you must set them using the standard set of ANSYS solution commands and the standard corresponding menu paths.
8.5.3.2.1. Creep Criteria If your structure exhibits creep behavior, you can specify a creep criterion for automatic time step adjustment [CRPLIM,CRCR, Option]. (If automatic time stepping [AUTOTS] is off, this creep criterion will have no effect.) The program will compute the ratio of creep strain increment (∆εcr, the change in creep strain in the last time step) to the elastic strain (εel), for all elements. If the maximum ratio is greater than the criterion CRCR, the program will then decrease the next time step size; if it is less, the program might increase the next time step size. (The program will also base automatic time stepping on the number of equilibrium iterations, impending element status change, and plastic strain increment. The time step size will be adjusted to the minimum size calculated for any of these items.) For explicit creep (Option = 0), if the ratio ∆εcr / εel is above the stability limit of 0.25, and if the time increment cannot be decreased, a divergent solution is possible and the analysis will be terminated with an error message. This problem can be avoided by making the minimum time step size sufficiently small [DELTIM and NSUBST]. For implicit creep (Option = 1), there is no maximum creep limit by default. You can however, specify any creep ratio control. Command(s): CRPLIM GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Creep Criterion Note — If you do not want to include the effects of creep in your analysis, use the RATE command with Option = OFF, or set the time steps to be longer than the previous time step, but not more than 1.0e-6 longer.
8.5.3.2.2. Time Step Open Control This option is available for thermal analysis. (Remember that you cannot perform a thermal analysis using the Solution Controls dialog box; you must use the standard set of ANSYS solution commands or the standard corresponding menu paths instead.) This option's primary use is in unsteady state thermal analysis where the final temperature stage reaches a steady state. In such cases, the time step can be opened quickly. The default is that if the TEMP increment is smaller than 0.1 in three (NUMSTEP = 3) contiguous substeps, the time step size can be "opened-up" (value = 0.1 by default). The time step size can then be opened continuously for greater solution efficiency. Command(s): OPNCONTROL GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Open Control
8.5.3.2.3. Solution Monitoring This option provides a facility to monitor a solution value at a specified node in a specified DOF. The command also provides the user with a means to quickly review the solution convergence efficiency, rather than attempting to gather this information from a lengthy output file. For instance, if an excessive number of attempts were made for a substep, the information contained in the file provides hints to either reduce the initial time step size or increase the minimum number of substeps allowed through the NSUBST command to avoid an excessive number of bisections. Command(s): MONITOR GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Monitor
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–55
Chapter 8: Nonlinear Structural Analysis
8.5.3.2.4. Birth and Death Specify birth and death options as necessary. You can deactivate [EKILL] and reactivate [EALIVE] selected elements to model the removal or addition of material in your structure. As an alternative to the standard birth and death method, you can change the material properties for selected elements [MPCHG] between load steps. Command(s): EKILL, EALIVE GUI: Main Menu> Solution> Load Step Opts> Other> Birth & Death> Kill Elements Main Menu> Solution> Load Step Opts> Other> Birth & Death> Activate Elem The program “deactivates” an element by multiplying its stiffness by a very small number (which is set by the ESTIF command), and by removing its mass from the overall mass matrix. Element loads (pressure, heat flux, thermal strains, and so on) for inactive elements are also set to zero. You need to define all possible elements during preprocessing; you cannot create new elements in SOLUTION. Those elements to be “born” in later stages of your analysis should be deactivated before the first load step, and then reactivated at the beginning of the appropriate load step. When elements are reactivated, they have a zero strain state, and (if NLGEOM,ON) their geometric configuration (length, area, and so on) is updated to match the current displaced positions of their nodes. See the ANSYS Advanced Analysis Techniques Guide for more information on birth and death. Another way to affect element behavior during solution is to change the material property reference number for selected elements: Command(s): MPCHG GUI: Main Menu> Solution> Load Step Opts> Other> Change Mat Props> Change Mat Num Note — Use MPCHG with caution. Changing material properties in a nonlinear analysis may produce unintended results, particularly if you change nonlinear [TB] material properties.
8.5.3.2.5. Output Control In addition to OUTRES, which you can set on the Solution Controls dialog box, there are several other output control options that you can set for an analysis: Command(s): OUTPR, ERESX GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Output Ctrls> Solu Printout Main Menu> Solution> Unabridged Menu> Load Step Opts> Output Ctrls> Integration Pt Printed output [OUTPR] includes any results data on the output file (Jobname.OUT). Extrapolation of results [ERESX] copies an element's integration point stress and elastic strain results to the nodes instead of extrapolating them, if nonlinear strains (plasticity, creep, swelling) are present in the element. The integration point nonlinear strains are always copied to the nodes. See Chapter 2, “Loading” in the ANSYS Basic Analysis Guide for more information on these options.
8.5.4. Apply the Loads Apply loads on the model. See Chapter 2, “Structural Static Analysis” in this guide and Chapter 2, “Loading” in the ANSYS Basic Analysis Guide for load information. Remember that inertia and point loads will maintain constant direction, but surface loads will "follow" the structure in a large-deformation analysis. You can apply complex boundary conditions by defining a one-dimensional table (TABLE type array parameter). See Section 2.3.4.2.1: Applying Loads Using TABLE Type Array Parameters in this guide for more information.
8–56
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.5: Performing a Nonlinear Static Analysis
8.5.5. Solve the Analysis You solve a nonlinear analysis using the same commands and procedure as you do in solving a linear static analysis. See Section 2.3.5: Solve the Analysis in Chapter 2, “Structural Static Analysis”. If you need to define multiple load steps, you must respecify time settings, load step options, and so on, and then save and solve for each of the additional load steps. Other methods for multiple load steps - the load step file method and the array parameter method - are described in the ANSYS Basic Analysis Guide.
8.5.6. Review the Results Results from a nonlinear static analysis consist mainly of displacements, stresses, strains, and reaction forces. You can review these results in POST1, the general postprocessor, or in POST26, the time-history postprocessor. Remember that in POST1, only one substep can be read in at a time, and that the results from that substep should have been written to Jobname.RST. (The load step option command OUTRES controls which substep results are stored on Jobname.RST.) A typical POST1 postprocessing sequence is described below.
8.5.6.1. Points to Remember •
To review results in POST1, the database must contain the same model for which the solution was calculated.
•
The results file (Jobname.RST) must be available.
8.5.6.2. Reviewing Results in POST1 1.
Verify from your output file (Jobname.OUT) whether or not the analysis converged at all load steps. •
If not, you probably will not want to postprocess the results, other than to determine why convergence failed.
•
If your solution converged, then continue postprocessing.
2.
Enter POST1. If your model is not currently in the database, issue RESUME. Command(s): /POST1 GUI: Main Menu> General Postproc
3.
Read in results for the desired load step and substep, which can be identified by load step and substep numbers or by time. (Note, however, that arc-length results should not be identified by time.) Command(s): SET GUI: Main Menu> General Postproc> Read Results> load step You can also use the SUBSET or APPEND commands to read in or merge results data for selected portions of the model only. The LIST argument on any of these commands lists the available solutions on the results file. You can also limit the amount of data written from the results file to the database through the INRES command. Additionally, you can use the ETABLE command to store result items for selected elements. See the individual command descriptions in the ANSYS Commands Reference for more information. Caution: If you specify a TIME value for which no results are available, the ANSYS program will perform a linear interpolation to calculate the results at that value of TIME. Realize that this interpolation will usually cause some loss of accuracy in a nonlinear analysis (see Figure 8.23: “Linear Interpolation of Nonlinear Results Can Introduce Some Error”). Thus, for a nonlinear analysis, you should usually postprocess at a TIME that corresponds exactly to the desired substep. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–57
Chapter 8: Nonlinear Structural Analysis
Figure 8.23 Linear Interpolation of Nonlinear Results Can Introduce Some Error
4.
Display the results using any of the following options: Option: Display Deformed Shape Command(s): PLDISP GUI: Main Menu> General Postproc> Plot Results> Deformed Shape In a large deformation analysis, you might prefer to use a true scale display [/DSCALE,,1]. Option: Contour Displays Command(s): PLNSOL or PLESOL GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu Use these options to display contours of stresses, strains, or any other applicable item. If you have adjacent elements with different material behavior (such as can occur with plastic or multilinear elastic material properties, with different material types, or with adjacent deactivated and activated elements), you should take care to avoid nodal stress averaging errors in your results. Selecting logic (described in the ANSYS Basic Analysis Guide) provides a means of avoiding such errors. The KUND field on PLNSOL and PLESOL gives you the option of overlaying the undeformed shape on the display. You can also contour element table data and line element data: Command(s): PLETAB, PLLS GUI: Main Menu> General Postproc> Element Table> Plot Element Table Main Menu> General Postproc> Plot Results> Contour Plot> Line Elem Res Use PLETAB to contour element table data and PLLS to contour line element data. Option: Tabular Listings Command(s): PRNSOL (nodal results) PRESOL (element-by-element results) PRRSOL (reaction data) PRETAB PRITER (substep summary data), and so on. NSORT ESORT GUI: Main Menu> General Postproc> List Results> Nodal Solution Main Menu> General Postproc> List Results> Element Solution Main Menu> General Postproc> List Results> Reaction Solution Use the NSORT and ESORT commands to sort the data before listing them.
8–58
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.6: Performing a Nonlinear Transient Analysis Other Capabilities Many other postprocessing functions - mapping results onto a path, report quality listings, and so on are available in POST1. See The General Postprocessor (POST1) in the ANSYS Basic Analysis Guide for details. Load case combinations usually are not valid for nonlinear analyses.
8.5.6.3. Reviewing Results in POST26 You can also review the load-history response of a nonlinear structure using POST26, the time-history postprocessor. Use POST26 to compare one ANSYS variable against another. For instance, you might graph the displacement at a node versus the corresponding level of applied load, or you might list the plastic strain at a node and the corresponding TIME value. A typical POST26 postprocessing sequence might follow these steps: 1.
Verify from your output file (Jobname.OUT) whether or not the analysis converged at all desired load steps. You should not base design decisions on unconverged results.
2.
If your solution converged, enter POST26. If your model is not currently in the database, issue RESUME. Command(s): /POST26 GUI: Main Menu> TimeHist Postpro
3.
Define the variables to be used in your postprocessing session. The SOLU command will cause various iteration and convergence parameters to be read into the database, where you can incorporate them into your postprocessing. Command(s): NSOL, ESOL, RFORCE GUI: Main Menu> TimeHist Postpro> Define Variables
4.
Graph or list the variables. Command(s): PLVAR (graph variables) PRVAR EXTREM (list variables) GUI: Main Menu> TimeHist Postpro> Graph Variables Main Menu> TimeHist Postpro> List Variables Main Menu> TimeHist Postpro> List Extremes
Other Capabilities Many other postprocessing functions are available in POST26. See Chapter 6, “The Time-History Postprocessor (POST26)” in the ANSYS Basic Analysis Guide for details. See the NLGEOM, SSTIF, NROPT, TIME, NSUBST, AUTOTS, KBC, CNVTOL, NEQIT, NCNV, PRED, OUTRES, and SOLU command descriptions for more information.
8.5.7. Terminating a Running Job; Restarting You can stop a nonlinear analysis by creating an "abort" file (Jobname.ABT). See Chapter 3, “Solution” in the ANSYS Basic Analysis Guide for details. The program will also stop upon successful completion of the solution, or if a convergence failure occurs. You can often restart an analysis if it successfully completed one or more iterations before it terminated. Restart procedures are covered in Section 3.16: Restarting an Analysis in the ANSYS Basic Analysis Guide.
8.6. Performing a Nonlinear Transient Analysis Many of the tasks that you need to perform in a nonlinear transient analysis are the same as (or similar to) those that you perform in nonlinear static analyses (described in Section 8.5: Performing a Nonlinear Static Analysis) and linear full transient dynamic analyses (described in Chapter 2, “Structural Static Analysis”). However, this section describes some additional considerations for performing a nonlinear transient analysis. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–59
Chapter 8: Nonlinear Structural Analysis Remember that the Solution Controls dialog box, which is the method described in Section 8.5: Performing a Nonlinear Static Analysis, cannot be used to set solution controls for a thermal analysis. Instead, you must use the standard set of ANSYS solution commands and the standard corresponding menu paths.
8.6.1. Build the Model This step is the same as for a nonlinear static analysis. However, if your analysis includes time-integration effects, be sure to include a value for mass density [MP,DENS]. If you want to, you can also define material-dependent structural damping [MP,DAMP].
8.6.2. Apply Loads and Obtain the Solution 1.
2.
Specify transient analysis type and define analysis options as you would for a nonlinear static analysis: •
New Analysis or Restart [ANTYPE]
•
Analysis Type: Transient [ANTYPE]
•
Large Deformation Effects [NLGEOM]
•
Large Displacement Transient (if using the Solution Controls dialog box to set analysis type)
Apply loads and specify load step options in the same manner as you would for a linear full transient dynamic analysis. A transient load history usually requires multiple load steps, with the first load step typically used to establish initial conditions (see the ANSYS Basic Analysis Guide). The general, nonlinear, birth and death, and output control options available for a nonlinear static analysis are also available for a nonlinear transient analysis. In a nonlinear transient analysis, time must be greater than zero. See Chapter 5, “Transient Dynamic Analysis” for procedures for defining nonzero initial conditions. For a nonlinear transient analysis, you must specify whether you want stepped or ramped loads [KBC]. See the ANSYS Basic Analysis Guide for further discussion about ramped vs. stepped loads. You can also specify dynamics options: alpha and beta damping, time integration effects, and transient integration parameters. Command(s): ALPHAD, BETAD, TIMINT, TINTP GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Transient Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Damping Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Time Integration An explanation of the dynamics options follows. •
Damping Rayleigh damping constants are defined using the constant mass [ALPHAD] and stiffness [BETAD] matrix multipliers. In a nonlinear analysis the stiffness may change drastically - do not use BETAD, except with care. See Section 5.10.3: Damping for details about damping.
•
Time Integration Effects [TIMINT] Time integration effects are ON by default in a transient analysis. For creep, viscoelasticity, viscoplasticity, or swelling, you should turn the time integration effects off (that is, use a static analysis). These
8–60
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.7: Sample Input for a Nonlinear Transient Analysis time-dependent effects are usually not included in dynamic analyses because the transient dynamic time step sizes are often too short for any significant amount of long-term deformation to occur. Except in kinematic (rigid-body motion) analyses, you will rarely need to adjust the transient integration parameters [TINTP], which provide numerical damping to the Newmark and HHT methods. (See your ANSYS, Inc. Theory Reference for more information about these parameters.) ANSYS' automatic solution control sets the defaults to a new time integration scheme for use by first order transient equations. This is typically used for unsteady state thermal problems where θ = 1.0 (set by SOLCONTROL, ON); this is the backward Euler scheme. It is unconditionally stable and more robust for highly nonlinear thermal problems such as phase changes. The oscillation limit tolerance defaults to 0.0, so that the response first order eigenvalues can be used to more precisely determine a new time step value. Note — If you are using the Solution Controls dialog box to set solution controls, you can access all of these options [ALPHAD, BETAD, KBC, TIMINT, TINTP, TRNOPT] on the Transient tab. 3.
Write load data for each load step to a load step file. Command(s): LSWRITE GUI: Main Menu> Solution> Load Step Opts> Write LS File
4.
Save a backup copy of the database to a named file. Command(s): SAVE GUI: Utility Menu> File> Save As
5.
Start solution calculations. Other methods for multiple load steps are described in Chapter 1, “Getting Started with ANSYS” in the ANSYS Basic Analysis Guide. Command(s): LSSOLVE GUI: Main Menu> Solution> Solve> From LS Files
6.
After you have solved all load steps, leave SOLUTION. Command(s): FINISH GUI: Close the Solution menu.
8.6.3. Review the Results As in a nonlinear static analysis, you can use POST1 to postprocess results at a specific moment in time. Procedures are much the same as described previously for nonlinear static analyses. Again, you should verify that your solution has converged before you attempt to postprocess the results. Time-history postprocessing using POST26 is essentially the same for nonlinear as for linear transient analyses. See the postprocessing procedures outlined in Chapter 5, “Transient Dynamic Analysis”. More details of postprocessing procedures can be found in the ANSYS Basic Analysis Guide.
8.7. Sample Input for a Nonlinear Transient Analysis A sample input listing for a nonlinear transient analysis is shown below: ! Build the Model: /PREP7 --------FINISH !
! Similar to a linear full transient model, with ! these possible additions: nonlinear material ! properties, nonlinear elements
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–61
Chapter 8: Nonlinear Structural Analysis ! Apply Loads and Obtain the Solution: /SOLU ANTYPE,TRANS ! TRNOPT,FULL by default --! Establish initial conditions as in linear full --! transient analysis LSWRITE ! Initial-condition load step NLGEOM,ON ! Nonlinear geometric effects (large deformations) SSTIF,ON ! Stress stiffening effects ! NROPT=AUTO by default: Program will choose appropriate Newton-Raphson and ! Adaptive Descent options, depending on ! nonlinearities encountered ! Loads: F,... D,... ! Load Step Options: TIME,... ! TIME at end of load step DELTIM,... ! Time step controls (starting, min, max) AUTOTS,ON ! Automatic time stepping, including bisection ! KBC=0 by default (ramped loading) ! Dynamic Options: ALPHAD,... ! Mass damping TIMINT,ON ! TIMINT,ON by default, unless you turned it OFF for ! initial-condition load step ! Nonlinear Options: CNVTOL,... ! Convergence criteria ! NEQIT=25 by default NCNV,,,... ! Nonconvergence termination controls PRED,ON ! Predictor ON OUTRES,ALL,ALL ! Results for every substep written to database LSWRITE ! First "real" transient load step --! Additional load steps, as needed --LSSOLVE,1,3 ! Initiate multiple l.s. solution SAVE FINISH ! ! Review the Results: /POST26 ! Time-History Postprocessor SOLU,2,CNVG ! Check convergence SOLU,3,FOCV PRVAR,2,3 NSOL,... ! Store results (displacements, stresses, etc.) as ! variables PLVAR,... ! Graph results vs. TIME to evaluate general quality ! of analysis, determine critical time step, etc. FINISH ! /POST1 ! General Postprocessor SET,... ! Read results from desired time step PLDISP,... ! Postprocess as desired PLNSOL,... NSORT,... PRNSOL,... FINISH
See the ANTYPE, TRNOPT, LSWRITE, NLGEOM, SSTIF, NROPT, TIME, DELTIM, AUTOTS, KBC, ALPHAD, TIMINT, CNVTOL, NEQIT, NCNV, PRED, OUTRES, LSSOLVE, and SOLU command descriptions for more information.
8.8. Restarts Restart procedures for a transient analysis are essentially the same as for a static analysis; see Section 3.16: Restarting an Analysis in the ANSYS Basic Analysis Guide.
8–62
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.10: Tips and Guidelines for Nonlinear Analysis
8.9. Using Nonlinear (Changing-Status) Elements Nonlinear elements display an abrupt change in stiffness when they experience a change in status. For example, when a cable goes slack, its stiffness suddenly drops to zero. When two separate bodies come into contact, their overall stiffness changes drastically. These and other status-dependent stiffness changes can be modeled by using nonlinear elements (described below), by applying birth and death options to applicable elements (see the ANSYS Advanced Analysis Techniques Guide), or by changing material properties [MPCHG]. Some of the nonlinear element features described below are available only in the ANSYS Multiphysics, ANSYS Mechanical, and ANSYS Structural products only. See the ANSYS Elements Reference for details. •
COMBIN7
•
COMBIN14
•
COMBIN37
•
COMBIN39
•
COMBIN40
•
CONTAC12 and CONTAC52
•
TARGE169, TARGE170, CONTA171, CONTA172, CONTA173, CONTA174, and CONTA175
•
LINK10
•
SHELL41
•
SOLID65
8.9.1. Element Birth and Death Sometimes, an element's status changes between "existent" and "nonexistent." The birth and death options [EKILL, EALIVE, ESTIF] (Main Menu> Solution> Load Step Opts> Other) can be used to deactivate or reactivate selected elements in such cases. The birth and death feature is discussed in detail in Chapter 11, “Element Birth and Death” in the ANSYS Advanced Analysis Techniques Guide.
8.10. Tips and Guidelines for Nonlinear Analysis This section describes tips and guidelines that can help you to perform a nonlinear analysis.
8.10.1. Starting Out with Nonlinear Analysis By taking your time and proceeding with reasonable caution, you can avoid many difficulties commonly associated with nonlinear analyses. The following suggestions should be useful.
8.10.1.1. Be Aware of How the Program and Your Structure Behave If you have not used a particular nonlinear feature before, construct a very simple model (that is, containing only a few elements), and make sure you understand how to handle this feature before you use it in a large, complicated model. •
Gain preliminary insight into your structure's behavior by analyzing a preliminary simplified model first. For nonlinear static models, a preliminary linear static analysis can reveal which regions of your model will first experience nonlinear response, and at what load levels these nonlinearities will come into play. For nonlinear transient dynamic analyses, a preliminary model of beams, masses, and springs can provide insight into the structure's dynamics at minimal cost. Preliminary nonlinear static, linear transient dynamic,
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–63
Chapter 8: Nonlinear Structural Analysis and/or modal analyses can also help you to understand various aspects of your structure's nonlinear dynamic response before you undertake the final nonlinear transient dynamic analysis. •
Read and understand the program's output messages and warnings. At a minimum, before you try to postprocess your results, make sure your problem converged. For path-dependent problems, the printout's equilibrium iteration record can be especially important in helping you to determine if your results are valid or not.
8.10.1.2. Keep It Simple •
Keep your final model as simple as possible. If you can represent your 3-D structure as a 2-D plane stress, plane strain, or axisymmetric model, do so. If you can reduce your model size through the use of symmetry or antisymmetry surfaces, do so. (However, if your model is loaded antisymmetrically, you can generally not take advantage of antisymmetry to reduce a nonlinear model's size. Antisymmetry can also be rendered inapplicable by large deflections.) If you can omit a nonlinear detail without affecting results in critical regions of your model, do so.
•
Model transient dynamic loading in terms of static-equivalent loads whenever possible.
•
Consider substructuring the linear portions of your model to reduce the computational effort required for intermediate load or time increments and equilibrium iterations.
8.10.1.3. Use an Adequate Mesh Density •
Recognize that regions undergoing plastic deformation require a reasonable integration point density (mesh density is particularly important in plastic-hinge regions). Higher-order elements use only the corner integration points for nonlinear analyses, thus lower-order elements provide the same accuracy as higherorder elements. However, the 18x elements are recommended for nonlinear analyses.
•
Provide an adequate mesh density on contact surfaces to allow contact stresses to be distributed in a smooth fashion.
•
Provide a mesh density adequate for resolving stresses. Areas where stresses or strains are of interest require a relatively fine mesh compared to that needed for displacement or nonlinearity resolution.
•
Use a mesh density adequate to characterize the highest mode shape of interest. The number of elements needed depends on the elements' assumed displacement shape functions, as well as on the mode shape itself.
•
Use a mesh density adequate to resolve any transient dynamic wave propagation through your structure. If wave propagation is important, then provide at least 20 elements to resolve one wavelength.
8.10.1.4. Apply the Load Gradually •
For nonconservative, path-dependent systems, you need to apply the load in small enough increments to ensure that your analysis will closely follow the structure's load-response curve.
•
You can sometimes improve the convergence behavior of conservative systems by applying the load gradually, so as to minimize the number of Newton-Raphson equilibrium iterations required.
8.10.2. Overcoming Convergence Problems When performing a nonlinear analysis you may encounter convergence difficulties due to a number of reasons. Some examples may be initially open contact surfaces causing rigid body motion, large load increments causing nonconvergence, material instabilities, or large deformations causing mesh distortion that result in element shape errors. Solution control (SOLCONTROL) automatically adjusts solution parameters and attempts to obtain
8–64
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.10: Tips and Guidelines for Nonlinear Analysis a robust, accurate solution. In addition, several tools are available in ANSYS that can help you identify potential problems before, during, and after a solution. CHECK, MCHECK, and CNCHECK commands help you verify if there are any obvious problems with the model before you start the solution. The CHECK command does an overall verification of the model, including missing elastic properties, unconstrained model, and element shape checks. The MCHECK command can help you identify defects in the mesh such as holes or cracks, especially when the mesh is imported from a third party software. The CNCHECK command provides the initial contact status of contact pairs, identifying whether the contacts are initially open or closed. If, for example, a part in your model is constrained only through contact with other parts and if the contact surfaces are open, the CNCHECK command can help you identify this potential error condition. When you analyze models with large deformations, some portions of the initial mesh can become highly distorted. Highly distorted elements can take on unacceptable shapes, providing inaccurate results. This can cause your nonlinear solution to stop. When this happens, use the ESCHECK command to perform shape checking of deformed elements in the postprocessor (based on the current set of results in database). This deformed-shape checker will help you to identify the portions of your model that require different meshing, thereby allowing them to retain acceptable shapes. Using ESCHECK at different time points will help you to identify the load conditions that cause mesh deterioration. A convergence failure can also indicate a physical instability in the structure, or it can merely be the result of some numerical problem in the finite element model. The following sections detail some of the techniques that you can use to attempt to improve the convergence performance of your analysis.
8.10.2.1. Performing Nonlinear Diagnostics The nonlinear diagnostics tool NLDIAG can help you find problems in your model when an analysis will not converge. Identify Regions of High Residual Forces Issue the NLDIAG,NRRE command to write the Newton-Raphson residuals from equilibrium iterations to a file. You can then contour plot the residual forces via the PLNSOL,NRRE command, which will help to identify regions of high residual forces. Such a capability can be useful when you experience convergence difficulties in the middle of a load step, where the model has a large number of contact surfaces and other nonlinearities. You can restart the analysis and issue an NLDIAG,NRRE command to write out the residuals. By tracking the way the residuals change over several equilibrium iterations you can identify a portion of your model where large residuals persist. You can then focus on the nonlinearities in that area (for example, a contact pair's properties) instead of having to deal with the entire model. Identify Problem Elements
Typically, nonlinear analyses fail to converge for the following reasons:
•
Too large a distortion
•
Elements contain nodes that have near zero pivots (nonlinear analyses)
•
Too large a plastic or creep strain increment
•
Elements where mixed u-P constraints are not satisfied (mixed U-P option of 18x solid elements only)
ANSYS has default limits which, when exceeded, determine when convergence criteria have been violated. Some limits are user-controlled; for example, the CUTCONTROL command sets the maximum plastic/creep strain increments allowed in an iteration. Other limits are fixed.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–65
Chapter 8: Nonlinear Structural Analysis The NLDIAG,EFLG command identifies elements that violate the above criteria and records them in a file (Jobname.ndxxx). Process the Tracked Results Issue the NLDPOST command to process the .ndxxx nonlinear diagnostics files. The command creates components of elements that violate a certain criterion for a particular equilibrium iteration (or iterations). Monitor the Diagnostics Results in Real Time The NLHIST command allows you to monitor results of interest in real time during solution. Before starting the solution, you can request nodal data such as displacements or reaction forces at specific nodes. You can also request element nodal data such as stresses and strains at specific elements to be graphed. Pair-based contact data are also available. The result data are written to a file named Jobname.nlh. For example, a reaction force-deflection curve could indicate when possible buckling behavior occurs. Nodal results and contact results are monitored at every converged substep while element nodal data are written as specified via the OUTRES setting. You can also track results during batch runs. Either access the ANSYS Launcher and select File Tracking from the Tools menu, or type nlhist81 at the command line. Use the supplied file browser to navigate to your Jobname.nlh file, and click on it to invoke the tracking utilty. You can use this utilty to read the file at any time, even after the solution is complete (the data in the file must be formatted correctly).
8.10.2.2. Tracking Convergence Graphically As a nonlinear structural analysis proceeds, ANSYS computes convergence norms with corresponding convergence criteria each equilibrium iteration. Available in both batch and interactive sessions, the Graphical Solution Tracking (GST) feature displays the computed convergence norms and criteria while the solution is in process. By default, GST is ON for interactive sessions and OFF for batch runs. To turn GST on or off, use either of the following: Command(s): /GST GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> Grph Solu Track Figure 8.24: “Convergence Norms Displayed By the Graphical Solution Tracking (GST) Feature” shows a typical GST display:
8–66
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.10: Tips and Guidelines for Nonlinear Analysis
Figure 8.24 Convergence Norms Displayed By the Graphical Solution Tracking (GST) Feature
8.10.2.3. Using Automatic Time Stepping •
•
Be sure to place an upper limit on the time step size using DELTIM or NSUBST, especially for complicated models. This ensures that all of the modes and behaviors of interest will be accurately included. This can be important in the following situations: –
Problems that have only localized dynamic behavior (for example, turbine blade and hub assemblies) in which the low-frequency energy content of the system could dominate the high-frequency areas.
–
Problems with short ramp times on some of their loads. If the time step size is allowed to become too large, ramped portions of the load history may be inaccurately characterized.
–
Problems that include structures that are continuously excited over a range of frequencies (for example, seismic problems).
Take care when modeling kinematic structures (systems with rigid-body motions). These guidelines can usually help you obtain a good solution: –
Incorporate significant numerical damping (0.05 < γ < 0.1 on the TINTP command) into the solution to filter out the high frequency noise, especially if a coarse time step is used. Do not use α-damping (mass matrix multiplier, ALPHAD command) in a dynamic kinematic analysis, as it will dampen the rigid body motion (zero frequency mode) of the system.
– Avoid imposed displacement history specifications, because imposed displacement input has (theoretically) infinite jumps in acceleration, which causes stability problems for the Newmark time-integration algorithm. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–67
Chapter 8: Nonlinear Structural Analysis
8.10.2.4. Using Line Search Line search [LNSRCH] can be useful for enhancing convergence, but it can be expensive (especially with plasticity). You might consider setting line search on in the following cases: •
When your structure is force-loaded (as opposed to displacement-controlled).
•
If you are analyzing a "flimsy" structure which exhibits increasing stiffness (such as a fishing pole).
•
If you notice (from the program output messages) oscillatory convergence patterns.
8.10.2.5. Using the Arc-Length Method You can use the arc-length method [ARCLEN and ARCTRM] to obtain numerically stable solutions for many physically unstable structures. When using the arc-length method, please keep in mind the following considerations: •
The arc-length method is restricted to static analyses with proportional (ramped) loads only.
•
The program calculates the reference arc-length radius from the load (or displacement) increment of the first iteration of the first substep, using the following formula:
Reference Arc -Length Radius =
(Total Load or Displacement) NSB BSTP
where NSBSTP is the number of substeps specified in the NSUBST command. When choosing the number of substeps, consider that more substeps will result in a longer solution time. Ideally, you want to choose the minimum number of substeps required to produce an optimally efficient solution. You might have to take an "educated guess" of the desired number of substeps, and adjust and re-analyze as needed. •
Do not use line search [LNSRCH], the predictor [PRED], adaptive descent [NROPT,,,ON], automatic time stepping [AUTOTS, TIME, DELTIM], or time-integration effects [TIMINT] when the arc-length method is active.
•
Do not attempt to base convergence on displacement [CNVTOL,U]. Use the force criteria [CNVTOL,F] instead.
•
To help minimize solution time with the arc-length method, the maximum number of equilibrium iterations in a single substep [NEQIT] should be less than or equal to 15.
•
If an arc-length solution fails to converge within the prescribed maximum number of iterations [NEQIT], the program will automatically bisect and continue the analysis. Bisection will continue either until a converged solution is obtained, or until the minimum arc-length radius is used (the minimum radius is defined by NSBSTP [NSUBST] and MINARC [ARCLEN]).
•
In general, you cannot use this method to obtain a solution at a specified load or displacement value because the value changes (along the spherical arc) as equilibrium is achieved. Note in Figure 8.4: “Traditional Newton-Raphson Method vs. Arc-Length Method” how the specified load point. The actual load at convergence is somewhat less.
•
8–68
F1a
is only used as a starting
Similarly, it can be difficult to determine a value of limiting load or deflection within some known tolerance when using the arc-length method in a nonlinear buckling analysis. You generally have to adjust the reference arc-length radius (using NSUBST) by trial-and-error to obtain a solution at the limit point. It might
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.10: Tips and Guidelines for Nonlinear Analysis be more convenient to use standard Newton-Raphson iterations with bisection [AUTOTS] to determine values of nonlinear buckling loads. •
You should usually avoid using the JCG solver [EQSLV] in conjunction with the arc-length method, because the arc-length procedure might result in a negative definite stiffness matrix (negative pivot), which can cause a solution failure with this solver.
•
You can freely switch from the Newton-Raphson iteration method to the arc-length method at the start of any load step. However, to switch from arc-length to Newton-Raphson iterations, you must terminate the analysis and restart, deactivating the arc-length method in the first load step of the restart [ARCLEN,OFF]. An arc-length solution terminates under these conditions: – When limits defined by the ARCTRM or NCNV commands are reached – When the solution converges at the applied load – When you use an abort file (Jobname.ABT) See the ANSYS Basic Analysis Guide for a discussion of termination and restart procedures.
•
Use the load-deflection curve as a guide for evaluating and adjusting your analysis to help you achieve the desired results. It is usually good practice to graph your load-deflection curve (using POST26 commands) with every analysis.
•
Often, an unsuccessful arc-length analysis can be traced to an arc-length radius that is either too large or too small. "Drifting back," in which the analysis retraces its steps back along the load-deflection curve, is one typical difficulty that is caused by using too large or too small an arc-length radius. Study the loaddeflection curve to understand this problem. You can then use the NSUBST and ARCLEN commands to adjust the arc-length radius size and range, as appropriate.
•
The total arc-length load factor (item ALLF on the SOLU command) can be either positive or negative. Similarly, TIME, which in an arc-length analysis is related to the total arc-length load factor, can also be either positive or negative. Negative values of ALLF or TIME indicate that the arc-length feature is applying load in the reverse direction, in order to maintain stability in the structure. Negative ALLF or TIME values can be commonly encountered in various snap-through analyses.
•
When reading arc-length results into the database for POST1 postprocessing [SET], you should always reference the desired results data set by its load step and substep number (LSTEP and SBSTEP) or by its data set number (NSET). Do not reference results by a TIME value, because TIME in an arc-length analysis is not always monotonically increasing. (A single value of TIME might reference more than one solution.) Additionally, the program cannot correctly interpret negative TIME values (which might be encountered in a snap-through analysis).
•
If TIME becomes negative, remember to define an appropriate variable range [/XRANGE or /YRANGE] before creating any POST26 graphs.
8.10.2.6. Artificially Inhibit Divergence in Your Model's Response If you do not want to use the arc-length method to analyze a force-loaded structure that starts at, or passes through, a singular (zero stiffness) configuration, you can sometimes use other techniques to artificially inhibit divergence in your model's response: •
In some cases, you can use imposed displacements instead of applied forces. This approach can be used to start a static analysis closer to the equilibrium position, or to control displacements through periods of unstable response (for example, snap-through or postbuckling).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–69
Chapter 8: Nonlinear Structural Analysis •
Another technique that can be effective in circumventing problems due to initial instability is running a static problem as a "slow dynamic" analysis (that is, using time-integration effects in an attempt to prevent the solution from diverging in any one load step).
•
You can also apply temporary artificial stiffness to unstable DOFs, using control elements (such as COMBIN37), or using the birth and death option on other elements. The idea here is to artificially restrain the system during intermediate load steps in order to prevent unrealistically large displacements from being calculated. As the system displaces into a stable configuration, the artificial stiffness is removed.
8.10.2.7. Turn Off Extra Element Shapes ANSYS provides "incompatible" modes" formulation (also referred to as "extra shapes") for modeling bending applications. If your problem is predominantly bulk deformation, then you may choose to turn extra shapes off to reduce CPU/storage requirements and enhance convergence. However, doing so precludes the ability to model any bending.
8.10.2.8. Using Birth and Death Wisely Realize that any sudden change in your structure's stiffness matrix is likely to cause convergence problems. When activating or deactivating elements, try to spread the changes out over a number of substeps. (Use a small time step size if necessary to accomplish this.) Also be aware of possible singularities (such as sharp reentrant corners) that might be created as you activate or deactivate elements. Such singularities can cause convergence problems.
8.10.2.9. Read Your Output Remember that the ANSYS program performs a nonlinear analysis as a series of linear approximations with corrections. The program printout gives you continuous feedback on the progress of these approximations and corrections. (Printout either appears directly on your screen, is captured on Jobname.OUT, or is written to some other file [/OUTPUT].) You can examine some of this same information in POST1, using the PRITER command, or in POST26, using the SOLU and PRVAR commands. You should make sure that you understand the iteration history of your analysis before you accept the results. In particular, do not dismiss any program error or warning statements without fully understanding their meaning. A typical nonlinear output listing is shown in Figure 8.25: “Typical Nonlinear Output Listing”.
Figure 8.25 Typical Nonlinear Output Listing SOLVE command echo
*****
Checking Logic
*** NOTE *** CP= 13.891 TIME= 11:09:22 Nonlinear analysis, NROPT set to 1 (full Newton-Raphson solution procedure) for all DOFs.
Load step summary table
8–70
ANSYS SOLVE
COMMAND
L O A D
*****
S T E P
O P T I O N S
LOAD STEP NUMBER. . . . . . . . . . . . . TIME AT END OF THE LOAD STEP. . . . . . . AUTOMATIC TIME STEPPING . . . . . . . . . INITIAL NUMBER OF SUBSTEPS . . . . . . MAXIMUM NUMBER OF SUBSTEPS . . . . . . MINIMUM NUMBER OF SUBSTEPS . . . . . . MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS. STEP CHANGE BOUNDARY CONDITIONS . . . . . TERMINATE ANALYSIS IF NOT CONVERGED . . . CONVERGENCE CONTROLS. . . . . . . . . . . PRINT OUTPUT CONTROLS . . . . . . . . . . DATABASE OUTPUT CONTROLS ITEM FREQUENCY COMPONENT BASI -10
. . . . . . . . . . .
. . . . . . . . . . .
. 2 . 200.00 . ON . 100 . 10000 . 10 . 15 . NO .YES (EXIT) .USE DEFAULTS .NO PRINTOUT
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.11: Sample Nonlinear Analysis (GUI Method) Load step 2 substep 1
FORCE CONVERGENCE VALUE = 0.2006E+06 CRITERION= 1125. EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1272E-01 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.1272E-01 FORCE CONVERGENCE VALUE = 4267. CRITERION= 480.2 EQUIL ITER 2 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.9019E-03 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = -0.9019E-03 FORCE CONVERGENCE VALUE = 1751. CRITERION= 488.2 EQUIL ITER 3 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1746E-03 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.1746E-03 FORCE CONVERGENCE VALUE = 778.5 CRITERION= 497.7 EQUIL ITER 4 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.6943E-04 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.6943E-04 FORCE CONVERGENCE VALUE = 347.4 CRITERION= 507.7 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 4 *** LOAD STEP 2 SUBSTEP 1 COMPLETED. CUM ITER = 7 *** TIME = 101.000 TIME INC = 1.00000
Load step 2 substep 2
FORCE CONVERGENCE VALUE = 0.6674E+05 CRITERION= 594.3 EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.4318E-02 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.4318E-02 FORCE CONVERGENCE VALUE = 626.2 CRITERION= 502.9 EQUIL ITER 2 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.8570E-04 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.8570E-04 FORCE CONVERGENCE VALUE = 77.87 CRITERION= 512.9 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 2 *** LOAD STEP 2 SUBSTEP 2 COMPLETED. CUM ITER = 9 *** TIME = 102.000 TIME INC = 1.00000
Load step 2 substep 3 Equilbrium iteration summaries
FORCE CONVERGENCE VALUE = 0.1333E+05 CRITERION= 575.4 EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.5329E-02 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = -0.5329E-02 FORCE CONVERGENCE VALUE = 8237. CRITERION= 534.2 EQUIL ITER 2 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.3628E-02 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.3628E-02 FORCE CONVERGENCE VALUE = 3905. CRITERION= 532.9 EQUIL ITER 3 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1451E-02 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.1451E-02 FORCE CONVERGENCE VALUE = 1135. CRITERION= 540.3 EQUIL ITER 4 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1034E-03 LINE SEARCH PARAMETER = 0.9578 SCALED MAX DOF INC = 0.9905E-04 FORCE CONVERGENCE VALUE = 41.95 CRITERION= 551.4 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 4
Substep summary
*** LOAD STEP 2 *** TIME = 103.500
SUBSTEP
3 COMPLETED. TIME INC = 1.50000
CUM ITER =
13
8.10.2.10. Graph the Load and Response History This verification technique may be considered to be a graphical combination of two other techniques: checking for reasonableness, and reviewing the iteration history. POST26 graphs of load and response histories should agree with your informed expectations about your structure's behavior. The results of interest (displacements, reaction forces, stresses, and so on) should show relatively smooth response histories. Any non-smoothness may indicate that too coarse of a time step was used.
8.11. Sample Nonlinear Analysis (GUI Method) In this sample analysis, you will run a nonlinear analysis of an elastic-plastic circular plate under the action of a dead load and a cyclic point load. You will define a kinematic hardening plasticity curve, as well as load step options, the maximum and minimum number of substeps for a load step, and the various load steps that describe externally applied loads. You will also learn how to interpret the monitor file that ANSYS writes for a nonlinear analysis.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–71
Chapter 8: Nonlinear Structural Analysis ANSYS uses an incremental solution procedure to obtain a solution to a nonlinear analysis. In this example, the total external load within a load step is applied in increments over a certain number of substeps. As described earlier in this chapter, ANSYS uses a Newton-Raphson iterative procedure to solve each substep. You must specify the number of substeps for each load step, since this number controls the size of the initial load increment applied in the first substep of the each load step. ANSYS automatically determines the size of the load increment for each subsequent substep in a load step. You can control the size of the load increment for these subsequent substeps by specifying the maximum and minimum number of substeps. If you define the number of substeps, the maximum and minimum number of substeps all to be the same, then ANSYS uses a constant load increment for all substeps within the load step.
8.11.1. Problem Description In this example, you will use an axisymmetric model for the plate, using four-node PLANE42 elements with the axisymmetric option to mesh the model. You will perform a geometrically nonlinear analysis. Specify the kinematic constraints as follows: The nodes located at the center of the plate are constrained to have zero radial displacement. The nodes located at the outer edge are constrained to have zero radial and axial displacement. You will apply the dead load in load step 1 and the cyclic point load in six subsequent load steps. See Section 8.11.3: Problem Sketch. You will specify 10 substeps for the first load to ensure that the increment of the dead load applied over the first substep is 1/10 of the total load of 0.125 N/m2. You will also specify a maximum of 50 and a minimum of 5 substeps to ensure that if the plate exhibits a severe nonlinear behavior during the solution, then the load increment can be cut back to 1/50 the total load. If the plate exhibits mild nonlinear behavior, then the load increment can be increased up to 1/5 the size of the total load. For the subsequent six load steps that apply the cyclic point load, you will specify 4 substeps, with a maximum of 25 and a minimum of 2 substeps. For this example, you will monitor the history over the entire solution of the vertical displacement of the node at the location where the point cyclic load is applied and the reaction force at the node located at the bottom of the clamped edge.
8.11.2. Problem Specifications The circular plate has a radius of 1.0 m and a thickness of 0.1 m. The following material properties are used for this problem: EX = 16911.23 Pa PRXY = 0.3 The kinematic hardening plasticity curve for the material is: Log Strain
True Stress (Pa)
0.001123514
19.00
0.001865643
22.80
0.002562402
25.08
0.004471788
29.07
0.006422389
31.73
The plate has a dead load acting as a uniform pressure of 0.125N/m2. The history of the cyclic point load is shown here: 8–72
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.11: Sample Nonlinear Analysis (GUI Method)
Figure 8.26 Cyclic Point Load History
8.11.3. Problem Sketch 23 45563 4 ,7./ 098:1; <%=
!" # !%$&'# ()" &*+-,-.'/ .0..'1
" *><$ 4 +
8.11.3.1. Set the Analysis Title and Jobname 1.
Choose menu path Utility Menu> File> Change Title.
2.
Type the text "Cyclic loading of a fixed circular plate."
3.
Click on OK.
4.
Choose menu path Utility Menu> File> Change Jobname. The Change Jobname dialog box appears.
5.
Type the text “axplate” in the entry box and click OK.
8.11.3.2. Define the Element Types 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
In the list on the left, click once on "Structural Solid."
4.
In the list on the right, click once on "Quad 4node 42."
5.
Click on OK. The Library of Element Types dialog box closes.
6.
Click on Options. The PLANE42 element type options dialog box appears.
7.
In the scroll box for element behavior, scroll to "Axisymmetric" and select it.
8.
Click on OK.
9.
Click on Close in the Element Types dialog box.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–73
Chapter 8: Nonlinear Structural Analysis
8.11.3.3. Define Material Properties 1.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
2.
In the Material Models Available window, double-click on the icons next to the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
3.
Enter 16911.23 for EX (Young's modulus).
4.
Enter .3 for PRXY (Poisson's ratio).
5.
Click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
8.11.3.4. Specify the Kinematic Hardening material model (KINH) 1.
In the Material Models Available window, double-click on the following options: Nonlinear, Inelastic, Rate Independent, Kinematic Hardening Plasticity, von Mises Plasticity, Multilinear (General). A dialog box appears.
2.
Enter the following Strain/Stress value pair in the table: 0.00112, 19.0.
3.
Click on the Add Point button, and enter the next Strain/Stress value pair: 0.00187, 22.8.
4.
Repeat the previous step to enter the following Strain/Stress value pairs: 0.00256, 25.1; 0.00447, 29.1; 0.00642, 31.7.
5.
Click on OK.
6.
Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
8.11.3.5. Label Graph Axes and Plot Data Tables 1.
Choose menu path Utility Menu> PlotCtrls> Style> Graphs> Modify Axes. The Axes Modifications for Graph Plots dialog box appears.
2.
Enter Total Strain for the X-axis label.
3.
Enter True Stress for the Y-axis label and click OK.
4.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
5.
In the Material Models Defined window, double-click in Material Model Number 1, and Multilinear Kinematic (General). The dialog box appears that includes the Strain/Stress data pairs that you entered.
6.
Click on the Graph button. A graph of the data table values appears in the Graphics window. If necessary, revise the stress/strain values and click on the Graph button again. Repeat revisions and graphing as needed until you are satisfied with the graphed results. Click on OK.
7.
Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
8.
Click on SAVE_DB on the ANSYS Toolbar.
8.11.3.6. Create Rectangle 1.
Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.
2.
Type "radius=1.0" in the Selection field and click Accept. This value is the radius of the plate.
3.
Type "thick=0.1" in the Selection field and click Accept. This value is the thickness of the plate. Click Close.
8–74
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.11: Sample Nonlinear Analysis (GUI Method) 4.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Areas> Rectangle> By Dimensions. The Create Rectangle by Dimensions dialog box appears.
5.
Enter "0, radius" for X-coordinates.
6.
Enter "0, thick" for Y-coordinates and click on OK. A rectangle appears in the ANSYS Graphics window.
7.
Choose menu path Utility Menu> Plot> Lines.
8.11.3.7. Set Element Size 1.
Choose menu path Main Menu> Preprocessor> Meshing> MeshTool. The MeshTool dialog box appears.
2.
Click Size Controls> Lines> Set. The Element Size on Picked Lines picking menu appears. Click on the two vertical lines (2 and 4). Click OK on the picking menu. The Element Sizes on Picked Lines dialog box appears.
3.
Enter 8 for number of element divisions and click on OK.
4.
Repeat these steps (1-3), but choose horizontal lines 1 and 3, and specify 40 element divisions.
8.11.3.8. Mesh the Rectangle 1.
On the MeshTool, pick Quad and Map, then click MESH. The Mesh Areas picking menu appears.
2.
Click on Pick All.
3.
Click on SAVE_DB on the ANSYS Toolbar.
4.
Click on Close on the MeshTool.
8.11.3.9. Assign Analysis and Load Step Options 1.
Choose menu path Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options. The Static or Steady-State Analysis dialog box appears.
2.
Turn large deformation effects ON and click OK.
3.
Choose menu path Main Menu> Solution> Load Step Opts> Output Ctrls> DB/Results File. The Controls for Database and Results File Writing dialog box appears.
4.
Verify that All items are selected, and choose Every substep for the File write frequency. Click OK.
8.11.3.10. Monitor the Displacement In this step, you monitor the displacement of the node located at the axes of symmetry, as well as the reaction force at the fixed end of the plate. 1.
Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.
2.
Type "ntop = node(0,thick,0.0)" in the Selection field and click Accept.
3.
Type "nright = node(radius,0.0,0.0)" in the Selection field and click Accept, then Close.
4.
Choose menu path Main Menu> Solution> Load Step Opts> Nonlinear> Monitor. The Monitor picking menu appears.
5.
Type "ntop" in the picker and press RETURN. Click OK in the picking menu. The Monitor dialog box appears.
6.
In the scroll box for Quantity to be monitored, scroll to "UY" and select it. Click OK.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–75
Chapter 8: Nonlinear Structural Analysis 7.
Choose menu path Main Menu> Solution> Load Step Opts> Nonlinear> Monitor. The Monitor picking menu appears.
8.
Type "nright" in the picker and press RETURN. Click OK in the picking menu. The Monitor dialog box appears.
9.
In the scroll box for Variable to redefine, scroll to "Variable 2" and select it. In the scroll box for Quantity to be monitored, scroll to "FY" and select it. Click OK.
8.11.3.11. Apply Constraints 1.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears.
2.
Select Nodes and By Location in the first two selection boxes. Verify that X coordinates are selected, and enter "radius" in the Min, Max field. Click OK.
3.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears.
4.
Click Pick All. The Apply U,ROT on Nodes dialog box appears.
5.
Click on "All DOF" for DOFs to be constrained. Click OK.
6.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears. Verify that Nodes, By Location, and X coordinates are selected. Enter "0" in the Min, Max field and click OK. This will select the nodes at the X=0 position.
7.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears.
8.
Click Pick All. The Apply U,ROT on Nodes dialog box appears.
9.
Click on "UX" for DOFs to be constrained. Click on All DOF to deselect it.
10. Enter "0.0" as the Displacement value. Click OK. 11. Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears. Verify that Nodes and By Location are selected. 12. Click on Y coordinates and enter "thick" in the Min, Max field. Click OK. 13. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Pressure> On Nodes. The Apply PRES on Nodes picking menu appears. 14. Click on Pick All. The Apply PRES on nodes dialog box appears. 15. Enter "0.125" in the Load PRES value field and click OK. 16. Choose menu path Utility Menu> Select> Everything. 17. Click on SAVE_DB on the ANSYS Toolbar.
8.11.3.12. Solve the First Load Step 1.
Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Time and Substps. The Time and Substep Options dialog appears.
2.
Enter 10 as the number of substeps, enter 50 as the maximum number of substeps, and enter 5 as the minimum number of substeps. Click OK.
3.
Choose menu path Main Menu> Solution> Solve> Current LS. Review the information in the /STAT window, and click on Close.
4.
Click on OK on the Solve Current Load Step dialog box.
8–76
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.11: Sample Nonlinear Analysis (GUI Method) 5.
Click on Close on the Information dialog box when the solution is done.
6.
Choose Utility Menu> Plot> Elements.
8.11.3.13. Solve the Next Six Load Steps 1.
Choose Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.
2.
Enter "f = 0.010" in the Selection field and click on Accept. Click on Close.
3.
Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Time and Substps. The Time and Substep Options dialog appears.
4.
Enter "4" for the number of substeps, "25" for the maximum number of substeps, and "2" for the minimum number of substeps. Click OK.
5.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment> On Nodes. The Apply F/M on Nodes picking menu appears.
6.
Enter "ntop" in the picker and press RETURN. Click OK in the Apply F/M on Nodes picking menu. The Apply F/M on Nodes dialog box appears.
7.
Select "FY" in the Direction of force/mom selection box. Enter "-f" in the Force/moment value field. Click OK.
8.
Choose menu path Main Menu> Solution> Solve> Current LS. Review the information in the /STAT window, and click on Close.
9.
Click on OK on the Solve Current Load Step dialog box.
10. Click on Close on the Information dialog box when the solution is done. 11. Repeat Steps 5-10, entering "f" in the Force/moment value field at Step 7. 12. Repeat Steps 5-11 two more times, for a total of three cycles (six substeps). 13. Click on SAVE_DB on the ANSYS Toolbar.
8.11.3.14. Review the Monitor File 1.
Choose menu path Utility Menu> List> Files> Other. The List File dialog box appears. Select the axplate.mntr file and click on OK.
2.
Review the time step size, vertical displacement, and reaction force evolution over the entire solution.
3.
Click Close.
8.11.3.15. Use the General Postprocessor to Plot Results. 1.
Choose menu path Main Menu> General Postproc> Read Results> Last Set.
2.
Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears.
3.
Click on Def + undef edge for items to be plotted. Click OK. The deformed mesh appears in the ANSYS Graphics window.
4.
Choose menu path Main Menu> General Postproc> Plot Results> Contour Plot> Element Solu. The Contour Element Solution Data dialog box appears.
5.
In the selection box on the left, choose Strain-plastic. In the selection box on the right, choose Eqv plastic EPEQ. Click OK. The contour plot appears in the Graphics window.
6.
Choose Utility Menu> Plot> Elements. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–77
Chapter 8: Nonlinear Structural Analysis
8.11.3.16. Define Variables for Time-History Postprocessing 1.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears.
2.
Verify that Nodes and By Num/Pick are selected in the first two boxes. Click OK. The Select nodes picking menu appears.
3.
Type "ntop" in the picker and press RETURN. Click OK.
4.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears. Choose Elements in the first drop-down selection box. Choose Attached to in the second drop-down selection box. Verify that Nodes is selected. Click OK.
5.
Choose Utility Menu> Select> Everything.
6.
Choose Main Menu> TimeHist Postpro> Define Variables. The Defined Time-History Variables dialog box appears. Click on Add. The Add Time-History Variable dialog box appears.
7.
Click on Element results. Click OK. The Define Elemental Data picking menu appears.
8.
Click on the top left element in the ANSYS Graphics window. Click OK on the picking menu. The Define Nodal Data picking menu appears.
9.
Click on the top left node of the top left element. Click OK on the picking menu. The Define Element Results Variable dialog box appears.
10. Verify that the reference number of the variable is 2. 11. Choose Stress in the selection list on the left. Choose Y-direction SY in the selection list on the right. Click OK. The Defined Time-History Variables dialog box reappears, with a second variable listed (ESOL). The dialog box should show element number 281, node number 50, item S, component Y, and name SY. 12. Click on Add. Repeat steps 7-10, with variable reference number 3. 13. In the Define Element Results Variable dialog box, choose Strain-elastic in the selection list on the left. Choose Y-dir'n EPEL Y in the selection list on the right. Click OK. 14. Click on Add. Repeat steps 7-10, with variable reference number 4. 15. In the Define Element Results Variable dialog box, choose Strain-plastic in the selection list on the left. Choose Y-dir'n EPPL Y in the selection list on the right. Click OK. 16. Click on Close on the Defined Time-History Variables dialog box. 17. Choose menu path Main Menu> TimeHist Postpro> Math Operations> Add. The Add Time-History Variables dialog box appears. 18. Enter 5 for the reference number for result, enter 3 as the 1st variable, and enter 4 as the 2nd variable. Click OK. This adds the elastic and plastic strains that you stored as variables 3 and 4. Their sum is the total strain, and it is stored as variable 5.
8.11.3.17. Plot Time-History Results 1.
Choose menu path Main Menu> TimeHist Postpro> Settings> Graph. The Graph Settings dialog box appears.
2.
Click on Single variable for the X-axis variable and enter 5 as the single variable number. Click OK.
3.
Choose menu path Utility Menu> PlotCtrls> Style> Graphs> Modify Axes. The Axes Modifications for Graph Plots dialog box appears.
4.
Enter Total Y-Strain as the X-axis label.
5.
Enter Y-Stress as the Y-axis label. Click OK.
8–78
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.12: Sample Nonlinear Analysis (Command or Batch Method) 6.
Choose menu path Main Menu> TimeHist Postpro> Graph Variables. The Graph Time-History Variables dialog box appears.
7.
Enter 2 as the first variable to graph. Click OK.
8.11.3.18. Exit ANSYS 1.
Choose QUIT from the ANSYS Toolbar.
2.
Click on the save option you want, and click on OK.
8.12. Sample Nonlinear Analysis (Command or Batch Method) You can perform the example nonlinear static analysis of a copper cylinder impacting a rigid wall using the ANSYS commands shown below instead of GUI choices. Items prefaced by an exclamation point (!) are comments. /BATCH,LIST /title, Cyclic loading of a fixed circular plate /filnam,axplate /prep7 radius=1.0 ! Radius of the plate (m) thick=0.1 ! Thickness of plate (m) YM=16911.23 et,1,PLANE42,,,1 ! PLANE42 axisymmetric element mp,ex,1,YM mp,nuxy,1,0.3 ! Define a Kinematic Hardening Plasticity curve using the KINH material model tb,KINH,1,1,5 ! Define the true stress vs. total log strain curve for this material model ! using 5 points. First point defines the elastic limit tbpt,,0.001123514,19.00 tbpt,,0.001865643,22.80 tbpt,,0.002562402,25.08 tbpt,,0.004471788,29.07 tbpt,,0.006422389,31.73 ! Set the axles labels for the stress-strain curve plot /axlab,X,Log Strain (N/m^2) /axlab,Y,True Stress (N/m^2) tbpl,KINH,1
! Plot and verify the material stress-strain curve
! Define a rectangle which is the axisymmetric cross section of the plate. ! The rectangle has a length equal to the radius of the plate and a height equal ! to the thickness of the plate rect,,radius,,thick ! Select the left and right bounding lines of the created rectangle and set ! the line division to 8 (8 elements through the thickness of the plate) FLST,5,2,4,ORDE,2 FITEM,5,2 FITEM,5,4 CM,_Y,LINE LSEL, , , ,P51X !* CM,_Y1,LINE CMSEL,,_Y LESIZE,_Y1, , ,8,1, CMDEL,_Y CMDEL,_Y1 !*
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–79
Chapter 8: Nonlinear Structural Analysis
! Select the top and bottom bounding lines of the created rectangle and set ! the line division to 40 (40 elements through the radius of the plate) FLST,5,2,4,ORDE,2 FITEM,5,1 FITEM,5,3 CM,_Y,LINE LSEL, , , ,P51X !* CM,_Y1,LINE CMSEL,,_Y LESIZE,_Y1, , ,40,1, CMDEL,_Y CMDEL,_Y1 !* CM,_Y,AREA ASEL, , , , 1 CM,_Y1,AREA CHKMSH,'AREA' CMSEL,S,_Y amesh,all CMDEL,_Y CMDEL,_Y1 CMDEL,_Y2 fini /solve nlgeom,on! Turn on geometric nonlinearity ! Get the node numbers for the nodes located at the top ! of the axis of symmetry and at bottom right of the model ntop = node(0,thick,0) nright = node(radius,0,0) ! Activate the monitoring of the displacement and reaction force histories ! during the analysis. This will be written out to the monitor file ratch.mntr monitor,1,ntop,uy monitor,2,nright,fy outres,all,all
! Output all the results for all substeps to the ! results file for later postprocessing
! Select the nodes located at right end and constrain their radial (x) and ! axial (y) direction displacement to be zero. nsel,s,loc,x,radius d,all,all ! Select the nodes located at left end and constrain their radial (x) direction ! displacement to be zero. nsel,s,loc,x,0.0 d,all,ux,0.0 ! Define the load for Load Step 1. ! Select the nodes located at top surface of plate and apply a uniform pressure ! of 0.125 N/m^2 as dead load on the plate. nsel,s,loc,y,thick sf,all,pres,0.125 alls! Select all nodes ! Define the number of substeps (10). Also define maximum number of ! substeps (50), and the minimum number of substeps (5) for the automatic ! time stepping algorithm. nsub,10,50,5
8–80
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.12: Sample Nonlinear Analysis (Command or Batch Method) solve f = 0.01
! Solve load step 1 ! Define the parameter, f, used to apply ! the cyclic point load.
! Over six load steps apply a cyclic point load of magnitude f = 0.01 units ! applied at the center of the plate over three cycles ! Start Cycle 1 ! ---------------nsel,s,node,,ntop f,all,fy,-f nsel,all nsubst,4,25,2 solve nsel,s,node,,ntop f,all,fy,f nsel,all nsubst,4,25,2 solve
! Define load for load step 2 ! Set the number of substeps, max and min number ! of substeps ! Solve load step 2
! Define load for load step 3 ! Set the number of substeps, max and min number ! of substeps ! Solve load step 3
! Start Cycle 2 ! ---------------nsel,s,node,,ntop f,all,fy,-f nsel,all nsubst,4,25,2 solve nsel,s,node,,ntop f,all,fy,f nsel,all nsubst,4,25,2 solve
! Define load for load step 4 ! Set the number of substeps, max and min number ! of substeps ! Solve load step 4
! Define load for load step 5 ! Set the number of substeps, max and min number ! of substeps ! Solve load step 5
! Start Cycle 3 ! ---------------nsel,s,node,,ntop f,all,fy,-f nsel,all nsubst,4,25,2 solve nsel,s,node,,ntop f,all,fy,f nsel,all nsubst,4,25,2 solve save fini /post1 set,last ! (final state) pldi,2 ples,nl,epeq
! Define load for load step 6 ! Set the number of substeps, max and min number ! of substeps ! Solve load step 6 ! Define load for load step 7 ! Set the number of substeps, max and min number ! of substeps. ! Solve load step 7
! Read in the results from the last substep of ! the last step. ! ! ! !
Plot the deformed mesh with the undeformed edge only Plot the total accumulated equivalent plastic strains
fini /post26 eplo nsel,s,node,,ntop
! Plot the mesh ! Select the node where the point load is attached
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–81
Chapter 8: Nonlinear Structural Analysis esln elem=elnext(0) alls
! Select the element attached to this node ! Get the number of this element ! Select back everything in the model
! Define variable 2 to be Y component of stress at the node where the point ! load is applied ESOL,2,elem,ntop,S,Y,
! Define variable 3 to be Y component of elastic strain at the node where the ! point load is applied ESOL,3,elem,ntop,EPEL,Y, ! Define variable 4 to be Y component of plastic strain at the node where the ! point load is applied ESOL,4,elem,ntop,EPPL,Y, ! Add the elastic and plastic strains in variables 3 and 4 and store the total ! strain in variable 5. ADD,5,3,4, , , , ,1,1,0, xvar,5
! Set the axes for subsequent x-y plot to be variable 5
! Define the x and y axes labels for subsequent x-y plot /axlab,x,Total Y-Strain /axlab,y,Y-Stress plvar,2 fini /eof /exit,nosav
! Plot the Y-stress stored in variable 2
8.13. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional nonlinear analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS program. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual includes a variety of nonlinear analysis test cases: VM7 - Plastic Compression of a Pipe Assembly VM11 - Residual Stress Problem VM24 - Plastic Hinge in a Rectangular Beam VM38 - Plastic Loading of a Thick-Walled Cylinder Under Pressure VM56 - Hyperelastic Thick Cylinder Under Internal Pressure VM78 - Transverse Shear Stresses in a Cantilever Beam VM80 - Plastic Response to a Suddenly Applied Constant Force VM104 - Liquid-Solid Phase Change VM124 - Discharge of Water from a Reservoir VM126 - Heat Transferred to a Flowing Fluid VM132 - Stress Relaxation of a Bolt Due to Creep VM133 - Motion of a Rod Due to Irradiation Induced Creep VM134 - Plastic Bending of a Clamped I-Beam VM146 - Bending of a Reinforced Concrete Beam
8–82
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.13: Where to Find Other Examples VM185 - Current Carrying Ferromagnetic Conductor VM198 - Large Strain In-Plane Torsion Test VM199 - Viscoplastic Analysis of a Body Undergoing Shear Deformation VM200 - Viscoelastic Sandwich Seal Analysis VM218 - Hyperelastic Circular Plate VM220 - Eddy Current Loss in Thick Steel Plate
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–83
8–84
Chapter 9: Material Curve Fitting Use the ANSYS material curve fitting feature to evaluate experimental data for use as coefficients for certain nonlinear material models built into ANSYS. With this feature, you compare experimental stress data versus ANSYS-calculated stress data for different nonlinear models. Based on these comparisons, you decide which material model to use during solution. Curve fitting is based on the data table configurations outlined in the TB command. The data manipulations and constructions are performed by the TBFT command.
9.1. Applicable Material Behavior Types ANSYS supports Hyperelastic, Creep and Viscoelastic material behavior for Curve Fitting •
Section 9.2: Hyperelastic Material Curve Fitting For Hyperelastic material models, your stress-strain curves can be converted to any of the available ANSYSsupported hyperelastic models, including Mooney-Rivlin, Ogden, Neo-Hookean, Polynomial, Arruda-Boyce, Gent, and Yeoh. Compressible hyperelastic models Ogden hyper-foam and Blatz-Ko are also supported.
•
Section 9.3: Creep Material Curve Fitting For creep material models, your creep strain rate or creep strain as a function of time, stress or temperature can be converted to any of the thirteen ANSYS supported implicit creep models.
•
Section 9.4: Viscoelastic Material Curve Fitting For viscoelastic material models, your shear modulus vs time and/or bulk modulus vs. time data is converted to ANSYS supported Prony series format. Curve fitting for temperature dependency is supported using the SHIFT option.
9.2. Hyperelastic Material Curve Fitting Hyperelastic curve fitting is a tool for estimating the material constants for your material by inputting your experimental data and comparing it to the ANSYS supported hyperelastic material models. You perform curve fitting either through an interactive user interface or via batch commands. You input your experimental data, choose a model from one of nine hyperelastic models supplied, perform a regression analysis, graphically view the curve fitting results, compare the fits to the experimental data, and write the fitted coefficients as ANSYS nonlinear data table commands to the database for the subsequent finite elements analyses. ANSYS hyperelastic models can define three types of behavior: Purely Incompressible, Nearly Incompressible and Compressible. Curve fitting helps you estimate coefficients for these situations. Hyperelastic curve fitting is based on the HYPER option of the TB command.
9.2.1. Using Curve Fitting to Determine Your Hyperelastic Material Behavior The steps for Hyperelastic Curve Fitting are defined as follows: 1
Section 9.2.1.1: Prepare Experimental Data
The experimental data must be a plain text file delimited by a space or a comma.
2
Section 9.2.1.2: Input the Data into The experimental data can be read into ANSYS by browsing ANSYS to the file location in the GUI or by specifying the filename and path (batch) on the command line. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 9: Material Curve Fitting 3
Section 9.2.1.3: Select a Material Model Option
The material options for the applicable curve fitting regimen are defined in the TB command. Nine hyperelastic models are supported. Once you pick a model, you can still change to another model if an ideal fit is not realized.
4
Section 9.2.1.4: Initialize the Coeffi- Hyperelastic curve fitting can be a linear regression or a cients nonlinear regression process, depending on the model. The hyperelastic material models, and the associated process for each are listed in Table 9.3: “Hyperelastic Curve Fitting Model Types”.
5
Section 9.2.1.5: Specify Control Parameters and Solve
You will specify the type of error norm to be used to generate the curve fit.
6
Section 9.2.1.6: Plot Your Experimental Data and Analyze
You review and verify the results by comparing the experimental data and the regression errors. If the results you obtain are not acceptable repeat steps 3 to 5 to perform a new curve fitting solution.
7
Section 9.2.1.7: Write Data to TB Command
Write curve fitting results as the TB command to ANSYS database.
9.2.1.1. Prepare Experimental Data Curve fitting requires experimental test data. Your hyperelastic curve fitting data needs to be a comma or space delimited file, referencing your stress vs. strain values. Hyperelastic curve fitting does not support temperature dependent data. Hyperelastic curve-fitting supports three main behaviors: •
Case 1 - Totally Incompressible Models (see Table 9.1: “Experimental Details for Case 1 and 2 Models and Blatz-Ko”)
•
Case 2 - Nearly Incompressible Models (see Table 9.1: “Experimental Details for Case 1 and 2 Models and Blatz-Ko”)
•
Case 3 - Compressible Models (see Table 9.2: “Experimental Details for Case 3 Models”)
The types of data required for each of these cases is defined in the tables below.
Table 9.1 Experimental Details for Case 1 and 2 Models and Blatz-Ko Experimental Type
Column 1
Column 2
Uniaxial Test
Engineering Strain
Engineering Stress
Biaxial Test
Engineering Strain
Engineering Stress
Shear Test
Engineering Strain
Engineering Stress
Volumetric Test
Volumetric Strain(J)
True Stress
Table 9.2 Experimental Details for Case 3 Models Experimental Type
Column 1
Uniaxial Test
Longitudinal Engineering Lateral Direction Engineer- Engineering Stress Strain ing Strain
Biaxial Test
Biaxial Engineering Strain Thickness Direction Engin- Engineering Stress eering Strain
9–2
Column 2
Column 3
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.2: Hyperelastic Material Curve Fitting Experimental Type
Column 1
Column 2
Column 3
Shear Test
Shear Engineering Strain Thickness Direction Engin- Engineering Stress eering Strain
Volumetric Test
Volumetric Strain(J)
True Stress
Note — J is the ratio of current volume to the original volume. All stresses that ANSYS outputs in POST1/POST26 are true stresses and logarithmic strains.
9.2.1.2. Input the Data into ANSYS The EADD argument for the TBFT command determines how you input your data files. First you designate whether they are uniaxial, biaxial, shear or volumetric, and then you designate the location in the Option2, Option3, Option4 fields. All of the stress values will be engineering stress, except for the volumetric option (true stress). The file should be a simple, delimited set of stress and strain values similar to the following: 0.9703 0.9412 0.9127 0.8847
60.00 118.2 175.2 231.1
9.2.1.2.1. Batch TBFT,EADD,ID,Option1,Option2,Option3,Option4
Option1 = UNIA, BIAX, SHEA, or VOLU Option2 = name of file containing experimental data Option3 = file name extension Option4 = file directory
9.2.1.2.2. GUI The Material Properties GUI provides an input field where you can type the filename of your data file, and also include the appropriate path. You can also “Browse” to a file in a specified location. Separate input is performed for each Option1 value (UNIA, BIAX, SHEA, etc.).
9.2.1.3. Select a Material Model Option Table 9.3: “Hyperelastic Curve Fitting Model Types”, below lists the models that are available for hyperelastic curve fitting. When volumetric data is supplied, a compressible, or nearly incompressible model is implied, and only the available options will be available. When no volumetric data is supplied, the model is understood to be incompressible, and those model options will be available. Supplying zero coefficients for the volumetric data field will also denote an incompressible model.
Table 9.3 Hyperelastic Curve Fitting Model Types Model Name
Abbreviation
Order/Options
No. of Coefficients Linear/Nonlinear [1] Fitting
Mooney-Rivlin
moon
2, 3, 5, 9
2/3/5/9+1
Linear
Polynomial
poly
1 to N
see below [2]
Linear
Yeoh
yeoh
1 to N
N+N
Linear
Neo-Hookean
neoh
-
1+1
Linear
Ogden
ogde
1 to N
2*N+N
Nonlinear
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–3
Chapter 9: Material Curve Fitting Model Name
Abbreviation
Order/Options
No. of Coefficients Linear/Nonlinear [1] Fitting
Arruda-Boyce
boyc
-
2+1
Nonlinear
Gent
gent
-
2+1
Nonlinear
Blatz-Ko
blat
-
1
Nonlinear
1 to N
2*N+N
Nonlinear
Ogden Hyper-foam foam
1.
The number of coefficients is usually the sum of the number of deviatoric coefficients and the number of volumetric coefficients.
2.
The number of coefficients for a polynomial will be dependent on the polynomial order N. N
Number of Coefficients = ∑ (1 + i) + N i =1
Blatz-Ko and Ogden hyper-foam are compressible models. For Ogden hyper-foam, the experimental data you supply will require additional fields. More information on the hyperelastic models ANSYS supplies for curve fitting can be found in Section 2.5.2: Hyperelastic Material Constants.
9.2.1.3.1. Batch TBFT,FADD,ID,HYPER,Option2,Option3
Option2 = Model name, as specified in Table 9.3: “Hyperelastic Curve Fitting Model Types” (above). Option3 = Order or number of coefficients, where applicable. Table 9.3: “Hyperelastic Curve Fitting Model Types”
(above) specifies the number and type of coefficient(s) necessary for each hyperelastic model type.
9.2.1.3.2. GUI You can navigate to a pull-down selection menu in the material GUI to pick the applicable material model option. The options displayed will be dependent on the format of your experimental data file.
9.2.1.4. Initialize the Coefficients Depending on the model you choose, hyperelastic curve fitting can be a linear or a nonlinear regression process; the initial coefficients you supply will determine how accurate and efficient your curve fit will be. The initial values of the coefficients generally come from experience, and also from studying the function that defines the model you are attempting to compare/fit your data to. For most hyperelastic models, 1 or -1 is a good starting point. However, coefficient values can vary greatly depending on the model chosen. The Gent model, for instance, provides good fit with initial coefficient values as high as 1000. You can also fix (hold constant) your coefficients. You specify a value for a coefficient and keep it unchanged, while allowing the other coefficients to be operated on. You can then release the fixed coefficient later if desired. By default, all of the coefficients are free to vary.
9.2.1.4.1. Batch TBFT,SET,ID,HYPER,Option2,Option3,Option4,Option5
Option2 = Model name. See Table 9.3: “Hyperelastic Curve Fitting Model Types” (above) for the models available. Option3 = not applicable
9–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.2: Hyperelastic Material Curve Fitting Option4 = index of coefficient Option5 = entr “0” for variable, 1 for fixed.
9.2.1.4.2. GUI The GUI automatically updates your coefficient tables depending on the model you pick. You can modify these values to initialize them at values you believe more appropriate.
9.2.1.5. Specify Control Parameters and Solve Depending on the model, your hyperelastic curve fitting will be either a linear or nonlinear regression process (see Table 9.3: “Hyperelastic Curve Fitting Model Types” (above) for details). Your error norms can be either normalized and unnormalized. The normalized error norm is the default regression option. Normalized error norms generally give better results than the unnormalized error norms, since normalized error gives equal weight to all of your data points. The solution control parameters of a nonlinear regression include: 1.
number of iterations
2.
residual tolerance
3.
coefficient change tolerance
The solution stops when both residual tolerance of error norm and coefficient change tolerance is met or if the number of iterations criteria is met. Wherever nonlinear regression is used, you need to initialize your coefficients.
9.2.1.5.1. Batch TBFT,SOLVE,ID,HYPER,Option2,Option3,Option4, ..., Option7
Option2 = Model name. See Table 9.3: “Hyperelastic Curve Fitting Model Types” (above) for the models available. Option3 = The order or number of your coefficients. See Table 9.3: “Hyperelastic Curve Fitting Model Types”
(above) for possible values. Option4 = curve fitting procedure: 0 = unnormalized least squares, 1 = normalized least squares Option5 = maximum number of iterations Option6 = tolerance of residual changes Option7 = tolerance of coefficient changes
Other solution parameters are available. See the TBFT command for details.
9.2.1.5.2. GUI The GUI lets you specify all of your control parameters (error norm, solution control parameters, and the solver options) interactively. Select the options and Solve to generate the coefficients. Change the parameters and repeat the solution as necessary to ensure the accuracy of the results. The unused options are disabled whenever necessary.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–5
Chapter 9: Material Curve Fitting
9.2.1.6. Plot Your Experimental Data and Analyze After you initiate Solve, the coefficient tables will contain the fitted coefficients and also the residual errors. You can then plot your data and visually interpret the results. Column one is always your X- axis, with each additional column plotted separately as a function of column one.
9.2.1.6.1. Batch TBFT,PLOT,ID,Option1,HYPER,Option3,Option4
Option1 = UNIA, BIAX, SHEA, or VOLU Option3 = Model name. See Table 9.3: “Hyperelastic Curve Fitting Model Types” (above) for the models available. Option4 = The order or number of your coefficients. See Table 9.3: “Hyperelastic Curve Fitting Model Types”
(above) for possible values. You use the /WINDOW command to configure the graphs for each of the resultant curves for the individual stress types.
9.2.1.6.2. GUI Use the GRAPH button to plot the data. Your plots will show Columns 2 and above as separate curves, plotted as a function of column 1. The data in column 1 is always the X-axis. By default all the experiments are plotted in separated graphs in the GUI window. To view a specific data and its corresponding fitting result, you can use the right click of mouse button on the specific dataset, and pick a desired option to view the results. Other plotting utilities can be found by using the right click of mouse button on the listed data in the curve fitting GUI window. You can also turn the legend and/or axis displays on and off, and switch the scales between log scale and regular scale. You can use the middle-mouse button to eliminate a specific curve and clarify or refine the remaining curve.
9.2.1.6.3. Review/Verify After plotting the curve fitting results, you can then review them and also verify the error norm/residual values that are printed in the curve fitting GUI window. These values help you determine the quality of curve fitting and whether to accept the results. Error norm values are not always the best indicator of a valid curve fit. Plotting the curves and visually assessing the result is often the best indication. If the results are unacceptable, you may want to go back to step 3 and solve again, either by picking a different model, increasing the order, or redefining your initial values of the coefficients or other control parameters. Repeat steps 3-7 until you get an acceptable solution.
9.2.1.7. Write Data to TB Command After you are satisfied with your curve fitting results, you can write the curve fitting data to the ANSYS database using TBFT, FSET. The GUI or the command line converts the coefficients to the appropriate form before writing to ANSYS TB tables. ANSYS stores the data as part of the material property set for use in subsequent analyses.
9.2.1.7.1. Batch TBFT,FSET,ID,HYPER,Option2,Option3
Option2 = Model name. See Table 9.3: “Hyperelastic Curve Fitting Model Types” (above) for the models available.
9–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.3: Creep Material Curve Fitting Option3 = The order or number of your coefficients. See Table 9.3: “Hyperelastic Curve Fitting Model Types”
(above) for possible values.
9.2.1.7.2. GUI Once you complete the process and update your material data properties with the representative curve data, you are returned to the material properties dialog. The curve data can now be accessed for the full range of material behavior.
9.3. Creep Material Curve Fitting ANSYS provides a number of creep models, along with the tools to fit derived coefficients to your experimental data. You can use either the interactive user interface (GUI) or batch commands. You input your experimental data, choose a model from one of the supplied creep models, and then perform a regression analysis. You then graphically view the curve fitting result, and compare it for fit with your experimental data. If the curve is acceptable, you write the fitted coefficients as ANSYS nonlinear data table commands (ANSYS TB command format) to the database for the subsequent finite element analyses. All thirteen implicit creep models are supported.
9.3.1. Using Curve Fitting to Determine Your Creep Material Behavior The steps for creep curve fitting are defined as follows: 1
Section 9.3.1.1: Prepare Experimental Data
The experimental data must be a plain text file with headers to describe the data types and attributes. The test data must be delimited by a space or a comma.
2
Section 9.3.1.2: Input the Data into The experimental data can be read into ANSYS by browsing ANSYS to the file location in the GUI or by specifying the path (batch) on the command line.
3
Section 9.3.1.3: Select a Material Model Option
4
Section 9.3.1.4: Initialize the Coeffi- Creep curve fitting is a nonlinear regression; the initial values cients of the coefficients to be determined can be very important for a successful solution.
5
Section 9.3.1.5: Specify Control Parameters and Solve
You choose the error norm to be used for an acceptable curve fit.
6
Section 9.3.1.6: Plot the Experimental Data and Analyze
You review and verify the results by comparing them with the experimental data and the regression errors. If they are not acceptable, repeat steps 3 to 5 to obtain a new curve fitting solution.
7
Section 9.3.1.7: Write Data to TB Command
Write curve fitting results in the TB command format to the ANSYS database.
The material options for the applicable curve fitting regimen are defined in the TB command. Thirteen implicit creep models are supported. Once you pick a model, you can still switch to another model if an ideal fit is not realized.
9.3.1.1. Prepare Experimental Data You need to provide accurate experimental test data in order to achieve valid curve fitting results. For the creep analysis, you will use either the creep strain value or creep strain rate, derived as a function of time, temperature, stress and/or creep strain. The type of data you need to provide will depend on the creep model chosen. The experimental data is named “creep” to distinguish it from other types of data such as uniaxial, tension, biaxial, etc. The creep data must be a plain text file, which contains the headers and the test data as a table, delimited by a space or a comma. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–7
Chapter 9: Material Curve Fitting The header can be used to describe the data types that characterize the test data columns or attributes of the data. There are a total of five different creep data types, see Table 9.4: “Creep Data Types and Abbreviations”.
Table 9.4 Creep Data Types and Abbreviations Time
time
Equivalent Creep Strain
creq
Equivalent Creep Strain Rate
dcreq
Equivalent Stress
seqv
Temperature
temp
The header format that defines the type of data column is /n, abbr, where n is the index of the data column in the file, and abbr is the abbreviation for the type of data in the column, as described in Table 9.4: “Creep Data Types and Abbreviations”. An example of a typical data input is shown here: /1,seqv ! indicates first column is stress /2,creq ! indicates second column is creep strain /3,temp ! indicates third column is temperature /4,dcreq ! indicates fourth column is creep strain rate 4000 0.00215869 100 0.000203055 4000 0.00406109 100 0.000181314 4000 0.00664691 100 0.000165303 4000 0.0102068 100 0.000152217 4000 0.0151416 100 0.000140946
When a particular column is unchanged over the loading history, you can define it as an attribute. For instance, in the above example, the stress and temperature are constant throughout the range. You define a data attribute in the header as follows: The header format to define a data attribute is /attr, value, where attr is the abbreviation of data type, and value is the value of the attribute. An example of a typical input data using attributes is shown here: /seqv,4000 ! indicate this creep has a constant stress of 4000 /temp,100 ! indicate this creep data is at a constant temperature of 100 /1,creq ! indicate first column is creep strain /2,dcreq ! indicate second column is creep strain rate 0.00215869 0.000203055 0.00406109 0.000181314 0.00664691 0.000165303 0.0102068 0.000152217 0.0151416 0.000140946 0.0220102 0.000130945
There are thirteen model types available from ANSYS for creep curve fitting. The model you choose will determine the experimental data required for the curve fitting process. The following tables describe the creep data required to perform curve fitting for each model type. Please note that for strain hardening and modified strain hardening, you need to input both creep strain and creep strain rate in the experimental data.
Table 9.5 Creep Model and Data/Type Attribute Creep Model
creq
dcreq
Strain Hardening
x
x
time
seqv
temp
x
x
Time Hardening
x
x
x
x
Generalized Exponential
x
x
x
x
Generalized Graham
x
x
x
x
9–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.3: Creep Material Curve Fitting Creep Model
creq
Generalized Blackburn Modified Time Hardening
x
Modified Strain Hardening
x
dcreq
time
seqv
x
x
x
x
x
temp x
x
x
Generalized Garofalo
x
x
x
Exponential Form
x
x
x
Norton
x
x
x
x
x
x
Prim+Sec Time Hardening
x
Prim+Sec Rational Polynomial
x
x
x
Generalized Time Hardening
x
x
x
x
9.3.1.2. Input the Data into ANSYS The experimental data must be read into ANSYS from a plain text file. You prepare this file according to the previous section, including both header information and formatted test data. The header portion is absolutely required for creep analyses. Each file is viewed as a data set in ANSYS, and can be a complete set of experimental test data or a part of a series of files of experimental test data. You can include several data sets, such as tests performed at different stress levels and/or temperatures, to perform a creep curve fitting. There are two ways to input the experimental data.
9.3.1.2.1. Batch The EADD argument of the TBFT command is used to identify and specify the location of your data files. The command syntax is: TBFT,EADD,ID,Option1,Option2,Option3,Option4
Option1 = creep Option2 = name of file containing experimental data Option3 = file name extension Option4 = file directory
9.3.1.2.2. GUI In interactive mode you can input experimental data by typing the filename (with the appropriate path if the file is not in the default directory) into the appropriate area. You can also “Browse” to a file in a particular location. Use the Add Data Set button to add additional data sets for creep curve fitting. There is no restriction on the number of data sets you can add.
9.3.1.3. Select a Material Model Option There are thirteen models available for curve fitting. You pick the one that best satisfies your requirements. You will use the creep model abbreviation in subsequent equations to identify the creep model (see Table 9.6: “Creep Models and Abbreviations”). Use the creep models table (below) to view the formulae of the creep models and to determine the number of coefficients. You'll find it helpful to view the formula before you proceed to solve. It will tell you what initial coefficients you might use and also lets you determine the format of your experimental data. Also see Table 9.6: “Creep Models and Abbreviations” to determine a starting point for the initial creep model coefficients.
9.3.1.3.1. Batch TBFT,FADD,ID,CREEP,Option2,Option3 Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–9
Chapter 9: Material Curve Fitting Option2 = Creep model abbreviation, see Table 9.6: “Creep Models and Abbreviations”. Option3 = not used for creep curve fitting.
The following table describes the creep models available and their abbreviated names for Option2 (above).
Table 9.6 Creep Models and Abbreviations Model Number
Name
Fitting Name/Option2
1
Strain Hardening
shar
2
Time Hardening
thar
3
Generalized Exponential
gexp
4
Generalized Graham
ggra
5
Generalized Blackburn
gbla
6
Modified Time Hardening
mtha
7
Modified Strain Hardening
msha
8
Generalized Garofalo
ggar
9
Exponential Form
expo
10
Norton
nort
11
Prim+Sec Time Hardening
psth
12
Prim+Sec Rational Polynomial
psrp
13
Generalized Time Hardening
gtha
Note — It is very important for the experimental data to be consistent with the creep model you choose. See Table 9.5: “Creep Model and Data/Type Attribute” for the data types required for each creep model.
9.3.1.3.2. GUI You can pick the appropriate model option from a menu in the data entry area. All of the options and constraints listed for batch input apply.
9.3.1.4. Initialize the Coefficients Creep curve fitting is a nonlinear regression process. A successful curve fit depends greatly on the initial coefficient values. For some creep models the initial value of certain coefficients is critical to achieving a successful fit. This suggests that certain variances may cause your curve fit to fail to converge. When this happens you can adjust the initial value of specific coefficients and rerun the problem again. In general the more parameters a model has, the more difficult it is to get the solution to converge. You can also fix (hold constant) your coefficients. You specify a value for a coefficient and keep it unchanged, while allowing the other coefficients to be operated on. You can then release the fixed coefficients to obtain a solution. By default, all of the coefficients are free to vary.
9.3.1.4.1. Batch You define your coefficient values using the SET option of the TBFT command, as follows: TBFT,SET,ID,CREEP,Option2,Option3,Option4,Option5
Option2 = Creep model name Option3 = not applicable Option4 = index of coefficient
9–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.3: Creep Material Curve Fitting Option5 = value of coefficient
Then you can modify the coefficients with the FIX option of the TBFT command. TBFT,FIX,ID,CREEP,Option2,Option3,Option4,Option5
Option2 = Creep model name Option3 = not applicable Option4 = index of coefficient Option5 = 0 variable, 1 fixed
9.3.1.4.2. GUI You pick your creep model from the choices on the creep model tree. ANSYS automatically configures the coefficients for the model. You can then make modifications, including initializing and/or fixing certain coefficients.
9.3.1.5. Specify Control Parameters and Solve Error norm, maximum number of the allowed iterations and the error tolerance will affect the accuracy of your results. There are two available error norms available for the regression. Normalized curve fitting is the default option used to calculate error norms. It generally gives better results than unnormalized curve fitting since normalized fitting gives equal weight to all data points when minimizing the errors norms. Other available solve criteria are number of iterations, residual tolerance and coefficient change tolerance. The solution stops when both residual tolerance and coefficient change tolerance is met or if the number of iterations criteria is met. The coefficients are updated after every iteration during the solve process.
9.3.1.5.1. Batch The batch command is TBFT,SOLVE,ID,CREEP,Option2,Option3,Option4, ..., Option7
Option2 = Creep function name (See Table 9.6: “Creep Models and Abbreviations”) Option3 = not applicable for Creep models Option4 = error norm: 0 = unnormalized, 1 = normalized (default) Option5 = maximum number of iterations Option6 = tolerance of residual changes Option7 = tolerance of coefficient changes
Other solving parameters are available. See the TBFT command for details.
9.3.1.5.2. GUI The solution phase is entered automatically after you fill in the last set of coefficient values. Each of the options specified in the command line description is presented as a pull down menu or fill in box, and each option must be specified before Solve will begin. The coefficients are updated in the GUI after the solution is complete.
9.3.1.6. Plot the Experimental Data and Analyze After you initiate Solve, the coefficient tables will contain the fitted coefficients and also the residual errors. You can then plot your data and visually interpret the results. Column one is generally your X- axis, with each additional column plotted separately as a function of column one. The plot utility also incorporates many “right mouse click” context sensitive functions that will help you to configure and optimize your plot(s).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–11
Chapter 9: Material Curve Fitting Clicking in various areas of the display window brings up context sensitive functions that are particular to that area. (e.g., clicking on the legend area brings up controls to define and configure your graph legend). These functions change according to the type of graph you are creating and to the entity you click on in the graph. You can also use a middle mouse click to hide a particular curve within a graph.
9.3.1.6.1. Batch TBFT,PLOT,ID,Option1,Option2,Option3,Option4
Option1 = CREEP Option3 = Creep model name Option4 = Not Used
9.3.1.6.2. GUI You can simultaneously display many data sets for each function plotted. Each window of your display can be used to display each one of the data sets you are plotting against column one.
9.3.1.6.3. Analyze Your Curves for Proper Fit You use the GUI to graphically review the curve fitting result. In this way you can ensure a good fit throughout the range of data. Use the plotted curve fitting results both to determine the degree of fit at various locations, and also to verify the error norm/residual value. You can then determine the quality of a curve fitting and decide whether to accept the results. If the results are unacceptable, you may want to go back to step 3, and then solve again with a new model, redefining certain initial values of the coefficients, and also modifying some of the other control parameters. Repeat steps 3-6 until you obtain a satisfactory solution.
9.3.1.7. Write Data to TB Command After you are satisfied with your curve fitting results, you can write the curve fitting data to the ANSYS database using TBFT, FSET. The GUI or the command line converts the coefficients to the appropriate form before writing to ANSYS TB tables. ANSYS stores the data as part of the material property set for use in subsequent analyses.
9.3.1.7.1. Batch TBFT,FSET,ID,CREEP,Option2,Option3
Option2 = Creep Model Abbreviation Option3 = Not applicable
9.3.1.7.2. GUI When you complete the process, click the Write to Database button to write the fitted coefficients of your creep model as a creep data table in ANSYS material database. You are then returned to the material properties dialog. The curve data can now be accessed for the full range of material behavior.
9.3.2. Tips For Curve Fitting Creep Models The following are some useful tips that will ensure successful curve fitting. These tips are not hard and fast specifications, only suggestions. Also, following them does not guarantee a solution. Refer to Section 2.5.11: Creep Equations for additional details on each implicit creep model . Name
9–12
Notes
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.3: Creep Material Curve Fitting 1
Strain Hardening
Strain hardening has 4 coefficients. C4 is for temperature dependency. If you do not have temperature dependent data, set C4 to zero. If you have difficulty solving temperature dependent data. Use experimental data for only one temperature and fix C4 to zero. Then solve. Then add data for other temperature, release C4 and solve for all coefficients or just C4 by fixing the C1, C2 and C3.
2
Time Hardening
Time hardening has 4 coefficients. C4 is for temperature dependency. If you do not have temperature dependent data, set C4 to zero. If you have difficulty solving temperature dependent data. Use experimental data for only one temperature, fix C4 to zero. Then solve. Then add data for other temperature, release C4 and solve for all coefficients or just C4 by fixing the C1, C2 and C3.
3
Generalized Exponential
Generalized Exponential has 5 coefficients. C4 is for temperature dependency. If you do not have temperature dependent data, set C4 to zero. Use a low value of C5 (e.g., 1e-3) to avoid floating-point overflows in the exponential term of this model. If you have difficulty solving temperature dependent data. Use experimental data for only one temperature, fix C4 to zero. Then solve. Then add data for other temperature, release C4 and solve for all coefficients or just C4 by fixing the C1, C2 and C3.
4
Generalized Graham
Generalized Graham has 8 coefficients. You use C8 for temperature dependency. If you do not have temperature dependent data, set C8 to zero. If you have difficulty solving temperature dependent data, use experimental data for only one temperature, fix C8 to zero, and solve. Then add data for other temperatures, release C8 and solve for the remaining coefficients individually.
5
Generalized Blackburn
Generalized Blackburn has 7 coefficients. It is advisable to look at exponential term and try to keep them from floatingpoint overflows. To keep eC2σ within floating-point range, make sure the initial value of C2 is such that C2σ is close to 1. Similarly try to keep σ/C4 and C7σ close to 1.
6
Modified Time Hardening
Modified Time Hardening has 4 coefficients. C4 is for temperature dependency. If you do not have temperature dependent data, fix C4 to zero.
7
Modified Strain Hardening
Modified Strain Hardening has 3 coefficients. This model is complex as far as curve fitting is concerned. To keep the
C1σC2 [(C3 + 1)ε]C3 term from going negative, C1 was replaced with C12 but converted to the right form before it was written to ANSYS database. 8
Generalized Garofalo
Generalized Garofalo has 4 coefficients. C4 is for temperature dependency. If you do not have temperature dependent data, set C4 to zero. To keep the Sinh term within floating-point range, keep c2σ close to one when you initialize the coefficients.
9
Exponential Form
Exponential Term has 3 coefficients. C3 is for temperature dependency. If you do not have temperature dependent data, set C3 to zero. To keep eσC2 within floating-point range, keep σ/C2 close to one.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–13
Chapter 9: Material Curve Fitting 10
Norton
Norton model has 3 coefficients. C3 is for temperature dependency. If you do not have temperature dependent data, set C3 to zero.
11
Prim+Sec Time Hardening
Time Hardening has 7 coefficients. This is a complex model. Here it is advisable to solve for temperature independent data first and then introduce temperature related data.
12
Prim+Sec Rational Polynomial
Rational Polynomial is a very complex model for curve fitting with 10 coefficients. If you find it hard to fit this data, it is advisable for you to split experimental data into primary creep data and secondary creep data. Primary creep data is the initial part of the curve that covers the nonlinearity in the strain rate. Fit only the secondary data by fixing C1 to 1 and then set all other coefficients except C2, C3 and C4 to zero. Use a low value of C3 to keep 10C3σ within floating-point range. Coefficients C5 to C10 in curve fitting refers to coefficients C7 to C12 in the implicit creep equation. Then add the primary creep data, release all coefficients, and solve.
13
Generalized Time Hardening
Generalized Time Hardening has 6 coefficients. Set C6 to zero if you have temperature independent data. When initializing coefficients set C5σ close to 1 to avoid floating-point overflows.
9.4. Viscoelastic Material Curve Fitting Viscoelastic material curve fitting is a tool to determine the material constants of the Prony series expansion for both shear and bulk modulus of the ANSYS hypoviscoelastic material option from experimental data. Either through an interactive user interface or the batch commands, users can input the experimental data, define the order of Prony series expansion, perform nonlinear regression, view the curve fitting results graphically, compare to the experimental data, and write the fitted coefficients as ANSYS nonlinear data table commands to the database for the subsequent finite elements analyses. Currently the tools allow you to fit shear modulus and/or bulk modulus and/or shift functions.
9.4.1. Using Curve Fitting to Determine the Coefficients of Viscoelastic Material Model The steps for Viscoelastic Curve Fitting are defined as follows: 1
Section 9.4.1.1: Prepare Experimental Data
2
Section 9.4.1.2: Input the Data into The experimental data can be read into ANSYS from GUI or ANSYS batch command line as a plain text file.
3
Section 9.4.1.3: Select a Material Model Option
4
Section 9.4.1.4: Initialize the Coeffi- Viscoelastic curve fitting is a nonlinear regression, the initial cients values of the coefficients to be determined can be very important for a successful solution.
5
Section 9.4.1.5: Specify Control Parameters and Solve
9–14
The experimental data must be a plain text file delimited by a space or a comma.
This includes Prony series expansion of shear and/or bulk moduli as well as shift function. The supported shift functions include WLF and TN.
Specify the error norm to be used, the solution control parameters, and perform the nonlinear regression.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.4: Viscoelastic Material Curve Fitting 6
Section 9.4.1.6: Plot the Experimental Data and Analyze
View graphically the curve fitting results. Review and verify the results by comparing with the experimental data and the regression errors, if not acceptable, repeat steps 3 to 7 to perform a new curve fitting solution.
7
Section 9.4.1.7: Write Data to TB Command
Write curve fitting results as the TB command to ANSYS database.
9.4.1.1. Prepare Experimental Data Curve fitting requires experimental test data. For curve fitting viscoelastic materials, the experimental data must be shear modulus and/or bulk modulus as a function of time and temperature. The experimental data is named “viscoelastic” to distinguish it from other data types, such as hyperelasticity or creep. This also makes documenting your analyses more convenient. The viscoelastic test data must be a plain text file containing the headers, along with the test data as a table of data delimited by a space or a comma. The header is used to define the test data type and the temperature for your test data. For viscoelastic curve fitting with multiple temperatures, you don't calculate each temperature point and write it as a temperature-dependent Prony data table. Instead, when multiple temperatures are present, either WLF or TN shift functions are used to account for the temperature dependency. Each file must contain only one temperature, and the temperatures of each of the files can be the same or different. The viscoelastic test data have 4 data types, seeTable 9.7: “Viscoelastic Data Types and Abbreviations”.
Table 9.7 Viscoelastic Data Types and Abbreviations Time
time
Shear modulus
smod
Bulk modulus
bmod
Temperature
temp
The headers are used to describe the data types that characterize the test data columns or attributes of the data. The following listing contains the appropriate headers, followed by the delimited data: /temp,100 ! define temperature attribute 0.01 2992.53 1 2978.514207 2 2965.45541 4 2942.293214 6 2922.530649 8 2905.612202 10 2891.073456 20 2842.506984 40 2798.142793 60 2772.383729 80 2750.631843 100 2730.398114 200 2643.125432 400 2517.475394 600 2431.262053 800 2366.580897 1000 2313.955396 2000 2117.922594 4000 1833.734397 6000 1627.199197 8000 1470.6806 10000 1347.264527 20000 964.0141125 40000 586.1405449 60000 392.186777 80000 277.2706253 Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–15
Chapter 9: Material Curve Fitting 100000 202.0025278 200000 46.87056342 400000 2.669209118 600000 0.156653269 800000 0.0137224 1000000 0.005591539
9.4.1.2. Input the Data into ANSYS You use the EADD argument of the TBFT command to input your data files. The experimental data must be read into ANSYS from a plain text file. The experimental data must be prepared as discussed in the previous section, and include both the header information and the formatted test data. Each file is viewed as a dataset in ANSYS, and can be the complete set of experimental test data or a part of an experimental test data. You can include several datasets, including tests performed at different temperatures. Although different datasets can have the same/or different temperature, each file can have only one temperature. Multiple temperature datasets must be input with multiple files. Two types of data may be required for viscoelastic curve fitting, either shear modulus vs time and/or bulk modulus vs. time. The data can also be a function of temperature, which can then be accounted for by either WLF or TN shift function. You can use the GUI window or batch command to input your experimental data.
9.4.1.2.1. Batch TBFT,EADD,ID,Option1,Option2,Option3,Option4
ID = Index corresponding to the ANSYS material number. Option1 = Experimental Date Type, either shear or bulk Option2 = name of file containing experimental data Option3 = file name extension Option4 = file directory
Note — “sdec” refers to the shear modulus as a function of time and “bdec” refers to the bulk modulus as a function of time.
9.4.1.2.2. GUI Click on the Add Dataset button and type the filename into the area provided. You can also “Browse” to a file in a specified location. Separate input is performed for each data type (Option1 = sdec, or bdec)
9.4.1.3. Select a Material Model Option The TBFT command provides the curve fitting tools for viscoelastic material modeling. You represent your viscoelastic material behavior by a set of Prony series expansions of shear and/or bulk moduli to characterize the shear and the bulk deformation of the material. You can also use the shift functions to characterize the material's temperature dependency. First you define a case “casename” to associate the set of coefficients for the Prony expansions with the shift functions that characterize the material behavior. You can use the “casename” to define several different options that characterize the same test data, and then to compare the curve fitting results. To define the material model, you must first define a “casename”, and then specify the order of shear and bulk moduli and the type of the shift function(s), if required. You need to create an additional case to define different shear order, bulk order or shift options. Once you create a case, the number of shear terms, bulk terms, or shift options cannot be changed.
9–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.4: Viscoelastic Material Curve Fitting
9.4.1.3.1. Batch You define a viscoelastic material with the Prony series expansion by creating a case and setting the order of shear modulus, bulk modulus and shift options. You create the case with the TBFT, FCASE command. The first line will include FCASE, ID, NEW. Then you specify the number of shear terms, bulk terms, and the shift function. The case is actually created only after the option is issued. The follow syntax examples and argument descriptions illustrate the relationship of these activities. TBFT,FCASE,ID,NEW,Option2,Option3
Option2 = PVHE (Refers to Prony Viscohypoelastic) Option3 = User Specified casename TBFT,FADD,ID,CATEGORY,Option2,Option3
CATEGORY = VISCO Option2 = pshear or pbulk or shift Option3 = Dependent on Option2 as follows:
•
Option2 = pshear or bulk, Option3 = NONE, or 1 to N
•
Option2 = shift, Option3 = NONE or TN or WLF TBFT,FCASE,ID,FINI
9.4.1.3.2. GUI You can use the GUI to interactively navigate the tree structure of the curve fitting window. Each of the shear, bulk and shift options can be selected, and you can fill in the appropriate “casename” in a text box field. As you choose the options, the coefficient table is automatically created.
9.4.1.4. Initialize the Coefficients The initial values you choose for your coefficients will determine the success of your viscoelastic curve fitting operations. A complete model has (2*NG+1)+(2* Nk +1)+ NS number of the coefficients. NG is the order of the Prony series expansion of the Shear modulus. Nk is the order of the Prony series expansion of the bulk modulus. NS is the number of coefficients of the shift function (NS = 2 for the TN option and NS =3 for the WLF option). The coefficients are ordered as shear terms first, then the bulk terms, and then the shift function. The coefficients are ordered as α0G, α1G, τ1G, α2G, τ2G, … αnG, and τnG for shear modulus, and α0K, α1K, τ1K, α2K, τ2K, … αnK, and τnK for bulk modulus. A shift function must be used together with your shear and/or bulk modulus for temperature dependent experimental data. The default coefficient is set to “one,” but you should redefine the initial values before solving. While initializing the coefficients, you should set αnKs to 1 and τnKs to time values that are equally distributed in the log scale, spanning the data range from minimum to maximum time. For example, in the shear decay versus time data file, if the time values vary from 1 to 10000, and if you use 3rd order Prony, logical guesses for τ1G , τ2G and τ3G that span this range could be τ1G = 1, τ2G = 100, and τ3G = 10,000 (also (1), (10) and (10,000) or (1), (1,000) and (10,000), respectively). You should also note that αnG used in curve fitting is the square root of the αnG used in ANSYS TB tables. This was done to keep all αnG used in the TB tables positive. A good guess for the WLF or TN parameter is the reference temperature you used during your partial solve for shear and bulk. The index of the reference/base temperatures is the sum of NumShear + NumBulk + 1. You can also fix (hold constant) your coefficients. You specify a value for a coefficient and keep it unchanged, while allowing the other coefficients to be operated on. You can then release the fixed coefficient later if desired. By default, all of the coefficients are free to vary. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–17
Chapter 9: Material Curve Fitting
9.4.1.4.1. Batch TBFT,SET,ID,CASE,Option2,Option3,Option4,Option5
Option2 = casename Option3 = Not Applicable Option4 = index of coefficient Option5 = value of coefficient
For example: TBFT,SET,1, myvisco1,,1,1.2 TBFT,SET,1, myvisco1,,2,1.5
! Initialize the first coefficient to 1.2 ! Initialize the second coefficient to 1.5
Use the TBFT,FIX command to fix a coefficient to a value set by the TBFT, SET command or to release a previously fixed coefficient. By default, coefficients are not fixed. TBFT,FIX,ID,CASE,Option2,Option3,Option4,Option5
Option2 = casename Option3 = Not Applicable Option4 = Index of coefficient Option5 = 1 to fix, 0 to vary
For example: TBFT,FIX,1, myvisco1,,1,1. TBFT,FIX,1, myvisco1,,2,1
! Fix the first coefficient to a value set via TBFT,SET ! Fix the second coefficient to a value set via TBFT,SET
9.4.1.4.2. GUI The coefficients table is automatically updated in the viscoelastic curve fitting GUI window when the order of shear modulus and/or bulk modulus and/or shift function are defined. Specify values for your coefficients in the coefficients table in the curve fitting GUI window, and check the appropriate boxes to fix them or allow them to vary.
9.4.1.5. Specify Control Parameters and Solve Viscoelastic curve fitting is a nonlinear regression process. You can use either normalized or unnormalized error norm for the regression. The normalized error norm is the default regression option for calculation of the error. This error norm generally gives better results than the unnormalized error norm option, since the normalized error gives equal weight to all data points. The solution control parameter of a nonlinear regression includes number of iterations, residual tolerance and coefficient change tolerance. The solution stops when both residual tolerance of error norm and coefficient change tolerance is met or if the number of iterations criteria is met. The coefficients are updated when the solution is completed. In general it is very difficult to directly solve a complete case including coefficients of the shear modulus, the bulk modulus and the shift function. Three solver options including shear modulus only, bulk modulus, and shift function (or all) are provided to allow user to solve only Prony coefficients of the shear modulus, Prony coefficients of the bulk modulus and coefficients of the shift function. However the coefficients of shift function can't be solved before the shear or bulk modulus are solved. It is normal for a solution to not converge at first, but to stop as the maximum iterations criteria is reached. You can then examine the curve fitting results and the solution history before proceeding any further. You can then adjust parameters and resolve the problem whenever it is necessary. For viscoelastic curve fitting, you should follow these three steps to perform the regression:
9–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.4: Viscoelastic Material Curve Fitting 1.
Solve the shear coefficients (if there are any). Set the partial solve option using TBFT, SET,,,,,COMP, PSHEAR. Set the reference temperature at which your partial solution will be performed using TBFT, SET,,,,,TREF, TX. Only data at temperature TX will be used to estimate shear coefficients Solve
2.
Solve the bulk coefficients (if there are any). Set the partial solve option using TBFT, SET,,,,,COMP, PBULK. Set the reference temperature at which your partial solution will be performed using TBFT, SET,,,,,TREF, TX. The reference temperature should be the same for both shear and bulk. Only data at temperature TX will be used to estimate shear coefficients Solve
3.
Solve the shift function (or all) coefficients. Set the partial solve option using TBFT, SET,,,,,COMP, PVHE. TREF is not used when you solve for all parameters. All temperature data is used to estimate the coefficients. Solve
Note — When only the shear and bulk buttons are checked, only your shear coefficients are solved. To solve for both shear and bulk, you must check all three buttons.
9.4.1.5.1. Batch Solution option command is: TBFT,SET,ID,CASE,Option2,Option3,Option4,Option5
Option2 = casename Option3 = Not Applicable Option4 = comp Option5 = pshea (for Shear only) or pbulk (for bulk only).
The SOLVE command allows you to specify procedure types, tolerances and number of iterations. TBFT,SOLVE,ID,CASE,Option2,Option3,Option4, ..., Option7
Option2 = Creep Function Name (See Table 9.6: “Creep Models and Abbreviations”) Option3 = Not Applicable Option4 = Curve Fitting Procedure: 0 = unnormalized least squares, 1 = normalized least squares (default) Option5 = maximum number of iterations Option6 = tolerance of residual changes Option7 = tolerance of coefficient changes
Other solving parameters are available. See the TBFT command for details.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–19
Chapter 9: Material Curve Fitting
9.4.1.5.2. GUI The GUI provides access for you to choose your error norm, solution control parameters, and solver options. Once you complete these specifications and solve, you can go back and modify your parameters as necessary to obtain a good curve fit.
9.4.1.6. Plot the Experimental Data and Analyze The best way to verify a good fit between your experimental data and the provided curves is to plot your curves and visually inspect them.
9.4.1.6.1. Batch You enter the plotting parameters from the command line as follows: TBFT,PLOT,ID,ExpIndex,CASE,Option3
Option3 = casename
9.4.1.6.2. GUI Graph button provides direct means to plot the data.
9.4.1.6.3. Analyze Your Curves for Proper Fit All of your data is plotted as a function of column 1 for the X-axis. Columns 2 and above are each plotted in a separate graph, in a separate window, with the corresponding fitted data as a function of column 1. By default all the shear datasets and/or the bulk datasets as well as the corresponding fitting results are plotted in two separated graphs in a GUI window. To view a specific data and its corresponding fitting result, you click the right mouse button on the specific dataset, and pick a desired option. You can also use the right mouse button to turn the legend and/or axis on and off. The scales can be also switched between log scale and regular scale. With the middle button you can eliminate certain curves from each window's display in order to see the remaining data more clearly. Reviewing your curve fitting result graphically is the only way to ensure a good fit. After plotting the curve fitting results, you can then review it and also verify the error norm/residual value that is printed in the curve fitting GUI window. This information helps you determine the quality of a curve fitting and decide whether to accept the results. If not, you may want to go back to step 3, solve again by changing the order of the Prony series, redefining certain initial values of the coefficients, and possibly other control parameters. Repeat steps 3-7 until you are satisfied with the solution.
9.4.1.7. Write Data to TB Command After a successful curve fitting, the last step is to write the curve fitting data as ANSYS Prony data table (the TB,Prony command) to ANSYS database. The GUI or the command line converts the coefficients to the appropriate form before writing TB commands.
9.4.1.7.1. Batch TBFT,FSET,ID,Option2,Option3
Option2 = CASE Option3 = casename
9–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.4: Viscoelastic Material Curve Fitting
9.4.1.7.2. GUI Click the “Write to Database” button and the fitted coefficients are automatically written to the ANSYS material database according Prony data table. Please note that the coefficients you see in the curve fitting module are different from those in the TB tables. The τ values remain the same, but the α values are different. The α values shown in ANSYS are the square of the α values derived during curve fitting. They are also normalized to make α at time 0 = 1.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–21
9–22
Chapter 10: Gasket Joints Simulation 10.1. Overview of Gasket Joints Gasket joints are essential components in most structural assemblies. Gaskets as sealing components between structural components are usually very thin and made of many materials, such as steel, rubber and composites. From a mechanics point of view, gaskets act to transfer force between components. The primary deformation of a gasket is usually confined to one direction, namely, through thickness. The stiffness contributions from membrane (in plane) and transverse shear are much smaller in general compared to the through thickness. The stiffness contribution therefore is assumed to be negligible, although the TB command provides options to account for transverse shear. A typical example of a gasket joint is in engine assemblies. A thorough understanding of the gasket joint is critical in engine design and operation. This includes an understanding of the behavior of gasket joint components themselves in an engine operation, and the interaction of the gasket joint with other components. Elements within the ANSYS family of interface element are used to model gaskets. By default, these elements are designed to account for gasket through-thickness behavior. However, you can account for transverse shear behavior by using an element Keyopt setting and transverse shear option of the gasket material data table. See the TB command documentation and the specific element documentation for more information.
10.2. Performing a Gasket Joint Analysis A gasket joint analysis involves the same overall steps that are involved in any ANSYS nonlinear analysis procedure. Most of these steps however warrant special considerations for a gasket joint analysis. Presented below are the overall steps with the special considerations noted, along with links to applicable sections where more detailed information is included on that topic. 1.
Build or import the model. There are no special considerations for building or importing the model for a gasket joint analysis. You perform this step as you would in any typical ANSYS analysis. See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details on building the model, see the ANSYS Modeling and Meshing Guide.
2.
Define element type. To properly simulate gasket joints, you must define structural element types and corresponding interface element types. See Section 10.4: ANSYS Family of Interface Elements in this chapter for more details on this topic, and in particular, see Section 10.4.1: Element Selection for a table of corresponding structural and interface elements.
3.
Define material. Use TB,GASKET to define the gasket joint material. You can use TB,GASKET to define four types of data input: general parameters, transverse shear stiffness, compression (loading), and tension (unloading). You specify the type using TBOPT. You then input the sets of data using the TBDATA and TBPT commands, as applicable. You can also plot most of the gasket data types using the TBPLOT command. See Section 10.5: Material Definition in this chapter for more details on this topic.
4.
Mesh the model. Use the AMESH or VMESH commands to mesh the structural element types, and use the IMESH command to mesh the gasket layer. Special restrictions apply to the IMESH command in terms of matching the source and target. Also, the order in which you execute these commands is critical. You can also mesh interface layers using the VDRAG command, and can generate interface elements directly using the EGEN command. Each of these commands involve special considerations for interface elements. See Section 10.6: Meshing Interface Elements in this chapter for more details on this topic.
5.
Solve. There are special solving considerations when you perform a gasket joint analysis. These are primarily concerned with the gasket element stiffness loss, and the gasket element's use with contact
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 10: Gasket Joints Simulation elements. See Section 10.7: Solution Procedure and Result Output in this chapter for more details on this topic. 6.
Review Results. You can print or plot any of four gasket output items: stresses (also pressure), total closure, total inelastic closure, and thermal closure, using the PRESOL, PRNSOL, PLESOL, PLNSOL, or ESOL commands. You can also use these items with the *GET command in POST1. See Section 10.8: Reviewing the Results in this chapter for more details on this topic.
10.3. Finite Element Formulation The primary deformation behavior of gasket joints is through-thickness deformation. It is therefore difficult to use solid continuum elements to effectively model gasket joints. The interface elements, which are based on the relative deformation of the top and bottom surfaces, offer a direct means to quantify through-thickness deformation of the gasket joints. Thus the pressure versus closure behavior can be directly applied to characterize the gasket material. The element formulation is based on a corotational procedure. Refer to Gasket Material in the ANSYS, Inc. Theory Reference for further details.
10.3.1. Element Topologies An interface element is composed of bottom and top surfaces. ANSYS provides several types of interface elements for the analysis of the gasket joints. Figure 10.1: “Element Topology of a 3-D 8-Node Interface Element” shows the geometry of a 3-D 8-node interface element available in ANSYS. An element midplane is created by averaging the coordinates of node pairs from the bottom and top surfaces of the elements. The numerical integration of interface elements is performed in the element midplane. The Gauss integration scheme is used for the numerical integration.
Figure 10.1 Element Topology of a 3-D 8-Node Interface Element
10.3.2. Thickness Direction The thickness direction is defined as the normal direction of the mid plane of the element at the integration point, and computed inside of ANSYS. The positive direction is defined by the right-hand rule going around the nodes in the midplane. The through thickness deformation is quantified by the relative deformation of bottom and top surfaces along the thickness direction. The thickness direction is then noted as the X-direction according to the ANSYS notation convention. No ESYS coordinate system is allowed for the elements.
10–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.4: ANSYS Family of Interface Elements
10.4. ANSYS Family of Interface Elements ANSYS offers 4 types of elements to simulate gaskets. They are referred to as interface elements and are summarized as follows: •
INTER192 - 2-D, 4-node, linear element.
•
INTER193 - 2-D, 6-node, quadratic element.
•
INTER194 - 3-D, 16-node, quadratic element.
•
INTER195 - 3-D, 8-node, linear element
The 2-D elements, INTER192 and INTER193, use a KEYOPT to define various stress state options.
10.4.1. Element Selection The simulation of an entire gasket joint assembly, consisting of the gasket and the structural elements on either side of the gasket, involves choosing interface elements and structural elements that have the same characteristics. Use the following table as a guideline for choosing interface and structural elements that have the same characteristics: For elements with these characteristics:
... use this interface element:
... with one of these structural elements:
2-D, linear
INTER192
PLANE42, HYPER56, VISCO106, PLANE182
2-D, quadratic
INTER193
PLANE2, PLANE82, HYPER84, VISCO88, PLANE183
3-D, quadratic
INTER194
VISCO89, SOLID92, SOLID95, SOLID96, SOLID186, SOLID187
3-D, linear
INTER195
SOLID45, SOLID46, HYPER58, SOLID62, SOLID64, SOLID65, HYPER86, SOLID185
Proper element type is chosen based on the stress states of interest and structural element types used. Element selection is done by the element type command, ET, for example, ET,1,195
defines element type 1 as element INTER195.
10.4.2. Applications In general, linear and quadratic elements are chosen for the following reasons: •
Fewer nodes produce a smaller model that runs faster with less computer resources.
•
Quadratic elements are necessary if stress gradients are present in surrounding bodies.
•
If elements are to follow a curved boundary closely, quadratic elements are ideal because their edges are arcs.
•
With a free mesh (tetrahedral elements) the mid-node (quadratic) is required for an accurate solution.
When a surrounding structure can be considered as a 2-D structure, for example, plane stress / strain / axisymmetric, 2-D elements are the ideal choice. A good example of the use of 2-D element INTER192 or INTER193 is the gasket between the "flanged" ends of pipe line. In this case the gasket properties do not vary significantly with geometric location.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–3
Chapter 10: Gasket Joints Simulation For a 3-D structure such as an internal combustion engine, 3-D element INTER194 or INTER195 is a good choice for simulating the gasket between the cylinder head and block. In this case there is no "nice" geometry because the gasket must fill in between two complicated surfaces, in between cylinders, and around other holes and passages. Also the gasket properties can vary in different zones. For example in a cylinder head, there is usually a much stiffer zone immediately around the cylinder to contain combustion pressure (called the "fire ring"). The remainder of the gasket is much softer.
10.5. Material Definition 10.5.1. Material Characteristics The TB command option GASKET allows gasket joints to be simulated with the ANSYS interface elements, in which there is only one element through the thickness, and the through thickness deformation is decoupled from the in plane deformation. The gasket material is usually under compression. The material under compression is highly nonlinear. The gasket material also exhibits quite complicated unloading behavior when compression is released. The GASKET option allows you to directly input data for the experimentally measured complex pressure closure curve for the material model (compression curve), and also for several unloading pressure closure curves. When no unloading curves are defined, the material behavior follows the compression curve while it is unloaded. As it is a joint component, there often exists an initial gap or void. On the other hand, from a modeling point of view, it is a lot easier to fill the spaces or volumes between the adjacent components with the interface meshes, and then set an initial gap for the gasket material to account for it. As long as the closure is less than the initial gap, no pressure is acted on the gaskets. Also, when it is under tension loading, there will be an open gap. Therefore, gasket joints generally do not have tension pressure. A stress cap is used to restrict tension pressure in the gasket joint elements. The GASKET material option must be used with interface elements INTER192, INTER193, INTER194, and INTER195. Figure 10.2: “Pressure vs. Closure Behavior of a Gasket Material” shows the experimental pressure vs. closure (relative displacement of top and bottom gasket surfaces) data for a graphite composite gasket material. The sample was unloaded and reloaded 5 times along the loading path and then unloaded at the end of the test to determine the materials unloading stiffness.
10–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.5: Material Definition
Figure 10.2 Pressure vs. Closure Behavior of a Gasket Material
10.5.2. Input Format You input gasket material data using TB,GASKET. The material data consists of 2 main parts: general parameters and pressure closure behaviors. The general parameters define initial gasket gap, stable stiffness for numerical stabilization, and stress cap for a gasket in tension. The pressure closure behavior includes gasket compression (loading) and tension data (unloading). The TB command specification for defining a gasket material is: TB,GASKET,MAT,NTEMP,NPTS,TBOPT where TBOPT = one of the following types of gasket material data: •
PARA: gasket material general parameters.
•
COMP: gasket compression data.
•
LUNL: gasket linear unloading data.
•
NUNL: gasket nonlinear unloading data.
•
TSS: gasket transverse shear stiffness data.
You input the general parameters using the TBDATA command, then input the compression and unloading data using the TBPT command. Presented in the following sections are examples of inputs for the various types of gasket data.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–5
Chapter 10: Gasket Joints Simulation
10.5.2.1. Define General Parameters (TBOPT = PARA) The gasket material general parameters include the initial gap, stable stiffness and the maximum tension stress cap. These parameters are defined as C1, C2, and C3 in the following example: TB,GASKET,MAT,NTEMP,NPTS,PARA TBDATA,1,C1,C2,C3
Refer to Gasket Materials in the ANSYS Elements Reference for further details on these parameters.
10.5.2.2. Define Compression Load Closure Curve (TBOPT = COMP) The compression pressure closure curve gasket material definition option is defined as follows: TB,GASKET,MAT,NTEMP,NPTS,COMP TBPT,,x1,y1 TBPT,,x2,y2 TBPT,,xi,yi
where: xi, yi are pairs of closure and pressure values. The following input listing is an example defining a compressive pressure vs. closure behavior of a gasket joint material with 10 data points. TB,GASKET,1, ,10,COMP TBPT,, 0.20000E-04, 0.54000E+08 TBPT,, 0.40000E-04, 0.15150E+09 TBPT,, 0.60000E-04, 0.24900E+09 TBPT,, 0.78000E-04, 0.30000E+09 TBPT,, 0.12000E-03, 0.37200E+09 TBPT,, 0.19000E-03, 0.47400E+09 TBPT,, 0.28600E-03, 0.58500E+09 TBPT,, 0.35800E-03, 0.67350E+09 TBPT,, 0.43200E-03, 0.78000E+09 TBPT,, 0.50500E-03, 0.89550E+09
! define compression data
10.5.2.3. Define Linear Unloading Data (TBOPT = LUNL) The linear unloading gasket material definition option is a simple way to define the gasket unloading behavior. Several unloading slopes can be defined to accommodate the comprehensive unloading behavior as follows: TB,GASKET,MAT,NTEMP,NPTS,LUNL TBPT,,x1,y1 TBPT,,x2,y2 TBPT,,xi,yi
where: NPTS is the number of unloading points; xi is the closure where unloading started, and yi is unloading slope. The following input listing is an example showing the linear unloading behavior of a gasket joint material with 3 unloading points TB,GASKET,1, ,3,LUNL ! define linear unloading data TBPT,, 0.78000E-04, 0.25100E+12
10–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.5: Material Definition TBPT,, 0.28600E-03, 0.25500E+12 TBPT,, 0.50500E-03, 0.10600E+13
A sample plot representing linear unloading curves is shown in Figure 10.3: “Gasket Material Input: Linear Unloading Curves”.
Figure 10.3 Gasket Material Input: Linear Unloading Curves
10.5.2.4. Define Nonlinear Unloading Data (TBOPT = NUNL) The nonlinear unloading gasket material definition option provides a more comprehensive way of defining gasket material unloading behavior. The input listing format is: TB,GASKET,MAT,NTEMP,NPTS,NUNL TBPT,,x1,y1 TBPT,,x2,y2 TBPT,,xi,yi
where: xi, yi are pairs of closure and pressure values. Several unloading curves can be defined. An example showing the nonlinear unloading behavior of a gasket joint material with 3 unloading points is as follows: TB,GASKET,1, ,5,NUNL ! define first nonlinear unloading data TBPT,, 0.78000E-04, 0.30000E+09 TBPT,, 0.66900E-04, 0.24750E+08 TBPT,, 0.63100E-04, 0.82500E+07 TBPT,, 0.54100E-04, 0.15000E+07 TBPT,, 0.00000E+00, 0.00000E+00 TB,GASKET,1, ,5,NUNL
! define second nonlinear unloading data
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–7
Chapter 10: Gasket Joints Simulation TBPT,, TBPT,, TBPT,, TBPT,, TBPT,,
0.28600E-03, 0.26400E-03, 0.26100E-03, 0.25600E-03, 0.00000E+00,
0.58500E+09 0.22350E+08 0.90000E+07 0.15000E+07 0.00000E+00
TB,GASKET,1, ,5,NUNL TBPT,, 0.50500E-03, 0.89550E+09 TBPT,, 0.47800E-03, 0.33900E+08 TBPT,, 0.47500E-03, 0.13500E+08 TBPT,, 0.46800E-03, 0.15000E+07 TBPT,, 0.00000E+00, 0.00000E+00
! define third nonlinear unloading data
A sample plot representing nonlinear unloading curves is shown in Figure 10.4: “Gasket Material Input: Nonlinear Unloading Curves”.
Figure 10.4 Gasket Material Input: Nonlinear Unloading Curves
10.5.3. Temperature Dependencies Inputting temperature dependent gasket material properties follows the standard ANSYS procedure for inputting temperature dependent data for other materials. The following format shows this procedure. TB,GASKET,MAT,NTEMP,NPTS,LUNL TBTEMP,T1 TBPT,,x1,y1 TBPT,,x2,y2 TBTEMP,T2 TBPT,,x1,y1 TBPT,,x2,y2
ANSYS will automatically interpolate the temperature data to the material points using linear interpolation. When the temperature is out of the specified range, the closest temperature point is used.
10–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.5: Material Definition The following is an example input listing defining a compressive pressure vs. closure behavior of a gasket joint material with 5 temperature points and up to 10 data points for each temperature point, and 3 nonlinear unloading curves with each curve having 5 temperatures and 5 data points. TB,GASKET,1, 5,10,COMP ! define compression data with 5 temperatures TBTEMP, 100.000 TBPT,, 0.20000E-04, 0.54000E+08 TBPT,, 0.40000E-04, 0.15150E+09 TBPT,, 0.60000E-04, 0.24900E+09 TBPT,, 0.78000E-04, 0.30000E+09 TBPT,, 0.12000E-03, 0.37200E+09 TBPT,, 0.19000E-03, 0.47400E+09 TBPT,, 0.28600E-03, 0.58500E+09 TBPT,, 0.35800E-03, 0.67350E+09 TBPT,, 0.43200E-03, 0.78000E+09 TBPT,, 0.50500E-03, 0.89550E+09 TBTEMP, 200.000 TBPT,, 0.20000E-04, TBPT,, 0.40000E-04, TBPT,, 0.60000E-04, TBPT,, 0.78000E-04, TBPT,, 0.12000E-03, TBPT,, 0.19000E-03, TBPT,, 0.28600E-03, TBPT,, 0.35800E-03, TBPT,, 0.43200E-03, TBPT,, 0.50500E-03,
0.18000E+08 0.50500E+08 0.83000E+08 0.10000E+09 0.12400E+09 0.15800E+09 0.19500E+09 0.22450E+09 0.26000E+09 0.29850E+09
TBTEMP, 300.000 TBPT,, 0.20000E-04, TBPT,, 0.40000E-04, TBPT,, 0.60000E-04, TBPT,, 0.78000E-04, TBPT,, 0.12000E-03, TBPT,, 0.19000E-03, TBPT,, 0.28600E-03, TBPT,, 0.35800E-03, TBPT,, 0.43200E-03, TBPT,, 0.50500E-03,
0.90000E+07 0.25250E+08 0.41500E+08 0.50000E+08 0.62000E+08 0.79000E+08 0.97500E+08 0.11225E+09 0.13000E+09 0.14925E+09
TBTEMP, 400.000 TBPT,, 0.20000E-04, TBPT,, 0.40000E-04, TBPT,, 0.60000E-04, TBPT,, 0.78000E-04, TBPT,, 0.12000E-03, TBPT,, 0.19000E-03, TBPT,, 0.28600E-03, TBPT,, 0.35800E-03, TBPT,, 0.43200E-03, TBPT,, 0.50500E-03,
0.36000E+07 0.10100E+08 0.16600E+08 0.20000E+08 0.24800E+08 0.31600E+08 0.39000E+08 0.44900E+08 0.52000E+08 0.59700E+08
TBTEMP, 500.000 TBPT,, 0.20000E-04, TBPT,, 0.40000E-04, TBPT,, 0.60000E-04, TBPT,, 0.78000E-04, TBPT,, 0.12000E-03, TBPT,, 0.19000E-03, TBPT,, 0.28600E-03, TBPT,, 0.35800E-03, TBPT,, 0.43200E-03, TBPT,, 0.50500E-03,
0.18000E+07 0.50500E+07 0.83000E+07 0.10000E+08 0.12400E+08 0.15800E+08 0.19500E+08 0.22450E+08 0.26000E+08 0.29850E+08
TB,GASKET,1, 5,5,NUNL ! define first nonlinear unloading data with 5 temperatures TBTEMP, 100.000 TBPT,, 0.78000E-04, 0.30000E+09 TBPT,, 0.66900E-04, 0.24750E+08 TBPT,, 0.63100E-04, 0.82500E+07 TBPT,, 0.54100E-04, 0.15000E+07
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–9
Chapter 10: Gasket Joints Simulation TBPT,, 0.00000E+00, 0.00000E+00 TBTEMP, 200.000 TBPT,, 0.78000E-04, TBPT,, 0.66900E-04, TBPT,, 0.63100E-04, TBPT,, 0.54100E-04, TBPT,, 0.00000E+00,
0.10000E+09 0.82500E+07 0.27500E+07 0.50000E+06 0.00000E+00
TBTEMP, 300.000 TBPT,, 0.78000E-04, TBPT,, 0.66900E-04, TBPT,, 0.63100E-04, TBPT,, 0.54100E-04, TBPT,, 0.00000E+00,
0.50000E+08 0.41250E+07 0.13750E+07 0.25000E+06 0.00000E+00
TBTEMP, 400.000 TBPT,, 0.78000E-04, TBPT,, 0.66900E-04, TBPT,, 0.63100E-04, TBPT,, 0.54100E-04, TBPT,, 0.00000E+00,
0.20000E+08 0.16500E+07 0.55000E+06 0.10000E+06 0.00000E+00
TBTEMP, 500.000 TBPT,, 0.78000E-04, TBPT,, 0.66900E-04, TBPT,, 0.63100E-04, TBPT,, 0.54100E-04, TBPT,, 0.00000E+00,
0.10000E+08 0.82500E+06 0.27500E+06 0.50000E+05 0.00000E+00
TB,GASKET,1, 5,5,NUNL ! define second nonlinear unloading data with 5 temperatures TBTEMP, 100.000 TBPT,, 0.28600E-03, 0.58500E+09 TBPT,, 0.26400E-03, 0.22350E+08 TBPT,, 0.26100E-03, 0.90000E+07 TBPT,, 0.25600E-03, 0.15000E+07 TBPT,, 0.00000E+00, 0.00000E+00 TBTEMP, 200.000 TBPT,, 0.28600E-03, TBPT,, 0.26400E-03, TBPT,, 0.26100E-03, TBPT,, 0.25600E-03, TBPT,, 0.00000E+00,
0.19500E+09 0.74500E+07 0.30000E+07 0.50000E+06 0.00000E+00
TBTEMP, 300.000 TBPT,, 0.28600E-03, TBPT,, 0.26400E-03, TBPT,, 0.26100E-03, TBPT,, 0.25600E-03, TBPT,, 0.00000E+00,
0.97500E+08 0.37250E+07 0.15000E+07 0.25000E+06 0.00000E+00
TBTEMP, 400.000 TBPT,, 0.28600E-03, TBPT,, 0.26400E-03, TBPT,, 0.26100E-03, TBPT,, 0.25600E-03, TBPT,, 0.00000E+00,
0.39000E+08 0.14900E+07 0.60000E+06 0.10000E+06 0.00000E+00
TBTEMP, 500.000 TBPT,, 0.28600E-03, TBPT,, 0.26400E-03, TBPT,, 0.26100E-03, TBPT,, 0.25600E-03, TBPT,, 0.00000E+00,
0.19500E+08 0.74500E+06 0.30000E+06 0.50000E+05 0.00000E+00
TB,GASKET,1, 5,5,NUNL ! define third nonlinear unloading data with 5 temperatures TBTEMP, 100.000 TBPT,, 0.50500E-03, 0.89550E+09 TBPT,, 0.47800E-03, 0.33900E+08 TBPT,, 0.47500E-03, 0.13500E+08 TBPT,, 0.46800E-03, 0.15000E+07
10–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.5: Material Definition TBPT,, 0.00000E+00, 0.00000E+00 TBTEMP, 200.000 TBPT,, 0.50500E-03, TBPT,, 0.47800E-03, TBPT,, 0.47500E-03, TBPT,, 0.46800E-03, TBPT,, 0.00000E+00,
0.29850E+09 0.11300E+08 0.45000E+07 0.50000E+06 0.00000E+00
TBTEMP, 300.000 TBPT,, 0.50500E-03, TBPT,, 0.47800E-03, TBPT,, 0.47500E-03, TBPT,, 0.46800E-03, TBPT,, 0.00000E+00,
0.14925E+09 0.56500E+07 0.22500E+07 0.25000E+06 0.00000E+00
TBTEMP, 400.000 TBPT,, 0.50500E-03, TBPT,, 0.47800E-03, TBPT,, 0.47500E-03, TBPT,, 0.46800E-03, TBPT,, 0.00000E+00,
0.59700E+08 0.22600E+07 0.90000E+06 0.10000E+06 0.00000E+00
TBTEMP, 500.000 TBPT,, 0.50500E-03, TBPT,, 0.47800E-03, TBPT,, 0.47500E-03, TBPT,, 0.46800E-03, TBPT,, 0.00000E+00,
0.29850E+08 0.11300E+07 0.45000E+06 0.50000E+05 0.00000E+00
Sample plots of compression and unloading curves for gasket data to two temperatures is shown in Figure 10.5: “Gasket Compression and Unloading Curves at Two Temperatures”.
Figure 10.5 Gasket Compression and Unloading Curves at Two Temperatures
"
#
!
!$ #
10.5.4. Plotting Gasket Data You can plot gasket compression, linear unloading and nonlinear unloading data using the TBPLOT command. The use of this command to plot gasket data is as follows: Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–11
Chapter 10: Gasket Joints Simulation TBPLOT,GASKET,MAT,TBOPT,TEMP,SEGN where TBOPT specifies the gasket material option to be plotted, TEMP specifies plotting either all of the temperature dependent data curves, or a curve at a specified temperature, and SEGN specifies whether or not to add the segment numbers to the curves.
10.6. Meshing Interface Elements Three options are available for meshing interface elements: •
For meshing gasket layers as an area or volume, use the IMESH command.
•
For meshing gasket layers by dragging an area mesh along a path, use the VDRAG command.
•
For generating interface elements directly from a pattern, use the EGEN command.
There are special requirements for meshing interface elements. See Section 7.5.6: Generating an Interface Mesh for Gasket Simulations in the ANSYS Modeling and Meshing Guide for further details on this type of meshing. The following example input listing shows the use of the IMESH command. /batch,list /title, Test to demonstrate the use of IMESH command /com, ************************************************************ /com, * * /com, * This is a simple test to demonstrate the use of IMESH * /com, * command to generate gasket elements. The model consists * /com, * of two blocks with gasket elements (INTER194) defined * /com, * between them. * /com, * * /com, ************************************************************ /prep7 !*+++++++++++++++++++++++++++++++++++++++ !* Define Element Types !*+++++++++++++++++++++++++++++++++++++++ et,1,187 ! Solid tetrahedral element et,2,194 ! Interface layer element !*+++++++++++++++++++++++++++++++++++++++ !* Define Parameters !*+++++++++++++++++++++++++++++++++++++++ EH=1.0 IH=0.1 DX=0 DY=0 DZ=IH Z1=EH Z2=Z1+IH Z3=Z2+EH !*+++++++++++++++++++++++++++++++++++++++ !* Generate Keypoints !*+++++++++++++++++++++++++++++++++++++++ k,1,0,0 k,2,1,0 k,3,1,1 k,4,0,1 k,5,0,0,z1 k,6,1,0,z1 k,7,1,1,z1 k,8,0,1,z1 k,9,0,0,z2 k,10,1,0,z2 k,11,1,1,z2 k,12,0,1,z2
10–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.6: Meshing Interface Elements k,13,0,0,z3 k,14,1,0,z3 k,15,1,1,z3 k,16,0,1,z3 !*+++++++++++++++++++++++++++++++++++++++ !* Generate First Volume !*+++++++++++++++++++++++++++++++++++++++ v,1,2,3,4,5,6,7,8 !*+++++++++++++++++++++++++++++++++++++++ !* Generate Second Volume !*+++++++++++++++++++++++++++++++++++++++ v,9,10,11,12,13,14,15,16 !*+++++++++++++++++++++++++++++++++++++++ !* Generate Middle Volume !*+++++++++++++++++++++++++++++++++++++++ v,5,6,7,8,9,10,11,12 !*+++++++++++++++++++++++++++++++++++++++ !* Define Element Size !*+++++++++++++++++++++++++++++++++++++++ esize,,4 ! !*+++++++++++++++++++++++++++++++++++++++ !* Mesh First Volume with Element Type 1 !*+++++++++++++++++++++++++++++++++++++++ type,1 mat,1 vmesh,1 !*++++++++++++++++++++++++++++++++++++++++++++ !* Generate Interface Layer with IMESH command !* using Element Type 2 (INTER194) !*++++++++++++++++++++++++++++++++++++++++++++ type,2 mat,2 imesh,area,6,7,0,DX,DY,DZ,TOL !*+++++++++++++++++++++++++++++++++++++++ !* Mesh Second Volume with Element Type 1 !*+++++++++++++++++++++++++++++++++++++++ type,1 mat,1 vmesh,2 !*+++++++++++++++++++++++++++++++++++++++ !* Plot Elements !*+++++++++++++++++++++++++++++++++++++++ /view,1 ,1,1,1 eplot finish
Figure 10.6: “Gasket Finite Element Model Geometry” shows the geometry of the finite element model, a thin interface layer between two block volumes. Figure 10.7: “Whole Model Mesh with Brick Element” shows the mesh with solid brick element, SOLID185, in top and bottom of block volumes, and Figure 10.8: “Interface Layer Mesh” shows the mesh of interface element, INTER195, in the interface layer between the two blocks. Figure 10.9: “Whole Model Tetrahedral Mesh” shows the mesh with solid tetrahedral element, SOLID187, in top and bottom of block volumes, and Figure 10.10: “Interface Layer Mesh with Degenerated Wedge Elements” shows the mesh of interface element (degenerated wedge), INTER194, in the interface layer between the two blocks.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–13
Chapter 10: Gasket Joints Simulation
Figure 10.6 Gasket Finite Element Model Geometry
Figure 10.7 Whole Model Mesh with Brick Element
10–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.6: Meshing Interface Elements
Figure 10.8 Interface Layer Mesh
Figure 10.9 Whole Model Tetrahedral Mesh
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–15
Chapter 10: Gasket Joints Simulation
Figure 10.10 Interface Layer Mesh with Degenerated Wedge Elements
10.7. Solution Procedure and Result Output Gasket material behavior is highly nonlinear. The full Newton-Raphson solution procedure (the standard ANSYS nonlinear method), is the default method for performing this type of analysis. Other solution procedures for gasket solutions are not recommended. Like most nonlinear problems, convergence behavior of a gasket joint analysis depends strongly on the particular problem to be solved. ANSYS has provided a comprehensive solution hierarchy, therefore it is always recommended that you use the ANSYS default solution options, unless you are sure about the benefits of the changes. Some special considerations for solving a gasket problem are as follows: •
By default a zero stress cap has been enforced on the gasket. When the element goes into tension, it will lose its stiffness and may cause numerical instability.
•
It is always a good practice to place the lower and upper limit on the time step size using the DELTIM or NSUBST commands, and to start with a small time step, then subsequently ramp it up . This ensures that all of the modes and behaviors of interest will be accurately included and that the problem is solved effectively.
•
Gasket elements must be configured to support transverse shear. Even if you do so, errors can result, especially for contact and other nonlinear applications. You should not use gasket elements with contact elements unless you configure the elements accordingly, and ascertain the mesh compatibility of the gasket layer and its mating components.
Like any other type of nonlinear analysis, the ANSYS program performs a series of linear approximations with corrections. A convergence failure can indicate a physical instability in the structure, or it can merely be the result of some numerical problem in the finite element model. The program printout gives you continuous feedback on the progress of these approximations and corrections. (The printout either appears directly on your screen, is captured on Jobname.OUT, or is written to some other file [/OUTPUT].) You can examine some of this same information in POST1, using the PRITER command, or in POST26, using the SOLU and PRVAR commands. You should make sure that you understand the iteration history of your analysis before you accept the results. In 10–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.7: Solution Procedure and Result Output particular, do not dismiss any program error or warning statements without fully understanding their meaning. A typical output listing with gasket nonlinearity only is shown in Section 10.7.1: Typical Gasket Solution Output Listing. When other types of nonlinearity such as contact or materials are included, additional information will be printed out.
10.7.1. Typical Gasket Solution Output Listing S O L U T I O N PROBLEM DIMENSIONALITY. . . DEGREES OF FREEDOM. . . . . ANALYSIS TYPE . . . . . . . PLASTIC MATERIAL PROPERTIES NEWTON-RAPHSON OPTION . . .
. . . . . . UX UY . . . . . INCLUDED. . . . . .
O P T I O N S . . . UZ . . . . . . . . .
. .3-D . .STATIC (STEADY-STATE) . .YES . .PROGRAM CHOSEN
*** NOTE *** CP= 0.000 TIME= 00:00:00 Present time 0 is less than or equal to the previous time. Time will default to 1. *** NOTE ***
CP=
0.000
TIME= 00:00:00
Nonlinear analysis, NROPT set to the FULL Newton-Raphson solution procedure for ALL DOFs. *** NOTE ***
CP=
0.000
The conditions for direct assembly have been met. files will be produced. L O A D
S T E P
TIME= 00:00:00
No .emat or .erot
O P T I O N S
LOAD STEP NUMBER. . . . . . . . . . . . . TIME AT END OF THE LOAD STEP. . . . . . . AUTOMATIC TIME STEPPING . . . . . . . . . INITIAL NUMBER OF SUBSTEPS . . . . . . MAXIMUM NUMBER OF SUBSTEPS . . . . . . MINIMUM NUMBER OF SUBSTEPS . . . . . . MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS. STEP CHANGE BOUNDARY CONDITIONS . . . . . TERMINATE ANALYSIS IF NOT CONVERGED . . . CONVERGENCE CONTROLS. . . . . . . . . . . COPY INTEGRATION POINT VALUES TO NODE . .
. . . . . . . . . . .
. . . . . . . . . . .
. 1 . 1.0000 . ON . 200 . 20000 . 20 . 15 . NO .YES (EXIT) .USE DEFAULTS .YES, FOR ELEMENTS WITH ACTIVE MAT. NONLINEARITIES PRINT OUTPUT CONTROLS . . . . . . . . . . . . .NO PRINTOUT DATABASE OUTPUT CONTROLS ITEM FREQUENCY COMPONENT ALL ALL SVAR ALL
Range of element maximum matrix coefficients in global coordinates Maximum= 4.326388889E+11 at element 0. Minimum= 388758681 at element 0. *** ELEMENT MATRIX FORMULATION TIMES TYPE NUMBER ENAME TOTAL CP AVE CP 1 2 SOLID185 0.000 0.000000 2 1 INTER195 0.000 0.000000 Time at end of element matrix formulation CP= 0. ALL CURRENT ANSYS DATA WRITTEN TO FILE NAME= FOR POSSIBLE RESUME FROM THIS POINT FORCE CONVERGENCE VALUE = 0.4200E+07 CRITERION= 0.2143E+05 SPARSE MATRIX DIRECT SOLVER. Number of equations = 24, Memory available (MB) = 0.0 DISP CONVERGENCE VALUE EQUIL ITER 1 COMPLETED.
Maximum wavefront = , Memory required (MB)
0 =
0.0
= 0.1130E-04 CRITERION= 0.2000E-06 NEW TRIANG MATRIX. MAX DOF INC= -0.4000E-05
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–17
Chapter 10: Gasket Joints Simulation
FORCE CONVERGENCE VALUE = 0.1367E-08 CRITERION= 51.35 <<< CONVERGED DISP CONVERGENCE VALUE = 0.3257E-20 CRITERION= 0.2000E-06 <<< CONVERGED EQUIL ITER 2 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC = -0.2234E-20 >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 2 *** ELEMENT RESULT CALCULATION TIMES TYPE
NUMBER 1 2
ENAME 2 1
SOLID185 INTER195
TOTAL CP 0.000 0.000
*** NODAL LOAD CALCULATION TIMES TYPE NUMBER ENAME TOTAL CP 1 2
2 1
SOLID185 INTER195
0.000 0.000
AVE CP 0.000000 0.000000
AVE CP 0.000000 0.000000
*** LOAD STEP 1 SUBSTEP 1 COMPLETED. CUM ITER = *** TIME = 0.500000E-02 TIME INC = 0.500000E-02 *** AUTO STEP TIME: NEXT TIME INC = 0.50000E-02 UNCHANGED
2
FORCE CONVERGENCE VALUE = 0.7716E-09 CRITERION= 100.6 DISP CONVERGENCE VALUE = 0.1951E-20 CRITERION= 0.2000E-06 <<< CONVERGED EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1642E-20 FORCE CONVERGENCE VALUE = 0.4624E-09 CRITERION= 102.7 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 1 *** LOAD STEP 1 SUBSTEP 2 COMPLETED. CUM ITER = 3 *** TIME = 0.100000E-01 TIME INC = 0.500000E-02 *** AUTO TIME STEP: NEXT TIME INC = 0.75000E-02 INCREASED (FACTOR = 1.5000) FORCE CONVERGENCE VALUE = 0.1964E-08 CRITERION= 176.1 DISP CONVERGENCE VALUE = 0.3748E-20 CRITERION= 0.3000E-06 <<< CONVERGED EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.2744E-20 FORCE CONVERGENCE VALUE = 0.8307E-09 CRITERION= 179.7 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 1 *** LOAD STEP 1 SUBSTEP 3 COMPLETED. CUM ITER = 4 *** TIME = 0.175000E-01 TIME INC = 0.750000E-02 *** AUTO TIME STEP: NEXT TIME INC = 0.11250E-01 INCREASED (FACTOR = 1.5000) FORCE CONVERGENCE VALUE = 0.3713E-08 CRITERION= 289.4 DISP CONVERGENCE VALUE = 0.7198E-20 CRITERION= 0.4500E-06 <<< CONVERGED EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.4503E-20 FORCE CONVERGENCE VALUE = 0.1468E-08 CRITERION= 295.3 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 1 *** LOAD STEP 1 SUBSTEP 4 COMPLETED. CUM ITER = 5 *** TIME = 0.287500E-01 TIME INC = 0.112500E-01 *** AUTO TIME STEP: NEXT TIME INC = 0.16875E-01 INCREASED (FACTOR = 1.5000) FORCE CONVERGENCE VALUE = 0.1833E-07 CRITERION= 459.2 DISP CONVERGENCE VALUE = 0.3753E-19 CRITERION= 0.6750E-06 <<< CONVERGED EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1800E-19 FORCE CONVERGENCE VALUE = 0.3550E-08 CRITERION= 468.6 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 1 *** LOAD STEP 1 SUBSTEP 5 COMPLETED. CUM ITER = 6 *** TIME = 0.456250E-01 TIME INC = 0.168750E-01 *** AUTO TIME STEP: NEXT TIME INC = 0.25313E-01 INCREASED (FACTOR = 1.5000) FORCE CONVERGENCE VALUE = 0.2322E-07 CRITERION= 714.0 DISP CONVERGENCE VALUE = 0.4656E-19 CRITERION= 0.1013E-05 <<< CONVERGED EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.2664E-19 FORCE CONVERGENCE VALUE = 0.6406E-08 CRITERION= 728.5 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 1 *** LOAD STEP 1 SUBSTEP 6 COMPLETED. CUM ITER = 7 *** TIME = 0.709375E-01 TIME INC = 0.253125E-01 *** AUTO TIME STEP: NEXT TIME INC = 0.37969E-01 INCREASED (FACTOR = 1.5000)
10–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.8: Reviewing the Results
10.8. Reviewing the Results Results from a gasket joint analysis consist mainly of displacements, stresses, strains and reaction forces of the structural components and the gasket joint layer information (gasket pressure, closure, etc.). You can review these results in POST1, the general postprocessor, or in POST26, the time-history postprocessor. See the Output Data sections of the element descriptions for any of the interface elements (for example INTER192) for a description of the available output components. Note that in POST1, only one substep can be read in at a time, and that the results from that substep should have been written to Jobname.RST. (The load step option command OUTRES controls which substep results are stored on Jobname.RST.) A typical POST1 postprocessing sequence is described below.
10.8.1. Points to Remember •
To review results in POST1, the database must contain the same model for which the solution was calculated.
•
The results file (Jobname.RST) must be available.
10.8.2. Reviewing Results in POST1 1.
Verify from your output file (Jobname.OUT) whether or not the analysis converged at all load steps. •
If not, you probably won't want to postprocess the results, other than to determine why convergence failed.
•
If your solution converged, then continue postprocessing.
2.
Enter POST1. If your model is not currently in the database, issue RESUME. Command(s): /POST1 GUI: Main Menu> General Postproc
3.
Read in results for the desired load step and substep, which can be identified by load step and substep numbers or by time. Command(s): SET GUI: Main Menu> General Postproc> Read Results> load step
4.
Display the results using any of the following options. Note that gasket results, such as pressure and closure, are always displayed and listed in the local coordinate system. Option: Display Deformed Shape Command(s): PLDISP GUI: Main Menu> General Postproc> Plot Results> Deformed Shape Option: Contour Displays Command(s): PLNSOL or PLESOL GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu Use these options to display contours of stresses, strains, or any other applicable item. When displaying the gasket pressure distribution, if other structural mating components are not included, ANSYS will plot the geometry of those components in gray. To have a better visualization of a gasket pressure plot, it is better for you to select gasket elements only.
Option: Tabular Listings Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–19
Chapter 10: Gasket Joints Simulation Command(s): PRNSOL (nodal results) PRESOL (element-by-element results) PRRSOL (reaction data) PRITER (substep summary data), etc. GUI: Main Menu> General Postproc> List Results> Nodal Solution Main Menu> General Postproc> List Results> Element Solution Main Menu> General Postproc> List Results> Reaction Solution Option: Animation You can also animate gasket results over time: Command(s): ANTIME GUI: Utility Menu> PlotCtrls> Animate> Over Time Other Capabilities Many other postprocessing functions are available in POST1. See The General Postprocessor (POST1) in the ANSYS Basic Analysis Guide for details. Load case combinations usually are not valid for nonlinear analyses.
10.8.3. Reviewing Results in POST26 You can also review the load-history response of a nonlinear structure using POST26, the time-history postprocessor. Use POST26 to compare one ANSYS variable against another. For instance, you might graph the gasket closure vs. gasket pressure, which should correspond to the material behavior defined by TB,GASKET. You might also graph the displacement at a node versus the corresponding level of applied load, or you might list the gasket pressure at a node and the corresponding TIME value. A typical POST26 postprocessing sequence for a gasket analysis is the same as the sequence for a typical nonlinear analysis. See steps 1 through 4 in Section 8.5.6.3: Reviewing Results in POST26 included in Chapter 8, “Nonlinear Structural Analysis”.
10.9. Sample Gasket Element Verification Analysis (Command or Batch Method) This is a simple finite element model created to demonstrate the gasket material simulation. Two block elements with element type SOLID185 were generated as supporters and a gasket element INTER195 was created. The whole system is fixed along one side of each axes to prevent rigid body motion. A prescribed displacement is placed on top of the supporter element. The gasket material is assumed to have a nonlinear compression behavior with 5 different linear unloading slopes. A pressure stress cap of 1.0e-5 is imposed so that no tension stress is generated. Two load steps were used. The ANSYS commands are shown below. /batch,list /title, Test to Verify Gasket Material and Element /com, ************************************************************** /com, * * /com, * This is a simple test case to verify gasket material and * /com, * element. * /com, * * /com, * The test case is set up with two solid SOLID185 elements * /com, * with gasket element (INTER195) defined between them. * /com, * Displacement is applied to one SOLID185 element while the * /com, * other SOLID185 element is fixed. * /com, * The problem is solved in two load steps. In the first * /com, * load step negative z-displacement is applied to one * /com, * SOLID195 element causing compression of gasket elements. * /com, * Then, in the second load step, a reverse displacement is * /com, * applied causing the unloading (tension) of gasket element. * /com, * A Stress Cap of 1.0E-05 is enforced so that there is no * /com, * tension pressure in gasket material. * /com, * *
10–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.9: Sample Gasket Element Verification Analysis (Command or Batch Method) /com, ************************************************************** /prep7 !*+++++++++++++++++++++ !* Define Element Types !*+++++++++++++++++++++ et,1,185 et,2,195 !*++++++++++++++++++++++++++++++++++++++ !* Define Linear Elastic Material Type 1 !*++++++++++++++++++++++++++++++++++++++ mp,ex,1,2.1E12 mp,nuxy,1,0.0 !*+++++++++++++++++++++++++++++++++++++++++++++++++ !* Define Initial Gap, Stable Stiffness, Stress Cap !*+++++++++++++++++++++++++++++++++++++++++++++++++ delta0 = 0.00e-3 stiff0 = 0.0e7 scap = 1.0e-5 tb,gasket,2,,,para tbdata, 1,delta0,stiff0,scap !*++++++++++++++++++++++++++++++++ !* Define Gasket Compression Curve !*++++++++++++++++++++++++++++++++ tb,gask,2,1,13,comp tbpt,,0.460800E-03, 0.161226E+07 tbpt,,0.511600E-03, 0.520884E+07 tbpt,,0.562400E-03, 0.113134E+08 tbpt,,0.613200E-03, 0.200499E+08 tbpt,,0.664000E-03, 0.259960E+08 tbpt,,0.714800E-03, 0.290345E+08 tbpt,,0.765600E-03, 0.357453E+08 tbpt,,0.816400E-03, 0.440064E+08 tbpt,,0.867200E-03, 0.563189E+08 tbpt,,0.918000E-03, 0.748254E+08 tbpt,,0.968800E-03, 0.967287E+08 tbpt,,0.101960E-02, 0.129001E+09 tbpt,,0.109326E-02, 0.157147E+09 !*+++++++++++++++++++++++++++++++++++++ !* Define Gasket Linear Unloading Curve !*+++++++++++++++++++++++++++++++++++++ tb,gask,2,1,5,lunl tbpt,,0.460800E-03, 2.430000E+11 tbpt,,0.714800E-03, 3.565000E+11 tbpt,,0.816400E-03, 5.92300E+11 tbpt,,0.968800E-03, 1.088000e+12 tbpt,,0.109326E-02, 1.490000E+12 !*+++++++++++++++++++++++++++ !* List Gasket Material Model !*+++++++++++++++++++++++++++ tblist,gask,all !*++++++++++++++++++ !* Define Parameters !*++++++++++++++++++ n1 = 20 n2 = n1*100 n3 = n1 dis1 = -0.0008 dis2 = -0.000001 pres = 1.0e7 pres2 = 10 pres3 = 1.4E8 dp = -2.0e7 elb = 1.0 elg = 0.1
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–21
Chapter 10: Gasket Joints Simulation !*+++++++++++++++ !* Generate Nodes !*+++++++++++++++ n,1, n,2,1.0 n,3,1.0,1.0 n,4,0.0,1.0 ngen,2,4,1,4,,0.0,0.0,elb ngen,2,8,1,4,,0.0,0.0,elb+elg ngen,2,12,1,4,,0.0,0.0,2*elb+elg !*+++++++++++++++++++++++++++++++++++++++++ !* Generate Front and Back SOLID185 Element !*+++++++++++++++++++++++++++++++++++++++++ et,1,185,,1 mat,1 e,1,2,3,4,5,6,7,8 e,9,10,11,12,13,14,15,16 !*+++++++++++++++++++++++++++++++++ !* Generate Middle INTER195 Element !*+++++++++++++++++++++++++++++++++ et,2,195,, type,2 mat,2 e,5,6,7,8,9,10,11,12 !*++++++++++++++++++++++++++ !* Define Boundary Condition !*++++++++++++++++++++++++++ nsel,s,loc,z d,all,uz nsel,all nsel,s,loc,x d,all,ux nsel,all nsel,s,loc,y d,all,uy nsel,all finish /solu !*+++++++++++++++++++ !* Apply Displacement !*+++++++++++++++++++ nsel,s,loc,z,elb*2+elg d,all,uz,dis1 nsel,all !*+++++++++++++++++++++++++++++++++++++++++++++ !* Solve First Load Step, Compress the Elements !*+++++++++++++++++++++++++++++++++++++++++++++ nsubst,n1,n2,n3 outres,all,all outres,svar,all solve !*++++++++++++++++++++++++++++++++++++++++++ !* Solve Second Load Step, Open the Elements !*++++++++++++++++++++++++++++++++++++++++++ nsubst,n1,n2,n3 outres,all,all outres,svar,all nsel,s,loc,z,elb*2+elg d,all,uz,dis2 nall solve finish !*++++++++++++++++++++++++ !* Postprocess the Results !*++++++++++++++++++++++++
10–22
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.9: Sample Gasket Element Verification Analysis (Command or Batch Method) /post1 set,last pres,s pres,epto pres,epel prns,epel finish !*++++++++++++++++++++++++++++++++++++++++++++++ !* Post26, Print and Plot Gasket Element Results !*++++++++++++++++++++++++++++++++++++++++++++++ /post26 esol,2,3, ,s,x,press esol,3,3, ,epel,x,delta add,4,2, , ,press,,,-1, ! change sign for plotting add,5,3,,,delta,,,-1, ! change sign for plotting prvar,2,3,4,5 xvar,5 plvar,4 finish /exit,nosave
Presented below is the POST26 output resulting from this analysis. -----------------------------------------------------------------------***** ANSYS POST26 VARIABLE LISTING ***** TIME 0.50000E-01 0.10000 0.15000 0.20000 0.25000 0.30000 0.35000 0.40000 0.45000 0.50000 0.55000 0.60000 0.65000 0.70000 0.75000 0.80000 0.85000 0.90000 0.95000 1.0000 1.0500 1.1000 1.1500 1.2000 1.2500 1.3000 1.3500 1.4000 1.4500 1.5000 1.5500 1.6000 1.6500 1.7000 1.7500 1.8000 1.8500 1.9000 1.9500 2.0000
3 S X press -139488. -278977. -418465. -557953. -697442. -836930. -976418. -0.111591E+07 -0.125539E+07 -0.139488E+07 -0.153437E+07 -0.278389E+07 -0.557968E+07 -0.989280E+07 -0.152775E+08 -0.208613E+08 -0.250737E+08 -0.277640E+08 -0.310936E+08 -0.357955E+08 -0.227277E+08 -0.965988E+07 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04
3 EPELX delta -0.398672E-04 -0.797343E-04 -0.119601E-03 -0.159469E-03 -0.199336E-03 -0.239203E-03 -0.279070E-03 -0.318937E-03 -0.358804E-03 -0.398672E-03 -0.438539E-03 -0.477349E-03 -0.514686E-03 -0.550578E-03 -0.585450E-03 -0.620132E-03 -0.656120E-03 -0.693558E-03 -0.730387E-03 -0.765909E-03 -0.738405E-03 -0.710900E-03 -0.680150E-03 -0.640200E-03 -0.600250E-03 -0.560300E-03 -0.520350E-03 -0.480400E-03 -0.440450E-03 -0.400500E-03 -0.360550E-03 -0.320600E-03 -0.280650E-03 -0.240700E-03 -0.200750E-03 -0.160800E-03 -0.120850E-03 -0.809000E-04 -0.409500E-04 -0.100000E-05
4 ADD press 139488. 278977. 418465. 557953. 697442. 836930. 976418. 0.111591E+07 0.125539E+07 0.139488E+07 0.153437E+07 0.278389E+07 0.557968E+07 0.989280E+07 0.152775E+08 0.208613E+08 0.250737E+08 0.277640E+08 0.310936E+08 0.357955E+08 0.227277E+08 0.965988E+07 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04
5 ADD delta 0.398672E-04 0.797343E-04 0.119601E-03 0.159469E-03 0.199336E-03 0.239203E-03 0.279070E-03 0.318937E-03 0.358804E-03 0.398672E-03 0.438539E-03 0.477349E-03 0.514686E-03 0.550578E-03 0.585450E-03 0.620132E-03 0.656120E-03 0.693558E-03 0.730387E-03 0.765909E-03 0.738405E-03 0.710900E-03 0.680150E-03 0.640200E-03 0.600250E-03 0.560300E-03 0.520350E-03 0.480400E-03 0.440450E-03 0.400500E-03 0.360550E-03 0.320600E-03 0.280650E-03 0.240700E-03 0.200750E-03 0.160800E-03 0.120850E-03 0.809000E-04 0.409500E-04 0.100000E-05
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–23
10–24
Chapter 11: Contact This chapter covers the following topics: 11.1. Contact Overview 11.2. General Contact Classification 11.3. ANSYS Contact Capabilities 11.4. Performing a Surface-to-Surface Contact Analysis 11.5. GUI Aids for Contact Analyses 11.6. Performing a Node-to-Surface Contact Analysis 11.7. Using the Internal MPC Approach for Assemblies and Kinematic Constraints 11.8. Performing a Node-to-Node Contact Analysis
11.1. Contact Overview Contact problems are highly nonlinear and require significant computer resources to solve. It is important that you understand the physics of the problem and take the time to set up your model to run as efficiently as possible. Contact problems present two significant difficulties. First, you generally do not know the regions of contact until you've run the problem. Depending on the loads, material, boundary conditions, and other factors, surfaces can come into and go out of contact with each other in a largely unpredictable and abrupt manner. Second, most contact problems need to account for friction. There are several friction laws and models to choose from, and all are nonlinear. Frictional response can be chaotic, making solution convergence difficult. In addition to these two difficulties, many contact problems must also address multi-field effects, such as the conductance of heat, electrical currents, and magnetic flux in the areas of contact. If you do not need to account for friction in your model, and the interaction between the bodies is always bonded, you may be able to use the internal multipoint constraint (MPC) feature (available for certain contact elements) to model various types of contact assemblies and surface-based constraints (see Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints for more information). Another alternative is to use constraint equations or coupled degrees of freedom instead of contact to model these situations (see Chapter 12, “Coupling and Constraint Equations” in the ANSYS Modeling and Meshing Guide for more information). Constraint equations are only available for small strain applications (NLGEOM,off).
11.1.1. Explicit Dynamics Contact Capabilities In addition to the implicit contact capabilities discussed in this chapter, ANSYS also offers explicit contact capabilities with the ANSYS LS-DYNA explicit dynamics product. Explicit capabilities are ideally suited for short-duration contact-impact problems. For more information on the ANSYS LS-DYNA product and its contact capabilities, see the ANSYS LS-DYNA User's Guide.
11.2. General Contact Classification Contact problems fall into two general classes: rigid-to-flexible and flexible-to-flexible. In rigid-to-flexible contact problems, one or more of the contacting surfaces are treated as rigid (i.e., it has a much higher stiffness relative to the deformable body it contacts). In general, any time a soft material comes in contact with a hard material, the problem may be assumed to be rigid-to-flexible. Many metal forming problems fall into this category. The other class, flexible-to-flexible, is the more common type. In this case, both (or all) contacting bodies are deformable (i.e., have similar stiffnesses). An example of a flexible-to-flexible contact is bolted flanges.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 11: Contact
11.3. ANSYS Contact Capabilities ANSYS supports three contact models: node-to-node, node-to-surface, and surface-to-surface. Each type of model uses a different set of ANSYS contact elements and is appropriate for specific types of problems as shown in Table 11.1: “ANSYS Contact Capabilities”.
Table 11.1 ANSYS Contact Capabilities
Point-to-Point
Node-to-Node
Node-to- Surface-to-Surface Surface
CONTAC CONTAC CONTA 12 52 178
CONTA CONTA CONTA 175, 171,172 173,174 TARGET TARGET TARGET 169, 170 169 170
Y
Y
Y
Point-to-Surface
Y
Surface-to-Surface
Y
Y
Y
Y
Y
Y
Y
Y
small
small
large
large
large
2-D
Y
3-D Sliding Cylindrical Gap
small Y
Y Y
Y
Pure Lagrange Multiplier
Y
Y
Y
Y
Augmented Lagrange Multiplier
Y
Y
Y
Y
Lagrange Multiplier on Normal and Penalty on Tangent
Y
Y
Y
Y
Y
Y
Y
Internal Multipoint Constraint (MPC) Contact Stiffness
Auto-meshing Tools Lower-Order
userdefined
usersemisemisemisemidefined automat- automat- automat- automatic ic ic ic
EINTF
EINTF
EINTF
ESURF
ESURF
ESURF
Y
Y
Y
Y
Y
Y
Y (2-D only)
Y
Y
Higher- Order Rigid-Flexible
Y
Y
Y
Y
Y
Y
Flexible- Flexible
Y
Y
Y
Y
Y
Y
Thermal Contact
Y
Y
Y
Electric Contact
Y
Y
Y
Magnetic Contact
Y
Y
Y
To model a contact problem, you first must identify the parts to be analyzed for their possible interaction. If one of the interactions is at a point, the corresponding component of your model is a node. If one of the interactions is at a surface, the corresponding component of your model is an element: either a beam, shell, or solid element. 11–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.3: ANSYS Contact Capabilities The finite element model recognizes possible contact pairs by the presence of specific contact elements. These contact elements are overlaid on the parts of the model that are being analyzed for interaction. The different contact elements that ANSYS uses, and procedures for using them, are described in the remainder of this chapter. An overview of the ANSYS contact elements and their capabilities follows. For detailed information on any of these elements, refer to the ANSYS Elements Reference and the ANSYS, Inc. Theory Reference.
11.3.1. Surface-to-Surface Contact Elements ANSYS supports both rigid-to-flexible and flexible-to-flexible surface-to-surface contact elements. These contact elements use a "target surface" and a "contact surface" to form a contact pair. •
The target surface is modeled with either TARGE169 or TARGE170 (for 2-D and 3-D, respectively).
•
The contact surface is modeled with elements CONTA171, CONTA172, CONTA173, and CONTA174.
To create a contact pair, assign the same real constant number to both the target and contact elements. You can find more details on defining these elements and their shared real constant sets in Section 11.4: Performing a Surface-to-Surface Contact Analysis. These surface-to-surface elements are well-suited for applications such as interference fit assembly contact or entry contact, forging, and deep-drawing problems. The surface-to-surface contact elements have several advantages over the node-to-node element CONTA175. These elements: •
Support lower and higher order elements on the contact and target surfaces (in other words, cornernoded or midside-noded elements).
•
Provide better contact results needed for typical engineering purposes, such as normal pressure and friction stress contour plots.
•
Have no restrictions on the shape of the target surface. Surface discontinuities can be physical or due to mesh discretization.
Using these elements for a rigid target surface, you can model straight and curved surfaces in 2-D and 3-D, often using simple geometric shapes such as circles, parabolas, spheres, cones, and cylinders. More complex rigid forms or general deformable forms can be modeled using special preprocessing techniques (see Step 3 of Section 11.4: Performing a Surface-to-Surface Contact Analysis for more information). Surface-to-surface contact elements are not well-suited for point-to-point, point-to-surface, or edge-to-surface contact applications, such as pipe whip or snap-fit assemblies. You should use the node-to-surface or node-tonode elements in these cases. You also can use surface-to-surface contact elements for most contact regions and use a few node-to-surface contact elements near contact corners. The surface-to-surface contact elements only support general static and transient analyses, buckling, harmonic, modal or spectrum analyses, or substructure analyses.
11.3.2. Node-to-Surface Contact Elements CONTA175 is a node-to-surface contact element. It supports large sliding, large deformation, and different meshes between the contacting components. CONTA175 is typically used to model point-to-surface contact applications, such as two beams contacting each other (at a beam tip or sharp corner node), and the corners of snap-fit parts.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–3
Chapter 11: Contact You can also use CONTA175 to model surface-to-surface contact, if the contacting surface is defined by a group of nodes and multiple elements are generated. The surfaces can be either rigid or deformable. An example of this type of contact problem is a wire inserted into a slot. Unlike the node-to-node contact elements, you do not need to know the exact location of the contacting area beforehand, nor do the contacting components need to have a compatible mesh. Large deformation and large relative sliding are allowed, although this capability can also model small sliding. CONTA175 does not support 3-D higher-order elements on the contact surface side. The element can fail if the target surface is severely discontinous. No contour plots are available for contact results.
11.3.3. Node-to-Node Contact Elements Node-to-node contact elements are typically used to model point-to-point contact applications. To use nodeto-node contact elements, you need to know the location of contact beforehand. These types of contact problems usually involve small relative sliding between contacting surfaces (even in the case of geometric nonlinearities). An example of a node-to-node contact application is the traditional pipe whip model, where the contact point is always located between the pipe tip and the restraint. Node-to-node contact elements can also be used to solve a surface-to-surface problem if the nodes of the two surfaces line up, the relative sliding deformation is negligible, and deflections (rotations) of the two surfaces remain small. These are typically problems with faceted and simple geometry. An interference fit problem is an example of a surface-to-surface problem where the use of node-to-node contact may be sufficient. Another use of node-to-node contact elements is in extremely precise analysis of surface stresses, such as in turbine blade analysis. ANSYS element CONTA178 is the best choice for most node-to-node problems. It offers a wider range of options and solver types than the other elements. CONTAC12 and CONTAC52 are available largely for reasons of backward compatibility with existing models.
11.4. Performing a Surface-to-Surface Contact Analysis You can use the surface-to-surface contact elements to model either rigid-flexible or flexible-flexible contact between surfaces. The Contact Manager provides an easy-to-use interface to help you construct and manage contact definitions. You can access the manager via the Contact Manager icon in the ANSYS Standard Toolbar, or via the menu path Main Menu> Preprocessor> Modeling> Create> Contact Pair. See Section 11.5: GUI Aids for Contact Analyses for more information on using the Contact Manager. The following sections explain how to set up a contact analysis using the both command and GUI approaches. Note — The following sections also apply to node-to-surface contact analyses using CONTA175, unless otherwise noted.
11.4.1. Using Surface-to-Surface Contact Elements In problems involving contact between two boundaries, one of the boundaries is conventionally established as the "target" surface, and the other as the "contact" surface. For rigid-flexible contact, the target surface is always the rigid surface, and the contact surface is the deformable surface. For flexible-to-flexible contact, both contact and target surfaces are associated with the deformable bodies. These two surfaces together comprise the "contact pair." Use TARGE169 with CONTA171, CONTA172, or CONTA175 to define a 2-D contact pair. For 3-D contact
11–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis pairs, use TARGE170 with CONTA173, CONTA174, or CONTA175. Each contact pair is identified via the same real constant number. Note — If you prefer a graphical approach to setting up your contact analysis, you can use the Contact Toolbar, as discussed in Section 11.5.1: The Contact Manager.
11.4.2. Steps in a Contact Analysis The basic steps for performing a typical surface-to-surface contact analysis are listed below. Each step is then explained in detail in the following pages. 1.
Create the model geometry and mesh
2.
Identify the contact pairs
3.
Designate contact and target surfaces
4.
Define the target surface
5.
Define the contact surface
6.
Set the element KEYOPTS and real constants
7.
Define/control the motion of the target surface (rigid-to-flexible only)
8.
Apply necessary boundary conditions
9.
Define solution options and load steps
10. Solve the contact problem 11. Review the results Each contact-specific step also has a corresponding GUI approach where you use functions and features on the Contact Toolbar.
11.4.3. Creating the Model Geometry and Mesh First, create solid model entities that represent the geometry of the contacting bodies. Set element types, real constants, and material properties as you would for any ANSYS analysis. Mesh the contacting bodies by meshing the areas or volumes with the element type that you have chosen. For more information, see the ANSYS Modeling and Meshing Guide. Command(s): AMESH, VMESH GUI: Main Menu> Preprocessor> Meshing> Mesh Note — You should avoid midside-noded elemets for 3-D contact surfaces when using node-to-surface element CONTA175.
11.4.4. Identifying Contact Pairs You must identify where contact might occur during the deformation of your model. Once you've identified potential contact surfaces, you define them via target and contact elements, which will then track the kinematics of the deformation process. Target and contact elements that make up a contact pair are associated with each other via a shared real constant set. The contact zone can be arbitrary; however, for the most efficient solution (primarily in CPU time), you may want to define smaller, localized contacting zones, but be sure your zones are adequate to capture all necessary contact. Different contact pairs must be defined by a different real constant set, even if the element real constant values do not change. There is no limit on the number of surfaces allowed. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–5
Chapter 11: Contact
Figure 11.1 Localized Contact Zones
Depending on the geometry of the model (and the potential deformation), multiple target surfaces could interact with the same zone of the contact surface. In such cases, you must define multiple contact pairs (using multiple overlapping contact elements), each with its own real constant number. See Figure 11.1: “Localized Contact Zones”.
11.4.5. Designating Contact and Target Surfaces Contact elements are constrained against penetrating the target surface. However, target elements can penetrate through the contact surface. For rigid-to-flexible contact, the designation is obvious: the target surface is always the rigid surface and the contact surface is always the deformable surface. For flexible-to-flexible contact, the choice of which surface is designated contact or target can cause a different amount of penetration and thus affect the solution accuracy. Consider the following guidelines when designating the surfaces: •
If a convex surface is expected to come into contact with a flat or concave surface, the flat/concave surface should be the target surface.
•
If one surface has a fine surface mesh and, in comparison, the other has a coarse mesh, the fine mesh should be the contact surface and the coarse mesh should be the target surface.
•
If one surface is stiffer then the other, the softer surface should be the contact surface and the stiffer surface should be the target surface.
11–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis •
If higher-order elements underly one of the external surfaces and lower-order elements underly the other surface, the surface with the underlying higher-order elements should be the contact surface and the other surface should be the target. However, for 3-D node-to-surface contact, the lower-order elements should be the contact surface. The higher-order elements should be the target surface.
•
If one surface is markedly larger than the other surface, such as in the instance where one surface surrounds the other surface, the larger surface should be the target surface.
These guidelines are true for asymmetric contact; however, asymmetric contact may not perform satisfactorily for your model. The following section details the difference between asymmetric and symmetric contact and outlines some of the situations that require symmetric contact.
11.4.5.1. Asymmetric Contact vs. Symmetric Contact 11.4.5.1.1. Background Asymmetric contact is defined as having all contact elements on one surface and all target elements on the other surface. This is sometimes called "one-pass contact." This is usually the most efficient way to model surfaceto-surface contact. However, under some circumstances asymmetric contact does not perform satisfactorily. In such cases, you can designate each surface to be both a target and a contact surface. You can then generate two sets of contact pairs between the contacting surfaces (or just one contact pair; for example, a self-contact case). This is known as symmetric contact (or "two-pass contact"). Obviously, symmetric contact is less efficient than asymmetric contact. However, many analyses will require its use (typically to reduce penetration). Specific situations that require symmetric contact include models where •
The distinction between the contact and target surfaces is not clear.
•
Both surfaces have very coarse meshes. The symmetric contact algorithm enforces the contact constraint conditions at more surface locations than the asymmetric contact algorithm.
If the meshes on both surfaces are identical and sufficiently refined, the symmetric contact algorithm may not significantly improve performance and may, in fact, be more "expensive" in CPU time. In such circumstances, pick one surface to be the target and the other the contact surface. For a symmetric contact definition, ANSYS may find one side of a contact surface as closed and the other side of the surface as closed. In this case, it can be difficult to interpret the results. The total contact pressure acting on both sides is the average of the contact pressures on each side of the surface.
11.4.5.1.2. Using KEYOPT(8) When there are several contact pairs involved in the model, and the graphical picking of contact and target surfaces is difficult, you can just define the symmetric contact pairs and, by setting KEYOPT(8) = 2, ANSYS will internally select which asymmetric pair is to be used at the solution stage based on the guidelines mentioned above in Designating Contact and Target Surfaces. Note — In any contact model, you can mix different types of contact pairs: rigid-to-flexible or flexible-toflexible contact; symmetric contact or asymmetric contact. However, only one type can exist with a contact pair.
11.4.6. Defining the Target Surface The target surface can be 2-D or 3-D and either rigid or deformable. For deformable target surfaces, you will normally use the ESURF command to generate the target elements along the boundaries of an existing mesh. You can follow the same method to generate the deformable contact surface (see Section 11.4.7: Defining the
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–7
Chapter 11: Contact Deformable Contact Surface for details). You should not use the following rigid target segments for a deformable target surface: ARC, CARC, CIRC, CYL1, CONE, SPHE, or PILO. For rigid target surfaces, the following provides general guidelines. In 2-D cases, the shape of the target surface is described by a sequence of straight lines, circular arcs, and parabolas, all of which can be represented with the target segment element TARGE169. You can use any combination to define the complex target surface geometry. In 3-D cases, the shape of the target surfaces is described by a sequence of triangles, quadrilaterals, cylinders, cones, and spheres, which can be represented with TARGE170. You can use any combination of low/high-order triangles and quadrilaterals to model a target surface with a complex, arbitrary geometry.
11.4.6.1. Pilot Nodes The rigid target surface can also be associated with a "pilot node," which is really an element with one node, whose motion governs the motion of the entire target surface. You can think of a pilot node as a handle for the rigid target surface. Forces/moments or rotations/displacements for the entire target surface can be prescribed on just the pilot node. The pilot node can be one of the nodes on the target element or a node at any arbitrary location. The location of the pilot node is important only when rotation or moment loading is required. If you define a pilot node, ANSYS checks for boundary conditions only on the pilot node and ignores any constraints on other nodes.
11.4.6.2. Primitives You can use circle, cylinder, cone, and sphere primitives to model the target (which require real constants to define the radius). You can combine primitive segments with general segments (such as lines, parabolas, triangles, and quadrilaterals) to define a target surface. Primitives cannot be defined directly in the Contact Wizard.
11.4.6.3. Element Types and Real Constants Before generating the target element, first define the element type (TARGE169 for 2-D or TARGE170 for 3-D): Command(s): ET GUI: Main Menu> Preprocessor> Element Type> Add/Edit/Delete
11.4.6.3.1. Defining Target Element Geometry You define characteristics of the target element geometry through real constants R1 and R2 as follows: •
•
For CONTA171 and CONTA172: –
R1 is the radius if the target shape (TARGE169) is a circle.
–
R2 is the element thickness if the underlying element is a superelement set as plane stress with thickness (KEYOPT(3) = 3). The default value is 1.
For CONTA173 and CONTA174 (also applies to node-to-surface element CONTA175): –
R1 is the radius if the target shape (TARGE170) is a cylinder, cone, or sphere.
–
R2 is the radius of a cone at the second node.
To set the real constant number for the target elements: Command(s): REAL GUI: Main Menu> Preprocessor> Real Constants
11–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis For TARGE169 and TARGE170, you need only set real constants R1 and R2 (if required). For a complete description of the target elements, element shapes, and real constants, see the description of TARGE169 and TARGE170 in the ANSYS Elements Reference. Note — Specifying real constants (R1, R2) manually is necessary only if you use direct generation to create your target elements. You can also use the ANSYS meshing tools to create the elements, or use the Contact Toolbar.
11.4.6.4. Using Direct Generation to Create Rigid Target Elements To generate target elements directly, use the following command or GUI path: Command(s): TSHAP GUI: Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes You then specify the element shape. Possible shapes are: •
Straight line (2-D)
•
Parabola (2-D)
•
Clockwise arc (2-D)
•
Counterclockwise arc (2-D)
•
Circle (2-D)
•
Three-node triangle (3-D)
•
Six-node triangle (3-D)
•
Four-node quadrilateral (3-D)
•
Eight-node quadrilateral (3-D)
•
Cylinder (3-D)
•
Cone (3-D)
•
Sphere (3-D)
•
Pilot node (both 2-D and 3-D)
Once you specify a target element shape, all subsequent elements will have that shape until you specify another shape. Note — You cannot mix 2-D and 3-D target elements on the same target surface. You cannot mix rigid target elements with deformable target elements on the same target surface. During solution, ANSYS assigns a deformable status to target elements with underlying elements and assigns a rigid status to target elements without underlying elements. If a portion of the underlying elements of a deformable surface are deleted, an error will occur in solution. You can generate the nodes and elements using standard ANSYS direct generation techniques. For more information on direct generation modeling techniques, see Chapter 9, “Direct Generation” in the ANSYS Modeling and Meshing Guide. Command(s): N, E GUI: Main Menu> Preprocessor> Modeling> Create> Nodes Main Menu> Preprocessor> Modeling> Create> Elements You can then verify your element shapes by listing the elements. Command(s): ELIST Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–9
Chapter 11: Contact GUI: Utility Menu> List> Elements> Nodes + Attributes
11.4.6.5. Using ANSYS Meshing Tools to Create Rigid Target Elements You can also let ANSYS generate the elements automatically using the standard ANSYS meshing capabilities. ANSYS will recognize the proper target element shape based on the solid model and will ignore the TSHAP setting. To generate a pilot node, use the following command or GUI path: Command(s): KMESH GUI: Main Menu> Preprocessor> Meshing> Mesh> Keypoints Note — KMESH always creates pilot nodes. To generate 2-D rigid target elements, use the following command or GUI path. ANSYS creates a single line over each line, parabolic segments over B-splines, and arc segments over each arc and line fillet (see Figure 11.2: “ANSYS Geometric Entities and Their Corresponding Rigid Target Elements”). If all the arcs form a closed circle, ANSYS creates a single circular segment (see Figure 11.3: “A Single Circular Target Segment Created From Arc Line Segments”). However, if the arcs that form a closed circle are created from imported or archived geometry (such as IGES), ANSYS might not create a single circular segment. Command(s): LMESH GUI: Main Menu> Preprocessor> Meshing> Mesh> Lines
Figure 11.2 ANSYS Geometric Entities and Their Corresponding Rigid Target Elements
11–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
Figure 11.3 A Single Circular Target Segment Created From Arc Line Segments
To generate 3-D rigid target elements, use the following command or GUI path. Command(s): AMESH GUI: Main Menu> Preprocessor> Meshing> Mesh> Areas If the surface segments on the solid model form a complete sphere, cylinder, or cone, then ANSYS automatically generates a single primitive 3-D target element through the AMESH command. By creating fewer elements, the analysis becomes more computationally efficient. For arbitrary surfaces, you should use AMESH to generate target elements. In these cases, the quality of the meshed target shape is not important. It is more important that the target elements represent the rigid surface geometry well. We recommend using mapped meshing on all possible areas. If there is no curvature on the edges of the surface, assign one division on that edge. TARGE169 with a rigid specification will always mesh with one element division, per line, ignoring any LESIZE setting. The default target element shape is quadrilateral. If you want a triangular target element shape, use MSHAPE,1. Figure 11.4: “Meshing Patterns for Arbitrary Target Surfaces” shows the meshing patterns for arbitrary target surfaces. The following command or GUI path will generate a mapped mesh wherever possible (otherwise, if not possible, it will generate a free mesh). Command(s): MSHKEY,2 GUI: Main Menu> Preprocessor> Meshing> Mesh> Areas> Target Surf If the target surface is flat (or nearly flat), you may select low-order target elements (3-node triangular or 4-node quadrilateral elements). If the target surface is curved you should select high-order target elements (6-node triangular or 8-node quadrilateral). By doing so, set KEYOPT(1) = 1 in the target element definition. Note — Low-order target elements result in "cheaper" CPU usage in getting penetration and gap; however, the meshed surface may not be smooth. Higher-order target elements are more "expensive" to use in getting the penetration and gap, but they need many fewer elements to discretize the whole curved target surface. Note — If target elements are created via program meshing (through the KMESH, LMESH, or ESURF commands) the TSHAP command is ignored and ANSYS chooses the correct shape codes automatically.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–11
Chapter 11: Contact
Figure 11.4 Meshing Patterns for Arbitrary Target Surfaces
11.4.6.5.1. Some Modeling and Meshing Tips A target surface can be made up of two or more disconnected regions. Where possible, you should localize the contact zone by defining multiple target surfaces (each with a different real constant number). There are no restrictions on the shape of the rigid surfaces. Smoothing is not required. However, you must ensure that the mesh discretization of the curved surfaces on the rigid target surface is adequate. Excessively coarse discretization can cause numerical convergence problems. It can be difficult to obtain a converged solution in a large sliding simulation if the target surface has sharp convex corners. To avoid such modeling problems, use line or area fillet functions on the solid model to smooth out the sharp corner, use a more refined mesh, or use high-order element in the region of abrupt curvature changes (see Figure 11.5: “Smoothing Convex Corner”).
11–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
Figure 11.5 Smoothing Convex Corner
11.4.6.5.2. Verifying Nodal Number Ordering (Contact Direction) of Target Surface The node order of the target surface elements is critical because it defines contact direction. For 2-D contact, the associated (deformable) contact elements must lie to the right of the target surface when moving from the first node to the second node along the target surface line (see Figure 11.6: “Correct Node Ordering”).
Figure 11.6 Correct Node Ordering
For 3-D contact, the target triangular element numbering should be such that the rigid surface's outward normal points toward the contact surface. The outward normal is determined by the right-hand rule. To check the direction of the normals, turn on the element coordinate systems. Command(s): /PSYMB,ESYS,1 Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–13
Chapter 11: Contact GUI: Utility Menu> PlotCtrls> Symbols If the element normals do not point toward the contact surface, select this element and reverse the direction of the surface normals. Command(s): ESURF,,REVE GUI: Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surf to Surf or, reorient the element normals: Command(s): ENORM GUI: Main Menu> Preprocessor> Modeling> Move/Modify> Elements> Shell Normals Note — Contact on target primitives (such as a complete circle, cylinder, cone, or sphere), can occur only on the outside surfaces of such target bodies.
11.4.7. Defining the Deformable Contact Surface To create the deformable contact surface, you must define that surface using contact elements CONTA171 or CONTA172 (for 2-D), or CONTA173 or CONTA174 (for 3-D), or CONTA175 for (2- or 3-D). The contact surface is defined by the set of contact elements that comprise the surface of the deformable body. These contact elements have the same geometric characteristics as the underlying elements of the deformable body. The contact surface elements are of the same order as the underlying elements (lower- or higher-order), with compatible nodes along the edges. The higher-order contact elements can match lower-order underlying elements by dropping the midside nodes. The underlying elements can be solid, shell, or 2-D beam elements. The contact surface can be on either side of the shell or beam elements. The underlying elements may also be a superelement. However, axisymmetric harmonic elements may not be used as underlying elements. As with the target surface elements, you must define the contact surface element type, then select the correct real constant number (the real constant number must be the same as the one used for the target surface for each contact pair), and finally generate the elements.
11.4.7.1. Element Type The four contact element types are listed below, along with a brief description. For complete information on these element types, see the ANSYS Elements Reference.
11–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
Figure 11.7 Contact Element Types
•
CONTA171: This element is a 2-D, 2-node, lower-order line element that can be located on the surfaces of 2-D solid, shell, or beam elements (such as BEAM3, PLANE42, or SHELL51).
•
CONTA172: This element is a 2-D, 3-node, higher-order parabolic element that can be located on the surfaces of 2-D solid or beam elements with midside nodes (such as PLANE82 or VISCO88).
•
CONTA173: This element is a 3-D, 4-node, lower-order quadrilateral element that can be located on the surfaces of 3-D solid or shell elements (such as SOLID45 or SHELL181). It can be degenerated to a 3-node triangular element.
•
CONTA174: This element is a 3-D, 8-node, higher-order quadrilateral element that can be located on the surfaces of 3-D solid or shell elements with midside nodes (such as SOLID92, SOLID95, or SHELL93). It can be degenerated to 3 - 7 node quadrilateral/triangular shapes.
•
CONTA175: This element is a 2- or 3-D 1-node element that can be located on the surface of 2-D low order and higher order solid or beam elements or 3-D low order solid or shell elements. Command(s): ET GUI: Main Menu> Preprocessor> Element Type> Add/Edit/Delete Note — Use CONTA175 for node-to-surface contact.
11.4.7.2. Real Constants and Material Properties After defining the element type, you need to select the correct real constant set. The real constant set for each contact surface must be the same one used for the corresponding target surface for each contact pair. Each contact pair must reference its own real constant number. ANSYS uses the material properties of the underlying elements to calculate an appropriate contact (or penalty) stiffness. In cases where the underlying element has TB plasticity material properties defined (whether active or not), the contact normal stiffness will be reduced by a factor of 100. ANSYS automatically defines a default value for tangent (sliding) contact stiffness that is proportional to MU and the normal stiffness. If the underlying element is a superelement, the material property set for the contact elements must be the same as that of the original structural elements used during the formation of the superelement. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–15
Chapter 11: Contact
11.4.7.3. Generating Contact Elements You can generate contact elements either through direct generation or by generating the surface automatically from the exterior faces of the underlying elements. We recommend that you use automatic generation; this approach is simpler and more reliable. To automatically generate contact elements, follow these steps: 1.
Select the nodes on the meshed deformable body. For each surface, view the node list. If you are certain that particular nodes will never come into contact, you can omit those nodes and reduce CPU time. However, you should always include more nodes than you think you'll need so that you don't miss unexpected areas of contact. Command(s): NSEL GUI: Utility Menu> Select> Entities
2.
Generate the contact elements. Command(s): ESURF GUI: Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surf to Surf If the contact surface is attached to areas or volumes that are meshed with solid elements, ANSYS automatically determines the outward normal needed for contact calculations. If the underlying elements are beam or shell elements, you must indicate which surface (top or bottom) is the target surface. Command(s): ESURF,,TOP or BOTTOM GUI: Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surf to Surf Use the TOP setting (default) to generate contact elements with their outward normals the same as the beam or shell elements' normals. Use the BOTTOM setting to generate contact elements with their outward normals opposite the beam or shell elements' normals. You must make sure that all elements in the beam or shell element selection have their normals consistently oriented. If the underlying elements are solid elements, then the TOP or BOTTOM setting has no effect.
3.
11–16
Check the direction of the outward normals for the contact elements. The direction of the contact surface's outward normal is critical for proper contact detection. For 3-D elements, the node numbering follows the right hand rule to define its outward normal. The contact surface's outward normal should point toward the target surface. Otherwise, ANSYS may detect over-penetration of the surfaces at the beginning of the analysis and have difficulty finding an initial solution. In most of these cases, the analysis will fail immediately. Figure 11.8: “Specification of the Contact Surface's Outward Normal” illustrates both proper and improper specification of the contact surface's outward normal. Command(s): /PSYMB,ESYS GUI: Utility Menu> PlotCtrls> Symbols
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
Figure 11.8 Specification of the Contact Surface's Outward Normal
If the surface normals are specified incorrectly, you must either change them by reversing the node number order of the selected elements. Command(s): ESURF,,REVE GUI: Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surf to Surf or, reorient the element normals. Command(s): ENORM GUI: Main Menu> Preprocessor> Modeling> Move/Modify> Elements> Shell Normals Note — ESURF,,TOP or BOTTOM and checking the direction of outward normals will not apply to nodeto-surface contact (CONTA175) because it is a single-node element with no surface normal associated with it.
11.4.8. Set the Real Constants and Element KEYOPTS ANSYS uses several real constants and KEYOPTs to control contact behavior using these surface-to-surface contact elements. For more information in addition to what is presented here, refer to the individual contact element descriptions in the ANSYS Elements Reference.
11.4.8.1. Real Constants Two real constants, R1 and R2, are used to define the geometry of the target surface elements. The remaining are used by the contact surface elements. •
R1 and R2 define the target element geometry.
•
FKN defines a normal contact stiffness factor.
•
FTOLN is a factor based on the thickness of the element which is used to calculate allowable penetration.
•
ICONT defines an initial closure factor (or adjustment band).
•
PINB defines a "pinball" region.
•
PMIN and PMAX define an allowable penetration range for initial penetration.
•
TAUMAX specifies the maximum contact friction.
•
CNOF specifies the positive or negative offset value applied to the contact surface.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–17
Chapter 11: Contact •
FKOP specifies the stiffness factor applied when contact opens.
•
FKT specifies the tangent contact stiffness.
•
COHE specifies the cohesion sliding resistance.
•
TCC specifies the thermal contact conductance coefficient.
•
FHTG specifies the fraction of frictional dissipated energy converted into heat.
•
SBCT specifies the Stefan-Boltzmann constant.
•
RDVF specifies the radiation view factor.
•
FWGT specifies the weight factor for the distribution of heat between the contact and target surfaces for thermal contact or for electric contact.
•
ECC specifies the electric contact conductance or capacitance per unit area.
•
FHEG specifies the fraction of electric dissipated energy converted into heat.
•
FACT specifies the ratio of static to dynamic coefficients of friction.
•
DC specifies the decay coefficient for static/dynamic friction.
•
SLTO controls maximum sliding distance when MU is nonzero and the tangent contact stiffness (FKT) is updated at each iteration (KEYOPT(10) = 2).
•
TNOP specifies the maximum allowable tensile contact pressure.
•
TOLS adds a small tolerance that extends the edge of the target surface.
•
MCC specifies the magnetic contact permeance (3-D only).
Real constant defaults can vary depending on the environment you are working in. The following table compares the default values between ANSYS and the ANSYS Workbench. See your ANSYS sales representative for more information about ANSYS Workbench.
Table 11.2 Summary of Real Constant Defaults in Different Environments Real Constants
Description
ANSYS Default ANSYS Workbench Default
No.
Name
1
R1
Target circle radius
0
n/a
2
R2
Superelement thickness
1
n/a
3
FKN
Normal penalty stiffness factor
1
[1]
4
FTOLN
Penetration tolerance factor
0.1
0.1
5
ICONT
Initial contact closure
0
0
6
PINB
Pinball region
[2]
[2]
7
PMAX
Upper limit of initial penetration
0
0
8
PMIN
Lower limit of initial penetration
0
0
9
TAUMAX
Maximum friction stress
1.00E+20
1.00E+20
10
CNOF
Contact surface offset
0
0
11
FKOP
Contact opening stiffness
1
1
12
FKT
Tangent penalty stiffness
1
1
13
COHE
Contact cohesion
0
0
14
TCC
Thermal contact conductance
0
[3]
11–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis Real Constants
Description
ANSYS Default ANSYS Workbench Default
No.
Name
15
FHTG
Frictional heating factor
1
1
16
SBCT
Stefan-Boltzmann constant
0
n/a
17
RDVF
Radiation view factor
1
n/a
18
FWGT
Heat distribution weighing factor
0.5
0.5
19
ECC
Electric contact conductance
0
n/a
20
FHEG
Joule dissipation weighting factor
1
n/a
21
FACT
Static/dynamic ratio
1
1
22
DC
Exponential decay coefficient
0
0
23
SLTO
Allowable elastic slip
1%
1%
24
(blank)
25
TOLS
Target edge extension factor
[4]
[4]
26
MCC
Magnetic contact permeance
0
n/a
1.
FKN = 10 for bonded. For all other, FKN = 1.0, but if bonded and other contact behavior exists, FKN = 1 for all.
2.
Depends on contact behavior (rigid vs. flex target), NLGEOM,ON or OFF, KEYOPT(9) setting, KEYOPT(12) setting, and the value of CNOF (see Section 11.4.8.9.2: Using PINB).
3.
Calculated as a function of highest conductivity and overall model size.
4.
10% of target length for NLGEOM,OFF. 2% of target length for NLGEOM,ON. Command(s): R GUI: Main Menu> Preprocessor> Real Constants
11.4.8.1.1. Positive and Negative Real Constant Values For the real constants FKN, FTOLN, ICONT, PINB, PMAX, PMIN, FKOP, FKT, SLTO, and TNOP, you can specify either a positive or negative value. ANSYS interprets a positive value as a scaling factor and interprets a negative value as the absolute value. ANSYS uses the depth of the underlying element as the reference value to be used for ICONT, FTOLN, PINB, PMAX, and PMIN. For example, a positive value of 0.1 for ICONT indicates an initial closure factor of 0.1 x depth of the underlying element. However, a negative value of 0.1 indicates an actual adjustment band of 0.1 units. When KEYOPT(10) = 0, 1, or 2, all the contact related settings (ICONT, FTOLN, PINB, PMAX, PMIN, FKN, FKT, SLTO) are averaged across all contact elements in a contact pair. However, when KEYOPT(10) = 3, 4, or 5, the settings are based on each individual contact element (geometry and material behaviors). Figure 11.9: “Depth of the Underlying Element” shows the depth of the underlying element for a solid element. If the underlying elements are shell or beam elements, the depth will usually be 4 times the element thickness.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–19
Chapter 11: Contact
Figure 11.9 Depth of the Underlying Element
When KEYOPT(10) = 0, 1, or 2, each contact pair has a pair-based depth which is obtained by averaging the depth of each contact element across all the contact elements in a contact pair. This can avoid the problem of very different element-based depths when there are meshes with large variations in element sizes. Note — When the contact pair depth is too small (for example, 10-5), the machine precision may not guarantee the accuracy of penetration to be calculated. You should scale the length unit in the model.
11.4.8.2. Element KEYOPTS Each contact element includes several KEYOPTS. We recommend using the default settings, which are suitable for most contact problems. For some specific applications, you can override the defaults. The element KEYOPTS allow you to control several aspects of contact behavior. •
Degrees of freedom (KEYOPT(1))
•
Contact algorithm (defaults to augmented Lagrangian) (KEYOPT(2))
•
Stress state when superelements are present (KEYOPT(3)) for 2-D surface-to-surface contact. Contact model for node-to-surface contact.
•
Location of contact detection point (KEYOPT(4))
•
CNOF Automated adjustment (KEYOPT(5))
•
Time step control (KEYOPT(7))
•
Asymmetric contact selection (KEYOPT(8))
•
Effect of initial penetration or gap (KEYOPT(9))
•
Contact stiffness update (KEYOPT(10))
•
Shell thickness effect (KEYOPT(11))
•
Behavior of contact surface (rough, bonded, etc.) (KEYOPT(12))
11–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis KEYOPT defaults can vary depending on the environment you are working in. The following table compares the default values between ANSYS, the ANSYS Contact Wizard, and the ANSYS Workbench. See your ANSYS sales representative for more information about ANSYS Workbench.
Table 11.3 Summary of KEYOPT Defaults in Different Environments KEYOPT Description
ANSYS
ANSYS Contact Wizard
ANSYS Workbench Default Linear (bonded, no sep)
ANSYS Workbench, Default Nonlinear (standard, rough)
1
Selects DOF*
Manual
Auto
Auto
Auto
2
Contact Algorithm
Aug. Lagr. Aug. Lagr. Pure Penalty
3
Stress state when superelement no super is present elem
no super elem
n/a
n/a
4
Location of contact detection point
gauss
gauss
gauss
gauss
5
CNOF/ICONT adjustment
No adjust
No adjust
No adjust
No adjust
6
(blank)
7
Element level time increment control
No control No control No control
No control
8
Asymmetric contact selection
No action
No action
9
Effect of initial penetration or gap
Include all Include all Exclude all
Include all/ramped
10
Contact stiffness update
Between Between load steps substeps
Between load steps
Between load steps
11
Beam/shell thickness effect
Exclude
Exclude
Exclude
Exclude
12
Behavior of contact surface
Standard
Standard
Bonded
n/a
No action
No action
Pure Penalty
*Manual: Requires user to define. Auto: Selection is based on DOF of underlying element. Command(s): KEYOPT, ET GUI: Main Menu> Preprocessor> Element Type> Add/Edit/Delete
11.4.8.3. Selecting a Contact Algorithm (KEYOPT(2)) 11.4.8.3.1. Background For surface-to-surface contact elements, ANSYS offers several different contact algorithms: •
Penalty method (KEYOPT(2) = 1)
•
Augmented Lagrangian (default) (KEYOPT(2) = 0)
•
Lagrange multiplier on contact normal and penalty on tangent (KEYOPT(2) = 3)
•
Pure Lagrange multiplier on contact normal and tangent (KEYOPT(2) = 4)
•
Internal multipoint constraint (MPC) (KEYOPT(2) = 2)
The penalty method uses a contact “spring” to establish a relationship between the two contact surfaces. The spring stiffness is called the contact stiffness. This method uses the following real constants: FKN and FKS for all values of KEYOPT(10), plus FTOLN and SLTO if KEYOPT(10) = 1 or 2. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–21
Chapter 11: Contact The augmented Lagrangian method (which is the default) is an iterative series of penalty methods. The contact tractions (pressure and frictional stresses) are augmented during equilibrium iterations so that the final penetration is smaller than the allowable tolerance (FTOLN). Compared to the penalty method, the augmented Lagrangian method usually leads to better conditioning and is less sensitive to the magnitude of the contact stiffness. However, in some analyses, the augmented Lagrangian method may require additional iterations, especially if the deformed mesh becomes too distorted. The pure Lagrange multiplier method enforces zero penetration when contact is closed and “zero slip” when sticking contact occurs. The pure Lagrange multiplier method does not require contact stiffness, FKN and FKS. Instead it requires chattering control parameters, FTOLN and TNOP. This method adds contact traction to the model as additional degrees of freedom and requires additional iterations to stabilize contact conditions. It often increases the computational cost compared to the augmented Lagrangian method. An alternative algorithm is the Lagrange multiplier method applied on the contact normal and the penalty method (tangential contact stiffness) on the frictional plane. This methods enforces zero penetration and allows a small amount of slip for the sticking contact condition. It requires chattering control parameters, FTOLN and TNOP, as well as the maximum allowable elastic slip parameter SLTO. Another method, the internal multipoint constraint (MPC) algorithm, is used in conjunction with bonded contact (KEYOPT(2) = 5 or 6) to model several types of contact assemblies and kinematic constraints. See Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints for more information on how to use this feature. Note — The Lagrange multiplier methods (KEYOPT(2) = 3, 4) and MPC approach (KEYOPT(2) = 2) do not support the Gauss point detection option (KEYOPT(4) = 0) for surface-to-surface contact. They support the nodal detection options for surface-to-surface contact and node-to-surface contact. When using these options, be careful not to overconstrain the model. The model is overconstrained when a contact node has prescribed boundary conditions, CE and CP equations. ANSYS usually detects and eliminates the overconstraints. However, there is no guarantee that the program will eliminate all the cases of overconstraint. You should always verify your model carefully to address this issue. The Lagrange multiplier also introduces more degrees of freedom which may result in spurious modes for modal and linear eigenvalue buckling analyses. The augmented Lagrangian method would be a better choice for these analysis types. Note — The Lagrange multiplier methods (KEYOPT(2) = 3, 4) introduce zero diagonal terms in the stiffness matrix. Any iterative solver (PCG or AMG) will encounter a preconditioning matrix singularity with these methods. Therefore, you should switch to sparse solver.
11.4.8.4. Determining Contact Stiffness and Allowable Penetration 11.4.8.4.1. Background For the augmented Lagrangian method and penalty method, normal and tangential contact stiffnesses are required. The amount of penetration between contact and target surfaces depends on the normal stiffness. The amount of slip in sticking contact depends on the tangential stiffness. Higher stiffness values decrease the amount of penetration/slip, but can lead to ill-conditioning of the global stiffness matrix and to convergence difficulties. Lower stiffness values can lead to a certain amount of penetration/slip and produce an inaccurate solution. Ideally, you want a high enough stiffness that the penetration/slip is acceptably small, but a low enough stiffness that the problem will be well-behaved in terms of convergence. ANSYS provides default values for contact stiffnesses (FKN, FKT), allowable penetration (FTOLN), and allowable slip (SLTO). In most cases, you do not need to define the contact stiffness. In addition, we recommend that you use KEYOPT(10) = 1 to allow the program to update the contact stiffness automatically. 11–22
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
11.4.8.4.2. Using FKN and FTOLN For certain contact problems, you may choose to use the real constant FKN to define a normal contact stiffness factor. The usual factor range is from 0.01-1.0, with a default of 1.0. The default value is appropriate for bulk deformation. If bending deformation dominates, we recommend using a smaller value (0.1). In cases where the underlying element has a TB plasticity material defined (whether plasticity is active or not), the contact normal stiffness will be reduced by a factor of 100. Use real constant FTOLN in conjunction with the augmented Lagrangian method. FTOLN is a tolerance factor to be applied in the direction of the surface normal. The range for this factor is less than 1.0 (usually less than 0.2), with a default of 0.1, and is based on the depth of the underlying solid, shell, or beam element (see Figure 11.9: “Depth of the Underlying Element”). This factor is used to determine if penetration compatibility is satisfied. Contact compatibility is satisfied if penetration is within an allowable tolerance (FTOLN times the depth of underlying elements). The depth is defined by the average depth of each individual contact element in the pair. If ANSYS detects any penetration larger than this tolerance, the global solution is still considered unconverged, even though the residual forces and displacement increments have met convergence criteria. You can also define an absolute allowable penetration by specifying a negative value for FTOLN. Note — When the contact stiffness is too large (for example, 1016), the machine precision may not guarantee good conditioning of the global stiffness matrix. In this case, you should scale the force unit in the model if possible. Note — FTOLN is also used in the Lagrange multiplier methods (KEYOPT(2) = 3, 4) as a chattering control parameter.
11.4.8.4.3. Using FKT and SLTO ANSYS automatically defines a default tangential contact stiffness that is proportional to MU and the normal stiffness FKN. The default tangential stiffness corresponds to a default value of FKT = 1.0. A positive value for FKT is a factor; a negative value indicates an absolute value of tangential stiffness. For KEYOPT(10) = 1 or 2, or when the Lagrange multiplier on normal and penalty on tangent option is used (KEYOPT(2) = 3), ANSYS updates tangential contact stiffness based on current contact normal pressure, PRES, and maximum allowable elastic slip, SLTO (FKT = MU* PRES/SLTO). The real constant SLTO is used to control maximum sliding distance when FKT is updated at each iteration. ANSYS provides default tolerance values which work well in most cases. You can override the default values for SLTO (1% of average contact length in pair) by defining a scaling factor (positive value when using command input) or an absolute value (negative value when using command input). A larger value will enhance convergence but compromise accuracy. Based on the tolerance, current normal pressure, and friction coefficient, the tangential contact stiffness FKT can be obtained automatically. In certain cases users can override FKT by defining a scaling factor (positive input value) or absolute value (negative input value) (see Positive and Negative Real Constants for more information).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–23
Chapter 11: Contact Note — FKN, FTOLN, FKT, and SLTO can be modified from one load step to another. They can also be adjusted in a restart run. Determining a good stiffness value may require some experimentation on your part. To arrive at a good stiffness value, you can try the following procedure as a “trial run”: 1.
Use a low value for the contact stiffness to start. In general, it is better to underestimate this value rather than overestimate it. Penetration problems resulting from a low stiffness are easier to fix than convergence difficulties that arise from a high stiffness.
2.
Run the analysis up to a fraction of the final load (just enough to get the contact fully established).
3.
Check the penetration and the number of equilibrium iterations used in each substep. If the global convergence difficulty is caused by too much penetration (rather than by residual forces and displacement increments), FKN may be underestimated or FTOLN may be too small. If the global convergence requires many equilibrium iterations for achieving convergence tolerances of residual forces and displacements rather than the resulting penetration, FKN or FKT may be overestimated.
4.
Adjust FKN, FKT, FTOLN, or SLTO as necessary and run the full analysis. If the penetration control becomes dominant in the global equilibrium iterations (that is, if more iterations were used to converge the problem to within the penetration tolerance than to converge the residual forces), you may increase FTOLN to permit more allowable penetration or increase FKN.
Note — Generally, the contact stiffness FKN, FKT has units FORCE/LENGTH3. However, for contact forcebased models (KEYOPT(3) = 0) in CONTA175, the contact stiffness has units FORCE/LENGTH.
11.4.8.4.4. Using KEYOPT(10) The normal and tangential contact stiffness can be updated during the course of an analysis, either automatically (due to large strain effects that change the underlying element's stiffness) or explicitly (by user-specified FKN or FKT values). KEYOPT(10) governs how the normal and tangential contact stiffness is updated when the augmented Lagrangian or penalty method is used. In most cases we recommend that you use KEYOPT(10) = 1 to allow the program to update contact stiffnesses automatically. The possible settings for KEYOPT(10) are outlined below. •
KEYOPT(10) = 0, the contact stiffness will be updated at each load step if FKN or FKT is redefined by the user. Stiffness and other settings (ICONT, FTOLN, SLTO, PINB, PMAX, and PMIN) are averaged across contact elements in a contact pair. The default contact stiffness is determined by underlying element depth and material properties.
•
KEYOPT(10) = 1 (covers KEYOPT(10) = 0), the normal contact stiffness will be updated at every substep based on the mean stress of the underlying elements from the previous substep and the allowable penetration, FTOLN, except in the first substep of the first load step. The default normal contact stiffness for the first substep of the first load step is the same as described for KEYOPT(10) = 0. If bisections occur in the beginning of the analysis, the normal contact stiffness will be reduced by a factor of 0.2 for each bisection. The tangential contact stiffness will be updated at each iteration based on the current contact pressure, MU, and allowable slip (SLTO).
•
KEYOPT(10) = 2 (covers KEYOPT(10) = 1), the normal contact stiffness will be updated at each iteration based on the current mean stress of the underlying elements and the allowable penetration, FTOLN, except in the very first iteration. The default normal contact stiffness for the first iteration is the same as described for KEYOPT(10) = 0. If bisections occur in the beginning of the analysis, the normal contact stiffness will be reduced by a factor of 0.2 for each bisection. The tangential contact stiffness will be updated at each iteration based on the current contact pressure, MU, and allowable slip (SLTO).
•
KEYOPT(10) = 3, same as KEYOPT(10) = 0, except stiffness and settings are not averaged across the contact elements in a contact pair. If bisections occur in the beginning of the analysis, the normal contact stiffness will be reduced by a factor of 0.2 for each bisection.
11–24
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis •
KEYOPT(10) = 4, same as KEYOPT(10) = 1, except stiffness and settings are not averaged across the contact elements in a contact pair.
•
KEYOPT(10) = 5, same as KEYOPT(10) = 2, except stiffness and settings are not averaged across the contact elements in a contact pair. Note — When a Lagrange multiplier method (KEYOPT(2) = 3, 4) or MPC algorithm (KEYOPT(2) = 2) is used, KEYOPT(10) is ignored.
11.4.8.4.5. Chattering Control Parameters The Lagrange multiplier methods (KEYOPT(2) = 3, 4) do not require contact stiffness, FKN and FKT. Instead they require chattering control parameters, FTOLN and TNOP, by which ANSYS assumes that the contact status remains unchanged. FTOLN is the maximum allowable penetration and TNOP is the maximum allowable tensile contact pressure. Note — A negative contact pressure occurs when the contact status is closed. A tensile contact pressure (positive) refers to a separation between the contact surfaces, but not necessarily an open contact status. The behavior can be described as follows: •
If the contact status from the previous iteration is open and the current calculated penetration is smaller than FTOLN, then contact remains open. Otherwise the contact status switches to closed and another iteration is processed.
•
If the contact status from the previous iteration is closed and the current calculated contact pressure is positive but smaller than TNOP, then contact remains closed. If the tensile contact pressure is larger than TNOP, then the contact status changes from closed to open and ANSYS continues to the next iteration.
ANSYS will provide reasonable defaults for FTOLN and TNOP. FTOLN defaults to the displacement convergence tolerance. TNOP defaults to the force convergence tolerance divided by contact area at contact nodes. Keep in mind the following when providing values for FTOLN and TNOP: •
A positive value is a scaling factor applied to the default values.
•
A negative value is used as an absolute value (which overrides the default).
The objective of FTOLN and TNOP is to provide stability to models which exhibit contact chattering due to changing contact status. If the values you use for these tolerances are too small, the solution will require more iterations. However, if the values are too large, the accuracy of the solution will be affected since a certain amount of penetration or tensile contact force is allowed.
11.4.8.5. Choosing a Friction Model 11.4.8.5.1. Background In the basic Coulomb friction model, two contacting surfaces can carry shear stresses up to a certain magnitude across their interface before they start sliding relative to each other. This state is known as sticking. The Coulomb friction model defines an equivalent shear stress τ, at which sliding on the surface begins as a fraction of the contact pressure p (τ = µp + COHE, where µ is the friction coefficient and COHE specifies the cohesion sliding resistance). Once the shear stress is exceeded, the two surfaces will slide relative to each other. This state is known as sliding. The sticking/sliding calculations determine when a point transitions from sticking to sliding or vice versa.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–25
Chapter 11: Contact For frictionless, rough, and bonded contact, the contact element stiffness matrices are symmetric. Contact problems involving friction produce unsymmetric stiffnesses. Using an unsymmetric solver is more computationally expensive than a symmetric solver for each iteration. For this reason, ANSYS uses a symmetrization algorithm by which most frictional contact problems can be solved using solvers for symmetric systems. If frictional stresses have a substantial influence on the overall displacement field and the magnitude of the frictional stresses is highly solution dependent, the symmetric approximation to the stiffness matrix may provide a low rate of convergence. In such cases, choose the unsymmetric solution option (NROPT,UNSYM) to improve convergence.
11.4.8.5.2. Using TAUMAX, FACT, DC, and COHE One of the material properties used for contact elements is input via the interface coefficient of friction, MU, for the Coulomb friction model. Use MU = 0 for frictionless contact. For rough or bonded contact (KEYOPT(12) = 1, 3, 5, or 6, see Selecting Surface Interaction Models), ANSYS assumes infinite frictional resistance regardless of specified value of µ. MU can be specified as a function of temperature. If the underlying element is a superelement (MATRIX50), the material property set must be the same as the one used for the original elements that were assembled into the superelement. ANSYS provides one extension of classical Coulomb friction: TAUMAX is maximum contact friction with units of stress. This maximum contact friction stress can be introduced so that, regardless of the magnitude of normal contact pressure, sliding will occur if the friction stress reaches this value. You typically use TAUMAX when the contact pressure becomes very large (such as in bulk metal forming processes). TAUMAX defaults to 1.0e20. σy Empirical data is often the best source for TAUMAX. Its value may be close to the material being deformed.
3
, where σy is the yield stress of
Another real constant used for the friction law is the cohesion, COHE (default COHE = 0), which has units of stress. It provides sliding resistance, even with zero normal pressure (see Figure 11.10: “Sliding Contact Resistance”).
Figure 11.10 Sliding Contact Resistance
Two other real constants, FACT and DC are involved in specifying static and dynamic friction coefficients, as described in the next section.
11.4.8.5.3. Static and Dynamic Friction Coefficients The coefficient of friction can depend on the relative velocity of the surfaces in contact. Typically, the static coefficient of friction is higher than the dynamic coefficient of friction. ANSYS provides the following exponential decay friction model:
µ = MU × (1 + (FACT − 1)exp( − DC × Vrel )) where: 11–26
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis µ = coefficient of friction. MU = dynamic coefficient of friction input using the MP command. FACT = ratio of static to dynamic coefficients of friction. It defaults to the minimum value of 1.0 DC = decay coefficient. It defaults to 0.0 and it has units of time/length. Therefore, time has some meaning in a static analysis. Vrel = slip rate calculated by ANSYS. Figure 11.11: “Friction Decay” shows the exponential decay curve where the static coefficient of friction is given by:
µs
= FACT × MU
Figure 11.11 Friction Decay
You can determine the decay coefficient if you know the static and dynamic coefficients of friction and at least one data point (µ1 ; Vrel1). The equation for friction decay can be rearranged to give:
DC = −
µ1 − MU × ln Vrel1 (FACT − 1) × MU 1
If you do not specify a decay coefficient and FACT is greater than 1.0, the coefficient of friction will change suddenly from the static to the dynamic value as soon as contact reaches the sliding state. This behavior is not recommended because the discontinuity may lead to convergence difficulties.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–27
Chapter 11: Contact
11.4.8.6. Selecting Location of Contact Detection 11.4.8.6.1. Background Contact detection points are located at the integration points of the contact elements which are interior to the element surface. The contact element is constrained against penetration into the target surface at its integration points. However, the target surface can, in principle, penetrate through into the contact surface, see Figure 11.12: “Contact Detection Located at Gauss Point”.
Figure 11.12 Contact Detection Located at Gauss Point
ANSYS surface-to-surface contact elements use Gauss integration points as a default, which generally provide more accurate results than the nodal detection scheme, which uses the nodes themselves as the integration points. The node-to-surface contact element CONTA175 always uses the nodal detection scheme.
11.4.8.6.2. Using KEYOPT(4) and TOLS The nodal detection algorithms require the smoothing of the contact surface (KEYOPT(4) = 1) or the smoothing of the target surface (KEYOPT(4) = 2), which is quite time consuming. You should use this option only to deal with corner, point-surface, or edge-surface contact (see Figure 11.13: “Contact Detection Point Location at Nodal Point”). KEYOPT(4) = 1 specifies that the contact normal be perpendicular to the contact surface. KEYOPT(4) = 2 specifies that the contact normal be perpendicular to the target surface. Use this option (KEYOPT(4) = 2) when the target surface is smoother than the contact surface.
11–28
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
Figure 11.13 Contact Detection Point Location at Nodal Point
Be aware, however, that using nodes as the contact detection points can lead to other convergence difficulties, such as "node slippage," where the node slips off the edge of the target surface, see Figure 11.14: “Node Slippage Using Nodal Integration KEYOPT(4) = 1 or 2”. In order to prevent node slippage, you can use real constant TOLS to extend the target surface when the default setting still cannot avoid the problem. For most point-to-surface contact problems, we recommend using CONTA175; see Section 11.6: Performing a Node-to-Surface Contact Analysis later in this chapter.
Figure 11.14 Node Slippage Using Nodal Integration KEYOPT(4) = 1 or 2
Smoothing is required for nodal detection algroithms, and it is performed by averaging surface normals connected to the node. As a result, the variation of the surface normal is continuous over the surface, which leads to a better calculation of friction behavior and a better convergence.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–29
Chapter 11: Contact Real constant TOLS is used to add a small tolerance that will internally extend the edge of the target surface when you define the contact detection at the nodal point (KEYOPT(4) = 1 or 2). TOLS is useful for problems where contact nodes are likely to lie on the edge of targets (as at symmetry planes or for models generated in a nodeto-node contact pattern). In these situations, the contact node may repeatedly "slip" off the target surface and go completely out of contact, resulting in convergence difficulties from oscillations. Units for TOLS are percent (1.0 implies a 1.0% increase in the target edge length). A small value of TOLS will usually prevent this situation from occurring. The default value is 10 for small deflection and 2 for large deflection (NLGEOM, ON). Note — The definition of KEYOPT(4) in node-to-surface contact element CONTA175 is different. KEYOPT(4) = 1 for surface-to-surface contact is equivalent to KEYOPT(4) = 1 for node-to-surface contact. However, KEYOPT(4) = 2 for surface-to-surface contact is equivalent to KEYOPT(4) = 0 for node-to surface contact. See Section 11.6.1.1.2: KEYOPT(4).
11.4.8.7. Adjusting Initial Contact Conditions 11.4.8.7.1. Background Rigid body motion is usually not a problem in dynamic analyses. However, in static analyses, rigid body motion occurs when a body is not sufficiently restrained. "Zero or negative pivot" warning messages and impractical, excessively large displacements indicate unconstrained motion in a static analysis. In simulations where rigid body motions are constrained only by the presence of contact, you must ensure that the contact pairs are in contact in the initial geometry. In other words, you want to build your model so that the contact pairs are "just touching." However, you can encounter various problems in doing so: •
Rigid body profiles are often complicated, making it difficult to determine where the first point of contact might occur.
•
Small gaps between element meshes on both sides of the element pair can be introduced by numerical round-off, even if the solid model is built in an initially-contacting state.
•
Small gaps can exist between the integration points of the contact elements and target surface elements.
For the same reasons, too much initial penetration between target and contact surfaces can occur. In such cases, the contact elements may overestimate the contact forces, resulting in nonconvergence or in breaking-away of the components in contact. The definition of initial contact is perhaps the most important aspect of building a contact analysis model. Therefore, you should always issue the CNCHECK command before starting the solution to verify the initial contact status. You may find that you need to adjust the initial contact conditions. ANSYS offers several ways to adjust the initial contact conditions of a contact pair.
11.4.8.7.2. Using PMIN, PMAX, CNOF, ICONT, KEYOPT(5), and KEYOPT(9) The following techniques can be performed independently or in combinations of one or more at the beginning of the analysis. They are intended to eliminate small gaps or penetrations caused by numerical round-off due to mesh generation. They are not intended to correct gross errors in either the mesh or in the geometric data. 1.
Use real constant CNOF to specify a contact surface offset. Specify a positive value to offset the entire contact surface towards the target surface. Use a negative value to offset the contact surface away from the target surface.
11–30
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis Note — If user-defined values are input for both CNOF and PINB, you must ensure that PINB is greater than CNOF. Otherwise, CNOF will be ignored. However, if a user-defined CNOF is input and the PINB value is left at its default value, the PINB value will be adjusted so that it is larger than the CNOF value, as described in Using PINB. ANSYS can automatically provide the CNOF value to either just close the gap or reduce initial penetration. Set KEYOPT(5) as follows: 1: Closes the gap 2: Reduces initial penetration 3: Either closes the gap or reduces initial penetration 2.
Use the real constant ICONT to specify a small initial contact closure. This is the depth of an "adjustment band" around the target surface. A positive value for ICONT indicates a scaling factor relative to the depth of the underlying elements. A negative value indicates an absolute contact closure value. The value of ICONT defaults to zero if KEYOPT(5) = 0, 1, 2, or 3. (The ICONT default is different when KEYOPT(12) = 6 for bonded-initial contact; see Section 11.4.8.11: Selecting Surface Interaction Models for more information). If KEYOPT(5) = 4, ANSYS provides a small (but meaningful) value for ICONT according to the geometric dimensions, and prints a warning message stating what value was assigned. Any contact detection points that fall within this adjustment band are internally shifted to be on the target surface (see Figure 11.15: “Contact Surface Adjustment With ICONT”(a)). Only a very small correction is suggested; otherwise, severe discontinuity may occur (see Figure (b)). The difference between CNOF and ICONT is that the former shifts the entire contact surface with the distance value CNOF, the latter moves all initially open contact points which are inside of adjustment band ICONT onto the target surface.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–31
Chapter 11: Contact
Figure 11.15 Contact Surface Adjustment With ICONT
!" # $%& '# A B& + $%& '#
0 1324%5
13678 9: 8 ;=<&>'? 9:@
!" ( #
* + , -
$%& ) #
, (# , &, /. A /B& + $=& '#
3.
Use real constants PMIN and PMAX to specify an initial allowable penetration range. When either PMAX or PMIN is specified, ANSYS brings the target surface into a state of initial contact at the beginning of the analysis (see Figure 11.16: “Contact Surface Adjustment (PMIN, PMAX)”). If the initial penetration is larger than PMAX, ANSYS adjusts the target surface to reduce penetration. If the initial penetration is smaller than PMIN (and within the pinball region), ANSYS adjusts the target surface to ensure initial contact. Initial adjustment for contact status is performed only in translational modes. Such adjustment of initial contact status will be performed for a rigid target surface that has either prescribed loads or displacements. Similarly, a target surface that has no boundary conditions specified may also be adjusted for initial contact. When all the target surface nodes have a prescribed value of zero, the initial adjustment using PMAX and PMIN will not be performed. Note that ANSYS treats applicable degrees of freedom for target surface nodes independently. For example, if you specify the UX degree of freedom to be "zero," then no initial adjustment is possible along the X direction. However, the PMAX and PMIN options will still be activated in the Y and Z directions.
11–32
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis The initial status adjustment is an iterative process. ANSYS uses a maximum of 20 iterations. If the target surface cannot be brought into an acceptable penetration range (i.e., in the range of PMIN to PMAX), the analysis proceeds with the original geometry. ANSYS issues a warning message in such circumstances, and you may need to manually adjust your initial geometry. Figure 11.17: “A Scenario in Which Initial Adjustment Will Fail” illustrates a problem in which initial contact adjustment iteration will fail. The UY degree of freedom for the target has been restrained. Therefore, the only possible adjustment for initial contact is in the X direction. However, in this problem, any movement of the rigid target surface in the X direction will not establish initial contact. For flexible-to-flexible contact, this technique not only moves the entire target surface but also moves the whole deformable body which attaches to the target surface. Make sure there is no other contact surface or target surface connecting with the deformable body.
Figure 11.16 Contact Surface Adjustment (PMIN, PMAX)
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–33
Chapter 11: Contact
Figure 11.17 A Scenario in Which Initial Adjustment Will Fail
4.
Set KEYOPT(9) to adjust initial penetration or gap; see Figure 11.18: “Ignoring Initial Penetration, KEYOPT(9) = 1”. True initial penetration includes two parts: •
Penetration or gap due to geometry
•
Penetration or gap due to user-defined contact surface offset (CNOF).
See Figure 11.19: “Components of True Penetration”. KEYOPT(9) provides the following capabilities: •
To include initial penetration from both geometry and contact surface offset, set KEYOPT(9) = 0. This is the default.
•
To ignore initial penetration from both effects, set KEYOPT(9) = 1. When KEYOPT(12) = 4 or 5, this setting for KEYOPT(9) will also ignore the initial force in open-gap springs, thus creating an initially "perfect" contacting surface having no initial forces acting across the contact interface.
•
To include the defined contact surface offset (CNOF) but ignore the initial penetration due to geometry, set KEYOPT(9) = 3. When KEYOPT(12) = 4 or 5, this setting for KEYOPT(9) will also ignore the initial force in open-gap springs, thus creating an initially "perfect" contacting surface having no initial forces acting across the contact interface.
For problems such as an interference fit, over-penetration is expected. These problems often have convergence difficulties if the initial penetration is step-applied in the first load step. You may overcome convergence difficulties by ramping the initial penetration over the first load step, see Figure 11.20: “Ramping Initial Interference”. The following KEYOPT(9) settings provide ramped capabilities:
11–34
•
To ramp the total initial penetration (CNOF + the offset due to geometry), set KEYOPT(9) = 2.
•
To ramp the defined contact surface penetration, but ignore the penetration due to geometry, set KEYOPT(9) = 4.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis For both of the above KEYOPT(9) settings, you should also set KBC,0 and not specify any external loads in the first load step. Also, be sure that the pinball region is big enough to capture the initial interference. You can use the above techniques in conjunction with each other. For example, you may wish to set a very precise initial penetration or gap but the initial coordinates of the finite element nodes may not be able to provide sufficient precision. To accomplish this, you could: 1.
Use ICONT to move the initial open contact points just onto the target surface.
2.
Use CNOF to specify a penetration (positive value) or gap (negative value).
3.
Use KEYOPT(9) = 3 to resolve the initial penetration in the first substep (or KEYOPT(9) = 4 to gradually resolve the initial penetration).
Figure 11.18 Ignoring Initial Penetration, KEYOPT(9) = 1
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–35
Chapter 11: Contact
Figure 11.19 Components of True Penetration
11–36
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
Figure 11.20 Ramping Initial Interference
ANSYS provides a printout (in the output window or file or via the CNCHECK) of the model's initial contact state for each target surface at the beginning of the analysis. This information is helpful for determining the maximum penetration or minimum gap for each target surface. If no contact is detected for a specific target surface, ANSYS issues a warning. This occurs when the target surface is far from contact (i.e., outside of the pinball region), or when the contact/target elements have been killed. See Positive and Negative Real Constants for more information on these real constants.
11.4.8.8. Physically Moving Contact Nodes Towards the Target Surface The initial contact status can be adjusted to close the gap by defining real constant ICONT or by ignoring the penetration (setting KEYOPT(9) = 1). However the initial contact adjustment is kept during the entire analysis as a rigid zone. The initial contact adjustment can cause a certain amount of residual force if a large rotation appears at the contact surface. This problem can be alleviated by issuing the CNCHECK,ADJUST command, which physically moves contact nodes towards the target surface under the following circumstances:
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–37
Chapter 11: Contact •
Only when using the nodal detection option (KEYOPT(4) = 1 or 2), or when using CONTA175.
•
Initially open contact nodes inside the ICONT zone.
•
Initially penetrated nodes with KEYOPT(9) = 1.
After issuing the CNCHECK,ADJUST command, the coordinates of the nodes that have been moved are modified as shown in Figure 11.21: “Effect of Moving Contact Nodes”. You can change other contact related settings in PREP7 (for example, set KEYOPT(4) = 0 to use the Gauss detection option) and save the db file. Issuing the SAVE command before issuing the CNCHECK,ADJUST command is recommended in order to resume the .DB file with the original contact configuration. For those contact pairs whose contact nodes you do not wish to physically move towards target surface, do not define KEYOPT(4) = 1 or 2.
Figure 11.21 Effect of Moving Contact Nodes
11.4.8.9. Determining Contact Status and the Pinball Region 11.4.8.9.1. Background The position and motion of a contact element relative to its associated target surface determines the contact element status. ANSYS monitors each contact element and assigns a status: •
STAT = 0 Open far-field contact
•
STAT = 1 Open near-field contact
•
STAT = 2 Sliding contact
•
STAT = 3 Sticking contact
A contact element is considered to be in near-field contact when its integration points (Gauss points or nodal points) are within a code-calculated (or user-defined) distance to the corresponding target surface. This distance 11–38
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis is referred to as the pinball region. The pinball region is a circle (in 2-D) or a sphere (in 3-D) centered about the Gauss point.
11.4.8.9.2. Using PINB Use real constant PINB to specify a scaling factor (positive value for PINB when using command input) or absolute value (negative value for PINB when using command input) for the pinball region. You can specify PINB to have any value. By default, and assuming that large deflection effects apply (NLGEOM,ON), ANSYS defines the pinball region as a circle for 2-D or a sphere for 3-D of radius 4*depth (if rigid-to-flexible contact) or 2*depth (if flexibleto-flexible contact) of the underlying element. (See the discussion of element depth in Section 11.4.8.1.1: Positive and Negative Real Constant Values.) If you include no large-deflection effects (NLGEOM,OFF), the default pinball region is half that of the large-deflection case. (For the no-separation (KEYOPT(12) = 4) and bonded-always (KEYOPT(12) = 5 options, the PINB default is different than described here. See Section 11.4.8.11: Selecting Surface Interaction Models for more information.) Note — If you input a value for real constant CNOF (contact surface offset) and the default PINB value (as described above) is less than the absolute value of CNOF, the default for PINB will be set to the absolute value of (1.1*CNOF). The computational cost of searching for contact depends on the size of the pinball region. Far-field contact element calculations are simple and add little computational demands. The near-field calculations (for contact elements that are nearly or actually in contact) are slower and more complex. The most complex calculations occur once the elements are in actual contact. Setting a proper pinball region is useful to overcome spurious contact definitions if the target surface has several convex regions. However, the default setting should be appropriate for most contact problems. See Positive and Negative Real Constants for more information on this real constant.
11.4.8.10. Avoiding Spurious Contact in Self Contact Problems In some cases of self contact, ANSYS may erroneously assume contact between a contact and target surface that are in very close geometrical position as shown below.
Figure 11.22 Auto Spurious Prevention
! ! " # $% &' !
( #*)+ '
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–39
Chapter 11: Contact ANSYS will alert you when it first detects spurious contact in each load step. If ANSYS encounters such contact on the first load step, you'll see the following error message: Contact element x has too much penetration related to target element y. We assume it (may be more elements) is spurious contact.
If ANSYS encounters an abrupt change in contact that it classifies as spurious contact, you'll see the following message: Contact element x status changed abruptly with target element y. We assume it (may be more elements) is spurious contact.
ANSYS issues such messages only once per load step. It does not notify you of additional cases of spurious contact that were ignored during the load step.
11.4.8.11. Selecting Surface Interaction Models 11.4.8.11.1. Background The surface-to-surface contact elements support normal unilateral contact models as well as other mechanical surface interaction models.
11.4.8.11.2. Using KEYOPT(12) and FKOP Use KEYOPT(12) to model different contact surface behaviors. •
KEYOPT(12) = 0 models standard unilateral contact; that is, normal pressure equals zero if separation occurs.
•
KEYOPT(12) = 1 models perfectly rough frictional contact where there is no sliding. This case corresponds to an infinite friction coefficient and ignores the material property MU.
•
KEYOPT(12) = 2 models no separation contact, in which the target and contact surfaces are tied (although sliding is permitted) for the remainder of the analysis once contact is established.
•
KEYOPT(12) = 3 models "bonded" contact, in which the target and contact surfaces are bonded in all directions (once contact is established) for the remainder of the analysis.
•
KEYOPT(12) = 4 models no separation contact, in which contact detection points that are either initially inside the pinball region or that once involve contact always attach to the target surface along the normal direction to the contact surface (sliding is permitted).
•
KEYOPT(12) = 5 models bonded contact, in which contact detection points that are either initially inside the pinball region or that once involve contact always attach to the target surface along the normal and tangent directions to the contact surface (fully bonded).
•
KEYOPT(12) = 6 models bonded contact, in which the contact detection points that are initially in a closed state will remain attached to the target surface and the contact detection points that are initially in an open state will remain open throughout the analysis.
For modeling either no-separation or bonded contact, you may need to set a value for the FKOP real constant. This provides a stiffness factor applied when contact opens. If FKOP is a scaling factor (positive value for command input), the true contact opening stiffness equals FKOP times the contact stiffness applied when contact closes. If FKOP is an absolute value (negative value for command input), the value is applied as an absolute contact opening stiffness. The default FKOP value is 1. No separation and bonded contact generate a "pull-back" force when contact opening occurs, and that force may not completely prevent separation. To reduce separation, define a larger value for FKOP. Also, in some cases separation is expected while connection between the contacting surfaces is required to prevent rigid body
11–40
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis motion. In such instances, you can specify a small value for FKOP to maintain the connection between the contact surfaces (this is a "weak spring" effect). For the no-separation option (KEYOPT(12) = 4) and the bonded-always option (KEYOPT(12) = 5), a relatively small PINB value (pinball region) may be used to prevent any false contact. For these KEYOPT(12) settings, the default for PINB is 0.25 (25% of the contact depth) for small deformation analysis (NLGEOM,OFF) and 0.5 (50% of the contact depth) for large deformation analysis (NLGEOM,ON). (The default PINB value may differ from what is described here if CNOF is input. See Section 11.4.8.9.2: Using PINB for more information.) For the bonded-initial option (KEYOPT(12) = 6), a relatively large ICONT value (initial contact closure) may be used to capture the contact. For this KEYOPT(12) setting, the default for ICONT is 0.05 (5% of the contact depth) when KEYOPT(5) = 0 or 4. See Positive and Negative Real Constants for more information on these real constants.
11.4.8.12. Modeling Contact with Superelements 11.4.8.12.1. Background The surface-to-surface contact elements can model a rigid body (or one linear elastic body) contacting another linear elastic body undergoing small motions. These elastic bodies can be modeled using superelements, which greatly reduces the number of degrees of freedom involved in the contact iteration. Remember that any contact or target nodes must be either all master nodes of the superelements or all slave nodes of the superelements. When the contact pair is built in original elements used to generate superelements, the contact status will not change from its initial status. Because the superelement consists only of a group of retained nodal degrees of freedom, it has no surface geometry on which ANSYS can define a contact and target surface. Therefore, the contact and target surface must be defined on the surface of the original elements before they are assembled into a superelement. Information taken from the superelement includes nodal connection and assembly stiffness, but no material property or stress states (whether axisymmetric, plane stress, or plane strain). One restriction is that the material property set used for the contact elements must be the same as the one used for the original elements before they were assembled into superelements.
11.4.8.12.2. Using KEYOPT(3) Use KEYOPT(3) to provide information for the 2-D analysis with superelements. In elements CONTA171 and CONTA172, the options are as follows: •
No superelement used (KEYOPT(3) = 0)
•
Axisymmetric, use with superelements only (KEYOPT(3) = 1)
•
Plane strain or plane stress with unit thickness, use with superelements only (KEYOPT(3) = 2)
•
Plane stress with thickness input use with superelements only (KEYOPT(3) = 3). Note that for this case, use real constant R2 to specify the thickness.
In 3-D contact analysis, KEYOPT(3) in elements CONTA173 and CONTA174 is ignored. ANSYS will automatically detect whether the underlying element is a superelement.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–41
Chapter 11: Contact Note — KEYOPT(3) in node-to surface contact element CONTA175 has a different meaning. In CONTA175, KEYOPT(3) = 1 defines the contact traction-based model. In this case, all of the real constant inputs and contact result quantities have the same units as the surface-to-surface contact elements. KEYOPT(3) = 0 (default) defines the contact force model. In this model, certain real constants and contact result quantities can have different units (a factor of AREA (Length2) difference). See Section 11.6.1.1.1: KEYOPT(3).
11.4.8.13. Accounting for Thickness Effect 11.4.8.13.1. Background You can account for the thickness of shells (2-D and 3-D) and beams (2-D) using KEYOPT(11). For rigid-to-flexible contact, ANSYS will automatically shift the contact surface to the bottom or top of the shell/beam surface. For flexible-to-flexible contact, ANSYS will automatically shift both the contact and target surfaces which are attached to shell/beam elements. By default, ANSYS does not account for the element thickness, and beams and shells are discretized at their mid-surface in which penetration distance is calculated from the mid-surface.
11.4.8.13.2. Using KEYOPT(11) When you set KEYOPT(11) = 1 to account for beam or shell thickness, the contact distance is calculated from either the top or the bottom surface as specified previously in Section 11.4.2: Steps in a Contact Analysis. Note — Only use KEYOPT(11) = 1 to account for thickness when you have shell or beam elements with nodes located at the middle surface (for example, KEYOPT(11) = 0 for SHELL91). When building your model geometry, if you are going to account for thickness, remember the offsets which may come from either the contact surface or target surface or from both. When you specify a contact offset (CNOF) along with setting KEYOPT(11) = 1, it is defined from the top or bottom of the shell/beam, not the mid-surface. When used with SHELL181, changes in thickness during deformation are also taken into account.
11.4.8.14. Using Time Step Control 11.4.8.14.1. Background Time step control is an automatic time stepping feature that predicts when the status of a contact element will change and cuts the current time step back.
11.4.8.14.2. Using KEYOPT(7) Use KEYOPT(7) to take one of four actions to control time stepping, where KEYOPT(7) = 0 provides no control (the default), and KEYOPT(7) = 3 provides the most control. •
KEYOPT(7) = 0: No control. The time step size is unaffected by the prediction. This setting is appropriate for most analyses when automatic time stepping is activated and a small time step size is allowed.
•
KEYOPT(7) = 1: Time step size is bisected if too much penetration occurs during an iteration, or if the contact status changes dramatically.
•
KEYOPT(7) = 2: Predict a reasonable increment for the next substep.
•
KEYOPT(7) = 3: Predict a minimal time increment for the next substep.
11.4.8.15. Using the Birth and Death Option The surface-to-surface contact and target elements allow birth and death and also follow the birth and death status of their underlying elements. The elements can be removed for part of an analysis and then reactivated 11–42
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis for a later stage. This feature is useful for modeling complex metal forming processes where multiple rigid target surfaces need to interact with the contact surface at different stages of the analysis. Springback modeling often requires removing the rigid tools at the end of the forming processes. This option cannot be used with "no separation" or bonded contact.
11.4.9. Controlling the Motion of the Rigid Target Surface (Rigid-to-Flexible Contact) Rigid target surfaces are defined in their original configuration, and the motion of the entire surface is then defined by the imposed displacements on the pilot node (or the different nodes of the target surface if no pilot node was defined). You must use a pilot node in any of the following situations to control the boundary conditions (and motion) of the entire target surface: •
The target surface is subjected to applied forces.
•
The target surface is subjected to rotations.
•
The target surface is connected to other elements (e.g., structural mass element MASS21).
•
The motion of the target surface is adjusted by the equilibrium condition.
The degrees of freedom of the pilot node represent the motion of the entire rigid surface, including two translational and one rotational degree of freedom in 2-D, and three translational and three rotational degrees of freedom in 3-D. You can apply boundary conditions (displacement, initial velocity), concentrated loads, rotations, etc. to the pilot node. To account for a rigid body's mass, define a mass element (MASS21) on the pilot node. Keep in mind the following restrictions on the target surface when using a pilot node: •
Each target surface can have only one pilot node.
•
ANSYS ignores all boundary conditions on all nodes other than the pilot node.
•
Only the pilot node can connect to other elements. If you need to attach the rigid surface to another element, you must use the pilot node to do so.
•
You cannot use constraint equations (CE) or node coupling (CP) to control the degree of freedom of the target surface when a pilot node has been defined. If you want to apply any loads or constraints on the rigid target surface, you must define a pilot node and apply the loads to that pilot node. If you do not use a pilot node, you can have rigid body motions only. Note — The pilot node can be one of the nodes on the target elements or a node at any arbitrary location. However, it should not be the node on the contact element. The location of the pilot node becomes important only when rotations or moments are to be applied. For each pilot node, ANSYS will automatically define an internal node and an internal constraint equation. The rotational DOF of the pilot node is connected to the translational DOF of the internal node by the internal constraint equation.
By default, KEYOPT(2) = 0 for the target element, ANSYS checks the boundary conditions for each target surface. If all of the following conditions are met, then ANSYS treats the target nodes along the respective degree of freedom as fixed: •
There are no explicit boundary conditions or prescribed forces for target surface nodes.
•
Target surface nodes are not connected to other elements.
•
Neither constraint equations nor node coupling have been used to constrain such nodes.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–43
Chapter 11: Contact At the end of each load step, ANSYS releases the constraint conditions that were set internally. The constraint conditions stored in the results file (Jobname.RST) and the database file (Jobname.DB) may be updated due to this change. You should carefully verify whether the current constraint conditions are expected before restarting an analysis or resolving the problem in interactive mode. If you wish, you can control the constraint conditions of target nodes by setting KEYOPT(2) = 1 in the target element definition.
11.4.10. Modeling Thermal Contact You can use surface-to-surface contact elements and the node-to-surface contact element, in combination with thermal-structural coupled field solid elements or thermal elements, to model heat transfer that occurs in the contact surface. To activate both the structural and thermal DOFs, set KEYOPT(1) = 1. To activate the thermal DOF only, set KEYOPT(1) = 2. The following thermal contact features are supported. •
Thermal contact conduction between two contacting surfaces.
•
Heat convection from a “free surface” to the environment or between two open surfaces separated by small gap (“near field” convection).
•
Heat radiation from a “free surface” to the environment or between two open surfaces separated by a small gap (“near field” radiation).
•
Heat generation due to frictional dissipation.
•
Heat flux input. Note — When KEYOPT(1) is set to 2, ANSYS ignores heat generation due to friction.
11.4.10.1. Thermal Contact Behavior vs. Contact Status Each contact pair can cover one or more thermal contact features. Which feature is active depends on the contact status: Closed Contact: Thermal contact conduction transfers heat between two contacting surfaces. Frictional Sliding: Frictional dissipated energy generates the heat to both the contact and target surfaces. Near-Field Contact: Both heat convection and radiation between the contact and target surfaces are taken into account. The external flux value contributes to the contact surface. Free-Surface Contact: Heat convection and radiation between the contact surface and the environment are taken into account. The external flux value only contributes to both contact and target surfaces.
11.4.10.2. Free Thermal Surface If you wish to model free surface convection, free surface radiation, or a surface with a supplied heat flux value, you can define a “free” thermal surface. A free thermal surface can be a contact surface with no associated target (that is, the contact pair lacks target elements). You can also set KEYOPT(3) = 1 of the target element type definition to define a free thermal surface. When this KEYOPT is set, both free surface radiation and convection are considered as long as open contact is detected. In this case, there is no convective and radiative heat transfer between the contact and target surfaces.
11–44
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
11.4.10.3. Temperature on Target Surface For interface heat conduction, near field convection, or near field radiation, a temperature for both the contact and target surfaces is required. The temperature at the intersection between the target surface and the normal from the contact detection point represents the target temperature. The temperature on the pilot node represents the entire rigid target surface temperature if the pilot node exists.
Figure 11.23 Target Temperature
!#"%$ & '
11.4.10.4. Modeling Conduction To take into account the conductive heat transfer between contact and target surfaces, you need to specify the thermal contact conductance coefficient TCC through a real constant table.
11.4.10.4.1. Using TCC The conductive heat transfer between two contacting surfaces is defined by q = TCC X (Tt -Tc) where: q: is the heat flux per area. TCC: is the thermal contact conductance coefficient, having units of HEAT/(TIME * TEMPERATURE * AREA) for force-based node-to-surface contact, or units of HEAT/(TIME * TEMPERATURE) for the traction-based model. Tt and Tc: are the temperatures of the contact points on the target and contact surfaces. The TCC value is input through a real constant, which can be made a function of temperature [(Tc + Tt)/2], pressure, time, and location by using the %TABLE% option. TCC has units of heat/(time x area x temp). If contact occurs, a small value of TCC yields a measure amount of imperfect contact and a temperature discontinuity across the interface. For large values of TCC, the resulting temperature discontinuity tends to vanish and perfect thermal contact is approached. When not in contact, however, it is assumed that no heat is transferred across the interface. To model contact conduction between two surfaces where a small gap exists, use KEYOPT(12) = 4 or 5 to define either the “bonded contact” or “no-separation contact” options (see Selecting Surface Interaction Models).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–45
Chapter 11: Contact
11.4.10.4.2. Using the Quasi Solver Option You can take advantage of the fast thermal transient solver option (THOPT,QUASI) in the contact analysis. (See Nonlinear Options in the ANSYS Thermal Analysis Guide for more information on this solver option.) To do so, you must use the following contact element key options: KEYOPT(1) = 2 - Temperature DOF only KEYOPT(12) = 5 or 6 - Bonded always or bonded initial The following solver options must also be set: ANTYPE,TRANS THOPT,QUASI EQSLV,JCG/ICCG The following two cases are supported: •
Thermal conductivity at contact. The only real constant used is TCC, which can be a function of time and temperature.
•
Perfect thermal contact which supports dissimilar meshes on both sides of the contacting interface (TCC = infinity). This case requires the internal MPC approach (KEYOPT(2) = 2) and contact nodal detections (KEYOPT(4) = 1 or 2) or CONTA175.
11.4.10.5. Modeling Convection To model convective heat transfer, you must specify the heat convection coefficient CONV using the SFE command. CONV can be a constant value (only uniform is allowed) or a function of temperature, time, and location as specified through tabular input. For free surface convection, you must specify bulk temperature through the SFE command. You can access this command through the following GUI paths: Main Menu> Preprocessor> Loads> Define Loads> Apply> Thermal> Convection> On Elements> Uniform Main Menu> Solution> Define Loads> Apply> Thermal> Convection> On Elements> Uniform
11.4.10.6. Modeling Radiation 11.4.10.6.1. Background To model radiative heat transfer, you need to specify one of the following: •
Emissivity value EMIS, specified through the material property definition.
•
Stefan-Boltzmann constant SBCT through a real constant.
•
Offset temperature TOFFST. If you define your data in terms of degrees Fahrenheit or degrees Celsius, you must specify a temperature offset using the TOFFST command. You can access this command through the following GUI paths: Main Menu> Preprocessor> Loads> Analysis Type> Analysis Options Main Menu> Preprocessor> Material Props
•
Radiation view factor RDVF, specified through a real constant.
•
Environment (ambient) temperature. It is only used for free radiation and input on the SFE command with KVAL = 2 and CONV as a table parameter (this is the same as the bulk temperature in free surface convection modeling).
11–46
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
11.4.10.6.2. Using SBCT and RDVF When contact is open, heat transfer through radiation can occur. The equation is defined by q = RDVF x EMIS x SBCT [(Te + TOFFST)4 - (Tc + TOFFST)4] Where TOFFST: The temperature offset from absolute zero to zero (defined through the TOFFST command.) EMIS: The surface emissivity (input as material property). SBCT: The Stefan-Boltzmann constant (input as a real constant). There is no default for SBCT, and if this is not defined the radiation effect is excluded. RDVF: The radiation view factor input as a real constant (defaults to 1). RDVF can be defined as a function of temperature, gap distance, time, and location by using the %TABLE% option. It is only used for near field radiation. For far field radiation, RDVF is set to 1.0 and a user-assigned value is ignored. Other freesurface conditions recognize user-specified RDVF. For “near field” radiation, when an intersection from a contact detection point to the target surface (in the direction of normal to the contact point) is detected, and the gap distance is smaller than the pinball radius, Te is the target temperature at the intersection. The radiation modeling here assumes that the radiative heat transfer occurs in the direction of the normal between two surfaces with a small gap. By defining RDVF as a function of gap, you can account for geometry effects. Use the Radiosity Solver method for more generalized radiation problems (see the ANSYS Thermal Analysis Guide for more information). For “free surface” radiation, Te becomes the “ambient” temperature defined by “bulk temperature” input from the SFE command (using KVAL = 2 and CONV as the table).
11.4.10.7. Modeling Heat Generation Due to Friction 11.4.10.7.1. Background In order to model heat generation due to frictional dissipated energy, you should perform a coupled transient thermal-structural analysis. If you wish you can turn off transient effects on structural DOFs by using TIMINT,STRUC,OFF. However, you must include transient effects on the thermal DOF. Two real constants are required: •
FHTG is the frictional dissipated energy converted into heat.
•
FWGT is the weight factor for the distribution of heat between contact and target surfaces.
11.4.10.7.2. Using FHTG and FWGT In the coupled thermal-structural contact modeling, the rate of frictional dissipation is given by q = FHTG x τ x V Where τ: The equivalent frictional stress. V: The sliding rate. FHTG: The fraction of frictional dissipated energy converted into heat. This value defaults to 1 and can be input as a real constant. For an input of true 0, you must enter a very small value (for example, 1E-8). If you enter 0, ANSYS interprets this as an input of the default value. The amount of frictional dissipation on contact and target surfaces is defined by
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–47
Chapter 11: Contact qc = FWGT x FHTG x τ x V and qT = (1 - FWGT) x FHTG x τ x V Where qc is the contact side and qT is the target side, and FWGT is the weight factor for the distribution of heat between the contact and target surfaces (input as a real constant). By default, FWGT = 0.5. For an input of true 0, you must enter a very small value (for example, 1E-8). If you enter 0, ANSYS interprets this as an input of the default value.
11.4.10.8. Modeling External Heat Flux You can apply heat flux on the contact elements through the SFE command. Only uniform flux can be applied. Heat flux cannot be applied on target elements. However, for near field contact, the external flux is applied on contact and will contribute to target elements. For a free thermal surface, if KEYOPT(3) of the target element is set to 1, the external flux is only applied on the contact side. On a given contact element either CONV or HFLUX (but not both) may be specified. However, you can define two different contact pairs: one models convection and the other models heat flux.
11.4.11. Modeling Electric Contact You can use surface-to-surface contact elements or the node-to-surface contact element, in combination with thermal-electric elements and solid coupled field elements to model electric current conduction. You can also use surface-to-surface contact elements, in combination with piezoelectric and electrostatic elements, to model electric charge across a contacting interface. KEYOPT(1) provides degree of freedom options for modeling electric contact. For combined structural/thermal/electric contact, set KEYOPT(1) = 3 to activate the structural, thermal, and electric current DOFs. For pure thermal/electric contact, set KEYOPT(1) = 4 to activate the thermal and electric current DOFs. For piezoelectric contact, set KEYOPT(1) = 5 to activate the structural and piezoelectric DOFs. For electrostatic contact, set KEYOPT(1) = 6 to activate the electrostatic DOF. The electric contact features are: •
Electric conduction between two contacting surfaces.
•
Heat generation due to electric dissipation.
•
Electric charge across the contacting interface.
11.4.11.1. Modeling Surface Interaction 11.4.11.1.1. Background To take into account the surface interaction for electric contact, you need to specify the electric contact conductance per unit area if you are using the electric current degree of freedom, or the electric contact capacitance per unit area if you are using the piezoelectric or electrostatic degrees of freedom. For either case, this parameter is ECC. You specify ECC through a real constant table. You can use a tabular input to define ECC as a function of contact pressure (pressure as a table), average temperature on contact detection point (temperature as a table), and time. If the “bonded contact” or “no-separation contact” option is set, contact interaction can occur between two surfaces separated by a narrow gap.
11–48
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
11.4.11.1.2. Using ECC The interaction between two contacting surfaces is defined by J = ECC x (Vt - Vc) where: J = current density for the electric potential (VOLT) degree of freedom (KEYOPT(1) = 3 or 4), or the electric charge density (KEYOPT(1) = 5, or 6). ECC = electric contact conductance for the electric potential (VOLT) degree of freedom (KEYOPT(1) = 3 or 4), or the electric contact capacitance per unit area for (KEYOPT(1) = 5, or 6). Vt and Vc = voltages at the contact points on the target and contact surfaces. The ECC value is input through a real constant, which can be a function of temperature [(Tt + Tc)/2], pressure, and time, by using the %TABLE% option. For the current conduction option, the electric contact conductance ECC has units of electric conductivity/length. For the piezoelectric and electrostatic options, the electric contact capacitance ECC has units of capacitance per unit area. To model surface interaction between two surfaces where a small gap exists, use KEYOPT(12) = 4 or 5 to define either the “bonded contact” or “no-separation contact” options (see Selecting Surface Interaction Models). Note — For force-based node-to-surface contact, ECC has units of (electric conductivity)(LENGTH) or the capacitance.
11.4.11.2. Modeling Heat Generation Due to Electric Current For electric current field analyses (KEYOPT(1) = 3 or 4), the heat generation due to electric current is given by q = FHEG x J x (VT - VC) Where FHEG: The fraction of electric dissipated energy converted into heat (Joule heating). This value defaults to 1 and can be input as a real constant. For an input of true 0, you must enter a very small value (for example, 1E-8). If you enter 0, ANSYS interprets this as an input of the default value. J: The current density. Vt and Vc: The voltages at the contact points on the target and contact surfaces. The amount of electric heat dissipation on contact and target surfaces is defined by qc = FWGT x q and qT = (1 - FWGT) x q Where qc is the contact side and qT is the target side, and FWGT is the weight factor for the contact heat dissipation between the contact and target surfaces (input as a real constant). FWGT is the same real constant used for frictional heat generation. By default, FWGT = 0.5. For an input of true 0, you must enter a very small value (for example, 1E-8). If you enter 0, ANSYS interprets this as an input of the default value.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–49
Chapter 11: Contact
11.4.12. Modeling Magnetic Contact You can use surface-to-surface contact elements or the node-to-surface contact element to model magnetic flux across two contacted bodies. The following situations are possible. •
Non-perfect contact to account for the effects of a small air gap between mating components. This typically occurs at the interface between adjoining bodies. In this situation, there is a gap permeance effect where an MMF drop occurs. You can model this effect by inputting the gap permeance real constant, MCC. This option works best if the magnetic flux is normal to the gap interface.
•
Perfect contact across dissimilar meshes. This is typically used to model the air gap in a machine, for example, where the rotor and stator meshes meet.
For both types of magnetic contact, you must set KEYOPT(1) = 7 to select the degree-of-freedom option. For the 2-D case, the magnetic potential degree of fredom, AZ, is active. For the 3-D case, only the scalar potential degree of freedom, MAG, is active, and scalar potential formulations (reduced (RSP), difference (DSP), or general (GSP)) are available (see MAGOPT). Note — 3-D magnetic contact is not supported for the MVP formulation (AX, AY, AZ), and the edge-based formulation (AZ). Note — Non-perfect magnetic contact is only available for the 3–D contact elements, CONTA173 and CONTA174. For more information on which element types should be used for a particular analysis, see the element discussions in the appropriate chapter of the ANSYS Low-Frequency Electromagnetic Analysis Guide. For information on the use of the AZ degree of freedom, see Section 2.3.1.3: Specifying Element Types and Options. For more information on the use of the MAG DOF, see Section 5.3.5: Building the Model. For details on how to set up a contact analysis, see Steps in a Contact Analysis. For an example input listing showing a 2-D static magnetic contact analysis, see Section 2.6: Doing an Example 2-D Static Magnetic Contact Analysis (Command Method).
11.4.12.1. Using MCC The magnetic flux across the contacting interface is defined by: MFLUX = MCC x (Mt - Mc) where: MFLUX = magnetic flux density Mt , Mc = magnetic potential at the contact points on the target and contact surfaces MCC = contact permeance coefficient (Henries/meters2 in MKS units) The MCC value is input through a real constant, which can be a function of temperature [(Tt + Tc)/2], pressure, and time, by using the %TABLE% option. MCC values can be approximated as µ/t, where µ is the gap permeability and t is the gap width. If the “no-separation contact” or “bonded contact” option is set (KEYOPT(12) = 4 or 5), contact interaction can occur between two surfaces separated by a narrow gap.
11–50
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
11.4.12.2. Modeling Perfect Magnetic Contact Perfect magnetic contact supports dissimilar meshes on both sides of the contacting interface (MCC = infinity). You must use the internal MPC approach by setting KEYOPT(2) = 2. You must also set KEYOPT(4) = 1 or 2 for contact nodal detection, and KEYOPT(12) = 5, 6 for bonded contact.
11.4.13. Applying Necessary Boundary Conditions to the Deformable Elements You can now apply any necessary boundary conditions as you would for any ANSYS analysis. For more information on applying boundary conditions, see the appropriate analysis descriptions in earlier chapters of this guide.
11.4.14. Defining Solution and Load Step Options Convergence behavior for contact problems depends strongly on the particular problem. The options listed below are either typical or recommended for most surface-to-surface contact analyses. Please see the ANSYS Commands Reference for further details. The time step size must be small enough to capture the proper contact zone. The smooth transfer of contact forces is disrupted if the time step size is too large. The time step size is specified by a number of substeps or the time step size itself. The following commands adjust these parameters. Command(s): NSUBST GUI: Main Menu> Preprocessor> Loads> Load Step Opts> Time/Frequenc> Freq and Substps Main Menu> Preprocessor> Loads> Load Step Opts> Time/Frequenc> Time and Substps Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Freq and Substps Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Time and Substps Command(s): DELTIM GUI: Main Menu> Preprocessor> Loads> Load Step Opts> Time/Frequenc> Time-Time Step Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc>Time-Time Step Note — A reliable way to set an accurate time step size is to turn automatic time stepping on. The following options are automatically invoked, but may override them if needed. Command(s): AUTOTS,ON GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Time-Time Step or Time and Substps If the contact status changes during the iteration process, discontinuity can occur. To avoid a slow convergence rate and use an updated stiffness matrix, set the Newton-Raphson option to FULL. Command(s): NROPT,FULL,,OFF GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–51
Chapter 11: Contact Also, do not use adaptive descent. Adaptive descent usually does not provide any help for surface-to-surface contact applications, and we recommend turning it off. In cases where frictional sliding dominates, set the unsymmetric solver option (NROPT, UNSYM,,OFF) to avoid slow convergence or divergence. Set the number of equilibrium equations to a number that is appropriate for a reasonable time step size. This command defaults to between 15 and 26 iterations, depending upon the physics of the problem. Command(s): NEQIT GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Nonlinear Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Equilibrium Iter Because the iterations tend to become unstable for large increments, use the line search option to stabilize the calculations. Command(s): LNSRCH GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Nonlinear Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Line Search Turn the predictor-corrector option on, except for large rotations or dynamic analyses. Command(s): PRED GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Nonlinear Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Predictor Many convergence failures in contact analyses are the result of using too large a value for contact stiffness (real constant FKN). Be sure to follow the recommendations given earlier in this chapter for estimating contact stiffness. If such estimated values lead to a convergence failure, reduce the contact stiffness and restart. Conversely, if overpenetration occurs in your contact analysis, you probably need a larger value of FKN. In this case, gradually increase the contact stiffness value to an appropriate level by redefining it using RMODIF commands over several load steps in a restart. Note — For most small strains, small displacements, and small sliding problems, set NLGEOM, OFF. This setting will speed up the searching time; however, if the contact problem involves large sliding, set NLGEOM, ON.
11.4.15. Solving the Problem You can now solve the analysis the same as you would for any nonlinear analysis. Keep the following points in mind: •
Always check the real constant sets which are related to contact pairs and check the constraint conditions on the target surfaces. Any previous "trial runs" could have changed the settings.
•
Always check the target surface contact status in the beginning of the analysis. If you detect any unexpected gap (or no contact) or overestimated penetration, abort the analysis and then check your geometric model. You can issue the CNCHECK command to verify the initial contact status.
•
If your model is experiencing convergence difficulties due to contact, use the NLHIST command as a debugging tool to monitor contact information during the solution. Before starting the solution, issue NLHIST to specify the pair-based contact items (such as contact penetration or gap, contact normal stiffness, etc.) to be tracked. The resulting data are written to a file named Jobname.nlh.
•
Always check your results carefully using standard engineering guidelines.
See Section 2.3.5: Solve the Analysis in Chapter 2, “Structural Static Analysis”. 11–52
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis If you are restarting a contact analysis, follow the normal restart procedures as discussed in Section 3.16: Restarting an Analysis in the ANSYS Basic Analysis Guide. However, be aware that the constraint conditions of target surfaces may have been set internally. Verify the constraints carefully before restarting an analysis. Only the real constants FKN, FTOLN, PINB, and FKOP can be changed, and they can only be changed at the point of restart or at the beginning of a new load step.
11.4.16. Reviewing the Results Results from a contact analysis consist mainly of displacements, stresses, strains, reaction forces, and the contact information (e.g., contact pressure, sliding, etc.). You can review these results in POST1, the general postprocessor, or in POST26, the time-history postprocessor. For contact-related results, you can select CONT as a plotting or list item. While in POST1, you can also review the results from within the Contact Manager (via the Contact Manager icon in the ANSYS Standard Toolbar). See the "Output Data" section of the element descriptions (the ANSYS Elements Reference) for the available output components. Remember that in POST1, only one substep can be read in at a time, and that the results from that substep should have been written to Jobname.RST (or Jobname.RCN for the initial contact configuration calculated by CNCHECK,POST). (The load step option command OUTRES controls which substep results are stored on Jobname.RST.) A typical POST1 postprocessing sequence is described below.
11.4.16.1. Points to Remember See Section 2.3.6.2: Points to Remember in Chapter 2, “Structural Static Analysis”.
11.4.16.2. Reviewing Results in POST1 The steps for reviewing results in POST1 are the same as those for a typical nonlinear analysis (see Section 8.5.6.2: Reviewing Results in POST1 in Chapter 8, “Nonlinear Structural Analysis”) with the following exceptions: For step 4, the following shows the various CONT options for the PLNSOL and PLESOL commands. CONT
STAT
Contact status. 3-closed and sticking, 2-closed and sliding, 1-open but near contact, 0-open and not near contact.
“
PENE
Contact penetration
“
PRES
Contact pressure
“
SFRIC
Contact friction stress
“
STOT
Contact total stress (pressure plus friction)
“
SLIDE
Contact sliding distance
“
GAP
Contact gap distance
“
FLUX
Heat flux at contact surface
“
CNOS
Total number of contact status changes during substep
Note — You can set these options through the Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu menu item. Choose Contact for Item, Comp and you'll see a list of the options detailed above. For rigid-to-flexible contact or asymmetric flexible-to-flexible contact, the contact element provides the true pressure and friction stress. However, for symmetric flexible-to-flexible contact, the true pressure and friction stress is the average of the pressures and friction stresses from both sides of the contact elements.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–53
Chapter 11: Contact Note — For the contact force-based model (KEYOPT(3) = 0) in CONTA175, PRES, SFRIC, and STOT are the contact normal force, contact friction force, and total contact force, respectively. Note that the contact-specific information (CONT) plots as follows. For 2-D contact analyses, the model will plot in gray and the requested item will be contoured as an area (trapezoid) along the edge of the model where the contact elements are located. Use the FACT item to scale 2-D contour size. For 3-D contact analyses, the model will plot in gray and the requested item will be contoured as a 2-D surface where the contact elements overlay the model. For tabular listings, you may also list contact-specific information by using the CONT label and its arguments with the PRNSOL or PRESOL commands or their related menu items You can also animate contact results over time. See the ANTIME command for details. Command(s): ANTIME GUI: Utility Menu> PlotCtrls> Animate> Over Time If you used CNCHECK,POST to evaluate the initial contact state, you can view the contact results items for the initial contact configuration as you would for any other load step. To do so, you must explicitly read the results of the first load step from the results file Jobname.RCN by issuing the FILE and SET,FIRST commands before postprocessing. Otherwise, the result file may be read improperly.
11.4.16.3. Reviewing Results in POST26 The steps for reviewing results in POST26 are the same as those for a typical nonlinear analysis See Section 8.5.6.3: Reviewing Results in POST26 in Chapter 8, “Nonlinear Structural Analysis”.
11.5. GUI Aids for Contact Analyses 11.5.1. The Contact Manager in the ANSYS Standard To use the GUI method, access the Contact Manager via the Contact Manager icon Toolbar, or via the menu path Preprocessor> Modeling> Create> Contact Pair. You can access the Contact Manager at the Begin level and in the following processors: preprocessor (PREP7), solution (SOLU), and general postprocessor (POST1). The Contact Manager Toolbar provides an intuitive interface for the creation and management of contact pairs. The manager supports surface-to-surface contact analysis, node-to-surface contact analysis (using CONTA175), and the internal multipoint constraint (MPC) method of contact .
Figure 11.24 Contact Manager Toolbar
•
Contact Wizard - Accesses the Contact Wizard GUI described in Section 11.5.2: The Contact Wizard. Allows you to manually define target and contact surfaces. Supports both 2-D and 3-D geometries as well as rigidflexible (with optional pilot node) or flexible-flexible contact. (Primitives are not supported by contact wizard.) The wizard also supports surface-based constraint contact pairs.
•
Contact Properties - Allows you to specify the properties of the contact pair(s) via real constants and KEYOPTs for the contact elements used.
11–54
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.5: GUI Aids for Contact Analyses •
Delete Contact Pairs - Deletes the contact pairs selected in the contact pair list.
•
Contact Selection Options - Specifies display of contact elements, target elements, or both.
•
Plot Elements/Results - Displays the elements of selected contact pairs; or displays the contact results, if available (POST1 only), specified in the Contact Results field for selected contact pairs. Results are displayed if Model Context is specified as “Result-”; otherwise, elements are displayed. The display can be limited to contact, or target, or both as specified in the Contact Selection Options field. (Note that CONTA175 results will not display graphically, but can be listed with the List Elements/Results icon.)
•
Show Normals - Specifies whether or not to display the normals on the elements when plotting contact pairs
•
Flip Normals - Flips the element normals of the selected contact pair. This action is limited to the elements specified in the Contact Selection Options field.
•
Switch Contact and Target - Inverts the target surface and the contact surface with each other. This is applicable only to flexible-to-flexible surface-to-surface contact pairs.
•
List Elements/Results - Lists the elements of the selected contact pairs; or lists the contact results, if available (POST1 only), specified in the Contact Results field for selected contact pairs. Results are listed if Model Context is specified as “Result-”; otherwise, elements are listed. The listing is restricted to the elements specified in the Contact Selection Options field.
•
Model Context - Displays the contact pairs in the context of the entire model using a translucent plot, or shows only the contact pairs. If set to “Result-” (POST1 only), controls display/listing of contact pair results.
•
Check Contact Status - Provides contact status information for selected contact pairs. Several options are available (click and hold down the Check Contact Status button to access these options):
•
–
Display a detailed listing of status information for each contact pair.
–
Run a partial solution of the initial contact state (CNCHECK,POST command) that can be subsequently postprocessed from the contact manager. (See CNCHECK for more information.)
–
Physically move contact nodes to the target surface (CNCHECK,ADJUST command) in order to close a gap or reduce a penetration (see Section 11.4.8.8: Physically Moving Contact Nodes Towards the Target Surface.)
Contact Results - Shows the contact result items for subsequent viewing using the Plot Elements/Results and List Elements/Results icons.
The bar below the toolbar icons minimizes or maximizes the Contact Pair list box below it. The Contact Pair list box displays the defined contact pairs. You can select contact pairs from this list for displaying or editing purposes.
11.5.2. The Contact Wizard This Contact Wizard will lead you through the process of manually creating contact pairs. The wizard supports rigid-flexible (with optional pilot node) and flexible-flexible contact, and supports both surface-to-surface and node-to-surface configurations. (Note that the wizard does not support rigid target primitives.) The Contact Wizard also supports surface-based constraint contact pairs. To use the Contact Wizard, access the Contact Manager Toolbar and click on the Contact Wizard icon. The wizard steps you through setting up the contact analysis. Below is an example of the screens you will see.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–55
Chapter 11: Contact
Figure 11.25 Example of a Contact Wizard Dialog
The Contact Wizard remains unavailable (dimmed) if you haven't meshed any portion of your model. If you wish to create a rigid-flexible model, mesh only those parts of the model which will be used as flexible contact surfaces (do not mesh the rigid target surfaces) before launching the wizard. If you wish to create a flexible-flexible model, mesh all parts of the model which will be used as contact surfaces (including target surfaces) before launching the wizard. You can specify target and contact surfaces using lines, areas, volumes, selected set of nodes, or node components. Note that the wizard allows you to choose more than one area for the target and contact surfaces, thus allowing multiple areas to form a single contact surface. If you specify a rigid target surface, you will then have the option to define a pilot node for that contact pair. (The pilot node step is mandatory if you define a surface-based constraint contact pair by picking the Pilot Node Only option.) After you specify the target and contact surfaces, you can specify properties of the contact pair (real constants and KEYOPTs) before creating the contact pair. When you finish specifying all the required data, click the Create button to create the contact and target element types, a unique real constant set with the real constant values, and the elements that make up the contact and target surfaces.
11.5.3. Managing Contact Pairs As discussed in Section 11.4: Performing a Surface-to-Surface Contact Analysis it is paramount that the contact elements be oriented correctly for proper contact detection. The contact manager provides tools that help you 1.
Verify that the normals of the contact and target surfaces are in the correct direction
2.
Reverse normals of elements that are not oriented correctly
11–56
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.6: Performing a Node-to-Surface Contact Analysis You can choose to display one or more contact pairs on which to perform the above listed operations. Then you have an additional option of only displaying the contact surface or the target surface when verifying or reversing the element normals. In addition these elements can be displayed independently or in the context of your entire model. In the later case the contact elements are highlighted in a translucent plot of your model. Another important function is to edit the properties of the contact pair(s) as needed. The properties include real constant values and key option values as discussed earlier. The Contact Properties button in the contact manager provides a simple to use interface that allows the properties of the selected contact pair(s) to be reviewed and modified if needed. Note that when you have multiple contact pairs, it is possible to have conflicts in the real constant values or in the KEYOPT settings. When you have such conflicts, the properties dialog for those real constants or KEYOPT settings is left blank. Finally, you can display or list specific contact result items (contact status, penetration, pressure, etc.) for the selected contact pairs. This option is only available in POST1, and only if a result set is available. The contact results can be displayed independently or in the context of your entire model. (For CONTA175, results can be listed but not displayed graphically.) Note — Prior to displaying or listing result items associated with the initial contact configuration resulting from the CNCHECK,POST command, you need to issue the appropriate FILE and SET,FIRST commands to read the results from the proper results file (see CNCHECK for details).
11.6. Performing a Node-to-Surface Contact Analysis You can use our node-to-surface contact element CONTA175 to model flexible-flexible or rigid-flexible contact between a surface and a node. Additionally, you can use these elements to represent contact between two surfaces by specifying one surface as a group of nodes. Node-to-surface contact is a phenomenon that occurs in most engineering applications: fasteners (nuts, bolts, rivets, pins), metal forming, rolling operations, dynamic pipe whip, etc. Engineers are interested in the stresses, deflections, forces, and temperature changes that occur due to contact between structural parts.
11.6.1. Using the Node-to-Surface Contact Elements Node-to-surface contact is represented in the ANSYS program by following the positions of points on one surface (the contact surface, modeled by CONTA175) relative to lines or areas of another surface (the target surface, modeled by TARGE169 or TARGE170). CONTA175, in two or three dimensions, is depicted in Figure 11.26: “Node-to-Surface Contact Elements”.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–57
Chapter 11: Contact
Figure 11.26 Node-to-Surface Contact Elements
: 64 5-7 '8.29 @BADCBE=F<@HGIDCJKAML !" # $% &')(+*-,+. / 0
> ;<=( <
465-7 '8.29
@NAMCNEOF<@HG
>
Presented below are characteristics of CONTA175: •
Has one node and its target surface is defined by TARGE169 or TARGE170. CONTA175 uses the same real constant set as the surface-to-surface contact elements. See Real Constants for more information.
•
Supports 2-D/3-D rigid-flexible and flexible-flexible contact.
•
Does not support 3-D contact surfaces with midside nodes, but can support 2-D/3-D target surfaces with midside nodes or 2-D contact surfaces with midside nodes.
•
Generates elements using the ESURF command, as do the surface-to-surface contact elements.
•
Supports structural, thermal, electric, and magnetic analyses. Note — CONTA175 is recommended for point-to-surface or edge-to-surface problems. It can also be used to supplement a surface-to-surface pair at strategic locations where edge contact exists. For general surface-to-surface contact, CONTA171 through CONTA174 are recommended.
CONTA175 follows the contact pair concept used by surface-to-surface elements CONTA171 through CONTA174. CONTA175 is paired off with target elements TARGE169 and TARGE170. See Identifying Contact Pairs for more information. CONTA175 uses most of the same element KEYOPTS and real constants as the surface-to-surface contact elements. These are described below. You should avoid midside-noded underlying elements of the contact surface, especially in 3-D. The “effective stiffness” at the contact surface nodes is very nonuniform. For instance, for the 20-node bricks SOLID95 or HYPER86, the corner nodes have a negative stiffness associated with them. However, the node-to-surface contact algorithm assumes that the stiffness is uniformly distributed across all the surface nodes when contact is made. This condition can lead to convergence difficulties when using midside-noded elements in contact. The midside-noded elements can only be used when bonded or no-separation contact is defined. You can still use midside nodes on 2-D contact surfaces or on 2-D/3-D target surfaces. The basic steps for performing a node-to-surface contact analysis using CONTA175 are the same as those used for a typical surface-to-surface analysis using CONTA171 through CONTA174. See Steps in a Contact Analysis for details. The Contact Manager provides an easy-to-use interface to help you construct and manage contact definitions. You can access the manager via the Contact Manager icon
11–58
in the ANSYS Standard Toolbar, or via the menu
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.6: Performing a Node-to-Surface Contact Analysis path Main Menu> Preprocessor> Modeling> Create> Contact Pair. See Section 11.5: GUI Aids for Contact Analyses for more information on using the Contact Manager. As mentioned, CONTA175 uses the ESURF command to generate elements between corresponding contact pairs, similar to the surface-to-surface contact elements. The GUI path is: Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Node to Surf Since CONTA175 is a one node element, you are not able to plot the contact results. However, you can list the results using the PLESOL,CONT or PRETAB commands.
11.6.1.1. CONTA175 KEYOPTS CONTA175 uses most of the same KEYOPTS that are used by the surface-to-surface contact elements CONTA171 through CONTA174. KEYOPT(3) and KEYOPT(4) are used but have different meanings when used with CONTA175. See Section 11.4.8.2: Element KEYOPTS for a listing of the remaining KEYOPTS.
11.6.1.1.1. KEYOPT(3) KEYOPT(3) in CONTA175 allows you to choose between a contact force-based model (KEYOPT(3) = 0, default), and a contact traction-based model (KEYOPT(3) = 1). For the contact traction-based model, ANSYS can determine the area associated with the contact node. For the single point contact case, a unit area will be used which is equivalent to the contact force-based model. When the traction-based model is defined, the real constants FKN, FKT, TCC, ECC, and MCC have the same units used in surface-to-surface contact elements (CONTA171 through CONTA174), as do postprocessing items PRES, TAUR, and TAUS. When the force-based model is defined, the units of these quantities have a factor of AREA with respect to those used in the traction-based model. For instance, contact stiffness FKN has units FORCE/LENGTH for the forcebased model, but FORCE/LENGTH3 for the traction-based model. PRES is the contact normal force in the forcebased model, but contact pressure in the traction-based model.
11.6.1.1.2. KEYOPT(4) KEYOPT(4) in CONTA175 allows you to choose the contact normal direction. The contact normal can be either perpendicular to the target surface (KEYOPT(4) = 0, default or KEYOPT(4) = 3), or perpendicular to the contact surface (KEYOPT(4) = 1, 2). When contact occurs on the bottom surface of a shell or beam, and shell thickness effect is included (KEYOPT(11) = 1), or CNOF is defined, KEYOPT(4) = 2 or 3 should be used in order to capture the contact. Real constant TOLS is used to add a small tolerance that will internally extend the edge of the target surface. TOLS is useful for problems where contact nodes are likely to lie on the edge of the target (as at symmetry planes or for models generated in a node-to-node contact pattern). In these situations, the contact node may repeatedly “slip” off the target surface and so completely out of contact, resulting in convergence difficulties from oscillations. Units for TOLS are percent (1.0 implies a 1.0% increase in the target edge length). A small value of TOLS will usually prevent this situation from occurring. The default value is 10 for small deflection and 2 for large deflection (NLGEOM,ON).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–59
Chapter 11: Contact
11.6.1.2. CONTA175 Real Constants CONTA175 uses the same real constants used by the surface-to-surface contact elements CONTA171 through CONTA174), except the units of TCC, ECC, and MCC for the contact force-based model. See a listing of the real constants in Section 11.4.8.1: Real Constants.
11.6.1.3. Multiphysics Contact You can use node-to-surface contact element CONTA175 to model thermal contact, electric contact, and magnetic contact as you would use the surface-to-surface contact elements. For multiphysics contact, we recommend that you use the contact traction-based model (KEYOPT(3) = 1), which allows you to use TCC, FCC, and MCC consistently with the surface-to-surface contact elements. If you use the contact force-based model (KEYOPT(3) = 0), you should adjust the values of TCC, ECC, and MCC up or down as you make the element mesh coarser or finer.
11.7. Using the Internal MPC Approach for Assemblies and Kinematic Constraints You can use the internal multipoint constraint (MPC) approach (KEYOPT(2) = 2), in conjunction with the bonded contact definition (KEYOPT(12) = 5 or 6), to define various contact assemblies and kinematic constraints. This capability is available for contact elements CONTA171, CONTA172, CONTA173, CONTA174, and CONTA175. By this method, the program builds MPC equations internally based on the contact kinematics. You can use this method to model the following contact assemblies and surface-based constraints: •
Solid-solid assembly - both contact and target surfaces paste onto solid element faces
•
Shell-shell assembly - both contact and target surfaces paste onto shell element faces
•
Shell-solid assembly - the contact surface pastes onto shell element faces and the target surfaces paste onto solid element faces
•
Rigid constraint surface - the contact nodes are constrained to the rigid body motion defined by the pilot node (similar to the CERIG command)
•
Force-distributed surface - the forces or displacements applied to the pilot node are distributed to contact nodes, in an average sense, through shape functions (similar to the RBE3 command)
•
Beam-solid assembly - one beam end-node is the pilot node which connects to the solid or shell surface (use the rigid constraint surface or force-distributed surface type of MPC)
The internal MPC approach can overcome the drawbacks of the traditional contact algorithms and other multipoint constraint tools available in ANSYS. For example: •
Degrees of freedom of the contact surface nodes are eliminated. This reduces the wave front size of the system equation solver.
•
No contact stiffness is required as input. For a small deformation problem, this represents true linear contact behavior; no iteration is needed in solving the system of equations. For large deformation problems, the MPC equations are updated during each iteration. This overcomes the small strain restriction in conventional constraint equations.
•
Both translational and rotational degrees of freedom can be constrained.
•
The generation of internal MPC is simple because it utilizes contact pair definitions.
•
Shape functions are taken into account automatically; no weight factor is needed for a force-distributed multipoint constraint (which is similar to the RBE3 command) if high order elements or axisymmetric
11–60
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints elements are used. In addition to forces, displacements can be applied on the pilot node for this type of MPC. The following sections describe how to use the internal MPC approach to define assemblies and surface-based constraints. Before using the internal MPC feature, be sure to review Section 11.7.4: Restrictions and Recommendations for Internal MPC.
11.7.1. Modeling Solid-solid and Shell-shell Assemblies To define solid-solid or shell-shell assemblies using the internal MPC approach, you must set the following key options on the contact elements: KEYOPT(2) = 2 - MPC based approach KEYOPT(12) = 5 or 6 - Bonded always or bonded initial KEYOPT(4) = 1 or 2 - Nodal detection for CONTA171, CONTA172, CONTA173, CONTA174 KEYOPT(4) = 0 or 1 - Contact normal direction for CONTA175 The following key options are ignored: KEYOPT(8) (it is always set to 2 internally), KEYOPT(10). The following real constants are used: R1, R2, ICONT, PINB, CNOF, PMAX, PMIN, TOLS. All other real constants are ignored. This function works similarly to the CEINTF command for small deformation analysis (NLGEOM,OFF). Comparing it to the CEINTF command, the contact surface acts as “region A nodes,” and the target surface acts as “region B elements.” As usual, the contact surface must be defined on the deformable bodies, and the target surface must be defined on either deformable or rigid bodies in the contact pair. In order to prevent over-constraint, only asymmetric contact is supported. If symmetric pairs are defined, ANSYS will automatically pick one pair and ignore the other pair (acting as KEYOPT(8) = 2). The self-contact pair definition is not supported. If the temperature degree of freedom is active in the model (KEYOPT(1) = 1 or 2), ANSYS will build MPC equations not only for structural degrees of freedom, but also for the temperature DOF. In this case, the real constant TCC is ignored. If only the temperature DOF is set (KEYOPT(1) = 2) and other solution options are defined (ANTYPE,,TRANS; THOPT,QUASI; EQSLV,JCG/ICCG), the internal MPC approach can support fast thermal transient analysis (see Section 3.5.4: Nonlinear Options in the ANSYS Thermal Analysis Guide). Internal MPC equations for temperature DOF are built to support heat transfer between the two bonded surfaces. For the “bonded always” option (KEYOPT(12) = 5), any contact node that lies inside the pinball region (PINB) can be the constrained node in the MPC definition if an intersection with the target surface is detected in the contact normal direction. This holds true at the beginning of deformation, as well as during the deformation process. A relatively small PINB may be used to prevent any false contact. When the “bonded always” option is set, the default for PINB is 0.25 (25% of the contact depth) for small deformation analysis (NLGEOM,OFF), and 0.5 (50% of the contact depth) for large deformation analysis (NLGEOM,ON). (The default PINB value may differ from what is described here if CNOF is input. See Section 11.4.8.9.2: Using PINB for more information.) For the “bonded initial” option (KEYOPT(12) = 6), only those contact nodes that are initially in contact or have a very small gap but lie inside the adjustment zone (ICONT) are always constrained via internal MPC. Those contact nodes that are initially open will never be constrained, even though they may later penetrate into the target surface during the deformation process. In order to capture contact, you should specify proper ICONT or CNOF values. Use CNCHECK in conjunction with ICONT to move all the contact nodes that are inside the ICONT zone onto the target surface in the initial configuration, without causing any strain. When the “bonded initial” option is set and KEYOPT(5) = 0 or 4, ICONT defaults to 0.05. See Section 11.4.8.7: Adjusting Initial Contact Conditions for more information on using KEYOPT(5), CNOF, and ICONT. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–61
Chapter 11: Contact In most cases, ANSYS will automatically constrain the translational degrees of freedom for a solid-solid assembly and constrain both translational and rotational degrees of freedom for a shell-shell assembly. However, you can use KEYOPT(5) of the target element (TARGE170) to explicitly define the type of constraint: KEYOPT(5) = 0 - Auto constraint type detection KEYOPT(5) = 1 - Solid-solid constraint (no rotational DOFs are constrained) KEYOPT(5) = 2 - Shell-shell constraint (both translational and rotational DOFs are constrained)
11.7.2. Modeling a Shell-solid Assembly The 3-D shell-solid assembly provides a transition from a shell element region to a solid element region. This approach is useful when local modeling requires a full three-dimensional model with a relatively fine mesh, but other parts of the structure can be represented by shell elements (see Figure 11.27: “Example of Shell-solid Assembly”). No alignment is required between the solid element mesh and the shell element mesh. The contact surface or edge must be built on the shell element side. The target surface must be built on the solid elements side.
Figure 11.27 Example of Shell-solid Assembly
!
To define a shell-solid assembly using the internal MPC approach, you must set the following key options on the contact elements: KEYOPT(2) = 2 - MPC based approach. KEYOPT(12) = 5 or 6 - Bonded always or bonded initial KEYOPT(4) = 1 or 2 - Nodal detection for CONTA171, CONTA172, CONTA173, CONTA174 KEYOPT(4) = 0 or 1 - Contact normal direction for CONTA175 11–62
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints The following real constants are also used: ICONT, FTOL, PINB, CNOF, PMAX, PMIN, TOLS. The following key options are ignored: KEYOPT(8), KEYOPT(10), KEYOPT(1)>0. In most cases, ANSYS will automatically constrain both translational and rotational degrees of freedom for a shell-solid assembly (see Figure 11.28: “Shell-solid Assembly (Original Mesh)”). However, you can use KEYOPT(5) of the target element (TARGE170) to explicitly define the type of constraint: KEYOPT(5) = 0 - Auto constraint type detection KEYOPT(5) = 1 - Solid-solid constraint; no rotational DOFs are constrained (see Figure 11.29: “Shell-solid Assembly with Solid-solid Constraint Option”) KEYOPT(5) = 2 - Shell-shell constraint; both translational and rotational DOFs are constrained (see Figure 11.30: “Shell-solid Assembly with Shell-shell Constraint Option”) KEYOPT(5) = 3 - Shell-solid constraint; both translational and rotational DOFs are constrained on shell nodes, only translational DOFs are constrained on solid nodes (see Figure 11.31: “Shell-solid Assembly with Shellsolid Constraint Option”) KEYOPT(5) = 4 - Shell-solid constraint, all directions. This option acts the same as KEYOPT(5) = 3 if an intersection is found from the contact normal to the target surface. Otherwise, constraint equations are still built as long as contact nodes and target segments are inside the pinball region. The solid-solid and shell-shell constraint types (KEYOPT(5) = 1 or 2) may require additional shell elements at the interface. These shell elements can be defined by typical modeling methods, or you can use the SHSD command to generate these elements automatically. SHSD is a meshing tool used to build solid-solid and shell-shell constraint types. This command can be used only when the contact pair consists of CONTA175 and TARGE170 elements. Additional shell elements (SHELL181) and/or contact elements (CONTA175) are created through this command (see the SHSD command description for more information). For the shell-solid constraint type, no special mesh tool is required.
Figure 11.28 Shell-solid Assembly (Original Mesh)
#%$ & ' ' & ' &()&*+-, .+$ / 021* &,,3 4 !" #65 ' / 78& ' &(&*+,
9!:;< &2+ & ' &(&*+, 9=?>A@B%CDE .5*F+5G)5 H ,!5 ' / 7 4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–63
Chapter 11: Contact
Figure 11.29 Shell-solid Assembly with Solid-solid Constraint Option
!"! $#&%('')*+) 4 !<J9 6 6 A"" 7 K#KK8L 2MN" !A> / 2!6 !D / : FEG )HI ,.-0/ 1 2!3 54 6 !3 7 2!98:<;92! => 5 ? @ 32 A< CB
Figure 11.30 Shell-solid Assembly with Shell-shell Constraint Option
O P3QRS TU VWX K YZ PX X P X P!["P!\U Y b n W!\
].^0_P`VWU7S a!\ Y b U T6W!\ Y X WU7S a!\
11–64
g s0f"t O b S \ i X VP!\ n PNj!S Y UW!\ n Ph
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints
Figure 11.31 Shell-solid Assembly with Shell-solid Constraint Option
! " # $
% &('*)+ , $-. / $- 0
For the shell-solid constraint option (KEYOPT(5) = 3 on TARGE170), ANSYS automatically creates an internal set of force-distributed constraints (similar to the RBE3 command) between nodes on the shell edges and nodes on the solid surface. The program uses the pinball region (PINB), initial adjustment zone (ICONT), and influence distance (FTOLN) to determine which nodes on the shell edge will be constrained with which nodes on the solid surface. Each shell node acts as the master node, and associated solid nodes act as slave nodes. For the “bonded always” option (KEYOPT(12) = 5), any shell node that lies inside the pinball region (PINB) will be included in the constraint if an intersection with the target surface is detected in the contact normal direction. This holds true at the beginning of deformation, as well as during the deformation process. A relatively small PINB value may be used to prevent any false contact. The default for PINB is 0.25 (25% of the contact depth) for small deformation analysis (NLGEOM,OFF), and 0.5 (50% of the contact depth) for large deformation analysis (NLGEOM,ON). (The default PINB value may differ from what is described here if CNOF is input. See Section 11.4.8.9.2: Using PINB for more information.) For the “bonded initial” option (KEYOPT(12) = 6), only the shell nodes that initially lie inside the adjustment zone (ICONT) are included in the constraint sets. Shell nodes that lie outside ICONT are not constrained with the solid nodes. The default for ICONT is 0.05 (5% of the contact depth). The influence distance (FTOLN) is used for the shell-solid constraint option (KEYOPT(5) =3 on TARGE170). Each solid node is included in the constraint set if the perpendicular distance from the solid node to any shell edge is smaller than the influence distance. FTOLN defaults to half the thickness of the shell. A positive FTOLN value represents a scaling factor on the shell half-thickness, and a negative value represents an absolute distance value. A shell-solid assembly can be used in a substructure analysis. However, if a superelement is defined to represent the shell elements, shell thickness is unknown in the use pass. In this case, you must overwrite the default setting of FTOLN (originally a factor of the shell thickness) to account for the zero thickness of the superelement. Input an absolute value for FTOLN (that is, input a negative value) to capture all constrained nodes when the constraint equations are built.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–65
Chapter 11: Contact Among the four constraint types, the shell-shell constraint approach (KEYOPT(5) = 2 on TARGE170) often provides a better solution. The solid-solid constraint (KEYOPT(5) = 1) can result in higher local stresses near the interface between the virtual shell surface and solid surface. The shell-solid constraint (KEYOPT(5) = 3 or 4 ) is not always capable of transmitting all components of the moment at the shell nodes due to transverse shear locking of shell elements. A typical example is the moment component that parallels to the normal of the solid surface. The KEYOPT(5) = 4 option (shell-solid constraint , all directions) is recommended for detecting contact in bodies that do not overlap or intersect. For the solid-solid and shell-shell constraint types (KEYOPT(5) = 1 or 2 on TARGE170), any initial penetration or gap is closed if KEYOPT(9) = 0; the initial penetration or gap remains if KEYOPT(9) = 1. However, for the shellsolid constraint type (KEYOPT(5) = 3 or 4), KEYOPT(9) is ignored, and initial penetration or gap always remains constant. In order to close the initial penetration or gap, issue the command CNCHECK,ADJUST in the beginning of the analysis.
11.7.3. Surface-based Constraints A surface-based constraint can be used to couple the motion of nodes on the contact surface to a single pilot node on the target surface. The multipoint constraint (MPC) capability of the contact elements (KEYOPT(2) = 2) allows you to define two types of surface-based constraints: •
Rigid constraint surface - In this type of constraint, the contact nodes are constrained to the rigid body motion defined by the pilot node (see Figure 11.32: “Rigid Constraint Surface”). This is similar to a constraint defined by the CERIG command.
•
Force-distributed constraint surface - In this type of constraint, forces or displacements applied on the pilot node are distributed to contact nodes (in an average sense) through shape functions (see Figure 11.33: “Force-distributed Surface”). This is similar to a constraint defined by the RBE3 command.
Figure 11.32 Rigid Constraint Surface "!$# %'&
*)+ ,- )/.0 ()0 1 )2 34
+ 5 1 6 (
11–66
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints
Figure 11.33 Force-distributed Surface !#"%$ &('
*+,- .,. /0 ,1*+
2
)
3 4 3
These surface-based constraints can be used in the following applications: •
To apply loads and boundary conditions to the pilot node (such as torque load or drill rotation). Example: a bolt head submitted to a torque force using a force-distributed surface constraint.
•
To model rigid end conditions. Example: using a rigid constraint surface to model a rigid end plate or rigid plane section of 3-D solid elements.
•
To define transitions between solid and structure elements. Example: a beam element connected to a solid element face.
11.7.3.1. Defining Surface-based Constraints The contact surface can be generated via the ESURF command. The contact nodes on the contact surface are the slave nodes of the MPC equations. The pilot node is the only target segment on the target surface side. It is the master node of the MPC equations. Forces and displacements can be applied on the pilot node. For a force-distributed surface constraint, use the following contact element key options: KEYOPT(2) = 2 - MPC based approach KEYOPT(12) = 5 or 6 - Bonded always or bonded initial (the two cases are the same) KEYOPT(4) = 1 - Nodal detection for CONTA171, CONTA172, CONTA173, CONTA174; Contact normal direction for CONTA175 For a rigid constraint surface, use the following contact element key options: KEYOPT(2) = 2 - MPC based approach KEYOPT(12) = 5 or 6 - Bonded always or bonded initial (the two cases are the same) KEYOPT(4) = 2 - Nodal detection for CONTA171, CONTA172, CONTA173, CONTA174 KEYOPT(4) = 0 - Contact normal direction for CONTA175 The following key options are ignored for surface-based constraints: KEYOPT(8), KEYOPT(5), KEYOPT(7), KEYOPT(10). Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–67
Chapter 11: Contact None of the standard contact real constants are used for surface-based constraints using internal MPC. KEYOPT(1) > 0 is ignored for a force-distributed surface constraint since only structural degree-of-freedom constraints are included. However, for a rigid constraint surface, you can use KEYOPT(1) to include other field degrees of freedom (in addition to the structural DOFs) in the constraint sets. You can specify the surface-based constraint in a local coordinate system. For the rigid constraint surface, rotate the contact nodes into a local coordinate system. For the force-distributed constraint, rotate the pilot node into a local coordinate system. You can apply the surface based constraint to a user-defined DOF set with respect to the global or the local coordinate system by using KEYOPT(4) of the target element (TARGE169 or TARGE170). For example, for the 3-D case (TARGE170), you might specify that only UX, UY, and ROTZ be used in the constraint. You can do this by entering a six digit value for KEYOPT(4). The first to sixth digits represent ROTZ, ROTY, ROTX, UZ, UY, UX, respectively. The number 1 (one) indicates the DOF is active, and the number 0 (zero) indicates the DOF is not active. Therefore, to specify that UX, UY, and ROTZ be used in the constraint, you would enter 100011 as the KEYOPT(4) value. For a force-distributed surface constraint, these additional guidelines apply: •
The pilot node is a dependent node (meaning the degrees of freedom for this node are removed). The contact nodes are independent nodes (the degrees of freedom are retained). If the pilot node has constraints applied to it, internally-generated MPCs are rewritten so that the degrees of freedom of the pilot node are no longer dependent DOF.
•
The pilot node has up to 3 degrees of freedom (2-D) or up to 6 degrees of freedom (3-D).
•
KEYOPT(4) of TARGE169 and TARGE170 controls the number of degrees of freedom of the pilot node.
•
The number of internally-generated MPCs is equal to the number of degrees of freedom defined by KEYOPT(4) of TARGE169 and TARGE170.
For a rigid constraint surface, these additional guidelines apply: •
The pilot node is an independent (retained) node in the constraint equation. The contact nodes are the dependent (removed) nodes. You should not apply any displacement constraints, coupling (CP command), or constraint equations (CE command) on the contact nodes.
•
The pilot node has 6 degrees of freedom (3-D) or 3 degrees of freedom (2-D).
•
KEYOPT(4) of TARGE169 and TARGE170 controls the DOF set (the number of DOF) of the contact (dependent) nodes used in the internally-generated MPCs.
•
The number of internally-generated MPCs is equal to (number of contact nodes) x (number of DOF).
11.7.3.2. Modeling a Beam-solid Assembly The surface-based constraint technique can be used to apply transitions between solid and structure elements; for example, a beam element connected to the solid or shell element face. One beam end node must be the pilot node and the solid/shell nodes must be the contact nodes. Generally speaking, the rigid constraint surface is well suited for the solid beam to solid surface case (see Figure 11.34: “Beam-solid Assembly Defined by Rigid Constraint Surface”) and the force-distributed constraint surface is well suited for the flexible beam (such as a thin wall beam) to solid/shell surface case (see Figure 11.35: “Beam-solid Assembly Defined by Force-distributed Surface”).
11–68
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints
Figure 11.34 Beam-solid Assembly Defined by Rigid Constraint Surface
!
Figure 11.35 Beam-solid Assembly Defined by Force-distributed Surface
"$# %& &'%& %( %)*!+ ./ & 0*) 0 1 %
, %-(%& %( %)*+
230)* - 4 *%& %( %)5*!+
11.7.4. Restrictions and Recommendations for Internal MPC The following restrictions apply when using the internal MPC approach.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–69
Chapter 11: Contact Generally speaking, displacement boundary conditions and other constraint equations or coupling equations should not be applied on the contact nodes for solid-solid, shell-shell, and shell-solid assemblies, and also for the rigid constraint surface MPC. Otherwise, over-constraint can occur since the degrees of freedom of contact nodes are eliminated through internal MPC equations. Sparse, PCG, and AMG solvers are recommended to solve models with constraint equations. In certain cases, the frontal solver may not solve problems containing constraint equations. The MPC based algorithm must work with nodal detection (KEYOPT(4) = 1 or 2) for CONTA171, CONTA172, CONTA173, and CONTA174. If nodal detection is not set, ANSYS will issue a warning message and automatically set KEYOPT(4) = 2. The internal MPC option does not support rigid-flexible contact when rigid surfaces are modeled by any primitive segments (such as circle, cylinder, cone, or sphere). The shell-solid assembly is usually used for the case where the solid mesh is fine with respect to the shell thickness. The shell-solid interface should be located in a region of the structure where shell theory is valid for an approximation. The accuracy of local stresses near the shell-solid interface (at least within the shell thickness range) is not guaranteed. We recommend you include at least two solid elements along the layer of the shell-solid interface. Using the force-distributed constraint type of MPC with a large number of contact nodes can result in a large wavefront for the global stiffness matrix. This may significantly increase the peak memory required during of element stiffness assembly. Consider reducing the number of contact nodes if real memory or virtual memory is limited. The contact related postprocessing items (ETABLE items, PRESOL,CONT, etc.) are not supported for the internal MPC option.
11.8. Performing a Node-to-Node Contact Analysis You can use node-to-node contact elements to model point-to-point contact (flexible-flexible or rigid-flexible). Additionally, you can use these elements to represent contact between two surfaces by specifying individual node-to-node contact between the opposing nodes of each surface. This use requires that the nodes of the two opposing surfaces match up geometrically and that the relative sliding between the two surfaces will be negligible. In addition, the deflections (rotations) of the two surfaces must remain small. The most commonly used node-to-node elements are shown in the following figure.
Figure 11.36 Node-to-Node Contact Elements
! " #
11–70
! %$ &
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.8: Performing a Node-to-Node Contact Analysis In terms of solution CPU time, the elements shown are the simplest and least expensive of all contact element types. When modeling conditions warrant their use, they can be an effective tool for modeling a variety of contact situations. CONTA178 offers more features and flexibility than CONTAC12 and CONTAC52. The following lists the features available with CONTA178: •
More contact algorithms, including the Lagrange method (KEYOPT(2))
•
Semiautomatic contact stiffness (real constants FKN-FKS)
•
More flexibility for defining contact normal
•
More contact behaviors (KEYOPT(10))
•
Cylindrical gap with friction (KEYOPT(4) = 4)
•
Damper (real constants CV1, CV2) Note — CONTA178 supports only elastic Coulomb friction behavior. For rigid Coulomb friction models, use CONTAC12 and CONTAC52
The procedure for performing a node-to-node contact analysis is similar to that described for the node-to-surface contact elements in Section 11.6: Performing a Node-to-Surface Contact Analysis. The following describes the typical steps in a node-to-node contact analysis. Each of these steps is explained in detail. 1.
Create the geometry and mesh the model.
2.
Generate the contact elements.
3.
Define the contact normal.
4.
Define the initial interference or gap.
5.
Select the contact algorithm.
6.
Apply the necessary boundary conditions.
7.
Define the solution options.
8.
Solve the problem.
9.
Review the results.
11.8.1. Creating Geometry and Meshing the Model Node-to-node contact elements transmit forces at the nodes (compared to surface-to-surface contact elements which transmit pressures at Gauss points). This feature limits their use to low order elements only. You must identify where contact might occur during the deformation of your model. The nodes on the two surfaces of potential contact must line up. Once you've identified potential contact surfaces and created an adequate mesh you can create the contact elements.
11.8.2. Generating Contact Elements You can generate node-to-node contact element in one of two ways: 1.
Use the direct generation method: Command(s): E GUI: Main Menu> Preprocessor> Modeling> Create> Elements> User Numbered> Thru Nodes
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–71
Chapter 11: Contact 2.
Use the EINTF command to generate the contact elements automatically at coincident nodes or offset nodes. This is discussed in detail in the following subsections.
11.8.2.1. Generating Contact Elements Automatically at Coincident Nodes If the two bodies are in the “just touching” position, you can use the EINTF command to automatically generate the contact elements. In this case, the menu path is Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> At Coincident Nodes. Only nodes within the tolerance value set in the first argument (TOLER) are considered as coincident. If you wish to check a subset of nodes for coincidence, first select all the nodes you wish to check using the NSEL command.
11.8.2.2. Generating Contact Elements Automatically at Offset Nodes If the two bodies are separated by a gap, the EINTF command can be used to create elements between offset nodes by specifying the node location increments (DX, DY, DZ) in the coordinate system KCN. The GUI path is Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Offset Nodes. If KOPT is set to 1, the nodes belonging to the contact elements created are rotated into the coordinate system KCN. For example, the following figure shows contact between two concentric pipes separated by a gap. In this example, KCN would be a cylindrical coordinate system centered in O, and DX would be set in ∆ (∆± TOLER).
Figure 11.37 Contact Between Two Concentric Pipes
11.8.2.3. Node Ordering Node ordering can be critical in determining the contact normal. You can use EINTF,,,LOW or EINTF,,,HIGH to control node ordering. When using the LOW argument, the 2-node elements are generated from the lowest numbered node to the highest numbered node. When using HIGH, 2-node elements are generated from the highest to the lowest. To check the contact normal, use /PSYMB,ESYS. If you discover that the ordering is incorrect, you can reverse it using EINTF,,,REVE. To determine which side of the interface contains the I nodes, use the following commands: ESEL,,ENAME,,178 NSLE,,POS,1 ESLN
11–72
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.8: Performing a Node-to-Node Contact Analysis NSLE EPLOT
11.8.3. Defining the Contact Normal The contact normal direction is of primary importance in a contact analysis with CONTA178. By default [KEYOPT(5) = 0 and NX, NY, NZ = 0], ANSYS will calculate the contact normal direction based on the initial positions of the I and J nodes, such that a positive displacement (in the element coordinate system) of node J relative to node I opens the gap. However, you must specify the contact normal direction for any of the following conditions: •
If nodes I and J have the same initial coordinates.
•
If the model has an initial interference condition in which the underlying elements' geometry overlaps.
•
If the initial open gap distance is very small.
In the above cases, the ordering of nodes I and J is critical. The correct contact normal usually points from node I toward node J unless contact is initially overlapped. You can specify the contact normal by means of real constants NX, NY, NZ (direction cosines related to the global Cartesian system) or element KEYOPT(5). The following lists the various options for KEYOPT(5): KEYOPT(5) = 0 The contact normal is either based on the real constant values of NX, NY, NZ or on node locations when NX, NY, NZ are not defined. For two dimensional contact, NZ = 0. KEYOPT(5) = 1 (2,3) The contact normal points in a direction which averages the direction cosines of the X (Y, Z) axis of the nodal coordinates on both nodes I and J. The direction cosines on nodes I and J should be very close. This option may be supported by the NORA and NORL commands, which rotate the X axis of the nodal coordinate system to point to the surface normal of solid models. The GUI paths for these commands are, respectively: Main Menu> Preprocessor> Modeling> Move/Modify> Rotate Node CS> To Surf Normal> On Areas Main Menu> Preprocessor> Modeling> Move/Modify> Rotate Node CS> To Surf Normal> On Lines Main Menu> Preprocessor> Modeling> Move/Modify> Rotate Node CS> To Surf Normal> With Area
Figure 11.38 Two Concentric Pipes, Normals Rotated Properly
For a pipe-within-a-pipe, this portrays the normals rotated properly. KEYOPT(5) = 4 (5,6) The contact normal points to X (Y, Z) of the element coordinate system issued by the ESYS command. If you use this option, make sure that the element coordinate system specified by ESYS is the Cartesian system. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–73
Chapter 11: Contact Note — For CONTAC12 you can define the orientation of the contact surface with real constant THETA. For CONTAC52, you can use real constants NX, NY, NZ.
11.8.4. Defining the Initial Interference or Gap With CONTA178, the gap size can be automatically calculated from the GAP real constant plus the node locations (projection of vector points from node I to J on the contact normal). This is the default (KEYOPT(4) = 0) This means that if you want the initial gap to be determined by the node locations only, set KEYOPT(4) = 0 and the real constant GAP to 0. If KEYOPT(4) = 1, the initial gap size is only based on the real constant GAP (it ignores the node location). A negative value for the gap size can be used to model initial interference. You can ramp initial interference using KEYOPT(9) = 1. This option isn't supported by CONTAC12 and CONTAC52. Note that CONTAC52's real constant GAP is the opposite of CONTAC12's real constant INTF, which defines an interference. KEYOPT(4) for CONTAC12 and CONTAC52 is also different from CONTA178.
11.8.5. Selecting the Contact Algorithm You can choose among the following four different contact algorithms for CONTA178: •
Pure Lagrange Multiplier
•
Lagrange multiplier on the contact normal, penalty on the frictional (tangential) direction.
•
Augmented Lagrange method
•
Pure penalty method.
CONTAC12 and CONTAC52 offer only the pure penalty method, in which you must specify the contact stiffness. The normal stiffness KN should be based upon the stiffness of the surface in contact. However, if you choose to use CONTA178 with the pure penalty method or the augmented Lagrange method, a “semiautomatic” setting is provided for the contact normal and tangential stiffnesses. ANSYS provides a default normal contact stiffness FKN, which is based on Young's modulus E and the size of the underlying elements. FKN and FKS are factors. If you want to import absolute values for FKN and FKS, use negative values.
11.8.6. Applying Necessary Boundary Conditions You can now apply necessary boundary conditions as you would do for any ANSYS analysis. For more information on applying boundary conditions, see the appropriate analysis description in earlier chapters of this guide. When using the Lagrange multiplier method, be careful not to overconstrain the model. The model is overconstrained when a contact constraint at a node conflicts with a prescribed boundary condition on that degree of freedom at the same node. The following figure illustrates this issue:
11–74
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.8: Performing a Node-to-Node Contact Analysis
Figure 11.39 Example of Overconstrained Contact Problem
Both nodes I and J are fixed in the X direction. The model is overconstrained only when the two bodies are in contact and bonded contact or rough friction has been defined. It can also occur if the contact status is “sticking,” In these cases, the constraint in the X-direction is duplicated which causes an overconstrained model. “Zero Pivot” and “Numerical Singularity” warning messages indicate overcontraints in a model. Overconstraints can lead to convergence difficulties and/or inaccurate results. They can be easily avoided by changing the contact definition or the boundary conditions.
11.8.7. Defining the Solution Options Convergence behavior for contact problems depends strongly on the particular problem. The options listed below are either typical or recommended for most node-to-node contact analyses. •
Set the appropriate auto time step behavior using KEYOPT(7). The SOLCONTROL command turns this off by default.
•
The time step size must be small enough to capture the proper contact zone. The smooth transfer of contact forces is disrupted if the time step size is too large. A reliable way to set an accurate time step size is to turn automatic time stepping on. The SOLCONTROL command turns this on by default. Command(s): AUTOTS,ON GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Time-Time Step Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Time and Substps
•
Set the number of equilibrium equations to a number that is appropriate for a reasonable time step size. With SOLCONTROL,ON, this command defaults to between 15 and 26 iterations, depending upon the physics of the problem. Command(s): NEQIT GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Nonlinear Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Equilibrium Iter
•
Turn the predictor-corrector option on, unless you expect large rotations. Command(s): PRED GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Nonlinear Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Predictor
•
Set the Newton-Raphson option to FULL, with adaptive descent on. Command(s): NROPT,FULL,,ON Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–75
Chapter 11: Contact GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options •
For analysis involving friction, using NROPT, UNSYM is useful (and sometimes required if the coefficient of friction µ is > 0.2) for problems where the normal and tangential (sliding) motions are strongly coupled.
•
NLGEOM, ON is supported but the contact normal is not updated during the analysis. Make sure that only small rotations occur along the contact surfaces (except for the cylindrical gap option).
•
Many convergence failures in contact analysis are the result of using too large a value for contact stiffness (real constant KN). Be sure to follow the recommendations given previously in this section for an initial estimate for contact stiffness. If such estimated values lead to a convergence failure, reduce the contact stiffness and restart. (You must also explicitly define the tangent stiffness - see the Note below.)
•
Conversely, if overpenetration occurred in your contact analysis, you probably used a value of KN that was too small. In this case, gradually increase the contact stiffness value to an appropriate level by redefining it using new R commands over several load steps in a restart. (You must also explicitly define the tangent stiffness - see the Note statement below.) Note — Although you can change the contact stiffness value (real constant KN), you cannot change any other real constants between load steps. Therefore, if you plan to change KN in a restart (or from one load step to the next), you cannot allow the value of the tangent (or "sticking") contact stiffness (real constant KT) to be defined by default, because the program would then attempt to redefine the tangent stiffness as the contact stiffness changed. You must explicitly define the tangent stiffness whenever you change the contact stiffness to maintain a consistent value for the tangent stiffness throughout all load steps.
11.8.8. Solving the Problem You can now solve the analysis the same as you would for any linear or nonlinear analysis. See Section 2.3.5: Solve the Analysis in Chapter 2, “Structural Static Analysis”.
11.8.9. Reviewing the Results Postprocessing of contact result items for these elements requires the use of ETABLE commands. The steps for reviewing results in POST26 are the same as those for a typical nonlinear analysis See Section 8.5.6.3: Reviewing Results in POST26 in Chapter 8, “Nonlinear Structural Analysis”. For general information on post processing, refer to the ANSYS Basic Analysis Guide.
11–76
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 12: Fracture Mechanics 12.1. Definition of Fracture Mechanics Cracks and flaws occur in many structures and components, sometimes leading to disastrous results. The engineering field of fracture mechanics was established to develop a basic understanding of such crack propagation problems. Fracture mechanics deals with the study of how a crack or flaw in a structure propagates under applied loads. It involves correlating analytical predictions of crack propagation and failure with experimental results. The analytical predictions are made by calculating fracture parameters such as stress intensity factors in the crack region, which you can use to estimate crack growth rate. Typically, the crack length increases with each application of some cyclic load, such as cabin pressurization-depressurization in an airplane. Further, environmental conditions such as temperature or extensive exposure to irradiation can affect the fracture propensity of a given material. Some typical fracture parameters of interest are: •
Stress intensity factors (KI, KII, KIII) associated with the three basic modes of fracture (see Figure 19.13: “The Three Basic Modes of Fracture” in the ANSYS, Inc. Theory Reference).
•
J-integral, which may be defined as a path-independent line integral that measures the strength of the singular stresses and strains near a crack tip
•
Energy release rate (G), which represents the amount of work associated with a crack opening or closure
12.2. Solving Fracture Mechanics Problems Solving a fracture mechanics problem involves performing a linear elastic or elastic-plastic static analysis and then using specialized postprocessing commands or macros to calculate desired fracture parameters. In this section, we will concentrate on two main aspects of this procedure: •
Modeling the Crack Region
•
Calculating Fracture Parameters
See Chapter 2, “Structural Static Analysis” for details about the general static analysis procedure. Also see Chapter 8, “Nonlinear Structural Analysis” for a discussion of structural nonlinearities.
12.2.1. Modeling the Crack Region The most important region in a fracture model is the region around the edge of the crack. We will refer to the edge of the crack as a crack tip in a 2-D model and crack front in a 3-D model. This is illustrated in Figure 12.1: “Crack Tip and Crack Front”.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 12: Fracture Mechanics
Figure 12.1 Crack Tip and Crack Front
In linear elastic problems, it has been shown that the displacements near the crack tip (or crack front) vary as
r , where r is the distance from the crack tip. The stresses and strains are singular at the crack tip, varying as r
. To pick up the singularity in the strain, the crack faces should be coincident, and the elements around 1/ the crack tip (or crack front) should be quadratic, with the midside nodes placed at the quarter points. Such elements are called singular elements. Figure 12.2: “Examples of Singular Elements” shows examples of singular elements for 2-D and 3-D models.
12–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 12.2: Solving Fracture Mechanics Problems
Figure 12.2 Examples of Singular Elements
(a) 2-D models and (b) 3-D models
12.2.1.1. 2-D Fracture Models The recommended element type for a 2-D fracture model is PLANE2, the 6-node triangular solid. The first row of elements around the crack tip should be singular, as illustrated in Figure 12.2: “Examples of Singular Elements” (a). The PREP7 KSCON command (Main Menu> Preprocessor> Meshing> Size Cntrls> Concentrat KPs> Create), which assigns element division sizes around a keypoint, is particularly useful in a fracture model. It automatically generates singular elements around the specified keypoint. Other fields on the command allow you to control
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
12–3
Chapter 12: Fracture Mechanics the radius of the first row of elements, number of elements in the circumferential direction, etc. Figure 12.3: “A Fracture Specimen and 2-D FE Model” shows a fracture model generated with the help of KSCON.
Figure 12.3 A Fracture Specimen and 2-D FE Model
Other modeling guidelines for 2-D models are as follows: •
Take advantage of symmetry where possible. In many cases, you need to model only one half of the crack region, with symmetry or antisymmetry boundary conditions, as shown below.
Figure 12.4 Taking Advantage of Symmetry
•
For reasonable results, the first row of elements around the crack tip should have a radius of approximately a/8 or smaller, where a is the crack length. In the circumferential direction, roughly one element every 30° or 40° is recommended.
•
The crack tip elements should not be distorted, and should take the shape of isosceles triangles.
12.2.1.2. 3-D Fracture Models The recommended element type for 3-D models is SOLID95, the 20-node brick element. As shown in Figure 12.2: “Examples of Singular Elements” (b), the first row of elements around the crack front should be singular elements. Notice that the element is wedge-shaped, with the KLPO face collapsed into the line KO.
12–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 12.2: Solving Fracture Mechanics Problems Generating a 3-D fracture model is considerably more involved than a 2-D model. The KSCON command is not available, and you need to make sure that the crack front is along edge KO of the elements. Other meshing guidelines for 3-D models are as follows: •
Element size recommendations are the same as for 2-D models. In addition, aspect ratios should not exceed approximately 4 to 1 in all directions.
•
For curved crack fronts, the element size along the crack front will depend on the amount of local curvature. As a rough guide, you should have at least one element every 15° to 30° along a circular crack front.
•
All element edges should be straight, including the edge on the crack front.
12.2.2. Calculating Fracture Parameters Once the static analysis is completed, you can use POST1, the general postprocessor, to calculate fracture parameters. As mentioned earlier, typical fracture parameters of interest are stress intensity factors, the J-integral, and the energy release rate.
12.2.2.1. Stress Intensity Factors The POST1 KCALC command (Main Menu> General Postproc> Nodal Calcs> Stress Int Factr) calculates the mixed-mode stress intensity factors KI, KII, and KIII. This command is limited to linear elastic problems with a homogeneous, isotropic material near the crack region. To use KCALC properly, follow these steps in POST1: 1.
Define a local crack-tip or crack-front coordinate system, with X parallel to the crack face (perpendicular to the crack front in 3-D models) and Y perpendicular to the crack face, as shown in the following figure. Note — This coordinate system must be the active model coordinate system [CSYS] and results coordinate system [RSYS] when KCALC is issued. Command(s): LOCAL (or CLOCAL, CS, CSKP, etc.) GUI: Utility Menu> WorkPlane> Local Coordinate Systems> Create Local CS> At Specified Loc
Figure 12.5 Crack Coordinate Systems
(a) 2-D Models and (b) 3-D Models 2.
Define a path along the crack face. The first node on the path should be the crack-tip node. For a halfcrack model, two additional nodes are required, both along the crack face. For a full-crack model, where
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
12–5
Chapter 12: Fracture Mechanics both crack faces are included, four additional nodes are required: two along one crack face and two along the other. The following figure illustrates the two cases for a 2-D model. Command(s): PATH, PPATH GUI: Main Menu> General Postproc> Path Operations> Define Path
Figure 12.6 Typical Path Definitions
(a) a half-crack model and (b) a full-crack model 3.
Calculate KI, KII, and KIII. The KPLAN field on the KCALC command specifies whether the model is planestrain or plane stress. Except for the analysis of thin plates, the asymptotic or near-crack-tip behavior of stress is usually thought to be that of plane strain. The KCSYM field specifies whether the model is a halfcrack model with symmetry boundary conditions, a half-crack model with antisymmetry boundary conditions, or a full-crack model. Command(s): KCALC GUI: Main Menu> General Postproc> Nodal Calcs> Stress Int Factr
12.2.2.2. J-Integral In its simplest form, the J-integral can be defined as a path-independent line integral that measures the strength of the singular stresses and strains near a crack tip. The following equation shows an expression for J in its 2-D form is shown below. It assumes that the crack lies in the global Cartesian X-Y plane, with X parallel to the crack (see Figure 12.7: “J-Integral Contour Path Surrounding a Crack-Tip”).
∂uy ∂u J = ∫r Wdy − ∫r t x x + t y ds ∂ y ∂ x where: γ = any path surrounding the crack tip W = strain energy density (that is, strain energy per unit volume) tx = traction vector along x axis = σxnx + σxy ny ty = traction vector along y axis = σyny + σxy nx σ = component stress n = unit outer normal vector to path γ u = displacement vector s = distance along the path γ
12–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 12.2: Solving Fracture Mechanics Problems
Figure 12.7 J-Integral Contour Path Surrounding a Crack-Tip
Follow these steps to calculate J for a 2-D model: 1.
Read in the desired set of results. Command(s): SET GUI: Main Menu> General Postproc> Read Results> First Set
2.
Store the volume and strain energy per element. Command(s): ETABLE GUI: Main Menu> General Postproc> Element Table> Define Table
3.
Calculate the strain energy density per element. Command(s): SEXP GUI: Main Menu> General Postproc> Element Table> Exponentiate
4.
Define a path for the line integral. Figure 12.8: “Examples of Paths for J-integral Calculation” shows examples of such paths. Command(s): PATH, PPATH GUI: Main Menu> General Postproc> Path Operations> Define Path
Figure 12.8 Examples of Paths for J-integral Calculation
5.
Map the strain energy density, which was stored in the element table in step 1, onto the path. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
12–7
Chapter 12: Fracture Mechanics Command(s): PDEF GUI: Main Menu> General Postproc> Path Operations> Map Onto Path 6.
Integrate it with respect to global Y. Command(s): PCALC GUI: Main Menu> General Postproc> Path Operations> Integrate
7.
Assign the final value of the integral to a parameter. This gives us the first term of equation 10.1. Command(s): *GET,Name,PATH,,LAST GUI: Utility Menu> Parameters> Get Scalar Data
8.
Map the component stresses SX, SY, and SXY onto the path. Command(s): PDEF GUI: Main Menu> General Postproc> Path Operations> Map Onto Path
9.
Define the path unit normal vector. Command(s): PVECT GUI: Main Menu> General Postproc> Path Operations> Unit Vector
10. Calculate TX and TY using the expressions shown with equation 10.1. Command(s): PCALC GUI: Main Menu> General Postproc> Path Operations> operation 11. Shift the path a small distance in the positive and negative X directions to calculate the derivatives of the displacement vector (δux/δx and δuy/δy). The following steps are involved (see Figure 19.13: “The Three Basic Modes of Fracture” in the ANSYS, Inc. Theory Reference): •
Calculate the distance by which the path is to be shifted, say DX. A rule of thumb is to use one percent of the total length of the path. You can obtain the total path length as a parameter using *GET,Name,PATH,,LAST,S.
•
Shift the path a distance of DX/2 in the negative X direction [PCALC,ADD,XG,XG,,,,-DX/2] and map the displacements UX and UY onto the path [PDEF], giving them labels UX1 and UY1, for example.
•
Shift the path a distance of DX in the positive X direction (that is, +DX/2 from its original position) and map UX and UY onto the path, giving them labels UX2 and UY2, for example.
•
Shift the path back to its original location (a distance of -DX/2) and calculate the quantities (UX2UX1)/DX and (UY2-UY1)/DX using PCALC. These quantities represent δux/δx and δuy/δy, respectively.
See the ANSYS Coupled-Field Analysis Guide for a discussion of the *GET, PCALC and PDEF commands. 12. Using the quantities calculated in steps 10 and 11, calculate the integrand in the second term of J [PCALC] and integrate it with respect to the path distance S [PCALC]. This gives the second term of equation 10.1. 13. Calculate J according to equation 10.1, using the quantities calculated in steps 5-7 and 12. You can simplify the J-integral calculations by writing a macro that performs the above operations. (Macros are described in the ANSYS APDL Programmer's Guide.)
12.2.2.3. Energy Release Rate Energy release rate is a concept used to determine the amount of work (change of energy) associated with a crack opening or closure. One method to calculate the energy release rate is the virtual crack extension method, outlined below. In the virtual crack extension method, you perform two analyses, one with crack length a and the other with crack length a +∆a. If the potential energy U (strain energy) for both cases is stored, the energy release rate can be calculated from 12–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 12.2: Solving Fracture Mechanics Problems U − Ua G = − a +∆a B∆a where B is the thickness of the fracture model. Extend the crack length by ∆a for the second analysis by selecting all nodes in the vicinity of the crack and scaling them in the X direction [NSCALE] (Main Menu> Preprocessor> Modeling> Operate> Scale) by the factor ∆a. Note — If you used solid modeling, you will first need to detach the solid model from the finite element model [MODMSH,DETACH] (Main Menu> Preprocessor> Checking Ctrls) before scaling the nodes. The "vicinity of the crack" is usually taken to mean all nodes within a radius of a/2 from the crack tip. Also, the factor ∆a for node scaling is usually in the range of 1/2 to 2 percent of the crack length.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
12–9
12–10
Chapter 13: Composites 13.1. Definition of Composites Composite materials have been used in structures for a long time. In recent times composite parts have been used extensively in aircraft structures, automobiles, sporting goods, and many consumer products. Composite materials are those containing more than one bonded material, each with different structural properties. The main advantage of composite materials is the potential for a high ratio of stiffness to weight. Composites used for typical engineering applications are advanced fiber or laminated composites, such as fiberglass, glass epoxy, graphite epoxy, and boron epoxy. ANSYS allows you to model composite materials with specialized elements called layered elements. Once you build your model using these elements, you can do any structural analysis (including nonlinearities such as large deflection and stress stiffening).
13.2. Modeling Composites Composites are somewhat more difficult to model than an isotropic material such as iron or steel. You need to take special care in defining the properties and orientations of the various layers since each layer may have different orthotropic material properties. In this section, we will concentrate on the following aspects of building a composite model: •
Choosing the proper element type
•
Defining the layered configuration
•
Specifying failure criteria
•
Following modeling and postprocessing guidelines
13.2.1. Choosing the Proper Element Type The following element types are available to model layered composite materials: SHELL99, SHELL91, SHELL181, SOLID46, and SOLID191. Which element you choose depends on the application, the type of results that need to be calculated, and so on. Check the individual element descriptions to determine if a specific element can be used in your ANSYS product. All layered elements allow failure criterion calculations. SHELL99 - Linear Layered Structural Shell Element SHELL99 is an 8-node, 3-D shell element with six degrees of freedom at each node. It is designed to model thin to moderately thick plate and shell structures with a side-to-thickness ratio of roughly 10 or greater. For structures with smaller ratios, you may consider using SOLID46. The SHELL99 element allows a total of 250 uniform-thickness layers. Alternately, the element allows 125 layers with thicknesses that may vary bilinearly over the area of the layer. If more than 250 layers are required, you can input your own material matrix. It also has an option to offset the nodes to the top or bottom surface. SHELL91 - Nonlinear Layered Structural Shell Element SHELL91 is similar to SHELL99 except that it allows only up to 100 layers and does not allow you to input a material property matrix. However, SHELL91 supports plasticity, large-strain behavior and a special sandwich option, whereas SHELL99 does not. SHELL91 is also more robust for large deflection behavior. SHELL181 - Finite Strain Shell Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 13: Composites SHELL181 is a 4-node 3-D shell element with 6 degrees of freedom at each node. The element has full nonlinear capabilities including large strain and allows 255 layers. The layer information is input using the section commands rather than real constants. Failure criteria is available using the FC commands. SOLID46 - 3-D Layered Structural Solid Element SOLID46 is a layered version of the 8-node, 3-D solid element, SOLID45, with three degrees of freedom per node (UX, UY, UZ). It is designed to model thick layered shells or layered solids and allows up to 250 uniform-thickness layers per element. Alternately, the element allows 125 layers with thicknesses that may vary bilinearly over the area of the layer. An advantage with this element type is that you can stack several elements to model more than 250 layers to allow through-the-thickness deformation slope discontinuities. The user-input constitutive matrix option is also available. SOLID46 adjusts the material properties in the transverse direction permitting constant stresses in the transverse direction. In comparison to the 8-node shells, SOLID46 is a lower order element and finer meshes may be required for shell applications to provide the same accuracy as SHELL91 or SHELL99 . SOLID191 - Layered Structural Solid Element SOLID191 is a layered version of the 20-node 3-D solid element SOLID95, with three degrees of freedom per node (UX, UY, UZ). It is designed to model thick layered shells or layered solids and allows up to 100 layers per element. As with SOLID46, SOLID191 can be stacked to model through-the-thickness discontinuities. SOLID191 has an option to adjust the material properties in the transverse direction permitting constant stresses in the transverse direction. In spite of its name, the element does not support nonlinear materials or large deflections. In addition to the layered elements mentioned above, other composite element capabilities exist in ANSYS, but will not be considered further in the chapter: •
SOLID95, the 20-node structural solid element, with KEYOPT(1) = 1 functions similarly to a single layered SOLID191 including the use of an orientation angle and failure criterion. It allows nonlinear materials and large deflections.
•
SHELL63, the 4-node shell element, can be used for rough, approximate studies of sandwich shell models. A typical application would be a polymer between two metal plates, where the bending stiffness of the polymer would be small relative to the bending stiffness of the metal plates. The bending stiffness can be adjusted by the real constant RMI to represent the bending stiffness due to the metal plates, and distances from the middle surface to extreme fibers (real constants CTOP, CBOT) can be used to obtain output stress estimates on the outer surfaces of the sandwich shell. It is not used as frequently as SHELL91, SHELL99, or SHELL181, and will not be considered for anything other than sandwich structures in this section.
•
SOLID65, the 3–D Reinforced Concrete Solid Element, models an isotropic medium with optional reinforcing in 3 different user-defined orientations.
•
BEAM188 and BEAM189, the 3–D finite strain beam elements, can have their sections built up with multiple materials.
13.2.2. Defining the Layered Configuration The most important characteristic of a composite material is its layered configuration. Each layer may be made of a different orthotropic material and may have its principal directions oriented differently. For laminated composites, the fiber directions determine layer orientation. Two methods are available to define the layered configuration: •
13–2
By specifying individual layer properties
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 13.2: Modeling Composites •
By defining constitutive matrices that relate generalized forces and moments to generalized strains and curvatures (available only for SOLID46 and SHELL99 )
13.2.2.1. Specifying Individual Layer Properties With this method, the layer configuration is defined layer-by-layer from bottom to top. The bottom layer is designated as layer 1, and additional layers are stacked from bottom to top in the positive Z (normal) direction of the element coordinate system. You need to define only half of the layers if stacking symmetry exists. At times, a physical layer will extend over only part of the model. In order to model continuous layers, these dropped layers may be modeled with zero thickness. Figure 13.1: “Layered Model Showing Dropped Layer” shows a model with four layers, the second of which is dropped over part of the model.
Figure 13.1 Layered Model Showing Dropped Layer
For each layer, the following properties are specified in the element real constant table [R, RMORE, RMODIF] (Main Menu> Preprocessor> Real Constants) (accessed with REAL attributes). •
Material properties (via a material reference number MAT)
•
Layer orientation angle commands (THETA)
•
Layer thickness (TK)
Layered sections may also be defined through the Section Tool (Prep>Sections>Shell — Add/edit). For each layer, the following are specified in the section definition through the section commands; or through the Section Tool (SECTYPE, SECDATA) (accessed with the SECNUM attributes). •
Material properties (via a material reference number MAT)
•
Layer orientation angle commands (THETA)
•
Layer thickness (TK)
•
Number of integration points per layer (NUMPT)
Material Properties - As with any other element, the MP command (Main Menu> Preprocessor> Material Props> Material Models> Structural> Linear> Elastic> Isotropic or Orthotropic) is used to define the linear material properties, and the TB command is used to define the nonlinear material data tables (plasticity is only available for elements SOLID191 and SHELL91). The only difference is that the material attribute number for each layer of an element is specified in the element's real constant table. For the layered elements, the MAT command (Main Menu> Preprocessor> Meshing> Mesh Attributes> Default Attribs) attribute is only used for the DAMP and REFT arguments of the MP command. The linear material properties for each layer may be either isotropic or orthotropic (see Linear Material Properties in the ANSYS Elements Reference). Typical fiber-reinforced composites contain orthotropic materials and these properties are most often supplied in the major Poisson's ratio form (see the ANSYS, Inc. Theory Reference). Material property directions are parallel to the layer coordinate system, which is defined by the element coordinate system and the layer orientation angle (described below). Layer Orientation Angle- This defines the orientation of the layer coordinate system with respect to the element coordinate system. It is the angle (in degrees) between X-axes of the two systems. By default, the layer coordinate system is parallel to the element coordinate system. All elements have a default coordinate system which you Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
13–3
Chapter 13: Composites can change using the ESYS element attribute [ESYS] (Main Menu> Preprocessor> Meshing> Mesh Attributes> Default Attribs). You may also write your own subroutines to define the element and layer coordinate systems (USERAN and USANLY); see the Guide to ANSYS User Programmable Features for details. Layer Thickness- If the layer thickness is constant, you only need to specify TK(I), the thickness at node I. Otherwise, the thicknesses at the four corner nodes must be input. Dropped layers may be represented with zero thickness. Number of integration points per layer- This allows you to determine in how much detail the program should compute the results. For very thin layers, when used with many other layers, one point would be appropriate. But for laminates with few layers, more would be needed. The default is 3 points. This feature applies only to sections defined through the section commands. Note — Currently, the GUI only allows layer real constant input of up to 100 layers. If more layers are needed for SHELL99 or SOLID46, the R and RMORE commands must be used.
13.2.2.2. Defining the Constitutive Matrices This is an alternative to specifying the individual layer properties and is available as an option [KEYOPT(2)] for SOLID46 and SHELL99. The matrices, which represent the force-moment and strain-curvature relationships for the element, must be calculated outside the ANSYS program as outlined in the ANSYS, Inc. Theory Reference. They can be included as part of the solution printout with KEYOPT(10). The main advantages of the matrix approach are: •
It allows you to incorporate an aggregate composite material behavior.
•
A thermal load vector may be supplied.
•
The matrices may represent an unlimited number of layers.
The terms of the matrices are defined as real constants. Mass effects are incorporated by specifying an average density (real constants AVDENS) for the element. If the matrix approach is used, detailed results in each layer cannot be obtained since individual layer information is not input.
13.2.2.3. Sandwich and Multiple-Layered Structures Sandwich structures have two thin faceplates and a thick, but relatively weak, core. Figure 13.2: “Sandwich Construction” illustrates sandwich construction.
Figure 13.2 Sandwich Construction
You can model sandwich structures with SHELL63, SHELL91, or SHELL181. SHELL63 has one layer but permits sandwich modeling through the use of real constants. You can modify the effective bending moment of inertia and the distance from the middle surface to the extreme fibers to account for the weak core. KEYOPT(9) = 1 of SHELL91 specifies the sandwich option. The core is assumed to carry all of the transverse shear; the faceplates carry none. Conversely, the faceplates are assumed to carry all (or almost all) of the bending load. Only SHELL91 has this sandwich option.
13–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 13.2: Modeling Composites SHELL181 models the transverse shear deflection using as energy equivalence method that makes the need for a sandwich option unnecessary
13.2.2.4. Node Offset For SHELL181 using sections defined through the section commands, nodes can be offset during the definition of the section, using the SECOFFSET command. For SHELL91, and SHELL99 the node offset option (KEYOPT(11)) locates the element nodes at the bottom, middle or top surface of the shell. The figures below illustrate how you can conveniently model ply drop off in shell elements that are adjacent to each other. In Figure 13.3: “Layered Shell With Nodes at Midplane”, the nodes are located at the middle surfaces (KEYOPT(11) = 0) and these surfaces are aligned. In Figure 13.4: “Layered Shell With Nodes at Bottom Surface”, the nodes are located at the bottom surfaces (KEYOPT(11) = 1) and these surfaces are aligned.
Figure 13.3 Layered Shell With Nodes at Midplane
Figure 13.4 Layered Shell With Nodes at Bottom Surface
13.2.3. Specifying Failure Criteria Failure criteria are used to learn if a layer has failed due to the applied loads. You can choose from three predefined failure criteria or specify up to six failure criteria of your own (user-written criteria). The three predefined criteria are: •
Maximum Strain Failure Criterion, which allows nine failure strains.
•
Maximum Stress Failure Criterion, which allows nine failure stresses.
•
Tsai-Wu Failure Criterion, which allows nine failure stresses and three additional coupling coefficients. You have a choice of two methods of calculating this criterion. The methods are defined in the ANSYS, Inc. Theory Reference.
The failure strains, stresses, and coupling coefficients may be temperature-dependent. See the ANSYS Elements Reference for details about the data required for each criterion. To specify a failure criterion, use either the family of TB commands or the family of FC commands. The TB commands areTB, TBTEMP, and TBDATA. (Main Menu> Preprocessor> Material Props> Failure Criteria). A typical sequence of commands to specify a failure criterion using these commands is shown below. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
13–5
Chapter 13: Composites TB,FAIL,1,2 ! Data table for failure criterion, material 1, ! no. of temperatures = 2 TBTEMP,,CRIT ! Failure criterion key TBDATA,2,1 ! Maximum Stress Failure Criterion (Const. 2 = 1) TBTEMP,100 ! Temperature for subsequent failure properties TBDATA,10,1500,,400,,10000 ! X, Y, and Z failure tensile stresses (Z value ! set to a large number) TBDATA,16,200,10000,10000 ! XY, YZ, and XZ failure shear stresses TBLIST TBTEMP,200 ! Second temperature TBDATA,...
The FC commands are FC, FCDELE, and FCLIST commands (Main Menu> Preprocessor> Material Props> Material Models> Structural> Nonlinear> Inelastic> Non-Metal Plasticity> Failure Criteria) and (Main Menu> General Postproc> Failure Criteria). A typical sequence of commands to specify a failure criterion using these commands is shown below. FC,1,TEMP,, 100, FC,1,S,XTEN, 1500, FC,1,S,YTEN, 400, FC,1,S,ZTEN,10000, FC,1,S,XY , 200, FC,1,S,YZ ,10000, FC,1,S,XZ ,10000, FCLIST, ,100 FCLIST, ,150 FCLIST, ,200 PRNSOL,S,FAIL
200 1200 500 8000 200 8000 8000
! Temperatures ! Maximum stress components
! ! ! !
List status List status List status Use Failure
of Failure Criteria at 100.0 degrees of Failure Criteria at 150.0 degrees of Failure Criteria at 200.0 degrees Criteria
Note — The TB commands (TB, TBTEMP, and TBDATA) can be used only for SHELL91, SHELL99, SOLID46, or SOLID191, but the FC and FCLIST commands can be used for any 2-D or 3-D structural solid element or any 3-D structural shell element. See the ANSYS Commands Reference for a discussion of the TB, TBTEMP, TBDATA, TBLIST, FC, FCDELE, and FCLIST commands. Some notes about specifying failure criteria: •
The criteria are orthotropic, so you must input the failure stress or failure strain values for all directions. (The exception is that compressive values default to tensile values.)
•
If you don't want the failure stress or strain to be checked in a particular direction, specify a large number in that direction (as shown in the previous example).
User-written failure criteria may be specified via user subroutines USRFC1 through USRFC6. These subroutines should be linked with the ANSYS program beforehand; see the ANSYS Advanced Analysis Techniques Guide for a brief description of user-programmable features.
13.2.4. Additional Modeling and Postprocessing Guidelines Some additional guidelines for modeling and postprocessing of composite elements are presented below. 1.
Composites exhibit several types of coupling effects, such as coupling between bending and twisting, coupling between extension and bending, etc. This is due to stacking of layers of differing material properties. As a result, if the layer stacking sequence is not symmetric, you may not be able to use model symmetry even if the geometry and loading are symmetric, because the displacements and stresses may not be symmetric.
2.
Interlaminar shear stresses are usually important at the free edges of a model. For relatively accurate interlaminar shear stresses at these locations, the element size at the boundaries of the model should be approximately equal to the total laminate thickness. For shells, increasing the number of layers per actual
13–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 13.2: Modeling Composites material layer does not necessarily improve the accuracy of interlaminar shear stresses. With elements SOLID46, SOLID95, and SOLID191, however, stacking elements in the thickness direction should result in more accurate interlaminar stresses through the thickness. Interlaminar transverse shear stresses in shell elements are based on the assumption that no shear is carried at the top and bottom surfaces of the element. These interlaminar shear stresses are only computed in the interior and are not valid along the shell element boundaries. Use of shell-to-solid submodeling is recommended to accurately compute all of the free edge interlaminar stresses. 3.
Because a large amount of input data is required for composites, you should verify the data before proceeding with the solution. Several commands are available for this purpose: •
ELIST (Utility Menu> List> Elements) lists the nodes and attributes of all selected elements.
•
EPLOT (Utility Menu> Plot> Elements) displays all selected elements. Using the /ESHAPE,1 command (Utility Menu> PlotCtrls> Style> Size and Shape) before EPLOT causes shell elements to be displayed as solids with the layer thicknesses obtained from real constants or section definition (see Figure 13.5: “Example of an Element Display”. This example uses element SHELL99 with /ESHAPE turned on). It also causes SOLID46 elements to be displayed with layers.
•
/PSYMB,LAYR,n (Utility Menu> PlotCrls> Symbols) followed by EPLOT displays layer number n for all selected layered elements. This can be used to display and verify each individual layer across the entire model.
•
/PSYMB,ESYS,1 followed by EPLOT displays the element coordinate system triad for those elements whose default coordinate system has been changed.
Figure 13.5 Example of an Element Display
•
LAYLIST (Utility Menu> List> Elements> Layered Elements) lists the layer stacking sequence from real constants and any two material properties for SHELL99, SHELL91, SOLID46, and SOLID191 elements. You can specify a range of layer numbers for the listing. LIST LAYERS 1 TO 4 IN REAL SET TOTAL LAYERS = 4 LSYM = 1 LP1 =
1 FOR ELEMENT TYPE 1 0 LP2 = 0 EFS = .000E+00
NO. ANGLE THICKNESS MAT --- ----- ---------- --1 45.0 0.250 1 2 -45.0 0.250 2 3 -45.0 0.250 2 4 45.0 0.250 1 -----------------------SUM OF THK 1.00
•
LAYPLOT (Utility Menu> Plot> Layered Elements) displays the layer stacking sequence from real constants in the form of a sheared deck of cards (see Figure 13.6: “Sample LAYPLOT Display for [45/Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
13–7
Chapter 13: Composites 45/ - 45/45] Sequence”). The layers are crosshatched and color coded for clarity. The hatch lines indicate the layer angle (real constant THETA) and the color indicates layer material number (MAT). You can specify a range of layer numbers for the display. •
4.
SECPLOT (Main Menu> Preprocessor> Sections> Shell> Plot Section) displays the section stacking sequence from sections in the form of a sheared deck of cards (see Figure 13.6: “Sample LAYPLOT Display for [45/-45/ - 45/45] Sequence”). The sections are crosshatched and color coded for clarity. The hatch lines indicate the layer angle (THETA) and the color indicates layer material number (MAT) defined by the SECDATA command. You can specify a range of layer numbers for the display.
By default, only data for the bottom of the first (bottom) layer, top of the last (top) layer, and the layer with the maximum failure criterion value are written to the results file. If you are interested in data for all layers, set KEYOPT(8) = 1. Be aware, though, that this may result in a large results file.
Figure 13.6 Sample LAYPLOT Display for [45/-45/ - 45/45] Sequence
5.
Use the ESEL,S,LAYER command to select elements that have a certain layer number. If an element has a zero thickness for the requested layer, the element is not selected. Note — For energy output, the results are applicable only to the entire element; you cannot get output results for individual layers.
6.
13–8
Use the LAYER command (Main Menu> General Postproc> Options for Outp) in POST1 (or LAYERP26 (Main Menu> TimeHist Postpro> Define Variables) in POST26) to specify the layer number for which results are to be processed. The SHELL command (Main Menu> General Postproc> Options for Outp or Main Menu> TimeHist Prostpro> Define Variables) specifies a TOP, MID, or BOT location within the layer. The default in POST1 is to store results for the bottom of the bottom layer, and the top of the top layer, and the layer with the maximum failure criterion value. In POST26, the default is layer 1. If KEYOPT(8) = 1 (that is, data stored for all layers), the LAYER and LAYERP26 commands store the TOP and BOT results for the specified layer number. MID values are then calculated by average TOP and BOT values. If KEYOPT (8) = 2 is set for SHELL181 during SOLUTION, then LAYER and LAYERP26 commands store the TOP,
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 13.2: Modeling Composites BOTTOM, and MID results for the specified layer number. In this case, MID values are directly retrieved from the results file. For transverse shear stresses with KEYOPT(8) = 0, therefore, POST1 can only show a linear variation, whereas the element solution printout or KEYOPT(8) = 2 can show a parabolic variation. 7.
By default, POST1 displays all results in the global Cartesian coordinate system. Use the RSYS command (Main Menu> General Postproc> Options for Outp) to transform the results to a different coordinate system. In particular, RSYS,SOLU allows you to display results in the layer coordinate system if LAYER is issued with a nonzero layer number.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
13–9
13–10
Chapter 14: Fatigue 14.1. Definition of Fatigue Fatigue is the phenomenon in which a repetitively loaded structure fractures at a load level less than its ultimate static strength. For instance, a steel bar might successfully resist a single static application of a 300 kN tensile load, but might fail after 1,000,000 repetitions of a 200 kN load. The main factors that contribute to fatigue failures include: •
Number of load cycles experienced
•
Range of stress experienced in each load cycle
•
Mean stress experienced in each load cycle
•
Presence of local stress concentrations
A formal fatigue evaluation accounts for each of these factors as it calculates how "used up" a certain component will become during its anticipated life cycle.
14.1.1. What the ANSYS Program Does The ANSYS fatigue calculations rely on the ASME Boiler and Pressure Vessel Code, Section III (and Section VIII, Division 2) for guidelines on range counting, simplified elastic-plastic adaptations, and cumulative fatigue summation by Miner's rule. For fatigue evaluations based on criteria other than those of the ASME Code, you can either write your own macro, or else interface your ANSYS results with an appropriate third-party program (see the ANSYS APDL Programmer's Guide for more information on these two features). The ANSYS program features the following fatigue-calculation capabilities: •
You can postprocess existing stress results to determine the fatigue usage factors for any solid-element or shell-element model. (You can also manually input stresses for fatigue evaluation of line-element models.)
•
You can store stresses at a preselected number of locations for a preselected number of events and loadings within the event.
•
You can define stress concentration factors for each location and scale factors for each event.
14.1.2. Basic Terminology A location is a node in your model for which fatigue stresses are to be stored. You would typically choose locations that represent points on the structure that would be susceptible to fatigue damage. An event is a set of stress conditions that occur at different times during a unique stress cycle. See Section 14.2.3.4: Guidelines for Obtaining Accurate Usage Factors later in this chapter for more information. A loading is one of the stress conditions that is part of an event. The alternating stress intensity is a measure of the difference in stress state between any two loadings. The program does not adjust the alternating stress intensity for mean-stress effects.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 14: Fatigue
14.2. Doing a Fatigue Evaluation You do a fatigue evaluation in POST1, the general postprocessor, after you have completed a stress solution. The procedure normally consists of five main steps: 1.
Enter POST1 and resume your database.
2.
Establish the size (the number of locations, events, and loadings), define the fatigue material properties, identify stress locations, and define stress concentration factors.
3.
Store stresses at locations of interest for various events and loadings; assign event repetitions and scale factors.
4.
Activate the fatigue calculations.
5.
Review the results.
14.2.1. Enter POST1 and Resume Your Database In order to perform a fatigue evaluation, you need to follow these steps: 1.
Enter POST1. Command(s): /POST1 GUI: Main Menu> General Postproc
2.
Read your database file (Jobname.DB) into active memory. (If your intended fatigue evaluation is a continuation of an ongoing ANSYS session, then Jobname.DB will already be in memory.) A results file (Jobname.RST) with nodal stress results should also be available; you will read results data into memory later. Command(s): RESUME GUI: Utility Menu> File> Resume from
14.2.2. Establish the Size, Fatigue Material Properties, and Locations Define the following data: •
Maximum number of locations, events, and loadings
•
Fatigue material properties
•
Stress locations and stress concentration factors (SCFs)
1.
Define the maximum number of stress locations, events, and loadings. By default, your fatigue evaluation can consider up to five nodal locations, ten events, and three loadings within an event. You can use the following option to establish larger dimensions (that is, allow more locations, events, or loadings), if necessary. Command(s): FTSIZE GUI: Main Menu> General Postproc> Fatigue> Size Settings
2.
Define material fatigue properties. In order to calculate usage factors, and to include the effect of simplified elastic-plastic computations, you must define material fatigue properties. The material properties of interest in a fatigue evaluation are: •
14–2
The S-N curve, a curve of alternating stress intensity ((Smax - Smin)/2) versus allowable number of cycles. The ASME S-N curves already account for maximum mean stress effects. You should adjust your S-N Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 14.2: Doing a Fatigue Evaluation curve to account for mean-stress effects, if necessary. If you do not input an S-N curve, alternating stress intensities will be listed in decreasing order for all possible combinations of stress conditions, but no usage factors will be calculated. Command(s): FP GUI: Main Menu> General Postproc> Fatigue> Property Table> S-N Table •
The Sm-T curve, a curve of design stress-intensity value versus temperature. This curve is needed if you want the program to detect whether or not the nominal stress range has gone plastic. Command(s): FP GUI: Main Menu> General Postproc> Fatigue> Property Table> Sm_T Table
•
Elastic-plastic material parameters M and N (strain hardening exponents). These parameters are required only if you desire simplified elastic-plastic code calculations. These parameters' values can be obtained from the ASME Code. Command(s): FP GUI: Main Menu> General Postproc> Fatigue> Property Table> Elas-plas Par The following example illustrates the use of the FP command to input material fatigue properties: ! Define the S-N table: FP,1,10,30,100,300,1000,10000 FP,7,100000,1000000 FP,21,650,390,240,161,109,59 FP,27,37,26 ! Define the Sm-T table: FP,41,100,200,300,400,500,600 FP,47,650,700,750,800 FP,51,20,20,20,18.7,17.4,16.4 FP,57,16.1,15.9.15.5,15.1
! Allowable Cycles, N ! " ! Alternating Stress! Intensity Range, S, ksi
! Temperature,°F ! " ! "Design Stress-Intensity ! Value", Sm (=2/3*Sy or ! 1/3 *Su), ksi ! Define the elastic-plastic material parameters: FP,61,1.7,.3 ! M and N
3.
Define stress locations and stress concentration factors. The following option allows you to explicitly define a nodal location of interest to your fatigue evaluation, define stress concentration factors (SCFs) for that location, and assign a short (20 character) title to that location. Command(s): FL GUI: Main Menu> General Postproc> Fatigue> Stress Locations
Note — Not all fatigue analyses will require the FL command. Locations are automatically defined for nodes when FS, FSNODE, or FSSECT are issued (see below). If your model contains sufficient grid detail, your stresses could be accurate enough that you would not need to apply calculated SCFs. (Supplemental SCFs for surface, size, or corrosion effects might still be required, however.) Where only one location is being examined, you could omit a title. If explicit definition of locations, SCFs, or titles are not required, you could forgo the FL command entirely. Here is an example of some FL commands for a cylinder with a global Y axis, having two wall thicknesses of interest, where SCFs are to be applied (to the axial linearized stresses) at the outside wall. FL,1,281,,,,Line 1 at inside FL,2,285,,1.85,,Line 1 at outside FL,3,311,,,,Line 2 at inside FL,4,315,,2.11,,Line 2 at outside
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
14–3
Chapter 14: Fatigue
Figure 14.1 Cylinder Wall with Stress Concentration Factors (SCFs)
14.2.3. Store Stresses and Assign Event Repetitions and Scale Factors 14.2.3.1. Storing Stresses In order to perform a fatigue evaluation, the program must know the stresses at different events and loadings for each location, as well as the number of repetitions of each event. You can store stresses for each combination of location, event, and loading, using the following options: •
Manually stored stresses
•
Nodal stresses from Jobname.RST
•
Stresses at a cross-section Caution: The program never assumes that a "zero" stress condition exists. If zero stress is one of the conditions to be considered, it must be explicitly input for each event in which it may occur.
The following command sequences schematically illustrate how to store stresses. In some situations, you might prefer to use LCASE instead of SET. Manually stored stresses:
FS
Nodal stresses retrieved from Jobname.RST:
SET, FSNODE
Stresses at a cross-section:
PATH, PPATH, SET, FSSECT
(Cross-section calculations also require data from Jobname.RST.)
You can use more than one method of storing stresses in an event. Each of these methods is explained in detail below.
14.2.3.1.1. Manually Stored Stresses You can use this option to store stresses and the temperature "manually" (without direct access to the results file Jobname.RST). In such cases, you are not using the fatigue module in POST1 as a postprocessor, but simply as a fatigue calculator. Line elements, such as beams, must be handled in this way since the fatigue module is not able to access data from a results file other than for solid elements or shell elements. Command(s): FS GUI: Main Menu> General Postproc> Fatigue> Store Stresses> Specified Val Command input for this option is demonstrated by the following example: FS,201,1,2,1,-2.0,21.6,15.2,4.5,0.0,0.0 FS,201,1,2,7,450.3
14–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 14.2: Doing a Fatigue Evaluation In this example, only the total stresses (items 1-6) and the temperature (item 7) are input. If the linearized stresses were also to be input, they would follow the temperatures as items 8 through 13. Note — In the special case of a beam element having only axial stress, you would input only one stress component (SX), leaving the rest of the stress fields blank.
14.2.3.1.2. Nodal Stresses from Jobname.RST When you use this option, you cause a nodal stress vector containing six stress components to be stored directly from the results database. Stress components stored with this option can be modified with a subsequent FS command. Note — You must issue a SET command, and possibly a SHELL command, before executing FSNODE. SET will read results for a particular load substep from the results file (Jobname.RST) into the database. SHELL allows you to select results from the top, middle, or bottom surfaces for shell elements (default is the top surface). Command(s): FSNODE GUI: Main Menu> General Postproc> Fatigue> Store Stresses> From rst File Input by means of FSNODE is demonstrated by the following example for an event at one nodal location: SET,1 FSNODE,123,1,1 SET,2 FSNODE,123,1,2 SET,3 FSNODE,123,1,3
! ! ! ! ! ! !
Define data set for load step 1 Stress vector at node 123 assigned to event 1, loading 1. Define data set for load step 2 ...event 1, loading 2 ...load step 3 ...event 1, loading 3
Figure 14.2 Three Loadings in One Event
14.2.3.1.3. Stresses at a Cross-Section This option calculates and stores total linearized stresses at the ends of a section path (as defined by a preceding PATH and PPATH command). Because you will normally want the linearization to take place over a thickness representing the shortest distance between the two surfaces, use only the two surface nodes to describe the path in the PPATH command. This option retrieves stress information from the results database; therefore
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
14–5
Chapter 14: Fatigue FSSECT must also be preceded by a SET command. Stress components stored with an FSSECT command can be modified with a subsequent FS command. Command(s): FSSECT GUI: Main Menu> General Postproc> Fatigue> Store Stresses> At Cross Sect Input by means of FSSECT is demonstrated in the following example. If node locations are not assigned with an FL command, the FSSECT commands in this example will automatically assign location numbers to the two path nodes, 391 and 395. (See Figure 14.3: “Surface Nodes are Identified by PPATH Prior to Executing FSSECT”.) PATH,Name,2 PPATH,1,391 PPATH,2,395 SET,1 FSSECT,,1,1
! Define the path using the two surface nodes
! Store stresses at nodes 391 and 395
Figure 14.3 Surface Nodes are Identified by PPATH Prior to Executing FSSECT
14.2.3.2. Listing, Plotting, or Deleting Stored Stresses Use the following options to list, plot, or delete stored stresses. •
List the stored stresses per location, per event, per loading, or per stress condition: Command(s): FSLIST GUI: Main Menu> General Postproc> Fatigue> Store Stresses> List Stresses
•
Display a stress item as a function of loading number for a particular location and event: Command(s): FSPLOT GUI: Main Menu> General Postproc> Fatigue> Store Stresses> Plot Stresses
•
Delete a stress condition stored for a particular location, event, and loading: Command(s): FSDELE GUI: Main Menu> General Postproc> Fatigue> Store Stresses> Dele Stresses
•
Delete all stresses at a particular location: Command(s): FL GUI: Main Menu> General Postproc> Fatigue> Stress Locations
•
Delete all stresses for all loadings in a particular event: Command(s): FE GUI: Main Menu> General Postproc> Fatigue> Erase Event Data
14.2.3.3. Assigning Event Repetitions and Scale Factors This option assigns the number of occurrences to the event numbers (for all loadings at all locations of the event). It can also be used to apply scale factors to all of the stresses that make up its loadings. Command(s): FE GUI: Main Menu> General Postproc> Fatigue> Assign Events
14–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 14.2: Doing a Fatigue Evaluation An example of this command usage is given below: FE,1,-1 FE,2,100,1.2 *REPEAT,3,1 FE,5,500
! Erase all parameters and fatigue stresses formerly ! used for event 1. ! Assign 100 occurrences to events 2, 3 and 4, ! and scale by 1.2. ! Assign 500 occurrences to event 5.
14.2.3.4. Guidelines for Obtaining Accurate Usage Factors Structures are usually subjected to a variety of maximum and minimum stresses, which occur in unknown (or even random) order. Therefore, you must take care to achieve an accurate count of the number of repetitions of all possible stress ranges, in order to obtain a valid fatigue usage factor. The ANSYS program automatically calculates all possible stress ranges and keeps track of their number of occurrences, using a technique commonly known as the "rain flow" range-counting method. At a selected nodal location, a search is made throughout all of the events for the pair of loadings (stress vectors) that produces the most severe stress-intensity range. The number of repetitions possible for this range is recorded, and the remaining number of repetitions for the events containing these loadings is decreased accordingly. At least one of the source events will be "used up" at this point; remaining occurrences of stress conditions belonging to that event will subsequently be ignored. This process continues until all ranges and numbers of occurrences have been considered. Caution: It can be surprisingly easy to misuse the range-counting feature of the fatigue module. You must take pains to assemble events carefully if you want your fatigue evaluation to yield accurate usage factors. Consider the following guidelines when assembling events: •
Understand the internal logic of the ANSYS range-counting algorithm. See the ANSYS, Inc. Theory Reference for more details on how the ANSYS program performs range counting.
•
Because it can be difficult to predict the exact load step at which a maximum (or minimum) 3-D stress state occurs, good practice often requires that you include several clustered loadings in each event, in order to successfully capture the extreme stress state. (See Figure 14.2: “Three Loadings in One Event”.)
•
You will obtain consistently conservative results if you include only one extreme stress condition (either a local maximum or a local minimum) in any given event. If you group more than one extreme condition in a single event, you will sometimes generate unconservative results, as illustrated by the following example:
Consider a load history made up of two slightly different cycles: Load Cycle 1: 500 repetitions of Sx = +50.0 to -50.1 ksi Load Cycle 2: 1000 repetitions of Sx = +50.1 to -50.0 ksi These load cycles will obviously sum to 1500 repetitions having an alternating stress intensity of about 50 ksi. However, carelessly grouping these loadings into only two events will result in an inaccurate range count. Let's see how this would happen: Event 1,
loading 1: Sx = 50.0 loading 2: Sx = -50.1
500 repetitions
Event 2,
loading 1: Sx = 50.1 loading 2: Sx = -50.0
1000 repetitions
The possible alternating stress intensities are: a.
From E1,L1 to E1,L2:
50.05 ksi Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
14–7
Chapter 14: Fatigue b.
From E1,L1 to E2,L1:
0.05 ksi
c.
From E1,L1 to E2,L2:
50.00 ksi
d.
From E1,L2 to E2,L1:
50.10 ksi
e.
From E1,L2 to E2,L2:
0.05 ksi
f.
From E2,L1 to E2,L2:
50.05 ksi
Sorting these combinations by decreasing alternating stress intensity gives: d.
From E1,L2 to E2,L1:
50.10 ksi
a.
From E1,L1 to E1,L2:
50.05 ksi
f.
From E2,L1 to E2,L2:
50.05 ksi
c.
From E1,L1 to E2,L2:
50.00 ksi
b.
From E1,L1 to E2,L1:
0.05 ksi
e.
From E1,L2 to E2,L2:
0.05 ksi
The range counting then proceeds as follows: d.
500 cycles of E1,L2 to E2,L1
- this uses up 500 cycles of E1 and E2
a.
0 cycles of E1,L1 to E1,L2
- E1 is all used up
f.
500 cycles of E2,L1 to E2,L2
- this uses up 500 more cycles of E2
c.
0 cycles of E1,L1 to E2,L2
- both events are all used up
b.
0 cycles of E1,L1 to E2,L1
- both events are all used up
e
0 cycles of E1,L2 to E2,L2
- both events are all used up
Thus, only 1000 repetitions of about 50 ksi range would be counted, instead of the known 1500 cycles. This error results solely from improper assembly of events. If the loadings had each been described as separate events (such that E1,L1 ≥ E1; E1,L2 ≥ E2; E2,L1 ≥ E3; and E2,L2 ≥ E4), then the following range counts would be obtained: d.
500 cycles of E2 to E3
- this uses up 500 cycles of E2 and E3
a.
0 cycles of E1 to E2
- E2 is all used up
f.
500 cycles of E3 to E4
- uses up 500 more cycles of E3, and 500 of E4
c.
500 cycles of E1 to E4
- uses up 500 more cycles of E4
b.
0 cycles of E1 to E3
- E3 is all used up
e.
0 cycles of E2 to E4
- E2 and E4 are both all used up
Cumulative fatigue damage in this case would properly be calculated for 1500 repetitions of about 50 ksi range. •
Conversely, using separate events for each maximum and each minimum stress condition could sometimes become too conservative. In such cases, carefully choose those loadings that should be counted together, and group them into the same events. The following example illustrates how some events can appropriately contain multiple extreme stress conditions:
Consider a load history made up of these two load cycles: •
Load Cycle 1: 500 repetitions of Sx = +100.1 to +100.0 ksi
•
Load Cycle 2: 1000 repetitions of Sx = +50.1 to +50.0 ksi
14–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 14.2: Doing a Fatigue Evaluation It is readily apparent that the worst possible combination of these cycles would yield 500 repetitions having alternating stress intensity of about 25 ksi range. Proceeding as in the above example, grouping these loadings into two events would produce an accurate count of 500 repetitions of about 25 ksi range. Treating each loading as a separate event would yield an over-conservative count of 1000 repetitions of about 25 ksi range.
14.2.4. Activate the Fatigue Calculations Now that you have locations, stresses, events, and material parameters all specified, you can execute the fatigue calculations at a specified location. The location is specified by either the location number or the node itself. Command(s): FTCALC GUI: Main Menu> General Postproc> Fatigue> Calculate Fatig
14.2.5. Review the Results Fatigue calculation results are printed in the output. If you have routed your output [/OUTPUT] to a file (for example Jobname.OUT), then you can review the results by listing that file. Command(s): *LIST GUI: Utility Menu> List> Files> Other> Jobname.OUT If you have input an S-N curve, output is in the form of a table of alternating stress intensities (listed in decreasing order) with corresponding pairs of event/loadings, as well as cycles used, cycles allowed, temperature, and partial usage factor. Following that, the cumulative usage factor is shown for that particular location. This information is repeated for all locations. As has been just mentioned, FTCALC output shows the contributing pairs of events and loadings for any given alternating stress-intensity range. This information can help you isolate the transients (events/loadings) causing the most fatigue damage. A convenient way to modify your events would be to write all stored fatigue data on Jobname.FATG. (This option could be executed either before or after FTCALC.) Data are written to Jobname.FATG in terms of equivalent fatigue module commands. You can modify your events by editing Jobname.FATG; then use the /INPUT command to reread the modified fatigue commands. Command(s): FTWRITE GUI: Main Menu> General Postproc> Fatigue> Write Fatig Data
14.2.6. Other Approaches to Range Counting Earlier, we discussed the "rain flow" range-counting method. This technique is useful whenever the exact timehistory of various loadings is not known. However, if in your fatigue analysis the time-history is known, you can avoid the undue conservatism of this procedure simply by running a separate fatigue analysis [FTCALC] for each sequential event and then adding the usage factors manually.
14.2.7. Sample Input A sample input listing for a fatigue evaluation is shown below: ! Enter POST1 and Resume the Database: /POST1 RESUME,... ! Number of Locations, Events, and Loadings FTSIZE,... ! Material Fatigue Properties: FP,1,.... ! N values
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
14–9
Chapter 14: Fatigue FP,21,... ! S values FP,41,... ! T values FP,51,... ! Sm values FP,61,... ! Elastic-plastic material parameters ! Locations, Stress Concentration Factors, and Location Titles FL,... ! Store Stresses (3 Different Methods) ! Store Stresses Manually: FS,... ! Retrieve Stresses from the Results File: SET,... FSNODE,... ! Store Stresses at a Cross-Section: PPATH,... SET,... FSSECT,... ! Event Repetitions and Scale Factors FE,... ! Activate the Fatigue Calculations FTCALC,... ! Review the Results (List the output file) FINISH
See the ANSYS Commands Reference for a discussion of the FTSIZE, FP, FL, FS, FSNODE, PPATH, FSSECT, FE, and FTCALC commands.
14–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 15: p-Method Structural Static Analysis 15.1. Definition of p-Method Analysis The p-method obtains results such as displacements, stresses, or strains to a user-specified degree of accuracy. To calculate these results, the p-method manipulates the polynomial level (p-level) of the finite element shape functions which are used to approximate the real solution. This feature works by taking a finite element mesh, solving it at a given p-level, increasing the p-level selectively, and then solving the mesh again. After each iteration the results are compared for convergence against a set of convergence criteria. You can specify the convergence criteria to include displacement, rotation, stress or strain at a point (or points) in the model, and global strain energy. The higher the p-level, the better the finite element approximation to the real solution. In order to capitalize on the p-method functionality, you don't have to work only within the confines of p-generated meshes. The p-method is most efficient when meshes are generated considering that p-elements will be used, but this is not a requirement. Of course, you might want to create and mesh your model using p-elements, but you can also perform a p-method solution using meshes that have been generated with h-elements (generated by ANSYS or your CAD package), if the elements are at least mid-noded. This provides you with the flexibility of taking advantage of the p-method solution option independently of how the mesh was created. The p-method can improve the results for any mesh automatically.
15.2. Benefits of Using the p-Method The p-method solution option offers many benefits for linear structural static analyses that are not available with the more traditional h-method, discussed in the preceding chapters. The most convenient benefit is the ability to obtain good results to a desired level of accuracy without rigorous user-defined meshing controls. If you are new to finite element analysis or do not have a solid background in mesh design, you might prefer this method since it relieves you of the task of manually designing an accurate mesh. In addition, the p-method adaptive refinement procedure offers error estimates that are more precise than those of the h-method, and can be calculated locally as well as globally (for example, stress at a point rather than strain energy). For example, if you need to obtain highly accurate solutions at a point, such as for fracture or fatigue assessments, the p-method offers an excellent means of obtaining these results to the required accuracy.
15.3. Using the p-Method The procedure for a p-method static analysis consists of four main steps: 1.
Select the p-method procedure.
2.
Build the model.
3.
Apply loads and obtain the solution.
4.
Review the results.
Each step is discussed in detail in the following sections.
15.3.1. Select the p-Method Procedure You can activate the p-method solution procedure in two ways: through the GUI or by defining a p-element [ET].
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 15: p-Method Structural Static Analysis •
Activating p-method through the GUI: Command(s): /PMETH GUI: Main Menu> Preferences> p-method
•
Defining a p-element: The p-method solution procedure can also be activated by defining a p-element. If you are working outside of the GUI, the definition of a p-element lets the program know that a p-method solution is to be done; no other commands are necessary to initiate p-method. From within the GUI, you can also issue the ET command in the "Input Window" to activate the p-method procedure. (Remember, the ET command must be entered in the "Input Window," since, by default, only h-elements are displayed in the GUI unless p-method is active.) Command(s): ET GUI: Main Menu> Preprocessor> Element Type> Add/Edit/Delete
15.3.2. Build the Model In order to build a model with p-elements, you must follow the procedure listed below. 1.
Define the element types.
2.
Specify material properties and/or real constants.
3.
Define the model geometry.
4.
Mesh the model into solid or shell elements.
The above steps are common to most analyses. The ANSYS Modeling and Meshing Guide explains those steps in detail. In this section we will explain the techniques that are unique to a p-analysis.
15.3.2.1. Define the Element Types You can use the following five p-elements to build your model: •
2-D Quadrilateral (PLANE145)
•
2-D Triangle (PLANE146)
•
3-D Brick (SOLID147)
•
3-D Tetrahedron (SOLID148)
•
3-D Shell (SHELL150) Note — H-elements and p-elements cannot be active at the same time in your model.
15.3.2.1.1. Specifying a p-Level Range Various options are available for use with p-elements. One important option is the ability to specify, either locally or globally, a range in which the p-level may vary. The range within which the p-level may vary can be controlled locally through the p-element KEYOPT settings (KEYOPT(1) and KEYOPT(2)), or globally across the entire model with PPRANGE. By default, the p-level range is 2 to 8. When both KEYOPT values and PPRANGE have been used to specify p-level ranges, the local p-level range [ET] will take precedence over the global p-level range [PPRANGE].
15–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.3: Using the p-Method For example, if you set a global p-level range between 3 and 8 with PPRANGE, then define a local p-level range of 4 to 6 for PLANE145 elements (ET,1,145,4,6), the p-level for the PLANE145 elements may only vary between 4 and 6, while the rest of the model may vary between 3 and 8. At the (default) starting p-level of 2, convergence checking is performed to determine those elements which are converged and may have their p-level fixed at 2. That is, these elements will remain at a p-level of 2, and will be eliminated from any further convergence checking. Additional checking is performed at each iteration to fix the p-levels of the elements which are converged. Note — Convergence checking for SHELL150 begins at a p-level of 3 instead of a p-level of 2. Use local p-range control to eliminate regions of little importance from high p-escalation. Use global p-range control for overall control of the p-level. These range controls are not necessary, but p-escalations to high plevels increase CPU time. Therefore, it is advantageous to have such controls available. •
Defining a local p-level range: Command(s): ET GUI: Main Menu> Preprocessor> Element Type> Add/Edit/Delete
•
Defining a global p-level range: Command(s): PPRANGE GUI: Main Menu> Preprocessor> Loads> Load Step Opts> p-Method> Set p-range
See the ANSYS Elements Reference for complete descriptions of each of the above element types.
15.3.2.2. Specify Material Properties and/or Real Constants 15.3.2.2.1. Material Properties Material properties for p-elements may be either constant or temperature-dependent, and isotropic or orthotropic. As with other structural analyses, if you plan to apply inertia loads (such as gravity or rotational velocity), you must also specify the density (DENS) that is required for mass calculations. Young's modulus (EX) must be defined, and if thermal loads (temperatures) are to be applied, a coefficient of thermal expansion (ALPX) must be specified. Command(s): MP GUI: Main Menu> Preprocessor> Material Props> Material Models> Structural> Density Main Menu> Preprocessor> Material Props> Material Models> Structural> Linear> Elastic> Isotropic Main Menu> Preprocessor> Material Props> Material Models> Structural> Thermal Expansion Coef> Isotropic Caution: Element coordinate systems [ESYS] used for orthotropic material directions are not supported by p-elements. All element coordinate systems are parallel to the global Cartesian coordinate system.
15.3.2.2.2. Real Constants You may define optional thicknesses for 2-D elements and thicknesses for SHELL150 as real constants. Thicknesses must be defined for SHELL150. Command(s): R GUI: Main Menu> Preprocessor> Real Constants
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–3
Chapter 15: p-Method Structural Static Analysis
15.3.2.3. Define the Model Geometry You can create your model using any of the various techniques outlined in the ANSYS Modeling and Meshing Guide, or you can import it from a CAD system using ANSYS Connection product. If you are generating your model from within ANSYS, you can use either solid modeling or direct generation techniques. Note — Using direct generation is not recommended when you plan to create a p-mesh since all p-elements require that midside nodes be included in their geometric definition. In cases where surface curvature is important, it would not only be tedious, but possibly imprecise to manually define each midside node. In addition, the EMID command does not place nodes on a curved line. It is much more convenient to let the program generate the midside nodes using solid modeling. You may not drop any midside nodes from p-elements. If you use direct generation or import your mesh from an outside source, keep the following guidelines in mind: •
A curved element edge should not cover more than a 30° arc.
•
The angles between adjacent edges should be between 10° and 170°. Element shape checking will warn that adjacent edges should be between 30° and 150°, but it is usually acceptable to have angles in the range of 10° to 170° for p-elements.
•
A good rule of thumb is to keep the aspect ratio (ratio of element length to width) less than 20:1.
15.3.2.4. Mesh the Model into Solid or Shell Elements 15.3.2.4.1. Using Program Defaults After you have generated your solid model, you are ready to mesh it with p-elements. The general procedure for meshing your solid model is outlined in Chapter 7, “Generating the Mesh” in the ANSYS Modeling and Meshing Guide. Compared to h-elements, the program will generate a coarser mesh under default settings for p-elements. Normally, you will not need to specify any meshing size controls because the program defaults will give you an adequate mesh. In addition, each element's p-level will be manipulated during solution to obtain accurate and efficient results. For engineering design studies, the accuracy obtained with a relatively coarse, ungraded mesh is usually sufficient. (A graded mesh is one where there are more elements near an area of interest. These elements are smaller relative to the other areas of the model, and a transition region occurs from the large to the smaller elements.) Note — Adaptive meshing is not valid with a p-method analysis.
15.3.2.4.2. Specifying Mesh Controls By default, the DESIZE command controls automatic element sizing. For free meshing, you have the option of using the SmartSize feature [SMRTSIZE] to control element sizing. SmartSizing generally produces a better quality mesh and is recommended for meshing a p-element model. (SmartSizing is not available for mapped meshing.) Command(s): SMRTSIZE GUI: Main Menu> Preprocessor> Meshing> Size Cntrls> SmartSize> Basic or Command(s): DESIZE GUI: Main Menu> Preprocessor> Meshing> Size Cntrls> Manual Size> Global> Other
15–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.3: Using the p-Method Note — Since p-method prefers a coarser mesh, the default element size values for a p-method analysis are different than those used for h-elements. See the SMRTSIZE and DESIZE commands for details. For fracture or fatigue assessments, you may still need to specify meshing controls because the mesh must be fine enough to obtain the desired accuracy near the areas of interest. In certain cases, such as when there are severe geometric transition regions, you may also need to specify mesh controls to avoid a meshing failure. You may also want to specify meshing controls for curved geometries, where successful meshes are more difficult to achieve with the default size settings. Under default conditions, badly shaped elements may be produced because of the difficulty of filling a curved domain with as few elements as possible. User-defined meshing controls can make the task less difficult.
15.3.2.4.3. Guidelines for Creating a Good Mesh •
Subdivide complex geometries, or build them as separate geometries. As a general rule, if you were to stand inside a volume, you should be able to see all of its vertices. If this is not possible, you might wish to consider subdividing the volume into more manageable pieces.
•
The number of divisions on lines "parallel" and near to each other should be fairly equivalent. The SmartSizing method of meshing [SMRTSIZE] handles this situation well. However, if the DESIZE method of element sizing is used, you should set local mesh controls to achieve a good mesh in these areas.
•
For beam-like or shell-like models, use one element through the thickness in the meshed model. SmartSizing will do this automatically. However, if you are using DESIZE for meshing, set the default element size [MINH] to 1 [DESIZE,,1].
Figure 15.1 Fan Model Showing p-Element vs. h-Element Meshes
15.3.3. Additional Information for Building Your Model 15.3.3.1. Viewing your element model A subgrid approach is used for plotting the model in which the amount of displayed element curvature can be controlled. You may display varying degrees of curvature in your model by specifying the number of facets to be used for element display. Facets are piecewise linear approximations of the actual curve represented by the element face or edge. A greater number of facets will result in a smoother representation of the element surface Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–5
Chapter 15: p-Method Structural Static Analysis for p-element plots. PowerGraphics is the default graphics display method used for p-method plots. This method will display the plot at a much faster speed than the Full Model method. See Chapter 10, “PowerGraphics” in the ANSYS Basic Analysis Guide for more information on PowerGraphics. For more information on /EFACET, see the discussion on the p-Element Subgrid later in this section. Command(s): /EFACET GUI: Utility Menu> PlotCtrls> Style> Size and Shape
15.3.3.2. Coupling You may couple degrees of freedom (DOFs) between nodes on p-elements to control nodal solution behavior. All coupled nodes are forced to assume the same displacement values in the specified nodal coordinate direction. The amount of this displacement is unknown until the analysis has been completed. Command(s): CP GUI: Main Menu> Preprocessor> Coupling/Ceqn> Couple DOFs The first degree of freedom defined on the coupled set is the "prime" degree of freedom. All other degrees of freedom in the coupled set are eliminated from the solution matrices as a result of their relationship to the prime degree of freedom. Note — For p-elements, only the corner nodes may be defined as prime degrees of freedom if midside nodes are also part of the same coupled set. For a p-method analysis, only the nodal combinations described below are permitted when coupling, and any deviation from these combinations will most likely result in singularities.
15.3.3.2.1. Coupling of Corner Nodes 1.
Two nodes are coupled within the same element.
Figure 15.2 Coupled Nodes on One Element
2.
Two nodes are coupled between adjacent element edges/faces.
Figure 15.3 Nodes Coupled Between Adjacent Elements
15–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.3: Using the p-Method
15.3.3.2.2. Midside Node Coupling 1.
Both corner nodes on the element's edge or face are part of the same coupled set. Only the corner nodes may be defined as prime degrees of freedom.
Figure 15.4 Both Corner Nodes are Coupled
2.
All nodes in the coupled set are midside nodes. In this case, a midside node must be defined as the prime degree of freedom, but this is only valid as long as there are no corner nodes defined as part of the same coupled set.
Figure 15.5 All Coupled Nodes are Midside Nodes
Note — If you have coupled faces or edges on a p-element (that is, all edges of the element's face or all nodes of the element's edge are coupled), the p-level of that edge or face will be held to 2. In addition, constraint equations (used to represent relatively rigid parts) are not available in a p-method analysis.
15.3.4. Apply Loads and Obtain the Solution In this section you will take the following steps to obtain a solution for your model: 1.
Enter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define the analysis options. Choose any of three options to solve the simultaneous equations generated by a p-method analysis. These solvers are discussed at length in Chapter 3, “Solution” in the ANSYS Basic Analysis Guide. •
Frontal equation solver
•
Jacobian Conjugate Gradient equation solver (JCG)
•
Preconditioned Conjugate Gradient equation solver (PCG) (recommended) Command(s): EQSLV Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–7
Chapter 15: p-Method Structural Static Analysis GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Sol'n Options Tab) Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options We generally recommend that you use the PCG solver for a p-element analysis. For most 3-D solid models and for very large 2-D models (usually greater than 40,000 DOF), the PCG solver is usually faster than the JCG and frontal solvers: •
The PCG solver is about 5 to 10 times faster than the frontal solver for p-elements.
•
The PCG solver is significantly faster than JCG for p-elements.
•
Computer-time savings will be greater with the PCG solver when p-levels of 4 and higher are active.
In certain cases, such as when your model contains elements with high aspect ratios or material type discontinuities, a greater number of iterations may be required to achieve convergence for the PCG solver. You may increase the maximum number of iterations by using the MULT option on the EQSLV command. This option is only valid when solving with the PCG solver. See the EQSLV command description in the ANSYS Commands Reference for more information on this capability. The PCG solver is not available for p-element shells. For more information on the general use of the PCG solver, refer to Chapter 3, “Solution” in the ANSYS Basic Analysis Guide. 3.
Apply the loads to the solid model (keypoints, lines, areas, etc.) or to the finite element model (nodes and elements), except for inertia loads (gravity, rotational velocity, etc.), which are independent of the model. For a general discussion of solid model loads versus finite element loads, see Chapter 2, “Loading” in the ANSYS Basic Analysis Guide. Internal Degrees of Freedom and Nodal Coordinate Systems In order to correctly apply boundary conditions, you need to understand nodal coordinate systems, and how degrees of freedom (DOFs) which are not attached to a node are handled. DOFs are the allowed motions or deformations of the elements. Those DOFs which are not attached to a node are referred to as internal degrees of freedom. •
Internal DOFs allow the elements to form a better approximation to the real solution. As the p-level is increased for each loop, more DOFs are added to the elements. Some of these DOFs act on the element boundary (edges and interior faces) resulting in deformations that vary from a polynomial order of 2 to 8. In many cases, the higher the p-level, the more complex the deformation, and the better the approximation to the real solution.
•
Nodal coordinate systems orient the degree of freedom directions at each node. Each node has its own nodal coordinate system, which, by default, is parallel to the global Cartesian system (regardless of the coordinate system in which the node was defined). Nodes may be rotated into a nodal coordinate system [NROTAT] (Main Menu> Preprocessor> Modeling> Move/Modify> Rotate Node CS> To Active CS). The constraints and forces are then applied to the nodes in the nodal coordinate systems. See the ANSYS Modeling and Meshing Guide for more details about nodal coordinate systems.
The program aligns the internal DOFs with the nodal coordinate systems as defined by the nodes on the element face or edge. Displacement constraints applied to nodes with rotated nodal coordinate systems are applied to the internal DOFs on an element edge or face only if ALL the nodes defining that edge or face are also rotated into that same coordinate system (see Figure 15.6: “Constraints on Rotated Nodes”). Therefore any symmetry/antisymmetry displacement boundary conditions applied to the nodes on adjoining surfaces 15–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.3: Using the p-Method should reference the same coordinate system. If you apply the symmetry/antisymmetry displacement boundary conditions to areas or lines, you should verify that the constraints all "point" in the same direction on each surface. If they do not, apply the boundary conditions to the individual nodes. Caution: If all of the DOFs of the nodes on an edge (or face) are not fully constrained (are only partially constrained, e.g. only UX is constrained) and the nodal rotations of these nodes are not the same, the stress results at these nodes may be inaccurate if the p-level of the attached elements exceeds 3. Nodal coordinate systems which are not necessarily parallel to the global Cartesian system are formed when you invoke symmetry or antisymmetry displacement constraints on model surfaces.
Figure 15.6 Constraints on Rotated Nodes
Loads Applicable to a p-Method Analysis Table 2.5: “Loads Applicable in a Static Analysis” of this manual describes the loads applicable to a static analysis. The following is a brief discussion of each type of loading. Displacements (UX, UY, UZ, ROTX, ROTY, ROTZ) are DOF constraints usually specified at model boundaries to define rigid support points. They are also used to indicate symmetry boundary conditions and points of known motion. The directions implied by the labels are in the nodal coordinate system. Displacement boundary conditions that are applied to all nodes on an element edge or face will also constrain the higher-order deformations along that edge or face. Conversely, if all of the nodes are not constrained in that direction, then those lower-order deformations will be constrained but not the higher-order ones. Never apply a displacement only at a midside node on an edge. (You may, however, apply a single constraint at a corner node.) Imposed motions may only vary linearly over an element edge or face. The program will ignore an imposed quadratic variation. Forces (FX, FY, FZ) are concentrated loads usually specified on the model exterior. The directions implied by the labels are in the nodal coordinate system. Moments (MX, MY, MZ) are concentrated loads usually specified on the model exterior. The directions implied by the labels are in the nodal coordinate system.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–9
Chapter 15: p-Method Structural Static Analysis Caution: Observe the following cautions: •
You should avoid applying single-point loads or constraints, since they cause stress singularities. If these loads or constraints are applied, exclude the elements attached to these nodes from the convergence computations. See the "Accounting for Stress Singularities" section later in this chapter.
•
Do not apply forces and moments to the midside nodes. You may only apply these loads at the corner nodes. In addition, out-of-plane (element ROTZ) moments may not be applied to SHELL150.
Pressures (PRES) are surface loads, also usually applied on the model exterior. Positive values of pressure act towards the element face (resulting in a compressive effect). Temperatures (TEMP) are applied to study the effects of thermal expansion or contraction (that is, thermal stresses). The coefficient of thermal expansion must be defined if thermal strains are to be calculated. You can read in temperatures from a thermal analysis, or you can specify temperatures directly on the nodes or the solid model keypoints. To obtain temperatures from a thermal analysis: •
Mesh the p-element model.
•
Convert the p-element types to the following thermal element types: PLANE145 to PLANE77, PLANE146 to PLANE35, SOLID147 to SOLID90, and SOLID148 to SOLID87. There is no thermal equivalent for SHELL150.
•
Run the thermal analysis.
•
Change the element types back to the p-element types in order to perform the p-method structural analysis.
•
For the remainder of the analysis, continue with the same procedure as defined for h-elements (see the ANSYS Thermal Analysis Guide).
Gravity, spinning, etc. are inertia loads that affect the entire structure. Density must be defined if inertia effects are to be included. 4.
Specify load step options. The following solution options are available to aid in solving a p-Method analysis: •
Convergence criteria specifications
•
Specifications for controlling p-levels
•
Accounting for stress singularities
As mentioned earlier in this section, a p-method analysis works with a series of iterations, or loops, checking for convergence each time. The PPRANGE command is used to specify the overall range where the p-level may vary (somewhere between 2 and 8). For analyses beginning at p=2, each element will have its solution checked for convergence against established criteria [PCONV]. If the solution is within the requested tolerance [PMOPTS], that element will have its p-level held to 2. Those elements that did not converge within the specified criteria (that is, not fixed at p=2 for the first iteration), will have their p-level increased, and another solution (iteration) will then be performed. At each iteration the convergence criteria (strain energy, displacement, stress, etc.) is checked, and if converged, the solution stops. Also, those elements whose individual solutions are considered to be converged will have their p-level held at the current p-level. This process is continued until all specified convergence criteria are met, or the maximum p-range has been reached. 15–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.3: Using the p-Method Convergence Criteria Specifications Convergence criteria may be global (for strain energy) or local. If you are specifically interested in the results at certain points in the model, then you should use local convergence criteria. Use this option to specify which areas of your model you would like to monitor for analysis convergence, as well as the type of criteria you would like to use to control convergence. Typically, you should select a few points of interest (nodes), at which to specify the convergence criteria (deflection, stress, strain, etc.). In most cases, the default convergence tolerance (5%) is sufficient for generally good results. You may want to lower this tolerance if you require a more accurate solution, such as for a fatigue evaluation. For a design study or optimization analysis, a higher tolerance will cut down on run times. Command(s): PCONV GUI: Main Menu> Preprocessor> Loads> Load Step Opts> p-Method> Convergence Crit For SHELL150, you also have the option to choose a layer (TOP, MID, or BOT) for stress or strain convergence criteria. If you are working with intersecting shells, it is recommended that you choose MID as the layer for convergence checking. Caution: Do not specify stress or strain criteria at nodes where there are singularities or at nodes along material interfaces. These locations will not converge due to the singularity. When choosing locations for specifying convergence criteria, you should concentrate your monitoring in the areas of high stress or at the point of maximum displacement rather than where stresses, strains, or displacements are relatively insignificant. Specifications for Controlling p-levels You may specify the starting (defaults to 2) and maximum (defaults to 8) p-levels that you wish to allow for your analysis [PPRANGE]. You may wish to start at a higher p-level if you have already completed an analysis and you want to perform a re-analysis (for a design change, for instance) and you know the final p-level where convergence will occur for most elements. You may also want to restrict the maximum plevel to less than 8 if conserving disk space or run time. Adjust the starting and maximum p-level in portions of your model using element KEYOPT selections. Accounting for Stress Singularities If the model contains any re-entrant (internal or concave) corners that are not modeled with a fillet radius, or contains point loads or any other areas of stress singularities, you should consider excluding these areas from the convergence computations. All elements that have a node at the singularity should be excluded. One exception applies to fracture mechanics. In that situation, you should not exclude elements at or near the crack tip. Command(s): PEXCLUDE GUI: Main Menu> Solution> Load Step Opts> p-Method> Strain Energy> Exclude Elems You can reassign, or re-include, elements for convergence checking. You may determine which elements have been included or excluded by listing [PINCLUDE,STAT; PEXCLUDE,STAT; or *GET] or plotting elements [EPLOT]. Excluded elements will appear `whited-out' in the plot. You may also select included or excluded elements by issuing the ESEL command directly [ESEL,,PEXC or ESEL,,PINC] (no GUI equivalent). This facilitates using these elements as a component [CM]. Command(s): PINCLUDE GUI: Main Menu> Solution> Load Step Opts> p-Method> Strain Energy> Include Elems 5.
Save a backup copy of the database. Command(s): SAVE Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–11
Chapter 15: p-Method Structural Static Analysis GUI: Utility Menu> File> Save As 6.
Start the p-level iterations and solution process. The output will provide a summary of each loop, indicating the current p-level, the convergence statistics, and the status of how many elements have converged. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
15.3.5. Helpful Hints for Common Problems If the analysis is not successful, try the following steps to identify and correct the cause for failure: Problem: "Negative Pivot" error encountered. Possible Cause: Insufficient constraints to prevent rigid-body motion (the component can slide or rotate in one direction because there are no constraints to prevent it from doing so). Solution: Add enough displacement constraints to prevent any rigid-body motion. Problem: Solution does not converge to within the requested tolerance. Possible Causes: There are several possible causes. You may use the general postprocessor [/POST1] to look at this solution in order to determine the difficulty. Possible Causes The convergence criteria is too tight for the maximum allowable plevel and the mesh.
Solution Relax the convergence criteria.
The convergence criterion was specified at a singularity (infinite stress Do not monitor a singularity point. or strain value, such as under a point load) or the elements near the singularity were not excluded. The mesh is too coarse, especially in the area where the stress is high. Refine the mesh. The maximum p-level was restricted lower than that required for convergence.
Allow the maximum p-level to go higher.
The convergence criterion is at a location where the angle made by Refine the mesh in that region. adjacent element edges is greater than 55° on a curved boundary.
Caution: You may not restart a p-method analysis.
15.3.6. Review the Results The fundamental procedures for general postprocessing of results [/POST1] in the ANSYS program are discussed in Chapter 4, “An Overview of Postprocessing” in the ANSYS Basic Analysis Guide. Although most of these capabilities are directly applicable to p-method analyses, some techniques for reviewing results are unique to pmethod, such as •
The p-Element Subgrid
•
Querying Subgrid Results
•
Printing and Plotting Node and Element Results
•
Specialized p-Method Displays and Listings
The results from a p-method analysis are written to the results file, Jobname.RST. They consist of the following data:
15–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.3: Using the p-Method Primary data Nodal displacements (UX, UY, ROTX, etc.) Derived data Nodal and element stresses, nodal and element strains, element forces Note — You must read the results data from the results file (Jobname.RST) into the database [SET] before displacements may be reviewed during postprocessing. Thermal strains are not available on the results file. The tools used for time-history postprocessing [/POST26] are also applicable to p-method analyses, but have limited functionality, since p-element technology is restricted to linear static analyses. In this section we will explain those procedures that deviate from standard postprocessing, such as some plotting and printing operations, etc. Before reading this section, it would be a good idea to review the chapters on postprocessing in the ANSYS Basic Analysis Guide for more details on postprocessing, in general.
15.3.6.1. The p-Element Subgrid As mentioned previously, p-method finite element models generally contain fewer elements than do models meshed with h-elements. Since fewer elements correspond to a coarser mesh, a subgrid approach has been devised for viewing results in POST1. In this approach, each element is divided into smaller, "h-like" elements. Both the display of geometric curvature and the display and printout of field quantities (displacements, stresses, etc.) are affected by this approach. In most cases, a greater number of facets will result in a smoother representation of the element surface and results contours for p-element plots. The key command involved in the subgrid approach is /EFACET,NUM where NUM represents the number of facets per element edge (GUI path Utility Menu> PlotCtrls> Style> Size and Shape). The example below illustrates how /EFACET subdivides a quadrilateral element. If NUM = 2, the element has 2 facets per edge and is divided into 4 subgrid facets by adding a pseudo node at the "center". If NUM = 4, the element has 4 facets per edge which means two pseudo nodes per edge and 9 interior pseudo nodes are added for each p-element, dividing the quadrilateral into 16 subgrid facets.
Figure 15.7 p-Element Subgrids for Quadrilateral Elements
As a general rule, for a model with a very coarse mesh or any model in which the p-levels are high (p>3) you should consider using NUM = 4 to view your field quantities. Since results are available at each subgrid location, more information will be available at NUM = 4.
15.3.7. Querying Subgrid Results You have the ability to directly and interactively query subgrid results. You can obtain all subgrid point results (or element results). Command(s): No command equivalent. GUI: Main Menu> General Postproc> Query Results Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–13
Chapter 15: p-Method Structural Static Analysis You may query stresses, strains, and displacements at all subgrid locations that have previously been activated by the /EFACET command.
15.3.8. Printing and Plotting Node and Element Results For elements PLANE145, PLANE146, SOLID147, and SOLID148, displacements, stresses, and strains can be listed [PRNSOL] at all node locations (both corner and midside nodes). For SHELL150, results can be listed (as controlled by the SHELL command) and plotted at the top/bottom and middle layer locations. Likewise, these nodal values can be contoured for display purposes [PLNSOL], with the contour resolutions being controlled by the/EFACET command. Note — Results values for SHELL150 are displayed for the top and bottom layer simultaneously. When viewing nodal field values across p-element boundaries ([PRNSOL, PLNSOL], or when using the Query function), results may be displayed in various ways. The results data may be averaged along element boundaries with the AVRES command. You can average results at all boundaries (the default), or at all boundaries except where real constant, and/or material type discontinuities exist. If a geometric discontinuity exists, results will not be averaged at those locations. Note — AVRES has no effect on the nodal degree of freedom solution values (UX, UY, UZ, ROTX, ROTY, ROTZ, etc.). For all of the p-elements, displacement plots are available with both undisplaced structure and undisplaced edge options [PLDISP]. When using PowerGraphics [/GRAPHICS,POWER], displaced shape plots reflect each calculated element subgrid [/EFACET] displacement. For PLANE145, PLANE146, SOLID147, and SOLID148, stresses and strains can be listed [PRESOL] at all node locations for each element. Results for SHELL150 are listed for the top, middle, and bottom layers with results for the bottom layer listed first. Printout is similar to that for h-elements, with nodal results being unaveraged and sorted by element number. Unlike higher order h-element printout, results are for all nodal locations (corner and midside nodes). Results may be printed or plotted for the entire model [/GRAPHICS,FULL] or for the model surface only [/GRAPHICS,POWER]. Note — Issuing the /PMETH,ON command or defining a p-element [ET] will activate PowerGraphics unless a prior /GRAPHICS,FULL command has been issued. Similarly, /PMETH,OFF will deactivate PowerGraphics unless /GRAPHICS,POWER has been issued previously.
15.3.8.1. Specialized p-Method Displays and Listings There are three commands specifically designed for listing or plotting p-element results data [PRCONV, PLCONV, PPLOT]. You may print [PRCONV] or plot [PLCONV] the previously-specified convergence values [PCONV] versus characteristic p-levels. The characteristic p-level refers to the p-level range from the minimum specified [PPRANGE] to the maximum p-level reached during SOLUTION. Final p-levels that were assigned to individual elements can be viewed by means of the PPLOT command. A convenient way to visualize local convergence criteria at specified locations in the model is to display a symbol at the location of interest, [/PSYMB,PCON], then issue an element or node plot.
15.4. Sample p-Method Analysis (GUI Method) Follow the steps below to perform a p-method analysis using the GUI.
15–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.4: Sample p-Method Analysis (GUI Method)
15.4.1. Problem Description In this sample problem, you will perform a p-method analysis on a steel plate with a hole.
15.4.2. Problem Specifications For this problem, you will use symmetry boundary conditions to constrain the left side and bottom of the model. This problem uses element type PLANE145. The material is 1/4" thick steel. Loading for this problem is: P = (100) (10) (.25) = 250 lbs (total force applied on the right side).
15.4.3. Problem Diagram Figure 15.8 Steel Plate With a Hole
15.4.3.1. Set the Analysis Title After you enter the ANSYS program, follow these steps to set the title. 1.
Choose menu path Utility Menu> File> Change Title.
2.
Type the text "p-Method Plate with Hole" and click on OK.
15.4.3.2. Select p-Method 1.
Choose menu path Main Menu> Preferences. The Preferences for GUI Filtering dialog box appears.
2.
Click the Structural method on. Click the p-Method Struct. option on.
3.
Click on OK.
15.4.3.3. Define the Element Type and Options 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
Click on OK to accept the default of "2D Quad 145."
4.
Click on Options. The PLANE145 element type options dialog box appears. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–15
Chapter 15: p-Method Structural Static Analysis 5.
In the scroll box for Analysis type, scroll down to "Plane Stress+TK" to select it.
6.
Click on OK.
7.
Click on Close in the Element Types dialog box.
15.4.3.4. Define the Real Constants 1.
Choose menu path Main Menu> Preprocessor> Real Constants> Add/Edit/Delete.
2.
Click on Add. The Element Type for Real Constants dialog box appears.
3.
Click on OK. The Real Constants for PLANE145 dialog box appears.
4.
Enter .25 for thickness and click on OK.
5.
Click on Close to close the Real Constants dialog box.
15.4.3.5. Define Material Properties 1.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
2.
In the Material Models Available window, double-click on the icons next to the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
3.
Enter 30e6 for EX (Young's modulus).
4.
Enter 0.29 for PRXY and click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
5.
Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
15.4.3.6. Create Plate with Hole 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Areas> Rectangle> By Dimensions. The Create Rectangle by Dimensions dialog box appears.
2.
Enter 0,20 for the X-coordinates and 0,10 for the Y-coordinates. Use the TAB key to move between fields.
3.
Click on OK. The rectangle appears in the ANSYS Graphics window.
4.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Areas> Circle> By Dimensions. The Circular Area by Dimensions dialog box appears.
5.
Enter 5 for outer radius.
6.
Click on OK. The circle appears on the ANSYS Graphics window, on the lower left corner of the rectangle.
7.
Choose menu path Main Menu> Preprocessor> Modeling> Operate> Booleans> Subtract> Areas. The Subtract Areas picking menu appears.
8.
Click once on the rectangle to select it.
9.
Click on OK in the picking menu. Another Subtract Areas picking menu appears.
10. Click once on the circle to select it. 11. Click on OK in the picking menu. A semicircle is removed from the lower left-hand corner of the plate.
15.4.3.7. Mesh the Areas 1.
Choose menu path Main Menu> Preprocessor> Meshing> MeshTool. The MeshTool appears.
2.
Click the SmartSize check box on. Set the SmartSize slider to 5.
15–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.4: Sample p-Method Analysis (GUI Method) 3.
In the Mesh section of the MeshTool, choose Areas and Free. Then click the MESH button. The Mesh Areas picking menu appears.
4.
Click on Pick All. A mesh for the plate is created.
5.
Click Close to close the MeshTool.
6.
Click on SAVE_DB on the ANSYS Toolbar.
15.4.3.8. Define Symmetry Boundary Conditions 1.
Choose menu path Utility Menu> Select> Entities.
2.
In the top two menus, pick "Nodes" and "By Location."
3.
Enter 0 for Min, Max and click on OK.
4.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> Symmetry B.C.> On Nodes. The Apply SYMM on Nodes dialog box appears.
5.
Click on OK to accept the default of symmetric surface normal to X-axis. The displacement symbols appear down the left edge of the drawing.
6.
Choose menu path Utility Menu> Select> Entities.
7.
Click the "Y coordinates" option on. Click OK.
8.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> Symmetry B.C.> On Nodes. The Apply SYMM on Nodes dialog box appears.
9.
In the drop down menu for Symm surface is normal to, select "Y-axis."
10. Click OK. The displacement symbols appear along the bottom of the drawing.
15.4.3.9. Define Pressure Load along Right Edge. 1.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears.
2.
Click the "X coordinates" option on.
3.
Enter 20 for Min, Max and click on OK.
4.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Pressure> On Nodes. The Apply PRES on Nodes picking menu appears.
5.
Click on Pick All. The Apply PRES on Nodes dialog box appears.
6.
Enter 100 for pressure value and click on OK.
7.
Choose menu path Utility Menu> Select> Everything.
15.4.3.10. Define Convergence Criteria 1.
Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.
2.
In the Selection field, enter NCVG = NODE(0,5,0) and click on Accept.
3.
Click on Close.
4.
In the ANSYS Input window, enter PCONV,1,S,X,NCVG and press ENTER.
15.4.3.11. Solve the Problem 1.
Choose menu path Main Menu> Solution> Solve> Current LS. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–17
Chapter 15: p-Method Structural Static Analysis 2.
Carefully review the information in the status window, and then close it.
3.
Click on OK in the Solve Current Load Step dialog box to begin the solution.
4.
Click on Close when the Solution is done window appears.
15.4.3.12. Review the Results and Exit ANSYS In this step, you will review results as deformed shape and SX contour plot. 1.
Choose menu path Main Menu> General Postproc> Read Results> First Set.
2.
Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears.
3.
Click the "Def + undeformed" option on. Click on OK. The deformed and undeformed shapes appear in the ANSYS Graphics window.
4.
Choose menu path Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu. The Contour Nodal Solution Data dialog box appears.
5.
In the scroll box on the left, click once on "Stress" to select it. In the scroll box on the right, click once on "X-direction SX" to select it.
6.
Click on OK. Review the graphic using the legend in the graphics window. Expected results are: Max displacement = .97x10-4 in, and Max stress in X direction = 437 psi.
7.
Click on QUIT on the ANSYS Toolbar.
8.
Choose a save option and click on OK.
15.5. Sample p-Method Analysis (Command or Batch Method) You can perform the example p-method analysis of a plate with a hole using the ANSYS commands shown below instead of GUI choices. All items prefaced by an exclamation point (!) are comments. /TITLE, p-method plate with hole problem /PREP7 ET,1,PLANE145,,,3 R,1,.25 MP,EX,1,30e6 MP,PRXY,1,0.29 RECTNG,0,20,0,10 PCIRC,5,,0,360 ASBA,1,2 SMRTSIZ,5 AMESH,3 SAVE FINISH /SOLU NSEL,S,LOC,X,0 DSYM,SYMM,X NSEL,S,LOC,Y,0 DSYM,SYMM,Y NSEL,S,LOC,X,20 SF,ALL,PRES,-100 ALLSEL NCVG=NODE(0,5,0) PCONV,1,S,X,NCVG SOLVE /POST1 SET,1 PLNSOL,S,X PLDISP,1 FINISH
15–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 16: Beam Analysis and Cross Sections 16.1. An Overview of Beams Beam elements are used to create a mathematical one-dimensional idealization of a 3-D structure. They offer computationally efficient solutions when compared to solid and shell elements. The discussion in this chapter applies only to BEAM44, which is a 3-D tapered unsymmetric beam; and BEAM188 and BEAM189, which are 3-D finite strain beams. These beams provide more robust nonlinear analysis capabilities, and significant improvements in cross section data definition, analysis, and visualization, as compared to other ANSYS beams. See the descriptions of the BEAM44, BEAM188, and BEAM189 elements in the ANSYS Elements Reference for more information. Note — If you are using the cross section capabilities described in this chapter with BEAM44 elements, be aware that you cannot use these capabilities to define tapered sections. In addition, the postprocessing visualization capabilities described in this chapter are not applicable to BEAM44 elements. Note — Custom cross sections may not be used with the CDWRITE command.
16.2. What Are Cross Sections? A cross section defines the geometry of the beam in a plane perpendicular to the beam axial direction. ANSYS supplies a library of eleven commonly-used beam cross section shapes, and permits user-defined cross section shapes. When a cross section is defined, ANSYS builds a numeric model using a nine node cell for determining the properties (Iyy, Izz, etc.) of the section and for the solution to the Poisson's equation for torsional behavior. Figure 16.1: “Plot of a Z Cross Section” shows the centroid and shear center of the cross section and the calculated section properties:
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 16: Beam Analysis and Cross Sections
Figure 16.1 Plot of a Z Cross Section
Cross sections and user section meshes may be saved and stored in cross section library files. You may assign beam cross sections as attributes of a line using the LATT command. These section definitions will be incorporated into the generated beam elements when the line is meshed with BEAM44, BEAM188, or BEAM189.
16.3. How to Create Cross Sections The general procedure for creating cross sections consists of the following steps: 1.
Define the section and associate a section ID number with the section subtype.
2.
Define the geometry data for the section.
ANSYS supplies the following commands for creating, viewing, and listing cross sections, and for managing cross section libraries:
Table 16.1 ANSYS Cross Section Commands Command
GUI Menu Path
Purpose
PRSSOL
Main Menu> General Postproc> List Results> Section Solution Utility Menu> List> Results> Section Solution
Prints beam section results (not supported for BEAM44)
SECTYPE
Main Menu> Preprocessor> Sections> Beam> Common Sectns Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Read Sect Mesh
Associates section Subtype with
16–2
SECID
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.3: How to Create Cross Sections Command
GUI Menu Path
Purpose
SECDATA
Main Menu> Preprocessor> Sections> Beam> Common Sectns
Defines section geometry data
SECOFFSET
Main Menu> Preprocessor> Sections> Beam> Common Sectns Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Read Sect Mesh
Defines section offset for beam cross sections
SECCONTROLS
Main Menu> Preprocessor> Sections> Beam> Sect Control
Overrides program calculated properties.
SECNUM
Main Menu> Preprocessor> Meshing> Mesh At- Identifies the SECID to be assigned to an element tributes> Default Attribs Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes
SECPLOT
Main Menu> Preprocessor> Sections> Beam> Plot Section
Plots geometry of a beam section to scale
SECWRITE
Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Write From Areas
Creates an ASCII file containing user mesh or a custom cross section
/SECLIB
Main Menu> Preprocessor> Sections> Section Library> Library Path
Sets default section library path for SECREAD
SECREAD
Main Menu> Preprocessor> Sections> Section Library> Import Library Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Read Sect Mesh
Reads a user defined section library, mesh, or custom cross section
SLIST
Main Menu> Preprocessor> Sections> List Sec- Summarizes section properties tions Utility Menu> List> Properties> Section Properties Utility Menu> List> Properties> Specified Section Properties
SDELETE
Main Menu> Preprocessor> Sections> Delete Section
Deletes a cross section
For complete documentation of the cross section commands, see the ANSYS Commands Reference.
16.3.1. Defining a Section and Associating a Section ID Number Use the SECTYPE command to define a section and associate it with a section ID number. For example, the following command assigns a section identification number (2) to a predefined cross section shape (circular solid): Command(s): SECTYPE, 2, BEAM, CSOLID GUI: Main Menu> Preprocessor> Sections> Beam> Common Sectns To define your own cross sections, use the subtype MESH. To define a cross section with integrated properties such as Iyy and Izz, use the subtype ASEC.
16.3.2. Defining Cross Section Geometry and Setting the Section Attribute Pointer Use the SECDATA command to define the geometry of a cross section. Continuing with the example SECTYPE command shown above, note that the CSOLID subtype has two dimensions: the radius and the number of cells along its circumference. Thus, the SECDATA command shown below specifies 5 as the radius of the circular Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–3
Chapter 16: Beam Analysis and Cross Sections solid beam, and 8 as the number of cells along its circumference. The SECNUM command sets the element section attribute pointer to 2. Command(s): SECDATA, 5, 8 and SECNUM, 2 GUI: Main Menu> Preprocessor> Sections> Beam> Common Sectns Main Menu> Preprocessor> Meshing> Mesh> Attributes> Default Attribs
16.3.2.1. Determining the Number of Cells to Define In general, you do not need to set the number of cells when building a cross section. ANSYS will calculate values for the cross section such as the area of the section and the moments of inertia about the coordinate axes using default integration rules and will produce results that are numerically exact. Since the torsion constant is derived from the mesh, the accuracy of the torsion constant is directly proportional to the mesh size of the cross section. The default mesh used by ANSYS yields acceptable engineering accuracy. There are two ways to specify the mesh size for common sections: •
invoking SECTYPE,,,,,REFINEKEY to set the level of mesh refinement for thin-walled sections (CTUBE, CHAN, I, Z, L, T, HATS, and HREC)
•
specifying the number of divisions using SECDATA for solid sections (RECT, QUAD, and CSOLID)
The thin wall sections have a minimum of two integration points through thickness, so results produced using thin wall sections should be acceptable for materially nonlinear analysis. However, when doing a plasticity analysis, the cell defaults may need to be changed for the solid sections. Here are examples of ANSYS-generated solid section cell meshes and the type of analysis you may wish to use them with.
Figure 16.2 Types of Solid Section Cell Mesh
16.3.3. Meshing a Line Model with BEAM44, BEAM188, or BEAM189 Elements Before you mesh a line with BEAM44, BEAM188, or BEAM189 elements, some of its attributes must be defined. These attributes include: •
The material set attribute pointer to be associated with the generated beam elements.
•
The beam element type to be used in meshing the line.
•
The orientation of the cross section with respect to the beam element axis. For detailed information about orientation nodes and beams, see Section 7.5.2: Generating a Beam Mesh With Orientation Nodes in the ANSYS Modeling and Meshing Guide.
16–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.4: Creating Cross Sections •
The cross section ID to be assigned to the generated beam elements.
Issue the LATT command to associate these attributes with the selected, unmeshed line: Command(s): LATT, MAT, , TYPE, , KB, KE, SECNUM GUI: Main Menu> Preprocessor> Meshing> Mesh Attributes> Picked Lines See the LATT command description for the meaning of MAT and TYPE. The following arguments are described here in terms of their applicability to beams. KB
Corresponds to any keypoint number in the model. All beam elements generated will have their beam section oriented such that the beam z-axis will lie in the plane defined by two line end keypoints and this keypoint number. KE
Corresponds to any keypoint number in the model (optional). This keypoint determines the beam orientation at the end of the line as described above. If KE is given, KB determines the beam orientation at the beginning of the line. This is useful for creating twisted beams. SECNUM
Corresponds to the beam section defined by the SECTYPE command with the section ID number as given by the SECNUM.
16.4. Creating Cross Sections There are two main types of beam cross sections: •
common sections
•
custom sections
Common sections are described by a standard geometry and a single material. Custom sections are defined by an arbitrary geometry and may consist of several isotropic materials. In addition, you can use defined sections to create tapered beams (for BEAM188 and BEAM189 only). See Section 16.4.5: Defining a Tapered Beam for more information.
16.4.1. Using the Beam Tool to Create Common Cross Sections The SECTYPE, SECDATA, and SECOFFSET commands (Main Menu> Preprocessor> Sections> Beam> Common Sectns) are all associated with the BeamTool in the GUI. The appearance of the BeamTool varies depending on the cross section subtype you select:
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–5
Chapter 16: Beam Analysis and Cross Sections
Figure 16.3 BeamTool with Subtypes Drop Down List Displayed
The top part of the BeamTool relates a section ID number to a subtype (and, optionally, a section name) [SECTYPE]. The middle of the BeamTool defines the section offset information, if needed [SECOFFSET]. The bottom contains the fields for section geometry information [SECDATA]. The dimensions defined by the SECDATA command are determined by the subtype selected. For documentation about a particular variant of the BeamTool, select the subtype that you want information about, and then click on the Help button on the BeamTool. The subtype dimensions are also documented in the SECDATA command description.
16.4.2. Creating Custom Cross Sections with a User-defined Mesh If you need to define a cross section that is not common, you must create a user mesh file. To create a user mesh file, create a 2-D solid model and save it using the SECWRITE command (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Write From Areas). This procedure is outlined in greater detail below: 1.
Create all areas (Main Menu> Preprocessor> Modeling> Create> Areas).
2.
Overlap the areas (Main Menu> Preprocessor> Modeling> Operate> Booleans> Overlap> Areas) or glue them (Main Menu> Preprocessor> Modeling> Operate> Booleans> Glue> Areas) where appropriate.
3.
Save the model.
16–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.4: Creating Cross Sections 4.
Set the number of line divisions for all lines (Main Menu> Preprocessor> Meshing> Size Cntrls> ManualSize> Lines> Picked Lines or use the MeshTool).
5.
Select Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Write From Areas. A picker appears. Pick the area(s) of the cells.
6.
ANSYS creates cells on the areas. ANSYS may display bad shape messages during the mesh - these messages can be ignored. However, you may see an "Unable to mesh area ...." message. If you do, clear the elements from all areas (Main Menu> Preprocessor> Meshing> Clear> Areas) and repeat steps 4 and 5.
7.
Write the .SECT file out to a unique name in the Write Section Library File dialog box and click on OK.
8.
Read in the user mesh file (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Read Sect Mesh) to calculate the section properties. Material properties must be defined to calculate the cross section shear correction factors, material-weighted centroids and the shear centers.
Note — Even if you have already set LESIZE, you will see the following message: Line element sizes may need to be specified for desired cross-section mesh. Please refer to the LESIZE command. If you have already set the line element size, click on the Close button to continue. If you have not already set it, issue LESIZE with the appropriate information. When creating cells on the area using the GUI, you do not need to define a plane element type. On the other hand, a plane element type must be defined if the user issues the SECWRITE command explicitly. MESH200 with KEYOPT(1) = 7 and PLANE82 are the only valid plane element types.
16.4.3. Creating Custom Cross Sections with Mesh Refinement and Multiple Materials When doing a plasticity analysis, you may need to refine the cross section mesh. A cross section consisting of more than one material may be defined to represent layers, reinforcements or sensors. When defining a multiplematerial cross section, you will need to specify the material that each cross section cell is made of. You may take a previously-created cross section and modify it. To create a custom cross section with a refined mesh and/or multiple materials, perform the following tasks: 1.
Either read a common section (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Built-up> Edit Common) from the ANSYS database or read a custom section from a .SECT file. (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Built-up> Edit Custom)
2.
ANSYS displays a MESH200 plot in the Graphics Window.
3.
Refine the section mesh. (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Builtup> Refine Mesh)
4.
Modify the cell materials. (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Builtup> Modify Material) If you want to create a multiple-material section, define the materials. This is necessary to calculate the shear correction factors and material-weighted centroids.
5.
Save the section to a .SECT file using SECWRITE (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Built-up> Save).
6.
To calculate the section properties and use a custom section in the analysis, read in the user mesh file (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Read Sect Mesh).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–7
Chapter 16: Beam Analysis and Cross Sections Note — If you redefine a material after creating the section, you must reissue the SECTYPE and SECREAD commands to recompute the cross section. When a cross section has multiple materials, and /ESHAPE is used to produce contour plots of stresses (and other quantities), the element averages the stresses across material boundaries. To limit this behavior, use small cross section cells around the material boundaries. When a cross section has multiple materials, the multiple materials will not be displayed in an element plot with /ESHAPE,1. The multiple materials can be verified by viewing the cross section in the Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Built-up> Edit Custom submenu. When using the SECWRITE command explicitly, a section with multiple materials can be created by assigning material attributes to the areas. During meshing, the elements inherit the material attribute from the area and this attribute is written to the .SECT file.
16.4.4. Defining Composite Cross Sections A composite cross section is a cross section consisting of at least two materials and meshed with a user-defined mesh. When creating a composite section, define the materials before running the SECREAD command. This is necessary to calculate the shear correction factors, material-weighted centroids and the shear centers. Note — If you redefine a material after creating the section, you must reissue the SECREAD command to recompute the cross section. You can save composite cross sections as custom cross sections. For information on custom cross sections, see Section 16.4.1: Using the Beam Tool to Create Common Cross Sections
16.4.5. Defining a Tapered Beam For BEAM188 and BEAM189, you can define tapered beams using the TAPER option on the SECTYPE command (Main Menu> Preprocessor> Sections> Beam> Taper Sections). The tapered section varies linearly between two specified locations, (x1, y1, z1) and (x2, y2, z2). Thus, two SECDATA commands are required to define the taper as shown below. At each of these end points, a valid beam section ID must be input (station-1 and station2 in the example below). SECTYPE,SECID,TAPER SECDATA,station-1,x1,y1,z1 SECDATA,station-2,x2,y2,z2 The following is a typical command input stream used to create a tapered cross section: sectype,1,beam,rect secdata,.0001,0.5 sectype,2,beam,rect secdata,3,0.5 sectype,3,taper secdata,1,0.0,0.0 secdata,2,0.0,20.0
! define cross section at first end point ! define cross section at far end ! new Section ID for tapered beam analysis ! section 1 at location (0,0,0) ! section 2 at location (0,20,0)
Continuing with this example, you can then use 3 as the taper section ID when assigning mesh attributes with the SECNUM or LATT command. The resulting beam cross section is (0.0001*0.5) at end 1, and linearly tapers to (3*0.5) at end 2. The following assumptions apply to tapered beams defined with this method: •
The end sections must be defined prior to defining the taper.
•
Sections defined at the end points must be topologically identical.
16–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.6: Sample Lateral Torsional Buckling Analysis (GUI Method) •
A section cannot taper to a point (or zero area) at either end.
•
The arbitrary beam section type (ASEC on the SECTYPE command) is not supported for tapered beams.
The program performs a number of checks (although not completely comprehensive) to ensure topological equality. The following items are compared: •
number of section nodes
•
number of section elements
•
section type
If both end stations refer to custom cross sections with multiple materials, you must ensure that material IDs for the cells are the same for both ends. At a Gauss point of integration, the BEAM188 and BEAM189 elements will find the closest point on the line defined by station-1 and station-2. Using this information, a linear interpolation is performed for the cross section mesh. Therefore, it is very important that the Gauss point be located within the end points. ANSYS will produce error messages when this is not the case. The tapered section treatment is significantly more expensive than a constant cross section (since recomputation is necessary). If this is a concern, use KEYOPT(12) of the beam element to specify the tapered section treatment. •
KEYOPT(12) = 0 - Linear tapered section analysis (more accurate, but expensive)
•
KEYOPT(12) = 1 - Average cross section analysis (an approximation of the order of the mesh size, but faster)
16.5. Managing Cross Section and User Mesh Libraries Cross section data for common sections such as CHAN and RECT can be stored in cross section libraries. To create standard cross sections for later use, create one or more cross sections, edit the Jobname.LOG file, and copy the appropriate SECTYPE, SECDATA, and SECOFFSET commands into a separate file with a SECT extension. These predefined cross sections can later be read into a model using the /SECLIB command (Main Menu> Preprocessor> Sections> Section Library> Import Library).
16.6. Sample Lateral Torsional Buckling Analysis (GUI Method) You can use BEAM188 and BEAM189 elements to model not only straightforward beam bending and shear response but also to model beam response that involves lateral-torsional buckling. To create this type of model, you will need to create an adequately fine mesh of beam elements. You typically need to model a single beam member using a series of short beam elements, as shown in Figure 16.4: “Lateral-Torsional Buckling of a Cantilever I-Beam”.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–9
Chapter 16: Beam Analysis and Cross Sections
Figure 16.4 Lateral-Torsional Buckling of a Cantilever I-Beam
Lateral-Torsional Buckling of a Cantilever I-Beam, Modeled With 60 BEAM188 Elements (Displayed Using /ESHAPE) Chapter 7, “Buckling Analysis” in the ANSYS Structural Analysis Guide documents buckling analysis in detail. This sample problem shows what happens when a cantilever beam is subjected to a concentrated end load, which causes lateral-torsional buckling.
16.6.1. Problem Description A straight, slender cantilever beam has one fixed end and one free end. A load is applied to the free end. The model is analyzed using eigenvalue buckling calculations, followed by a nonlinear load versus deflection study. The objective is to determine the critical value of the end load (indicated by P in Figure 16.5: “Diagram of a Beam With Deformation Indicated”) at which the beam undergoes a bifurcation indicated by a large displacement in the lateral direction.
16.6.2. Problem Specifications The following material properties are used for this problem: Young's modulus = 1.0 X 104 psi Poisson's ratio = 0.0 16–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.6: Sample Lateral Torsional Buckling Analysis (GUI Method) The following geometric properties are used for this problem: L = 100 in H = 5 in B = .2 in Loading for this problem is: P = 1 lb.
16.6.3. Problem Sketch Figure 16.5 Diagram of a Beam With Deformation Indicated
16.6.4. Eigenvalue Buckling and Nonlinear Collapse Eigenvalue buckling calculation is a linearized calculation, and is generally valid only for elastic structures. The yielding of materials occurs usually at loads lesser than that predicted by eigenvalue buckling analysis. This type of analysis tends to need less computation time than a full nonlinear buckling analysis. You can also perform a nonlinear load versus deflection study, which employs an arc length solution strategy to identify critical loads. While the approach is more general, a collapse analysis may be computationally intensive. The nonlinear collapse analysis must be performed on a structure with imperfections built in to the model, since a perfect model will not show signs of buckling. You can add imperfections by using eigenvectors that result from an eigenvalue buckling analysis. The eigenvector determined is the closest estimate of the actual mode of buckling. The imperfections added should be small when compared to a typical thickness of the beam being analyzed. The imperfections remove the sharp discontinuity in the load-deflection response. It is customary to use one to ten percent of the beam/shell thickness as the maximum imperfection introduced. The UPGEOM command adds displacements from a previous analysis and updates the geometry to the deformed configuration.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–11
Chapter 16: Beam Analysis and Cross Sections
16.6.5. Set the Analysis Title and Define Model Geometry 1.
Choose menu path Utility Menu> File> Change Title.
2.
Enter the text "Lateral Torsional Buckling Analysis" and click on OK.
3.
Start the model creation preprocessor and define the keypoints for the beam. Choose menu path Main Menu> Preprocessor> Modeling> Create> Keypoints> In Active CS, and enter these keypoint numbers and the coordinates in the dialog box as indicated: Keypoint Number
X Location
Y Location
Z Location
Click This Button to Accept Values
1
0
0
0
Apply
2
100.0
0
0
Apply
3
50
5
0
OK
4.
Create a straight line through keypoints 1 and 2. Choose menu path Main Menu> Preprocessor> Modeling> Create> Lines> Lines> Straight Line. The Create Straight Line picker appears. Select keypoints 1 and 2 in the Graphics window and click on OK in the Create Straight Line picker.
5.
Save the model. Choose menu path Utility Menu> File> Save As. Enter buckle.db in the Save Database to box and click on OK.
16.6.6. Define Element Type and Cross Section Information 1.
Choose menu path Main Menu> Preferences and select the "Structural" check box. Click on OK to continue.
2.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete. The Element Types dialog box appears.
3.
Click on Add ... The Library of Element Types dialog box appears.
4.
In the scroll box on the left, click on "Structural Beam" to select it.
5.
In the scroll box on the right, click on "3D finite strain, 3 node 189" to select BEAM189.
6.
Click on OK, and then click on Close in the Element Types dialog box.
7.
Define a rectangular cross section for the beam. Choose menu path Main Menu> Preprocessor> Sections> Beam> Common Sectns. The BeamTool is displayed. ANSYS sets the section ID to 1, and the subtype to RECT (signified by a rectangle on the subtype button) by default. Since you will be creating a rectangular cross section, there is no need to change the subtype.
8.
In the lower half of the BeamTool, you will see a diagram of the cross section shape with dimension variables labeled. Enter the width of the cross section, 0.2, in the box labeled B. Enter the height of the cross section, 5.0, in the box labeled H. Click on Apply to set the cross section dimensions.
9.
Use the BeamTool to display information about the cross section. Click on the Preview button on the BeamTool. A diagram and data summary of the cross section appear in the Graphics window. You can also preview the mesh of the cross section by selecting the Meshview button. Click on the Close button in the BeamTool to continue.
16.6.7. Define the Material Properties and Orientation Node 1.
16–12
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.6: Sample Lateral Torsional Buckling Analysis (GUI Method) 2.
In the Material Models Available window on the right, double-click on the following: Structural, Linear, Elastic, Isotropic. A dialog box appears.
3.
Enter 1E4 for EX (Young's modulus).
4.
Enter 0.0 for PRXY (Poisson's ratio), and click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
5.
Choose menu path Material> Exit to close the Define Material Model Behavior dialog box.
6.
Replot the line by choosing menu path Utility Menu> Plot> Lines.
7.
Select the line and define the orientation node of the line as an attribute. Choose menu path Main Menu> Preprocessor> Meshing> Mesh Attributes> Picked Lines. The Line Attributes picker appears. Select the line in the Graphics window and click on Apply in the Line Attributes picker.
8.
The Line Attributes dialog box appears. ANSYS includes the material attribute pointer to the material set 1, the element type attribute pointer to the local element type 1, and the section attribute pointer to the section ID 1 by default. Click on the radio button beside the Pick Orientation Keypoint(s) label to change it to Yes and click on OK.
9.
The Line Attributes picker reappears. Type 3 in the picker, press the Enter key, and click on OK.
10. Save the model. Choose menu path Utility Menu> File> Save As. If the buckle.db file is not already selected, select it. Select OK, and when ANSYS prompts you if you want to overwrite the existing file, click on OK.
16.6.8. Mesh the Line and Verify Beam Orientation 1.
Define the mesh size and number of divisions. Choose menu path Main Menu> Preprocessor> Meshing> Size Cntrls> ManualSize> Lines> All Lines. Enter 10 in the No. of Element Divisions box and click on OK.
2.
Mesh the line. Choose menu path Main Menu> Preprocessor> Meshing> MeshTool. Click on MESH on the MeshTool and the Mesh Lines picker appears. Pick the line in the Graphics window, and then click on OK in the Mesh Lines picker. Click on Close in the MeshTool to close it.
3.
Rotate the meshed line. Choose menu path Utility Menu> PlotCtrls> Pan, Zoom, Rotate. The Pan, Zoom, Rotate tool appears. Select ISO and click on Close. The beam is rotated in the Graphics window.
4.
Verify the beam orientation. Choose menu path Utility Menu> PlotCtrls> Style> Size and Shape. Select the radio button next to the /ESHAPE label to turn /ESHAPE on and click on OK.
16.6.9. Define the Boundary Conditions 1.
Define a boundary condition to the fixed end. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Keypoints. The Apply U,ROT on KPs picker appears.
2.
Define keypoint 1 as the fixed end. In the picker, type 1, press the Enter key, then click on OK. The Apply U,ROT on KPs dialog box appears.
3.
Click on "All DOF" to select it, and click on OK. The boundary condition information appears in the ANSYS Graphics window at keypoint 1.
4.
Apply a force to the free end. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment> On Keypoints. The Apply F/M on KPs picker appears.
5.
Identify keypoint 2 as the free end. Type 2 in the picker, press the Enter key, and then click on OK. The Apply F/M on KPs dialog box appears.
6.
In the drop down list for Direction of force/mom, select FY. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–13
Chapter 16: Beam Analysis and Cross Sections 7.
Enter 1 for the Force/moment value in the Apply F/M on KPs dialog box, and click on OK. The force symbol appears in the ANSYS Graphics window at keypoint 2.
8.
Save the model. Choose menu path Utility Menu> File> Save As. If the buckle.db file is not already selected, select it. Click on OK and when ANSYS prompts you if you want to overwrite the existing file, click on OK again.
16.6.10. Solve the Eigenvalue Buckling Analysis 1.
Set analysis options. Choose menu path Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options. The Static or Steady-State Analysis dialog box appears.
2.
Use the sparse solver for the solution. In the Static or Steady-State Analysis dialog box, make sure that Sparse solver is selected in the drop down box beside the Equation solver label.
3.
Include prestress effect, which will be stored for later use in the eigenvalue buckling calculation. In the drop down list labeled Stress stiffness or prestress, select "Prestress ON." Click on OK to close the Static or Steady-State Analysis dialog box.
4.
Choose menu path Main Menu> Solution> Solve> Current LS. Review the summary information in the /STAT command window, then select Close from its menu bar. Click on OK in the Solve Current Load Step window to begin the solution.
5.
When the Solution is Done! window appears, click on Close to close it.
6.
Choose menu path Main Menu> Finish.
7.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis.
8.
Select the "Eigen Buckling" option, then click on OK.
9.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Eigenvalue Buckling Options dialog box appears. Select the Block Lanczos option. Enter 4 in the No. of modes to extract box, then click on OK.
10. Set the element calculation key for the MXPAND command. Choose menu path Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> Expand Modes. 11. In the Expand Modes dialog box, enter 4 in the No. of modes to expand box, change the No to Yes beside the Calculate elem results label, and click on OK. 12. Choose menu path Main Menu> Solution> Solve> Current LS. Review the summary information in the /STAT command window, then select Close from its menu bar. Click on OK in the Solve Current Load Step window to begin the solution. 13. When the Solution is Done! window appears, click on Close to close it. 14. Choose menu path Utility Menu> PlotCtrls> Style> Size and Shape. Be sure the radio button beside the label Display of element shapes ... (/ESHAPE) is set to On and click on OK. 15. Display the results summary. Choose menu path Main Menu> General Postproc> Results Summary. After you have reviewed the results, click on Close to close the window. 16. Choose menu path Main Menu> General Postproc> Read Results> First Set. 17. Plot the first mode shape of the beam. Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears. Select Def + undef edge and click on OK. 18. Choose menu path Main Menu> Finish.
16–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.6: Sample Lateral Torsional Buckling Analysis (GUI Method)
16.6.11. Solve the Nonlinear Buckling Analysis 1.
Introduce model imperfections calculated by the previous analysis. Choose menu path Main Menu> Preprocessor> Modeling> Update Geom. In the Update nodes using results file displacements dialog box, enter 0.002 in the Scaling factor box, 1 in the Load step box, 1 in the Substep box, and file.rst in the Selection box. Click on OK.
2.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis.
3.
Select the "Static" option, then click on OK.
4.
Choose menu path Main Menu> Solution> Load Step Opts> Output Ctrls> DB/Results File and be sure the drop down lists display All Items and All entities respectively. Choose the Every substep for the File write frequency radio button and click on OK.
5.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. Select the radio button beside Large deform effects, then click on OK.
6.
Set the arc-length method, and set parameters for the termination of the solution. Choose menu path Main Menu> Solution> Load Step Opts> Nonlinear> Arc-Length Opts. Select the Arc-length method on/off radio button and set it to On. Choose the pull down menu next to the Lab label and select Displacement lim. Enter 1.0 in the Max desired U box. Enter 2 in the Node number for VAL box. Choose the pull down menu next to the Degree of freedom label and select UZ. Click on OK.
7.
Define the number of substeps to be run during this load step. Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Time and Substps. Enter 10000 in the Number of substeps box and click on OK.
8.
Solve the current model. Choose menu path Main Menu> Solution> Solve> Current LS. Review the summary information in the /STAT command window, then select Close from its menu bar. Click on OK in the Solve Current Load Step window to begin the solution. A Nonlinear Solution window with a Stop button appears. A convergence graph is built, and can take several minutes to complete.
9.
You may receive a warning message. You should review the information in the message but you do not need to close it. Continue waiting for the solution to complete. When the Solution is Done! window appears, click on Close to close it.
10. Choose menu path Main Menu> Finish.
16.6.12. Plot and Review the Results 1.
Replot the beam. Choose menu path Utility Menu> Plot> Elements.
2.
Define the load point deflection to be read from the results file. Choose menu path Main Menu> TimeHist PostPro> Define Variables. When the Defined Time-History Variables dialog box appears, select Add.
3.
When the Add Time-History Variable dialog box appears, be sure the Nodal DOF result option is selected. Click on OK.
4.
The Define Nodal Data picker appears. In the Graphics window, pick node 2 (the end node on the right side of the beam) and click on OK.
5.
The Define Nodal Data dialog box appears. Be sure the Ref number of variable and Node number are both set to 2. Enter TIPLATDI in the User-specified label box. Select Translation UZ from the menu and click on OK.
6.
Define the total reaction force to be read from the results file. Choose Add from the Defined Time-History Variables dialog box.
7.
When the Add Time-History Variable dialog box appears, choose the Reaction forces radio button and then click on OK. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–15
Chapter 16: Beam Analysis and Cross Sections 8.
The Define Reaction Force picker appears. Pick the end node on the left side of the beam and click on OK.
9.
The Define Reaction Force Variable dialog box appears. Be sure the Ref number of variable is set to 3 and Node number is set to 1. Select Struct Force FY from the menu and click on OK. Click on Close to close the Defined Time-History Variables dialog box.
10. Choose menu path Main Menu> TimeHist Postpro> Math Operations> Multiply. In the Multiply TimeHistory Variables dialog box, enter 4 in the Reference number for result box, -1.0 in the 1st Factor box, and 3 in the 1st Variable box. Click on OK. 11. Display the X variable. Choose menu path Main Menu> TimeHist Postpro> Settings> Graph. Choose the single variable button, enter 2 in the Single variable no. box, and click on OK. 12. Plot the load versus deflection curve to confirm the critical load calculated by the eigenvalue method. Choose menu path Main Menu> TimeHist PostPro> Graph Variables. Enter 4 in the 1st variable to graph box. Click on OK. 13. List the variables versus time. Choose menu path Main Menu> TimeHist PostPro> List Variables. Enter 2 in the 1st variable to list box and 4 in the 2nd variable box and click on OK. 14. Check the values in the PRVAR Command window to see how they compare against the values generated by the eigenvalue buckling analysis. Expected results are: Critical buckling load, Pcr = 0.01892. Close the PRVAR Command window. 15. Choose menu path Main Menu> Finish. 16. In the ANSYS Toolbar, click on Quit. 17. Choose a save option and click on OK.
16.7. Sample Problem with Cantilever Beams, Command Method Here is the input file for the problem described in the previous section: /GRAPHICS,POWER /GST,ON /SHOW,BUCKLE,GRPH /PREP7 K,1,0,0,0 K,2,100.0,0,0 K,3,50,5,0 LSTR,1,2 ET,1,BEAM189 SECTYPE,1, BEAM, RECT SECDATA, 0.2, 5.0 SLIST, 1, 1 MP,EX,1,1E4 MP,NUXY,1,0.0 LSEL,S, , , 1, 1, 1 LATT,1, ,1,0, 3, ,1 LESIZE, all, , ,10 SECNUM,1 LMESH,all /VIEW,,1,1,1 /ESHAPE,1 EPLOT DK,1, , , ,0,ALL FK,2,FY,1.0 FINISH /SOLU PSTRES,ON EQSLV,SPARSE ! EQSLV,SPARSE is the default for static and full transient SOLVE FINISH /SOLU
16–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.8: Where to Find Other Examples ANTYPE,BUCKLE BUCOPT,LANB,4 MXPAND,4,,,YES SOLVE FINISH /POST1 /ESHAPE,1 /VIEW, 1 ,1,1,1 /ANG, 1 SET,LIST SET,1,1 PLDISP,2 FINISH /PREP7 UPGEOM,0.002,1,1,file,rst /SOLU ANTYPE,STATIC OUTRES,ALL,ALL NLGEOM,ON ARCLEN,ON,25,0.0001 ARCTRM,U,1.0,2,UZ NSUBST,10000 SOLVE FINISH /POST26 NSOL,2,2,U,Z,TIPLATDI RFORCE,3,1,F,Y PROD,4,3, , , , , ,-1.0,1,1 XVAR,2 PLVAR,4 PRVAR,2,4 FINISH
16.8. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional beam analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS program. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual contains one beam test case: VM222 - Warped Cantilever Beam
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–17
16–18
Chapter 17: Shell Analysis and Cross Sections 17.1. An Overview of Shells Shell elements are used to create a mathematical 2-D idealization of a 3-D structure. They offer computationally efficient solutions for modelling shell structures when compared to solid elements. The discussion in this chapter applies to SHELL181, which is a 3-D finite strain shell element. This shell element provides more robust nonlinear analysis capabilities, and significant improvements in cross section data definition, analysis, and visualization, as compared to other ANSYS shells. The method for defining shell sections described here can also be used to define the cross-sectional properties of the layered thermal shell elements, SHELL131 and SHELL132. Discussions in this chapter relating to integration points (NUMPT on the SECDATA command) and section properties (SECCONTROLS command) do not apply to SHELL131 and SHELL132.
17.2. What Are Cross Sections? A cross section defines the geometry of the shell in a plane parallel to the shell x-y plane. Through the section family of commands, you can describe the z direction of the element by defining consecutive layers. Each layer may vary in thickness, material type, orientation (from element x-axis), and number of integration points.
17.3. How to Create Cross Sections The general procedure for creating cross sections consists of the following steps: 1.
Define the section and associate a section ID number with the section.
2.
Define the geometry data for the section.
ANSYS supplies the following commands for creating, viewing, and listing cross sections, and for managing cross section libraries:
Table 17.1 ANSYS Cross Section Commands Command
Purpose
GUI Menu Path
SECTYPE
Associates section with SECID (section number)
Main Menu> Preprocessor> Sections> Shell> Add/Edit
SECDATA
Defines section geometry Main Menu> Preprocessor> Sections> Shell> Add/Edit data
SECCONTROLS Overrides program calcu- Main Menu> Preprocessor> Sections> Shell> Add/Edit lated properties. SECFUNCTION Specifies shell section thickness as a tabular function.
Main Menu> Preprocessor> Sections> Shell> Add/Edit
SECNUM
Identifies the SECID (sec- Main Menu> Preprocessor> Meshing> Mesh Attributes> Default tion number) to be asAttribs signed to an element Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes
SECOFFSET
Defines section offset for Main Menu> Preprocessor> Sections> Shell> Add/Edit shell cross sections
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 17: Shell Analysis and Cross Sections Command
Purpose
GUI Menu Path
SECPLOT
Plots geometry of a shell Main Menu> Preprocessor> Sections> Shell> Plot Section section to scale
SLIST
Summarizes section prop- Main Menu> Preprocessor> Sections> List Sections erties Utility Menu> List> Properties> Section Properties Utility Menu> List> Properties> Specified Section Properties
SDELETE
Deletes a cross section
Main Menu> Preprocessor> Sections> Delete Section
For complete documentation of the cross section commands, see the ANSYS Commands Reference. Figure 17.1: “Plot of a Shell Section” shows the layer stacking of a shell section. The layer order, along with material and orientation of each layer, is represented here:
Figure 17.1 Plot of a Shell Section
17.3.1. Defining a Section and Associating a Section ID Number Use the SECTYPE command to define a section and associate it with a section ID number. For example, the following command assigns a section identification number (2) to a shell section: Command(s): SECTYPE, 2, SHELL GUI: Main Menu> Preprocessor> Sections> Shell> Add/Edit
17.3.2. Defining Layer Data Use the SECDATA command to define the layers of a shell section. Each consecutive SECDATA command defines the next layer's thickness, material, orientation, and number of integration points. (The number of integration points input on SECDATA is not used by thermal shell elements.) The layer orientation angle is the angle between the layer coordinate system and the x-axis of the element coordinate system.
17–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 17.3: How to Create Cross Sections You may designate the number of integration points (1, 3, 5, 7, or 9) located thru the thickness of each layer. When only 1, the point is always located midway between the top and bottom surfaces. If 3 or more points, 2 points are located on the top and bottom surfaces respectively and the remaining points are distributed equal distance between the 2 points. An exception occurs when designating 5 points, where the quarter point locations are moved 5 percent toward their nearest layer surface to agree with the locations selected with real constant input. The default for each layer is 3. If a shell section has only one layer, and the number of section integration points is equal to one, then the shell does not have any bending stiffness. This may result in solver difficulties, and may affect convergence adversely. Command(s): SECDATA, 0.5, 1, 45, 3 SECDATA, 0.5, 2, -45, 3 SECDATA, 0.5, 1, 45, 3 GUI: Main Menu> Preprocessor> Sections> Shell> Add/Edit
17.3.3. Overriding Program Calculated Section Properties Use the SECCONTROLS command to override the program calculated section properties. By default, the program calculates shear correction factors and mass for each element based on the input section geometry and material properties. Any values input on the SECCONTROLS command will replace the defaults. (SECCONTROLS does not apply to thermal shell elements.) Command(s): SECCONTROLS, 0.8, 0.0, 0.8, 1.0 GUI: Main Menu> Preprocessor> Sections> Shell> Add/Edit
17.3.4. Specifying a Shell Thickness Variation (Tapered Shells) Use the SECFUNCTION command to associate a tabular thickness variation with the section. A table that describes thickness with respect to the global Cartesian coordinate system may be associated with a shell section. This thickness is interpreted as the total thickness of a shell. The total thickness of a layered shell, and all layer thickness values, will be scaled according to the tabular function. Command(s): SECFUNCTION, %table_name% GUI: Main Menu> Preprocessor> Sections> Shell> Add/Edit
17.3.5. Setting the Section Attribute Pointer Use the SECNUM command to associate an element with a particular section. Any element created after the SECNUM command will have this section identification number (2) as its section attribute. Command(s): SECNUM, 2 GUI: Main Menu> Preprocessor> Meshing> Mesh Attributes> Define> Default Attribs
17.3.6. Associating an Area with a Section Use the AATT command to associate an area with a shell section type. When the area is meshed, the new elements are associated with the section specified on the AATT command. The section specified by the SECNUM command is ignored. Command(s): AATT, , , , , 2 GUI: Main Menu> Preprocessor> Meshing> Mesh Attributes> All Areas Main Menu> Preprocessor> Meshing> Mesh Attributes> Picked Areas
17.3.7. Using the Shell Tool to Create Sections The SECTYPE, SECDATA, SECOFFSET, SECFUNCTION, and SECCONTROLS commands (Main Menu> Preprocessor> Sections> Shell> Add/Edit) are all associated with the ShellTool in the GUI.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
17–3
Chapter 17: Shell Analysis and Cross Sections
Figure 17.2 Shell Tool With Layup Page Displayed
The top part of the Layup page of the ShellTool relates a section ID number to a Shell section type (and, optionally, a section name) [SECTYPE]. The middle part of the page of the ShellTool defines each layer in the positive Z direction of the element [SECDATA]. Note that the order of the rows in the spreadsheet ascends up the page, resembling that stacking of the layers. (Integration point data for each layer is ignored by thermal shell elements.) The bottom contains the fields for section offset information, if needed [SECOFFSET]. You can define tapered shells by specifying a section function relating thickness to global coordinates [SECFUNCTION].
Figure 17.3 Shell Tool With Section Controls Page Displayed
The transverse shear stiffness, hourglass coefficients and drill stiffness of the sections are calculated from the section geometry and material properties. The default added mass per unit area of the section is always zero. On the Section Controls page, you can override the program calculated quantities [SECCONTROLS]. (The Section Controls page does not apply to thermal shell elements.)
17–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 17.3: How to Create Cross Sections
Figure 17.4 Shell Tool With Summary Page Displayed
On the Summary page, you can review the section properties.
17.3.8. Managing Cross Section Libraries Cross section data for shell sections can be stored in cross section libraries. To create standard cross sections for later use, create one or more cross sections, edit the Jobname.LOG file, and copy the appropriate SECCONTROLS, SECDATA, SECFUNCTION, SECOFFSET, and SECTYPE commands into a separate file with a SECT extension.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
17–5
17–6
creep, 8–31 hyperelasticity, 8–21 large strain, 8–6 plasticity, 8–9
Index Symbols 2-D fracture models, 12–3 3-D fracture models, 12–4
B
A adaptive descent, 8–53 adequate mesh density, 8–64 alpha (mass) damping, 4–10, 5–36, 6–18 alternating stress intensity, 14–1 amplitude of harmonic loads, 4–5 analysis modal analysis options, 3–4 reduced transient dynamic, 5–19 analysis options harmonic response analysis, 4–25 mode superposition method, 4–25 modal analysis, 3–2, 4–4, 4–20 nonlinear static structural analysis, 8–49 single-point spectrum analysis, 6–3 transient dynamic analysis, 5–14, 5–20 mode superposition method, 5–14 reduced method, 5–20 analysis type buckling, 7–1 full transient, 5–7 harmonic response, 4–1 modal, 3–1 nonlinear structural, 8–1 p-method, 15–1 spectrum, 6–1 static structural, 2–1, 2–2 structural, 1–1 definition of, 1–1 transient dynamic, 5–1 animation gasket results, 10–19 anisotropic, 8–10 applying loads, 3–2, 4–4, 4–20, 8–56, 8–60 harmonic response analysis, 4–5 increments for buckling analysis, 7–2 modal analysis, 3–5 nonlinear analysis, 8–56 p-method, 15–7 structural static analysis, 2–8, 2–8 transient dynamic analysis, 5–9 using TABLE array parameters, 2–8 arc-length method, 2–5, 7–2, 7–3, 8–2, 8–68 automatic time stepping, 5–35, 7–2, 8–67
Bauschinger effect, 8–10 beam tool, 16–5 beams cross sections, 16–1 Besseling model, 8–10 beta (stiffness) damping, 4–10, 5–36, 6–3, 6–18 bilinear isotropic hardening, 8–10 bilinear kinematic hardening, 8–10 birth and death, 8–69, 8–70 element, 8–63 bisection, 8–5 Block Lanczos extraction method, 4–25 Block Lanczos method, 3–3, 3–17 bonlinear structural analysis restarts, 8–59 buckling analysis, 7–1, 7–1 eigenvalue, 7–3 procedure, 7–3 expand the solution, 7–6 expansion pass, 7–6 methods of solution, 7–1 nonlinear, 7–2 procedure, 7–2 obtain the eigenvalue buckling solution, 7–5 obtain the static solution, 7–4
C calculating covariance in POST26, 6–23 fracture parameters, 12–5 cast iron plasticity, 8–10 causes of nonlinear behavior, 8–1 changing status, 8–2 geometric nonlinearities, 8–2 material nonlinearities, 8–2 cells defining for a section, 16–4 Chaboche model, 8–10 changing status, 8–2 combinations material model, 8–35 composite cross section, 16–8 composites, 13–1 element types for, 13–1 guidelines, 13–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index how to model, 13–1 layer properties, 13–3 concrete, 8–10, 8–29, 8–63 constant damping ratio, 4–10, 5–36, 6–3, 6–18 constitutive matrices, 13–4 constraint equations, 15–7 with QR Damped method, 3–19 contact, 8–2 node-to-node, 8–63 contact analysis, 11–1 asymmetric vs. symmetric contact, 11–7 birth and death option, 11–42 boundary conditions for node-to-node contact, 11–74 boundary conditions for surface-to-surface contact, 11–51 chattering controls, 11–21 choosing surfaces, 11–6 conduction, 11–45 contact algorithm, 11–21, 11–74 contact direction, 11–13 contact location detection, 11–28 Contact Manager, 11–4, 11–54 contact pairs, 11–5, 11–56 contact status, 11–38, 11–44 contact stiffness, 11–21, 11–22 contact surface elements, 11–3 Contact Wizard, 11–55 convection, 11–46 deformable contact surface, 11–14 direct generation to create rigid target elements, 11–9 electric contact, 11–48 electrostatic elements, 11–48 emissivity, 11–46 explicit dynamics, 11–1 flexible-to-flexible, 11–1, 11–4 free surface convection, 11–44 free surface radiation, 11–44 free thermal surface, 11–44 friction model, 11–25 gap, 11–74 Gauss integration points, 11–28 generating node-to-node contact elements, 11–71 generating surface-to-surface contact elements, 11–16 heat flux, 11–44, 11–48 heat generation due to electric current, 11–49 heat generation due to friction, 11–47 initial contact conditions, 11–30 initial interference, 11–74 internal MPC, 11–60
Index–2
localized contact zone, 11–12 magnetic contact, 11–50 moving contact nodes, 11–37 node ordering in node-to-node analysis, 11–72 node-to-node, 11–2, 11–4, 11–70 node-to-surface, 11–2, 11–3, 11–57 node-to-surface KEYOPTS, 11–59 node-to-surface real constants, 11–60 normals, 11–13, 11–16, 11–54, 11–73 open far-field contact status, 11–38 open near-field contact status, 11–38 overall steps, 11–5 overconstrained contact problem, 11–74 penalty stiffness, 11–15 penetration, 11–21 piezoelectric elements, 11–48 pinball region, 11–38 point-to-point, 11–4 point-to-surface, 11–3 pseudo element technique, 11–57 radiation, 11–46 results, 11–53 rigid-to-flexible, 11–1, 11–4, 11–43 self contact, 11–7, 11–39 shells, 11–42 sliding contact status, 11–38 slippage, 11–28 solution options for node-to-node contact, 11–75 solution options for surface-to-surface contact, 11–51 solving, 11–52 spurious contact, 11–39 Stefan-Boltzmann constant, 11–46 sticking contact status, 11–38 summary of contact capabilities, 11–2 superelements, 11–41 surface interaction for electric contact, 11–48 surface interaction models, 11–40 surface-to-surface, 11–2, 11–3, 11–4, 11–14 surface-to-surface KEYOPTS, 11–20 surface-to-surface material properties, 11–15 surface-to-surface overview, 11–4 surface-to-surface real constants, 11–15, 11–17 symmetric/unsymmetric solver, 11–25 target element shapes, 11–9 target surface definition, 11–7 target surface element types and real constants, 11–8 target surface modeling and meshing tips, 11–12 target surface nodal number ordering, 11–13 target surface pilot node, 11–8, 11–43 target surface primitives, 11–8 temperature required, 11–45
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index thermal contact, 11–44 thickness effect, 11–42 time step control, 11–42 using meshing tools to create rigid target elements, 11–10 contour displays, 2–11, 3–11, 6–8, 7–7, 8–57, 10–19 control elements, 8–69 controlling cutbacks, 2–4 controlling p-levels, 15–7 controlling restarts, 2–4 convergence checking, 8–51 enhancements, 8–64 failure, 8–64 convergence criteria, 8–51 default value, 8–51 disjointed structures, 8–51 displacement checking, 8–51 force checking, 8–51 p-method, 15–7 vector norms, 8–51 convergence tolerances, 2–4 coupling, 13–6, 15–6 covariance calculating, 6–23 crack faces, 12–1 crack front, 12–1 crack region modeling, 12–1 crack tip, 12–1 creating sections, 16–2, 16–5, 17–1 beam tool, 16–5 creep, 8–8, 8–29 automatic time stepping, 8–31 explicit, 8–29, 8–55 explicit creep procedure, 8–31 implicit, 8–29, 8–55 implicit creep procedure, 8–30 material curve fitting, 9–7 ratio, 8–55 creep criteria, 2–7, 8–55 creep strain rate, 8–29 cross sections (see sections) (see Sections) composite, 16–8 custom convergence criteria, 8–51 cutback criteria, 2–4 CUTCONTROL command changes through SOLCONTROL, 8–53 cyclic hardening/softening, 8–10
D damped method modal analysis, 3–3, 3–18 damping, 5–9, 5–36, 8–60 harmonic response analysis, 4–10 spectrum analysis, 6–18 PSD, 6–18 table of options, 5–36 transient dynamic analysis, 5–7, 5–9, 5–14, 5–22 database output, 2–2, 3–8, 4–10, 4–21, 5–7, 5–14, 5–24, 7–6, 8–49 DDAM (see dynamic design analysis method) deep drawing, 8–32 deformed shape display, 2–11, 6–8, 7–7, 8–57 displaying, 10–19 deleting sections, 16–2, 17–1 deterministic analysis, 6–2 disjointed structures, 8–51 display deformed shape, 3–11, 4–12 displaying deformed shapes, 8–57 DOFs master, 3–4 Drucker-Prager, 8–10 dynamic analyses harmonic response, 4–1 spectrum, 6–1 transient, 5–1 dynamic design analysis method (DDAM), 6–2, 6–25
E eigenvalue analysis, 3–1 eigenvalue buckling, 7–1 eigenvalue buckling solution buckling analysis, 7–5 eigenvalue calculation shift point, 7–5 eigenvalue extraction methods, 7–5 eigenvalues, 3–1 number to be extracted, 7–5 eigenvectors, 3–1 elastomers, 8–17 element birth and death, 8–63 element damping, 5–36 element loads, 4–25 element types structural, 1–2 elements associating sec IDs with, 16–2, 17–1 energy release rate, 12–1, 12–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index–3
Index engineering strain, 8–7 engineering stress, 8–7 epoxy, 13–1 equation solvers, 2–4, 4–4, 8–50, 15–7 equilibrium iterations, 8–2, 8–52 number of, 2–4, 8–52 error estimation, 2–11 example problems beam analysis, 16–17 buckling analysis, 7–12 harmonic response analysis, 4–19 modal analysis, 3–14 nonlinear analysis, 8–82 reduced transient dynamic analysis, 5–40 single-point response spectrum analysis, 6–17 static analysis, 2–26 excitation direction, 6–3 expand single solution, 5–24 expand the modes single-point response spectrum analysis, 6–6 expand the solution buckling analysis, 7–6 reduced harmonic response analysis, 4–21 expanded modes number to use, 6–3 expanded solution review results, 5–25 expanding modes, 3–8 expansion frequency range, 3–8 expansion pass, 4–21 activating, 3–8, 4–21, 5–24 buckling analysis, 7–6 harmonic response analysis, 4–21, 4–27 mode superposition method, 4–27 reduced method, 4–21 transient dynamic analysis, 5–18, 5–24 mode superposition method, 5–18 reduced method, 5–24 expansion pass options harmonic response analysis (reduced), 4–21 modal analysis, 3–8 transient dynamic analysis (reduced), 5–24 explicit creep, 8–29 explicit creep procedure, 8–31 extra element shapes, 8–70 extracting modes, 3–1 extrapolation of results, 2–7, 4–10, 4–21, 5–24, 8–56
F failure criteria, 13–5 maximum strain, 13–5 Index–4
maximum stress, 13–5 Tsai-Wu, 13–5 failures convergence, 8–64 fatigue alternating stress intensity, 14–1 design stress-intensity value (Sm), 14–2 evaluation procedure, 14–2 event, 14–1 event repetitions, 14–6 fatigue data file (Jobname.FATG), 14–9 guidelines for assembling events, 14–7 loading, 14–1 location, 14–1 manually stored stresses, 14–4 material properties, 14–2 overview, 14–1 S-N curve, 14–2 sample input, 14–9 scale factors, 14–6 Sm-T curve, 14–2 strain hardening exponents, 14–2 stress concentration factors, 14–2 stress locations, 14–2 stresses at a cross-section, 14–5 stresses from results file, 14–5 with p-elements, 15–4 fatigue assessments, 15–4 fatigue calculations activating, 14–9 fiberglass, 13–1 files Jobname.FATG, 14–9 .SECT, 16–6 forced vibrations, 4–1 forcing frequency range, 4–10 fracture assessments, 15–4 fracture mechanics, 12–1, 12–1 solving problems, 12–1 fracture models 2-D, 12–3 3-D, 12–4 fracture parameters calculating, 12–5 free meshing, 15–4 free-body analysis (see inertia relief) frequency range for expansion, 3–8, 4–21 frequency vector, 6–23 frequency-dependent damping ratio, 6–18 full harmonic response analysis procedure, 4–3 full transient dynamic analysis
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index procedure, 5–3
Blatz-Ko foam model, 8–20 Gent model, 8–20 large strain, 8–17 material curve fitting, 9–1 Mooney-Rivlin model, 8–18, 8–21 neo-Hookean model, 8–19 Ogden compressible foam model, 8–20 Ogden model, 8–18 polynomial form model, 8–19 stability checks, 8–21 u-P formulation, 8–21 user-defined option, 8–21 Yeoh model, 8–20
G gap conditions, 5–14, 5–20 and QR Damped method, 5–14 gasket joints simulation, 10–1 applications, 10–3 element topologies, 10–2 elements, 10–3 formulation, 10–2 materials, 10–4 meshing, 10–12 output listing, 10–17 overview, 10–1 plotting data, 10–11 procedure, 10–1 results, 10–19 sample problem, 10–20 solution, 10–16 thickness, 10–2 gasket results animation, 10–19 POST1, 10–19 POST26, 10–20 reviewing, 10–19 tabular listing, 10–19 geometric nonlinearities, 8–2, 8–6 geometry data for sections, 16–2, 17–1 geometry data of a section, 16–3, 17–2 glass, 8–33 guyan reduction, 3–19
H harmonic forcing frequency, 4–5 harmonic response, 4–1 harmonic response analysis, 4–1 full method, 4–3, 4–3 procedure, 4–3 methods of solution, 4–2 mode superposition method, 4–25, 4–27 procedure, 4–25 sample input, 4–27 prestressed, 4–28 reduced method, 4–20, 4–24 sample input, 4–24 uses for, 4–1 harmonic solutions number of, 4–9 Hill anisotropy, 8–10 hyperelasticity, 8–8, 8–17 Arruda-Boyce model, 8–19 automatic time stepping, 8–21
I implicit creep, 8–29 implicit creep procedure, 8–30 inertia relief, 2–9 calculating, 2–9 output, 2–9 partial, 2–9 initial accelerations, 5–4 initial conditions transient dynamic analysis, 5–4, 5–14, 5–21 full method, 5–4 mode superposition method, 5–14 reduced method, 5–21 initial displacement, 5–4 initial velocity, 5–4 integration point, 8–56 integration time step, 5–1, 5–7, 5–14, 5–22 guidelines for, 5–33 interface material model, 1–2 internal MPC, 11–60
J J-integral, 12–1, 12–6
K kinematic analysis, 8–60, 8–67 KSPIN [OMEGA], 8–8
L large deflection and load direction, 8–6 large deformation effects, 2–2, 5–7, 7–2, 8–6, 8–8, 8–60 large strain analyses, 8–6, 8–10 automatic time stepping, 8–6 hyperelasticity, 8–17 logarithmic strain, 8–7
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index–5
Index true stress, 8–7 viscoplasticity, 8–32 layer orientation angle, 13–3 layer thickness, 13–3 layered elements, 13–1 libraries sections, 16–9, 17–5 library paths for cross sections, 16–2 line element results, 2–11, 3–11 line search option, 2–4, 8–53, 8–68 list master DOF, 3–11 listing section properties, 16–2, 17–1 section results, 16–2 load step options, 3–8, 4–21, 5–24 buckling analysis, 7–6 eigenvalue buckling, 7–5 harmonic response analysis, 4–9, 4–20, 4–25 full method, 4–9 mode superposition method, 4–25 reduced method, 4–20 modal analysis, 3–6 mode superposition transient dynamic analysis, 5–14 Newton-Raphson, 8–54 p-method, 15–7 reduced transient dynamic analysis, 5–21 spectrum analysis, 6–3, 6–18 PSD, 6–18 single-point, 6–3 time, 5–14 transient dynamic analysis, 5–10, 5–10, 5–14, 5–21 full method, 5–10 mode superposition method, 5–14 reduced method, 5–21 load steps, 8–2 applying for transient loading, 5–10 load types, 2–7, 3–5 harmonic response analysis, 4–5 p-method, 15–7 load vector, 4–25, 5–14, 5–14 load-versus-time curve, 5–4 loads applying, 2–8, 3–2, 3–5, 4–8, 4–20, 5–14, 7–2, 8–56, 8–60, 15–7 p-method, 15–7 applying for transient loading, 5–9 direction in a large-deflection analysis, 8–6 harmonic response analysis, 4–5, 4–20, 4–25 mode superposition method, 4–25 reduced method, 4–20 modal analysis, 3–5
Index–6
nonlinear analysis, 8–56 structural static analysis, 2–8, 2–8 transient dynamic analysis, 5–9, 5–9, 5–14, 5–21 full method, 5–9 mode superposition method, 5–14 reduced method, 5–21 Loads applying, 4–4 logarithmic strain, 8–7, 8–7
M macros, 2–10 magnetic analysis contact, 11–50 mass damping, 5–36 mass matrix formulation, 2–6, 3–4, 4–4, 5–9 master degrees of freedom selection of, 3–19 master DOF (MDOF), 3–19, 5–20 master DOFs definition of, 3–4 material curve fitting, 9–1 creep, 9–7 viscoelastic, 9–14 material model combinations, 8–35 material model interface, 1–2 material models shape memory alloy, 8–31 material nonlinearities, 8–2, 8–8 material properties, 15–3 fatigue, 14–2 material curve fitting, 9–1 nonlinear, 8–8 material-dependent damping, 5–36 matrix reduction, 3–19 theory of, 3–19 maximum strain failure criterion, 13–5 maximum stress failure criterion, 13–5 MDOF, 3–4 memory saving when generating stiffness matrix, 8–50 meshing a line for a section, 16–4 p-element, 15–4 metal forming, 8–32 midside nodes p-element, 15–4 MINREF [CNVTOL], 8–51 modal analysis, 3–1 applying loads, 3–5 mode-extraction methods, 3–3, 3–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index options for, 3–4 prestressed, 3–14 prestressed, large deflection, 3–15 procedure, 3–1 modal damping, 5–36, 6–3 modal solution obtaining, 5–13 single-point response spectrum analysis, 6–3 mode combination methods, 6–6 mode extraction methods QR Damped, 6–3 mode numbers, 2–7 mode superposition harmonic response analysis, 4–25 mode-extraction methods, 4–25 transient dynamic analysis, 5–13 mode superposition method, 4–3, 5–2 mode superposition transient dynamic analysis obtain the modal solution, 5–13 obtain the mode superposition transient solution, 5–14 mode-extraction methods, 3–3, 3–16 Block Lanczos, 3–3, 3–17, 4–25 damped, 3–3, 3–18 power dynamics, 3–3, 3–17 QR Damped, 3–3, 3–19, 4–25, 4–25, 5–13, 5–14 reduced, 3–3, 3–18 subspace, 3–3, 3–17 unsymmetric, 3–3, 3–18 mode-frequency analysis, 3–1 model geometry defining, 15–4 modeling the crack region, 12–1 modes expanding, 3–8 number of, 3–8 number to expand, 3–4 number to extract, 3–4 Mohr-Coulomb, 8–10 MONITOR command changes from SOLCONTROL, 8–55 Mooney-Rivlin constants, 8–21 MPRS analysis, 6–25 multi-point response spectrum, 6–1 multilinear elastic, 8–8 multilinear elasticity, 8–16 multilinear isotropic hardening, 8–10 multilinear kinematic hardening, 8–10 multipoint constraint, 11–60
N natural frequencies, 3–10
Newton-Raphson, 8–2 Newton-Raphson option, 2–6 Newton-Raphson options, 8–54 nodal coordinate systems p-method, 15–7 nodal forces and moments, 2–11 nodal solution listing format, 4–21 nonlinear analysis tips and guidelines, 8–63 nonlinear behavior causes, 8–1 nonlinear diagnostics, 8–64 nonlinear isotropic hardening, 8–10 nonlinear kinematic hardening, 8–10 nonlinear material properties material curve fitting, 9–1 nonlinear structural analysis automatic time stepping, 8–67 buckling, 7–2 conservative vs. nonconservative, 8–5 creep, 8–29 geometric nonlinearities, 8–6 hyperelasticity, 8–17 interpolation of results, 8–57 levels of operation, 8–2 load directions, 8–6 material nonlinearities, 8–8 nonlinear elements, 8–63 overview, 8–1 plasticity, 8–9 sample transient input, 8–61 swelling, 8–34 termination, 8–59 verifying results, 8–70 viscoelasticity, 8–33 viscoplasticity, 8–32 nonlinear transient analysis procedure, 8–59 number of eigenvalues to be extracted, 7–5 number of harmonic solutions, 4–9 number of integration points per layer, 13–3 number of solutions to expand, 4–21
O obtain the modal solution, 4–25 offsets for sections, 16–2, 17–1 OPNCONTROL command changes through SOLCONTROL, 8–55 output, 8–70 database and results file, 2–2, 3–8, 4–10, 4–21, 5–7, 5–14, 5–24, 7–6, 8–49
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index–7
Index printed, 2–7, 3–8, 4–10, 4–21, 5–14, 5–14, 5–23, 5–24, 7–6, 8–56 output control, 4–10, 5–14, 5–23, 7–6 output controls, 3–6, 3–8, 5–24, 7–5
P p-elements meshing, 15–4 real constants, 15–3 p-level error-estimation range, 15–2 error-estimation techniques, 15–2 p-method, 15–1 benefits of, 15–1 guidelines for meshing, 15–5 internal DOFs, 15–7 load step options, 15–7 loads, 15–7 meshing the model, 15–4 p-element subgrid, 15–12 printing and plotting results, 15–14 querying subgrid results, 15–12, 15–13 reviewing results, 15–12 solving common problems, 15–12 specialized displays and listings, 15–14 status of elements, 15–7 use of solvers, 15–7 using, 15–1 viewing the element model, 15–5 participation factor calculations, 3–6, 6–18 Peirce model, 8–32 penalty stiffness in contact analysis, 11–15 Perzyna model, 8–32 phase angle for expansion, 4–21 phase angle of harmonic loads, 4–5 pilot node in contact analysis, 11–8, 11–43 plastic, 8–8 plasticity, 8–9, 8–68 anisotropic, 8–10 automatic time stepping, 8–9 bilinear isotropic hardening, 8–10 bilinear kinematic hardening, 8–10 cast iron, 8–10 Drucker-Prager, 8–10 Hill anisotropic, 8–10 multilinear isotropic hardening, 8–10 multilinear kinematic hardening, 8–10 nonlinear isotropic hardening, 8–10 nonlinear kinematic hardening, 8–10 rate-dependent, 8–32 Index–8
plastics, 8–33 PLNSOL command with p-elements, 15–14 plotting sections, 16–2, 17–1 POST1, 2–11, 4–11, 4–23, 4–27, 5–11, 5–25, 6–8, 6–22, 7–7, 8–57, 12–5, 14–2 using, 4–12, 5–12 POST26, 2–11, 4–11, 4–21, 4–23, 4–27, 5–11, 5–23, 5–25, 6–23, 8–57 using, 4–12, 5–11 postprocessing fatigue, 14–1 for different analysis (see reviewing results) power dynamics method, 3–3, 3–17 power spectral density (PSD), 6–2 predictor, 8–52 predictor-corrector option, 2–4, 8–52 PRESOL command with p-elements, 15–14 pressure loads in a large-deflection analysis, 8–6 prestress effects calculation, 2–6, 3–4, 7–4 prestressed analysis harmonic response, 4–28 mode superposition harmonic response, 4–29 transient, 5–32 prestressed full transient dynamic analysis procedure, 5–32 prestressed harmonic response analysis procedure, 4–28 prestressed modal analysis, 3–14 prestressed modal analysis of a large deflection, 3–15 prestressed mode superposition harmonic response analysis procedure, 4–29 prestressed mode superposition transient dynamic analysis procedure, 5–33 prestressed reduced transient dynamic analysis procedure, 5–33 printed output, 2–7, 4–10, 4–21, 5–14, 5–14, 5–23, 5–24, 7–6, 8–56 printing and plotting node and element results p-method, 15–14 PRNSOL command with p-elements, 15–14 probabilistic analysis, 6–2 program-selected masters, 3–21 proportional limit, 8–9 PSD analysis, 6–18 PSD type, 6–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index PSD-versus-frequency table, 6–18
Q QR Damped extraction method harmonic analysis, 4–25 QR Damped method gap conditions, 5–14 harmonic analysis, 4–25 modal analysis, 3–3, 3–19 spectrum analysis, 6–3 transient analysis, 5–13, 5–14
R ramped loads, 4–9, 5–7, 5–14, 5–23, 8–60 random vibrations, 6–18 and power spectral density, 6–2 range counting, 14–9 ratcheting effect, 8–10 rate-dependent plasticity , 8–32 ratio creep, 8–55 Rayleigh damping constants, 5–36 reaction forces and moments, 2–11 reading user-defined mesh, 16–2 real constants for layered elements, 13–3 reduced (Householder) method, 3–3 reduced analysis (see matrix reduction) reduced harmonic response analysis expand the solution, 4–21 reduced method, 3–18, 4–2, 5–3 reduced transient dynamic analysis expansion pass, 5–24 load step options, 5–21 obtain the reduced solution, 5–19 review results of expanded solution, 5–25 reference temperature, 2–7 relative stress distributions buckling analysis, 7–7 response PSD calculating, 6–23 response spectrum multi-point, 6–1 single-point, 6–1 type, 6–3 restart control, 2–4 restarts, 8–62 results data from a PSD analysis, 6–22 extrapolation of, 2–7, 4–10, 4–21, 5–24, 8–56
results file output, 2–2, 3–8, 4–10, 4–21, 5–7, 5–14, 5–24, 7–6, 8–49 reviewing results eigenvalue buckling, 7–7 fatigue, 14–9 harmonic response analysis, 4–11, 4–21, 4–27 full method, 4–11 mode superposition method, 4–27 reduced method, 4–21 modal analysis, 3–10 nonlinear static structural, 8–57 nonlinear transient structural, 8–61 reduced harmonic analysis, 4–23 spectrum analysis, 6–8, 6–22 PSD, 6–22 single-point, 6–8 static structural analysis, 2–10 transient dynamic analysis, 5–11, 5–18, 5–23 full method, 5–11 mode superposition method, 5–18 reduced method, 5–23 Rice's model, 8–10 rock, 8–10 rolling, 8–32 rubber, 8–17
S sample buckling analysis command method, 7–12 GUI method, 7–8 sample harmonic response analysis command method, 4–18 GUI method, 4–13 sample input fatigue, 14–9 full transient dynamic analysis, 5–12 harmonic response analysis, 4–24, 4–27 mode superposition method, 4–27 reduced method, 4–24 mode superposition transient analysis, 5–18 nonlinear structural, 8–61 transient, 8–61 spectrum analysis, 6–24 PSD, 6–24 transient dynamic analysis, 5–18 mode superposition method, 5–18 sample modal analysis command method, 3–13 GUI method, 3–12 sample nonlinear analysis command method, 8–79 GUI method, 8–71
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index–9
Index sample p-method analysis command method, 15–18 GUI method, 15–14 sample spectrum analysis command method, 6–16 GUI method, 6–10 sample static analysis command method, 2–24 GUI method, 2–13 sample transient dynamic analysis command method, 5–31 GUI method, 5–26 sandwich structures, 13–4 scaling the load vector, 4–25 .SECT file, 16–6 sections, 16–1, 17–1 associating subtypes with IDs, 16–2, 17–1 creating, 16–2, 16–5, 17–1 beam tool, 16–5 defining dimensions, 16–2, 17–1 geometry data of, 16–3, 17–2 libraries of, 16–9, 17–5 meshing a line for, 16–4 solid, 16–4 thin wall, 16–4 shakedown effect, 8–10 shape memory alloy, 8–31 SHELL command with p-elements, 15–14 shells, 17–1 shift point for eigenvalue calculation, 7–5 significant modes expanding, 6–6 single solution to expand, 5–24 single-point response spectrum, 6–1 acceleration response, 6–6 CQC mode combination method, 6–6 displacement response, 6–6 DSUM mode combination method, 6–6 expanding significant modes, 6–6 GRP mode combination method, 6–6 mode combination methods, 6–6 NRLSUM mode combination method, 6–6 procedure, 6–2 SRSS mode combination method, 6–6 velocity response, 6–6 single-point spectrum analysis load step option for, 6–3 singular elements, 12–1 slave DOF, 3–19 small deflection, 8–6 small strain analyses, 8–6
Index–10
S-N curve, 14–2 soil, 8–10 solid sections, 16–4 solution obtain the mode superposition transient solution, 5–14 solution controls, 8–48 solution controls dialog box full transient analysis, 5–6, 5–6, 5–6 defining analysis type and options, 5–6 static analysis, 2–2 solution listing format, 4–4 solution method harmonic response, 4–4 solution methods, 4–2, 5–2 full, 4–2, 5–2 transient dynamic analysis, 4–2 mode superposition, 4–3, 5–2 reduced, 4–2, 5–3 solution termination, 2–5 solutions to be expanded, 5–24 solver, memory saving option, 8–50 solvers equation, 2–4, 8–50, 15–7 sparse direct solver, 4–4 specifying a p-level range, 15–2 specifying mesh controls, 15–4 spectral-value-versus-frequency curve, 6–3 spectrum, 6–1 spectrum analysis, 5–36, 6–1, 6–1 DDAM, 6–25 multi-point, 6–25 PSD, 6–18, 6–24 procedure, 6–18 sample input, 6–24 random vibration (PSD), 6–18 obtain the spectrum solution, 6–18 single-point, 6–2 procedure, 6–2 single-point response, 6–3, 6–3, 6–6 expand the modes, 6–6 obtain the modal solution, 6–3 obtain the spectrum solution, 6–3 spectrum data, 6–18 spectrum solution random vibration (PSD) analysis, 6–18 single-point response spectrum analysis, 6–3 spectrum type single-point response, 6–3 spin softening, 8–8 stability analysis, 7–1 static solution
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index buckling analysis, 7–4 static structural analysis, 2–1 loading, 2–8 procedure, 2–1 stepped loads, 4–9, 5–7, 5–14, 5–23, 8–60 stiffness matrix memory saving option, 8–50 strain creep, 8–29 strain energy, 12–6 strain rate creep, 8–29 strain rate effect, 2–4 stress calculations, 3–8, 4–21 stress concentration factors, 14–2 stress intensity factors, 12–1, 12–5 stress pass (see expansion pass) stress relaxation, 8–29 stress singularities accounting for in p-method, 15–7 PEXCLUDE command, 15–7 PINCLUDE command, 15–7 stress stiffening, 8–7 stress stiffening effects, 2–5, 5–32, 8–53 structural analyses buckling, 7–1 fatigue, 14–1 harmonic response, 4–1 modal, 3–1 nonlinear, 8–1 spectrum, 6–1 static, 2–1 transient dynamic, 5–1 structural analysis, 1–1 element types, 1–2 nonlinear, 8–1 structural energy error estimation, 2–11 STURM number, 3–7 subgrid results, 15–13 subspace method, 3–3, 3–17 substeps, 8–2, 8–5, 8–49 swelling, 8–8, 8–34 swelling subroutine, 8–34
T TABLE array parameters, 2–8 tabular listings, 2–11, 3–11, 4–12, 6–8, 8–57 tapered beams, 16–8 termination solution, 2–5 thin wall sections, 16–4 time, 5–23, 5–32
arc-length, 8–68 time integration effects, 5–7, 5–32, 8–60, 8–60 time step optimization thermal, 8–55 time steps, 8–2, 8–5, 8–6, 8–49 automatic, 2–2, 5–7, 5–35, 7–2, 8–51 number of, 2–2, 5–7, 8–67, 8–68 size of, 2–2, 5–7, 8–67 TOLER [CNVTOL], 8–51 transient dynamic analysis, 5–1 full method, 5–3 procedure, 5–3 load step options for, 5–10 methods of solution, 5–2 mode superposition method, 5–13 procedure, 5–13 preparing for, 5–1 prestressed, 5–32 reduced method, 5–19, 5–19 procedure, 5–19 reduced solution, 5–19 transient integration parameters, 5–7, 5–14, 5–22, 8–60 true strain, 8–7 true stress, 8–7, 8–7 Tsai-Wu failure criterion, 13–5
U unsymmetric method, 3–3, 3–18 user defined material, 8–16 user mesh files, 16–9 USERSW, 8–34
V vector displays, 2–11, 6–8 vector norms, 8–51 vector plots, 4–12 vibration analysis, 3–1 virtual crack extension method, 12–8 viscoelastic material curve fitting, 9–14 viscoelasticity, 8–8, 8–33 element types, 8–33 viscoplasticity, 8–8, 8–32, 8–32 element types, 8–32 large strain, 8–32 Voce hardening law, 8–10
W wave propagation effects, 5–33 writing user mesh, 16–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index–11
Index
Y yield point, 8–9
Index–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
001972 April 2004
ANSYS, Inc. is a UL registered ISO 9001: 2000 Company
Structural Analysis Guide ANSYS Release 8.1
ANSYS, Inc. Southpointe 275 Technology Drive Canonsburg, PA 15317 [email protected] http://www.ansys.com (T) 724-746-3304 (F) 724-514-9494
Revision History Number 001612 001695* 001788* 001901* 001972*
Release ANSYS 6.1 ANSYS 7.0 ANSYS 7.1 ANSYS 8.0 ANSYS 8.1
Date April 2002 October 2002 May 2003 October 2003 April 2004
* ANSYS Documentation on CD.
Trademark Information ANSYS, DesignSpace, DesignModeler, ANSYS DesignXplorer VT, ANSYS DesignXplorer, ANSYS Emax, ANSYS Workbench environment, CFX, AI*Environment, CADOE and any and all ANSYS, Inc. product names referenced on any media, manual or the like, are registered trademarks or trademarks of subsidiaries of ANSYS, Inc. located in the United States or other countries. Copyright © 2004 SAS IP, Inc. All rights reserved. Unpublished rights reserved under the Copyright Laws of the United States. ANSYS, Inc. is a UL registered ISO 9001: 2000 Company ANSYS Inc. products may contain U.S. Patent No. 6,055,541 Microsoft, Windows, Windows 2000 and Windows XP are registered trademarks of Microsoft Corporation. Inventor and Mechanical Desktop are registered trademarks of Autodesk, Inc. SolidWorks is a registered trademark of SolidWorks Corporation. Pro/ENGINEER is a registered trademark of Parametric Technology Corporation. Unigraphics, Solid Edge and Parasolid are registered trademarks of Electronic Data Systems Corporation (EDS). ACIS and ACIS Geometric Modeler are registered trademarks of Spatial Technology, Inc. "FLEXlm License Manager" is a trademark of Macrovision Corporation. Other product and company names mentioned herein are the trademarks or registered trademarks of their respective owners. This ANSYS, Inc. software product and program documentation is ANSYS Confidential Information and are furnished by ANSYS, Inc. under an ANSYS software license agreement that contains provisions concerning non-disclosure, copying, length and nature of use, warranties, disclaimers and remedies, and other provisions. The Program and Documentation may be used or copied only in accordance with the terms of that license agreement. See the ANSYS, Inc. online documentation or the ANSYS, Inc. documentation CD for the complete Legal Notice. If this is a copy of a document published by and reproduced with the permission of ANSYS, Inc., it might not reflect the organization or physical appearance of the original. ANSYS, Inc. is not liable for any errors or omissions introduced by the copying process. Such errors are the responsibility of the party providing the copy.
Table of Contents 1. Overview of Structural Analyses ......................................................................................................... 1–1 1.1. Definition of Structural Analysis .................................................................................................... 1–1 1.2. Types of Structural Analysis ........................................................................................................... 1–1 1.3. Elements Used in Structural Analyses ............................................................................................ 1–2 1.4. Material Model Interface ............................................................................................................... 1–2 1.5. Types of Solution Methods ............................................................................................................ 1–2 2. Structural Static Analysis .................................................................................................................... 2–1 2.1. Definition of Static Analysis ........................................................................................................... 2–1 2.2. Linear vs. Nonlinear Static Analyses ............................................................................................... 2–1 2.3. Performing a Static Analysis .......................................................................................................... 2–1 2.3.1. Build the Model ................................................................................................................... 2–1 2.3.1.1. Points to Remember .................................................................................................... 2–1 2.3.2. Set Solution Controls ............................................................................................................ 2–2 2.3.2.1. Access the Solution Controls Dialog Box ...................................................................... 2–2 2.3.2.2. Using the Basic Tab ..................................................................................................... 2–2 2.3.2.3. The Transient Tab ........................................................................................................ 2–3 2.3.2.4. Using the Sol'n Options Tab ......................................................................................... 2–4 2.3.2.5. Using the Nonlinear Tab .............................................................................................. 2–4 2.3.2.6. Using the Advanced NL Tab ......................................................................................... 2–5 2.3.3. Set Additional Solution Options ........................................................................................... 2–5 2.3.3.1. Stress Stiffening Effects ................................................................................................ 2–5 2.3.3.2. Newton-Raphson Option ............................................................................................. 2–6 2.3.3.3. Prestress Effects Calculation ......................................................................................... 2–6 2.3.3.4. Mass Matrix Formulation ............................................................................................. 2–6 2.3.3.5. Reference Temperature ............................................................................................... 2–7 2.3.3.6. Mode Number ............................................................................................................. 2–7 2.3.3.7. Creep Criteria .............................................................................................................. 2–7 2.3.3.8. Printed Output ............................................................................................................ 2–7 2.3.3.9. Extrapolation of Results ............................................................................................... 2–7 2.3.4. Apply the Loads ................................................................................................................... 2–7 2.3.4.1. Load Types .................................................................................................................. 2–7 2.3.4.1.1. Displacements (UX, UY, UZ, ROTX, ROTY, ROTZ) ................................................... 2–7 2.3.4.1.2. Forces (FX, FY, FZ) and Moments (MX, MY, MZ) .................................................... 2–7 2.3.4.1.3. Pressures (PRES) .................................................................................................. 2–8 2.3.4.1.4. Temperatures (TEMP) .......................................................................................... 2–8 2.3.4.1.5. Fluences (FLUE) .................................................................................................. 2–8 2.3.4.1.6. Gravity, Spinning, Etc. ......................................................................................... 2–8 2.3.4.2. Apply Loads to the Model ............................................................................................ 2–8 2.3.4.2.1. Applying Loads Using TABLE Type Array Parameters ........................................... 2–8 2.3.4.3. Calculating Inertia Relief .............................................................................................. 2–9 2.3.4.3.1. Inertia Relief Output ............................................................................................ 2–9 2.3.4.3.2. Partial Inertia Relief Calculations .......................................................................... 2–9 2.3.4.3.3. Using a Macro to Perform Inertia Relief Calculations ........................................... 2–10 2.3.5. Solve the Analysis .............................................................................................................. 2–10 2.3.6. Review the Results ............................................................................................................. 2–10 2.3.6.1. Postprocessors .......................................................................................................... 2–11 2.3.6.2. Points to Remember .................................................................................................. 2–11 2.3.6.3. Reviewing Results Data .............................................................................................. 2–11 2.3.6.4. Typical Postprocessing Operations ............................................................................. 2–11 2.4. A Sample Static Analysis (GUI Method) ........................................................................................ 2–13 Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 2.4.1. Problem Description .......................................................................................................... 2–13 2.4.2. Problem Specifications ....................................................................................................... 2–13 2.4.3. Problem Sketch .................................................................................................................. 2–14 2.4.3.1. Set the Analysis Title .................................................................................................. 2–14 2.4.3.2. Set the System of Units .............................................................................................. 2–14 2.4.3.3. Define Parameters ..................................................................................................... 2–14 2.4.3.4. Define the Element Types .......................................................................................... 2–15 2.4.3.5. Define Material Properties ......................................................................................... 2–15 2.4.3.6. Create Hexagonal Area as Cross-Section ..................................................................... 2–15 2.4.3.7. Create Keypoints Along a Path ................................................................................... 2–16 2.4.3.8. Create Lines Along a Path .......................................................................................... 2–16 2.4.3.9. Create Line from Shank to Handle .............................................................................. 2–17 2.4.3.10. Cut Hex Section ....................................................................................................... 2–17 2.4.3.11. Set Meshing Density ................................................................................................ 2–17 2.4.3.12. Set Element Type for Area Mesh ............................................................................... 2–17 2.4.3.13. Generate Area Mesh ................................................................................................ 2–18 2.4.3.14. Drag the 2-D Mesh to Produce 3-D Elements ............................................................ 2–18 2.4.3.15. Select BOTAREA Component and Delete 2-D Elements ............................................. 2–18 2.4.3.16. Apply Displacement Boundary Condition at End of Wrench ...................................... 2–19 2.4.3.17. Display Boundary Conditions ................................................................................... 2–19 2.4.3.18. Apply Pressure on Handle ........................................................................................ 2–19 2.4.3.19. Write the First Load Step .......................................................................................... 2–21 2.4.3.20. Define Downward Pressure ...................................................................................... 2–21 2.4.3.21. Write Second Load Step ........................................................................................... 2–22 2.4.3.22. Solve from Load Step Files ....................................................................................... 2–22 2.4.3.23. Read First Load Step and Review Results .................................................................. 2–22 2.4.3.24. Read the Next Load Step and Review Results ............................................................ 2–23 2.4.3.25. Zoom in on Cross-Section ........................................................................................ 2–23 2.4.3.26. Exit ANSYS ............................................................................................................... 2–23 2.5. A Sample Static Analysis (Command or Batch Method) ................................................................ 2–24 2.6. Where to Find Other Examples .................................................................................................... 2–26 3. Modal Analysis .................................................................................................................................... 3–1 3.1. Definition of Modal Analysis .......................................................................................................... 3–1 3.2. Uses for Modal Analysis ................................................................................................................. 3–1 3.3. Overview of Steps in a Modal Analysis ........................................................................................... 3–1 3.4. Build the Model ............................................................................................................................ 3–1 3.5. Apply Loads and Obtain the Solution ............................................................................................ 3–2 3.5.1. Enter the Solution Processor ................................................................................................. 3–2 3.5.2. Define Analysis Type and Options ......................................................................................... 3–2 3.5.2.1. Option: New Analysis [ANTYPE] .................................................................................... 3–2 3.5.2.2. Option: Analysis Type: Modal [ANTYPE] ........................................................................ 3–3 3.5.2.3. Option: Mode-Extraction Method [MODOPT] ............................................................... 3–3 3.5.2.4. Option: Number of Modes to Extract [MODOPT] ........................................................... 3–4 3.5.2.5. Option: Number of Modes to Expand [MXPAND] .......................................................... 3–4 3.5.2.6. Option: Mass Matrix Formulation [LUMPM] .................................................................. 3–4 3.5.2.7. Option: Prestress Effects Calculation [PSTRES] .............................................................. 3–4 3.5.2.8. Additional Modal Analysis Options .............................................................................. 3–4 3.5.3. Define Master Degrees of Freedom ....................................................................................... 3–4 3.5.4. Apply Loads ......................................................................................................................... 3–5 3.5.4.1. Applying Loads Using Commands ............................................................................... 3–5 3.5.4.2. Applying Loads Using the GUI ..................................................................................... 3–5 3.5.4.3. Listing Loads ............................................................................................................... 3–6
vi
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 3.5.5. Specify Load Step Options .................................................................................................... 3–6 3.5.6. Participation Factor Table Output ......................................................................................... 3–6 3.5.7. Solve ................................................................................................................................... 3–7 3.5.7.1. Output ........................................................................................................................ 3–7 3.5.7.1.1. Output From Subspace Mode-Extraction Method ................................................ 3–7 3.5.8. Exit the Solution Processor ................................................................................................... 3–8 3.6. Expand the Modes ........................................................................................................................ 3–8 3.6.1. Points to Remember ............................................................................................................ 3–8 3.6.2. Expanding the Modes .......................................................................................................... 3–8 3.7. Review the Results ...................................................................................................................... 3–10 3.7.1. Points to Remember ........................................................................................................... 3–10 3.7.2. Reviewing Results Data ...................................................................................................... 3–10 3.7.3. Option: Listing All Frequencies ........................................................................................... 3–10 3.7.4. Option: Display Deformed Shape ........................................................................................ 3–11 3.7.5. Option: List Master DOF ...................................................................................................... 3–11 3.7.6. Option: Line Element Results .............................................................................................. 3–11 3.7.7. Option: Contour Displays ................................................................................................... 3–11 3.7.8. Option: Tabular Listings ...................................................................................................... 3–11 3.7.9. Other Capabilities .............................................................................................................. 3–12 3.8. A Sample Modal Analysis (GUI Method) ....................................................................................... 3–12 3.8.1. Problem Description .......................................................................................................... 3–12 3.8.2. Problem Specifications ....................................................................................................... 3–12 3.8.3. Problem Sketch .................................................................................................................. 3–12 3.9. A Sample Modal Analysis (Command or Batch Method) ............................................................... 3–13 3.10. Where to Find Other Examples .................................................................................................. 3–14 3.11. Prestressed Modal Analysis ....................................................................................................... 3–14 3.12. Prestressed Modal Analysis of a Large-Deflection Solution ......................................................... 3–15 3.13. Comparing Mode-Extraction Methods ....................................................................................... 3–16 3.13.1. Block Lanczos Method ...................................................................................................... 3–17 3.13.2. Subspace Method ............................................................................................................ 3–17 3.13.3. PowerDynamics Method .................................................................................................. 3–17 3.13.4. Reduced Method .............................................................................................................. 3–18 3.13.5. Unsymmetric Method ....................................................................................................... 3–18 3.13.6. Damped Method .............................................................................................................. 3–18 3.13.6.1. Damped Method-Real and Imaginary Parts of the Eigenvalue ................................... 3–18 3.13.6.2. Damped Method-Real and Imaginary Parts of the Eigenvector .................................. 3–18 3.13.7. QR Damped Method ........................................................................................................ 3–19 3.14. Matrix Reduction ...................................................................................................................... 3–19 3.14.1. Theoretical Basis of Matrix Reduction ................................................................................ 3–19 3.14.1.1. Guidelines for Selecting Master DOF ........................................................................ 3–19 3.14.1.2. A Note About Program-Selected Masters .................................................................. 3–21 4. Harmonic Response Analysis .............................................................................................................. 4–1 4.1. Definition of Harmonic Response Analysis ..................................................................................... 4–1 4.2. Uses for Harmonic Response Analysis ............................................................................................ 4–1 4.3. Commands Used in a Harmonic Response Analysis ........................................................................ 4–2 4.4. The Three Solution Methods ......................................................................................................... 4–2 4.4.1. The Full Method ................................................................................................................... 4–2 4.4.2. The Reduced Method ........................................................................................................... 4–2 4.4.3. The Mode Superposition Method ......................................................................................... 4–3 4.4.4. Restrictions Common to All Three Methods .......................................................................... 4–3 4.5. How to Do Harmonic Response Analysis ........................................................................................ 4–3 4.5.1. Full Harmonic Response Analysis .......................................................................................... 4–3
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
vii
Structural Analysis Guide 4.5.2. Build the Model ................................................................................................................... 4–4 4.5.2.1. Points to Remember .................................................................................................... 4–4 4.5.3. Apply Loads and Obtain the Solution ................................................................................... 4–4 4.5.3.1. Enter the ANSYS Solution Processor ............................................................................. 4–4 4.5.3.2. Define the Analysis Type and Options .......................................................................... 4–4 4.5.3.3. Apply Loads on the Model ........................................................................................... 4–5 4.5.3.3.1. Applying Loads Using Commands ....................................................................... 4–8 4.5.3.3.2. Applying Loads and Listing Loads Using the GUI ................................................. 4–9 4.5.3.4. Specify Load Step Options ........................................................................................... 4–9 4.5.3.4.1. General Options .................................................................................................. 4–9 4.5.3.4.2. Dynamics Options ............................................................................................. 4–10 4.5.3.4.3. Output Controls ................................................................................................ 4–10 4.5.3.5. Save a Backup Copy of the Database to a Named File ................................................. 4–11 4.5.3.6. Start Solution Calculations ......................................................................................... 4–11 4.5.3.7. Repeat for Additional Load Steps ............................................................................... 4–11 4.5.3.8. Leave SOLUTION ....................................................................................................... 4–11 4.5.4. Review the Results ............................................................................................................. 4–11 4.5.4.1. Postprocessors .......................................................................................................... 4–11 4.5.4.2. Points to Remember .................................................................................................. 4–11 4.5.4.3. Using POST26 ............................................................................................................ 4–12 4.5.4.4. Using POST1 .............................................................................................................. 4–12 4.6. Sample Harmonic Response Analysis (GUI Method) ..................................................................... 4–13 4.6.1. Problem Description .......................................................................................................... 4–13 4.6.2. Problem Specifications ....................................................................................................... 4–13 4.6.3. Problem Diagram ............................................................................................................... 4–14 4.6.3.1. Set the Analysis Title .................................................................................................. 4–14 4.6.3.2. Define the Element Types .......................................................................................... 4–14 4.6.3.3. Define the Real Constants .......................................................................................... 4–15 4.6.3.4. Create the Nodes ....................................................................................................... 4–15 4.6.3.5. Create the Spring Elements ........................................................................................ 4–15 4.6.3.6. Create the Mass Elements .......................................................................................... 4–16 4.6.3.7. Specify the Analysis Type, MDOF, and Load Step Specifications .................................. 4–16 4.6.3.8. Define Loads and Boundary Conditions ...................................................................... 4–16 4.6.3.9. Solve the Model ........................................................................................................ 4–17 4.6.3.10. Review the Results ................................................................................................... 4–17 4.6.3.11. Exit ANSYS ............................................................................................................... 4–18 4.7. Sample Harmonic Response Analysis (Command or Batch Method) ............................................. 4–18 4.8. Where to Find Other Examples .................................................................................................... 4–19 4.9. Reduced Harmonic Response Analysis ......................................................................................... 4–20 4.9.1. Apply Loads and Obtain the Reduced Solution ................................................................... 4–20 4.9.2. Review the Results of the Reduced Solution ........................................................................ 4–21 4.9.3. Expand the Solution (Expansion Pass) ................................................................................. 4–21 4.9.3.1. Points to Remember .................................................................................................. 4–21 4.9.3.2. Expanding the Modes ................................................................................................ 4–21 4.9.4. Review the Results of the Expanded Solution ...................................................................... 4–23 4.9.5. Sample Input ..................................................................................................................... 4–24 4.10. Mode Superposition Harmonic Response Analysis ..................................................................... 4–25 4.10.1. Obtain the Modal Solution ................................................................................................ 4–25 4.10.2. Obtain the Mode Superposition Harmonic Solution .......................................................... 4–25 4.10.3. Expand the Mode Superposition Solution ......................................................................... 4–27 4.10.4. Review the Results ........................................................................................................... 4–27 4.10.5. Sample Input ................................................................................................................... 4–27
viii
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 4.11. Other Analysis Details ............................................................................................................... 4–28 4.11.1. Prestressed Harmonic Response Analysis .......................................................................... 4–28 4.11.1.1. Prestressed Full Harmonic Response Analysis ........................................................... 4–28 4.11.1.2. Prestressed Reduced Harmonic Response Analysis ................................................... 4–29 4.11.1.3. Prestressed Mode Superposition Harmonic Response Analysis ................................. 4–29 5. Transient Dynamic Analysis ................................................................................................................ 5–1 5.1. Definition of Transient Dynamic Analysis ....................................................................................... 5–1 5.2. Preparing for a Transient Dynamic Analysis ................................................................................... 5–1 5.3. Three Solution Methods ................................................................................................................ 5–2 5.3.1. Full Method ......................................................................................................................... 5–2 5.3.2. Mode Superposition Method ................................................................................................ 5–2 5.3.3. Reduced Method ................................................................................................................. 5–3 5.4. Performing a Full Transient Dynamic Analysis ................................................................................ 5–3 5.4.1. Build the Model ................................................................................................................... 5–4 5.4.1.1. Points to Remember .................................................................................................... 5–4 5.4.2. Establish Initial Conditions ................................................................................................... 5–4 5.4.3. Set Solution Controls ............................................................................................................ 5–6 5.4.3.1. Access the Solution Controls Dialog Box ...................................................................... 5–6 5.4.3.2. Using the Basic Tab ..................................................................................................... 5–7 5.4.3.3. Using the Transient Tab ............................................................................................... 5–7 5.4.3.4. Using the Remaining Solution Controls Tabs ................................................................ 5–8 5.4.4. Set Additional Solution Options ........................................................................................... 5–8 5.4.4.1. Prestress Effects ........................................................................................................... 5–9 5.4.4.2. Damping Option ......................................................................................................... 5–9 5.4.4.3. Mass Matrix Formulation ............................................................................................. 5–9 5.4.5. Apply the Loads ................................................................................................................... 5–9 5.4.6. Save the Load Configuration for the Current Load Step ....................................................... 5–10 5.4.7. Repeat Steps 3-6 for Each Load Step ................................................................................... 5–10 5.4.8. Save a Backup Copy of the Database .................................................................................. 5–10 5.4.9. Start the Transient Solution ................................................................................................ 5–10 5.4.10. Exit the Solution Processor ............................................................................................... 5–11 5.4.11. Review the Results ........................................................................................................... 5–11 5.4.11.1. Postprocessors ........................................................................................................ 5–11 5.4.11.2. Points to Remember ................................................................................................ 5–11 5.4.11.3. Using POST26 .......................................................................................................... 5–11 5.4.11.4. Other Capabilities .................................................................................................... 5–12 5.4.11.5. Using POST1 ............................................................................................................ 5–12 5.4.12. Sample Input for a Full Transient Dynamic Analysis ........................................................... 5–12 5.5. Performing a Mode Superposition Transient Dynamic Analysis .................................................... 5–13 5.5.1. Build the Model .................................................................................................................. 5–13 5.5.2. Obtain the Modal Solution ................................................................................................. 5–13 5.5.3. Obtain the Mode Superposition Transient Solution ............................................................. 5–14 5.5.3.1. Points to Remember .................................................................................................. 5–14 5.5.3.2. Obtaining the Solution .............................................................................................. 5–14 5.5.4. Expand the Mode Superposition Solution ........................................................................... 5–18 5.5.5. Review the Results ............................................................................................................. 5–18 5.5.6. Sample Input for a Mode Superposition Transient Dynamic Analysis ................................... 5–18 5.6. Performing a Reduced Transient Dynamic Analysis ...................................................................... 5–19 5.6.1. Obtain the Reduced Solution .............................................................................................. 5–19 5.6.1.1. Define the Analysis Type and Options ........................................................................ 5–20 5.6.1.2. Define Master Degrees of Freedom ............................................................................ 5–20 5.6.1.3. Define Gap Conditions ............................................................................................... 5–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
ix
Structural Analysis Guide 5.6.1.3.1. Gap Conditions ................................................................................................. 5–20 5.6.1.4. Apply Initial Conditions to the Model ......................................................................... 5–21 5.6.1.4.1. Dynamics Options ............................................................................................. 5–22 5.6.1.4.2. General Options ................................................................................................ 5–22 5.6.1.4.3. Output Control Options .................................................................................... 5–23 5.6.1.5. Write the First Load Step to a Load Step File ............................................................... 5–23 5.6.1.6. Specify Loads and Load Step Options ......................................................................... 5–23 5.6.1.7. Obtaining the Solution .............................................................................................. 5–23 5.6.2. Review the Results of the Reduced Solution ........................................................................ 5–23 5.6.3. Expand the Solution (Expansion Pass) ................................................................................. 5–24 5.6.3.1. Points to Remember .................................................................................................. 5–24 5.6.3.2. Expanding the Solution ............................................................................................. 5–24 5.6.4. Review the Results of the Expanded Solution ...................................................................... 5–25 5.7. Sample Reduced Transient Dynamic Analysis (GUI Method) ......................................................... 5–26 5.7.1. Problem Description .......................................................................................................... 5–26 5.7.2. Problem Specifications ....................................................................................................... 5–26 5.7.3. Problem Sketch .................................................................................................................. 5–27 5.7.3.1. Specify the Title ......................................................................................................... 5–27 5.7.3.2. Define Element Types ................................................................................................ 5–27 5.7.3.3. Define Real Constants ................................................................................................ 5–27 5.7.3.4. Define Material Properties ......................................................................................... 5–28 5.7.3.5. Define Nodes ............................................................................................................ 5–28 5.7.3.6. Define Elements ........................................................................................................ 5–28 5.7.3.7. Define Analysis Type and Analysis Options ................................................................. 5–29 5.7.3.8. Define Master Degrees of Freedom ............................................................................ 5–29 5.7.3.9. Set Load Step Options ............................................................................................... 5–29 5.7.3.10. Apply Loads for the First Load Step .......................................................................... 5–29 5.7.3.11. Specify Output ........................................................................................................ 5–29 5.7.3.12. Solve the First Load Step .......................................................................................... 5–30 5.7.3.13. Apply Loads for the Next Load Step .......................................................................... 5–30 5.7.4. Solve the Next Load Step .................................................................................................... 5–30 5.7.4.1. Set the Next Time Step and Solve ............................................................................... 5–30 5.7.4.2. Run the Expansion Pass and Solve .............................................................................. 5–30 5.7.4.3. Review the Results in POST26 .................................................................................... 5–31 5.7.4.4. Review the Results in POST1 ...................................................................................... 5–31 5.7.4.5. Exit ANSYS ................................................................................................................. 5–31 5.8. Sample Reduced Transient Dynamic Analysis (Command or Batch Method) ................................. 5–31 5.9. Performing a Prestressed Transient Dynamic Analysis .................................................................. 5–32 5.9.1. Prestressed Full Transient Dynamic Analysis ........................................................................ 5–32 5.9.2. Prestressed Mode Superposition Transient Dynamic Analysis .............................................. 5–33 5.9.3. Prestressed Reduced Transient Dynamic Analysis ................................................................ 5–33 5.10. Other Analysis Details ............................................................................................................... 5–33 5.10.1. Guidelines for Integration Time Step ................................................................................. 5–33 5.10.2. Automatic Time Stepping ................................................................................................. 5–35 5.10.3. Damping .......................................................................................................................... 5–36 5.11. Where to Find Other Examples .................................................................................................. 5–40 6. Spectrum Analysis ............................................................................................................................... 6–1 6.1. Definition of Spectrum Analysis .................................................................................................... 6–1 6.2. What is a Spectrum? ..................................................................................................................... 6–1 6.2.1. Response Spectrum ............................................................................................................. 6–1 6.2.1.1. Single-Point Response Spectrum (SPRS) ....................................................................... 6–1 6.2.1.2. Multi-Point Response Spectrum (MPRS) ....................................................................... 6–1
x
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 6.2.2. Dynamic Design Analysis Method (DDAM) ............................................................................ 6–2 6.2.3. Power Spectral Density ........................................................................................................ 6–2 6.2.4. Deterministic vs. Probabilistic Analyses ................................................................................. 6–2 6.3. Steps in a Single-Point Response Spectrum (SPRS) Analysis ............................................................ 6–2 6.3.1. Build the Model ................................................................................................................... 6–3 6.3.1.1. Points to Remember .................................................................................................... 6–3 6.3.2. Obtain the Modal Solution ................................................................................................... 6–3 6.3.3. Obtain the Spectrum Solution .............................................................................................. 6–3 6.3.4. Expand the Modes ............................................................................................................... 6–6 6.3.5. Combine the Modes ............................................................................................................. 6–6 6.3.6. Review the Results ............................................................................................................... 6–8 6.4. Sample Spectrum Analysis (GUI Method) ..................................................................................... 6–10 6.4.1. Problem Description .......................................................................................................... 6–10 6.4.2. Problem Specifications ....................................................................................................... 6–10 6.4.3. Problem Sketch .................................................................................................................. 6–11 6.4.4. Procedure .......................................................................................................................... 6–11 6.4.4.1. Set the Analysis Title .................................................................................................. 6–11 6.4.4.2. Define the Element Type ............................................................................................ 6–11 6.4.4.3. Define the Real Constants .......................................................................................... 6–11 6.4.4.4. Define Material Properties ......................................................................................... 6–12 6.4.4.5. Define Keypoints and Line ......................................................................................... 6–12 6.4.4.6. Set Global Element Density and Mesh Line ................................................................. 6–12 6.4.4.7. Set Boundary Conditions ........................................................................................... 6–13 6.4.4.8. Specify Analysis Type and Options ............................................................................. 6–13 6.4.4.9. Solve the Modal Analysis ........................................................................................... 6–13 6.4.4.10. Set Up the Spectrum Analysis .................................................................................. 6–13 6.4.4.11. Define Spectrum Value vs. Frequency Table ............................................................. 6–14 6.4.4.12. Solve Spectrum Analysis .......................................................................................... 6–14 6.4.4.13. Set up the Expansion Pass ........................................................................................ 6–14 6.4.4.14. Expand the Modes ................................................................................................... 6–14 6.4.4.15. Start Expansion Pass Calculation .............................................................................. 6–15 6.4.4.16. Set Up Mode Combination for Spectrum Analysis ..................................................... 6–15 6.4.4.17. Select Mode Combination Method ........................................................................... 6–15 6.4.4.18. Combine the Modes ................................................................................................ 6–15 6.4.4.19. Postprocessing: Print Out Nodal, Element, and Reaction Solutions ............................ 6–15 6.4.4.20. Exit ANSYS ............................................................................................................... 6–16 6.5. Sample Spectrum Analysis (Command or Batch Method) ............................................................. 6–16 6.6. Where to Find Other Examples .................................................................................................... 6–17 6.7. How to Do a Random Vibration (PSD) Analysis ............................................................................. 6–18 6.7.1. Expand the Modes ............................................................................................................. 6–18 6.7.2. Obtain the Spectrum Solution ............................................................................................ 6–18 6.7.3. Combine the Modes ........................................................................................................... 6–21 6.7.4. Review the Results ............................................................................................................. 6–22 6.7.4.1. Reviewing the Results in POST1 ................................................................................. 6–22 6.7.4.1.1. Read the Desired Set of Results into the Database .............................................. 6–22 6.7.4.1.2. Display the Results ............................................................................................ 6–23 6.7.4.2. Calculating Response PSDs in POST26 ........................................................................ 6–23 6.7.4.3. Calculating Covariance in POST26 .............................................................................. 6–23 6.7.5. Sample Input ..................................................................................................................... 6–24 6.8. How to Do DDAM Spectrum Analysis .......................................................................................... 6–25 6.9. How to Do Multi-Point Response Spectrum (MPRS) Analysis ........................................................ 6–25 7. Buckling Analysis ................................................................................................................................ 7–1
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xi
Structural Analysis Guide 7.1. Definition of Buckling Analysis ...................................................................................................... 7–1 7.2. Types of Buckling Analyses ........................................................................................................... 7–1 7.2.1. Nonlinear Buckling Analysis .................................................................................................. 7–1 7.2.2. Eigenvalue Buckling Analysis ................................................................................................ 7–1 7.3. Commands Used in a Buckling Analysis ......................................................................................... 7–2 7.4. Procedure for Nonlinear Buckling Analysis ..................................................................................... 7–2 7.4.1. Applying Load Increments ................................................................................................... 7–2 7.4.2. Automatic Time Stepping ..................................................................................................... 7–2 7.4.3. Important ............................................................................................................................ 7–2 7.4.4. Points to Remember ............................................................................................................ 7–3 7.5. Procedure for Eigenvalue Buckling Analysis ................................................................................... 7–3 7.5.1. Build the Model ................................................................................................................... 7–3 7.5.1.1. Points to Remember .................................................................................................... 7–4 7.5.2. Obtain the Static Solution .................................................................................................... 7–4 7.5.3. Obtain the Eigenvalue Buckling Solution .............................................................................. 7–5 7.5.4. Expand the Solution ............................................................................................................. 7–6 7.5.4.1. Points to Remember .................................................................................................... 7–6 7.5.4.2. Expanding the Solution ............................................................................................... 7–6 7.5.5. Review the Results ............................................................................................................... 7–7 7.6. Sample Buckling Analysis (GUI Method) ........................................................................................ 7–8 7.6.1. Problem Description ............................................................................................................ 7–8 7.6.2. Problem Specifications ......................................................................................................... 7–8 7.6.3. Problem Sketch .................................................................................................................... 7–9 7.6.3.1. Set the Analysis Title .................................................................................................... 7–9 7.6.3.2. Define the Element Type ............................................................................................. 7–9 7.6.3.3. Define the Real Constants and Material Properties ...................................................... 7–10 7.6.3.4. Define Nodes and Elements ....................................................................................... 7–10 7.6.3.5. Define the Boundary Conditions ................................................................................ 7–11 7.6.3.6. Solve the Static Analysis ............................................................................................. 7–11 7.6.3.7. Solve the Buckling Analysis ........................................................................................ 7–11 7.6.3.8. Review the Results ..................................................................................................... 7–12 7.6.3.9. Exit ANSYS ................................................................................................................. 7–12 7.7. Sample Buckling Analysis (Command or Batch Method) ............................................................... 7–12 7.8. Where to Find Other Examples .................................................................................................... 7–12 8. Nonlinear Structural Analysis ............................................................................................................. 8–1 8.1. What is Structural Nonlinearity? .................................................................................................... 8–1 8.1.1. Causes of Nonlinear Behavior ............................................................................................... 8–1 8.1.1.1. Changing Status (Including Contact) ............................................................................ 8–2 8.1.1.2. Geometric Nonlinearities ............................................................................................. 8–2 8.1.1.3. Material Nonlinearities ................................................................................................. 8–2 8.1.2. Basic Information About Nonlinear Analyses ......................................................................... 8–2 8.1.2.1. Conservative versus Nonconservative Behavior; Path Dependency ............................... 8–5 8.1.2.2. Substeps ..................................................................................................................... 8–5 8.1.2.3. Load Direction in a Large-Deflection Analysis ............................................................... 8–6 8.1.2.4. Nonlinear Transient Analyses ....................................................................................... 8–6 8.2. Using Geometric Nonlinearities ..................................................................................................... 8–6 8.2.1. Stress-Strain ......................................................................................................................... 8–7 8.2.1.1. Large Deflections with Small Strain .............................................................................. 8–7 8.2.2. Stress Stiffening ................................................................................................................... 8–7 8.2.3. Spin Softening ..................................................................................................................... 8–8 8.3. Modeling Material Nonlinearities .................................................................................................. 8–8 8.3.1. Nonlinear Materials .............................................................................................................. 8–8
xii
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 8.3.1.1. Plasticity ..................................................................................................................... 8–9 8.3.1.1.1. Plastic Material Options ..................................................................................... 8–10 8.3.1.2. Multilinear Elasticity ................................................................................................... 8–16 8.3.1.3. User Defined Material ................................................................................................ 8–16 8.3.1.4. Hyperelasticity .......................................................................................................... 8–17 8.3.1.4.1. Mooney-Rivlin Hyperelastic Option (TB,HYPER) .................................................. 8–18 8.3.1.4.2. Ogden Hyperelastic Option ............................................................................... 8–18 8.3.1.4.3. Neo-Hookean Hyperelastic Option .................................................................... 8–19 8.3.1.4.4. Polynomial Form Hyperelastic Option ............................................................... 8–19 8.3.1.4.5. Arruda-Boyce Hyperelastic Option ..................................................................... 8–19 8.3.1.4.6. Gent Hyperelastic Option .................................................................................. 8–20 8.3.1.4.7. Yeoh Hyperelastic Option ................................................................................. 8–20 8.3.1.4.8. Blatz-Ko Foam Hyperelastic Option ................................................................... 8–20 8.3.1.4.9. Ogden Compressible Foam Hyperelastic Option ................................................ 8–20 8.3.1.4.10. User-Defined Hyperelastic Option ................................................................... 8–21 8.3.1.4.11. Mooney-Rivlin Hyperelastic Option (TB,MOONEY) ............................................ 8–21 8.3.1.5. Creep ........................................................................................................................ 8–29 8.3.1.5.1. Implicit Creep Procedure ................................................................................... 8–30 8.3.1.5.2. Explicit Creep Procedure ................................................................................... 8–31 8.3.1.6. Shape Memory Alloy .................................................................................................. 8–31 8.3.1.7. Viscoplasticity ........................................................................................................... 8–32 8.3.1.8. Viscoelasticity ............................................................................................................ 8–33 8.3.1.9. Swelling .................................................................................................................... 8–34 8.3.2. Material Model Combinations ............................................................................................. 8–35 8.3.2.1. BISO and CHAB Example ............................................................................................ 8–35 8.3.2.2. MISO and CHAB Example ........................................................................................... 8–35 8.3.2.3. NLISO and CHAB Example .......................................................................................... 8–35 8.3.2.4. BISO and RATE Example ............................................................................................. 8–36 8.3.2.5. MISO and RATE Example ............................................................................................ 8–36 8.3.2.6. NLISO and RATE Example ........................................................................................... 8–37 8.3.2.7. BISO and CREEP Example ........................................................................................... 8–37 8.3.2.8. MISO and CREEP Example .......................................................................................... 8–37 8.3.2.9. NLISO and CREEP Example ......................................................................................... 8–38 8.3.2.10. BKIN and CREEP Example ......................................................................................... 8–38 8.3.2.11. HILL and BISO Example ............................................................................................ 8–38 8.3.2.12. HILL and MISO Example ........................................................................................... 8–39 8.3.2.13. HILL and NLISO Example .......................................................................................... 8–39 8.3.2.14. HILL and BKIN Example ............................................................................................ 8–39 8.3.2.15. HILL and MKIN Example ........................................................................................... 8–40 8.3.2.16. HILL and KINH Example ............................................................................................ 8–40 8.3.2.17. HILL and CHAB Example .......................................................................................... 8–41 8.3.2.18. HILL and BISO and CHAB Example ............................................................................ 8–41 8.3.2.19. HILL and MISO and CHAB Example ........................................................................... 8–41 8.3.2.20. HILL and NLISO and CHAB Example .......................................................................... 8–42 8.3.2.21. HILL and RATE and BISO Example ............................................................................. 8–43 8.3.2.22. HILL and RATE and MISO Example ............................................................................ 8–44 8.3.2.23. HILL and RATE and NLISO Example ........................................................................... 8–44 8.3.2.24. HILL and CREEP Example .......................................................................................... 8–45 8.3.2.25. HILL and CREEP and BISO Example ........................................................................... 8–46 8.3.2.26. HILL and CREEP and MISO Example .......................................................................... 8–47 8.3.2.27. HILL and CREEP and NLISO Example ......................................................................... 8–47 8.3.2.28. HILL and CREEP and BKIN Example ........................................................................... 8–47
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xiii
Structural Analysis Guide 8.4. Running a Nonlinear Analysis in ANSYS ....................................................................................... 8–48 8.5. Performing a Nonlinear Static Analysis ........................................................................................ 8–48 8.5.1. Build the Model .................................................................................................................. 8–49 8.5.2. Set Solution Controls .......................................................................................................... 8–49 8.5.2.1. Using the Basic Tab: Special Considerations ............................................................... 8–49 8.5.2.2. Advanced Analysis Options You Can Set on the Solution Controls Dialog Box ............. 8–50 8.5.2.2.1. Equation Solver ................................................................................................ 8–50 8.5.2.3. Advanced Load Step Options You Can Set on the Solution Controls Dialog Box .......... 8–51 8.5.2.3.1. Automatic Time Stepping ................................................................................. 8–51 8.5.2.3.2. Convergence Criteria ........................................................................................ 8–51 8.5.2.3.3. Maximum Number of Equilibrium Iterations ...................................................... 8–52 8.5.2.3.4. Predictor-Corrector Option ............................................................................... 8–52 8.5.2.3.5. Line Search Option ........................................................................................... 8–53 8.5.2.3.6. Cutback Criteria ................................................................................................ 8–53 8.5.3. Set Additional Solution Options .......................................................................................... 8–53 8.5.3.1. Advanced Analysis Options You Cannot Set on the Solution Controls Dialog Box ........ 8–53 8.5.3.1.1. Stress Stiffness .................................................................................................. 8–53 8.5.3.1.2. Newton-Raphson Option .................................................................................. 8–54 8.5.3.2. Advanced Load Step Options You Cannot Set on the Solution Controls Dialog Box ..... 8–55 8.5.3.2.1. Creep Criteria .................................................................................................... 8–55 8.5.3.2.2. Time Step Open Control .................................................................................... 8–55 8.5.3.2.3. Solution Monitoring .......................................................................................... 8–55 8.5.3.2.4. Birth and Death ................................................................................................ 8–56 8.5.3.2.5. Output Control ................................................................................................. 8–56 8.5.4. Apply the Loads ................................................................................................................. 8–56 8.5.5. Solve the Analysis .............................................................................................................. 8–57 8.5.6. Review the Results ............................................................................................................. 8–57 8.5.6.1. Points to Remember .................................................................................................. 8–57 8.5.6.2. Reviewing Results in POST1 ....................................................................................... 8–57 8.5.6.3. Reviewing Results in POST26 ..................................................................................... 8–59 8.5.7. Terminating a Running Job; Restarting ............................................................................... 8–59 8.6. Performing a Nonlinear Transient Analysis ................................................................................... 8–59 8.6.1. Build the Model .................................................................................................................. 8–60 8.6.2. Apply Loads and Obtain the Solution .................................................................................. 8–60 8.6.3. Review the Results ............................................................................................................. 8–61 8.7. Sample Input for a Nonlinear Transient Analysis .......................................................................... 8–61 8.8. Restarts ...................................................................................................................................... 8–62 8.9. Using Nonlinear (Changing-Status) Elements ............................................................................... 8–63 8.9.1. Element Birth and Death .................................................................................................... 8–63 8.10. Tips and Guidelines for Nonlinear Analysis ................................................................................. 8–63 8.10.1. Starting Out with Nonlinear Analysis ................................................................................. 8–63 8.10.1.1. Be Aware of How the Program and Your Structure Behave ........................................ 8–63 8.10.1.2. Keep It Simple ......................................................................................................... 8–64 8.10.1.3. Use an Adequate Mesh Density ................................................................................ 8–64 8.10.1.4. Apply the Load Gradually ......................................................................................... 8–64 8.10.2. Overcoming Convergence Problems ................................................................................. 8–64 8.10.2.1. Performing Nonlinear Diagnostics ............................................................................ 8–65 8.10.2.2. Tracking Convergence Graphically ........................................................................... 8–66 8.10.2.3. Using Automatic Time Stepping ............................................................................... 8–67 8.10.2.4. Using Line Search .................................................................................................... 8–68 8.10.2.5. Using the Arc-Length Method .................................................................................. 8–68 8.10.2.6. Artificially Inhibit Divergence in Your Model's Response ........................................... 8–69
xiv
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 8.10.2.7. Turn Off Extra Element Shapes ................................................................................. 8–70 8.10.2.8. Using Birth and Death Wisely ................................................................................... 8–70 8.10.2.9. Read Your Output .................................................................................................... 8–70 8.10.2.10. Graph the Load and Response History .................................................................... 8–71 8.11. Sample Nonlinear Analysis (GUI Method) ................................................................................... 8–71 8.11.1. Problem Description ........................................................................................................ 8–72 8.11.2. Problem Specifications ..................................................................................................... 8–72 8.11.3. Problem Sketch ................................................................................................................ 8–73 8.11.3.1. Set the Analysis Title and Jobname .......................................................................... 8–73 8.11.3.2. Define the Element Types ........................................................................................ 8–73 8.11.3.3. Define Material Properties ........................................................................................ 8–74 8.11.3.4. Specify the Kinematic Hardening material model (KINH) ........................................... 8–74 8.11.3.5. Label Graph Axes and Plot Data Tables ..................................................................... 8–74 8.11.3.6. Create Rectangle ..................................................................................................... 8–74 8.11.3.7. Set Element Size ...................................................................................................... 8–75 8.11.3.8. Mesh the Rectangle ................................................................................................. 8–75 8.11.3.9. Assign Analysis and Load Step Options .................................................................... 8–75 8.11.3.10. Monitor the Displacement ..................................................................................... 8–75 8.11.3.11. Apply Constraints .................................................................................................. 8–76 8.11.3.12. Solve the First Load Step ........................................................................................ 8–76 8.11.3.13. Solve the Next Six Load Steps ................................................................................. 8–77 8.11.3.14. Review the Monitor File ......................................................................................... 8–77 8.11.3.15. Use the General Postprocessor to Plot Results. ........................................................ 8–77 8.11.3.16. Define Variables for Time-History Postprocessing ................................................... 8–78 8.11.3.17. Plot Time-History Results ....................................................................................... 8–78 8.11.3.18. Exit ANSYS ............................................................................................................. 8–79 8.12. Sample Nonlinear Analysis (Command or Batch Method) ........................................................... 8–79 8.13. Where to Find Other Examples .................................................................................................. 8–82 9. Material Curve Fitting ......................................................................................................................... 9–1 9.1. Applicable Material Behavior Types ............................................................................................... 9–1 9.2. Hyperelastic Material Curve Fitting ................................................................................................ 9–1 9.2.1. Using Curve Fitting to Determine Your Hyperelastic Material Behavior ................................. 9–1 9.2.1.1. Prepare Experimental Data .......................................................................................... 9–2 9.2.1.2. Input the Data into ANSYS ........................................................................................... 9–3 9.2.1.2.1. Batch .................................................................................................................. 9–3 9.2.1.2.2. GUI ..................................................................................................................... 9–3 9.2.1.3. Select a Material Model Option .................................................................................... 9–3 9.2.1.3.1. Batch .................................................................................................................. 9–4 9.2.1.3.2. GUI ..................................................................................................................... 9–4 9.2.1.4. Initialize the Coefficients .............................................................................................. 9–4 9.2.1.4.1. Batch .................................................................................................................. 9–4 9.2.1.4.2. GUI ..................................................................................................................... 9–5 9.2.1.5. Specify Control Parameters and Solve .......................................................................... 9–5 9.2.1.5.1. Batch .................................................................................................................. 9–5 9.2.1.5.2. GUI ..................................................................................................................... 9–5 9.2.1.6. Plot Your Experimental Data and Analyze ..................................................................... 9–6 9.2.1.6.1. Batch .................................................................................................................. 9–6 9.2.1.6.2. GUI ..................................................................................................................... 9–6 9.2.1.6.3. Review/Verify ..................................................................................................... 9–6 9.2.1.7. Write Data to TB Command ......................................................................................... 9–6 9.2.1.7.1. Batch .................................................................................................................. 9–6 9.2.1.7.2. GUI ..................................................................................................................... 9–7
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xv
Structural Analysis Guide 9.3. Creep Material Curve Fitting ......................................................................................................... 9–7 9.3.1. Using Curve Fitting to Determine Your Creep Material Behavior ........................................... 9–7 9.3.1.1. Prepare Experimental Data .......................................................................................... 9–7 9.3.1.2. Input the Data into ANSYS ........................................................................................... 9–9 9.3.1.2.1. Batch .................................................................................................................. 9–9 9.3.1.2.2. GUI ..................................................................................................................... 9–9 9.3.1.3. Select a Material Model Option .................................................................................... 9–9 9.3.1.3.1. Batch .................................................................................................................. 9–9 9.3.1.3.2. GUI ................................................................................................................... 9–10 9.3.1.4. Initialize the Coefficients ............................................................................................ 9–10 9.3.1.4.1. Batch ................................................................................................................ 9–10 9.3.1.4.2. GUI ................................................................................................................... 9–11 9.3.1.5. Specify Control Parameters and Solve ........................................................................ 9–11 9.3.1.5.1. Batch ................................................................................................................ 9–11 9.3.1.5.2. GUI ................................................................................................................... 9–11 9.3.1.6. Plot the Experimental Data and Analyze ..................................................................... 9–11 9.3.1.6.1. Batch ................................................................................................................ 9–12 9.3.1.6.2. GUI ................................................................................................................... 9–12 9.3.1.6.3. Analyze Your Curves for Proper Fit ..................................................................... 9–12 9.3.1.7. Write Data to TB Command ....................................................................................... 9–12 9.3.1.7.1. Batch ................................................................................................................ 9–12 9.3.1.7.2. GUI ................................................................................................................... 9–12 9.3.2. Tips For Curve Fitting Creep Models ................................................................................... 9–12 9.4. Viscoelastic Material Curve Fitting ............................................................................................... 9–14 9.4.1. Using Curve Fitting to Determine the Coefficients of Viscoelastic Material Model ................. 9–14 9.4.1.1. Prepare Experimental Data ........................................................................................ 9–15 9.4.1.2. Input the Data into ANSYS ......................................................................................... 9–16 9.4.1.2.1. Batch ................................................................................................................ 9–16 9.4.1.2.2. GUI ................................................................................................................... 9–16 9.4.1.3. Select a Material Model Option .................................................................................. 9–16 9.4.1.3.1. Batch ................................................................................................................ 9–17 9.4.1.3.2. GUI ................................................................................................................... 9–17 9.4.1.4. Initialize the Coefficients ............................................................................................ 9–17 9.4.1.4.1. Batch ................................................................................................................ 9–18 9.4.1.4.2. GUI ................................................................................................................... 9–18 9.4.1.5. Specify Control Parameters and Solve ........................................................................ 9–18 9.4.1.5.1. Batch ................................................................................................................ 9–19 9.4.1.5.2. GUI ................................................................................................................... 9–20 9.4.1.6. Plot the Experimental Data and Analyze ..................................................................... 9–20 9.4.1.6.1. Batch ................................................................................................................ 9–20 9.4.1.6.2. GUI ................................................................................................................... 9–20 9.4.1.6.3. Analyze Your Curves for Proper Fit ..................................................................... 9–20 9.4.1.7. Write Data to TB Command ....................................................................................... 9–20 9.4.1.7.1. Batch ................................................................................................................ 9–20 9.4.1.7.2. GUI ................................................................................................................... 9–21 10. Gasket Joints Simulation ................................................................................................................. 10–1 10.1. Overview of Gasket Joints ......................................................................................................... 10–1 10.2. Performing a Gasket Joint Analysis ............................................................................................ 10–1 10.3. Finite Element Formulation ....................................................................................................... 10–2 10.3.1. Element Topologies ......................................................................................................... 10–2 10.3.2. Thickness Direction .......................................................................................................... 10–2 10.4. ANSYS Family of Interface Elements .......................................................................................... 10–3
xvi
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 10.4.1. Element Selection ............................................................................................................ 10–3 10.4.2. Applications ..................................................................................................................... 10–3 10.5. Material Definition .................................................................................................................... 10–4 10.5.1. Material Characteristics .................................................................................................... 10–4 10.5.2. Input Format .................................................................................................................... 10–5 10.5.2.1. Define General Parameters ...................................................................................... 10–6 10.5.2.2. Define Compression Load Closure Curve .................................................................. 10–6 10.5.2.3. Define Linear Unloading Data .................................................................................. 10–6 10.5.2.4. Define Nonlinear Unloading Data ............................................................................. 10–7 10.5.3. Temperature Dependencies ............................................................................................. 10–8 10.5.4. Plotting Gasket Data ....................................................................................................... 10–11 10.6. Meshing Interface Elements .................................................................................................... 10–12 10.7. Solution Procedure and Result Output ..................................................................................... 10–16 10.7.1. Typical Gasket Solution Output Listing ............................................................................ 10–17 10.8. Reviewing the Results ............................................................................................................. 10–19 10.8.1. Points to Remember ....................................................................................................... 10–19 10.8.2. Reviewing Results in POST1 ............................................................................................ 10–19 10.8.3. Reviewing Results in POST26 .......................................................................................... 10–20 10.9. Sample Gasket Element Verification Analysis (Command or Batch Method) .............................. 10–20 11. Contact ............................................................................................................................................ 11–1 11.1. Contact Overview ..................................................................................................................... 11–1 11.1.1. Explicit Dynamics Contact Capabilities .............................................................................. 11–1 11.2. General Contact Classification ................................................................................................... 11–1 11.3. ANSYS Contact Capabilities ....................................................................................................... 11–2 11.3.1. Surface-to-Surface Contact Elements ................................................................................ 11–3 11.3.2. Node-to-Surface Contact Elements ................................................................................... 11–3 11.3.3. Node-to-Node Contact Elements ...................................................................................... 11–4 11.4. Performing a Surface-to-Surface Contact Analysis ...................................................................... 11–4 11.4.1. Using Surface-to-Surface Contact Elements ....................................................................... 11–4 11.4.2. Steps in a Contact Analysis ............................................................................................... 11–5 11.4.3. Creating the Model Geometry and Mesh ........................................................................... 11–5 11.4.4. Identifying Contact Pairs .................................................................................................. 11–5 11.4.5. Designating Contact and Target Surfaces .......................................................................... 11–6 11.4.5.1. Asymmetric Contact vs. Symmetric Contact ............................................................. 11–7 11.4.5.1.1. Background .................................................................................................... 11–7 11.4.5.1.2. Using KEYOPT(8) ............................................................................................. 11–7 11.4.6. Defining the Target Surface .............................................................................................. 11–7 11.4.6.1. Pilot Nodes .............................................................................................................. 11–8 11.4.6.2. Primitives ................................................................................................................ 11–8 11.4.6.3. Element Types and Real Constants ........................................................................... 11–8 11.4.6.3.1. Defining Target Element Geometry ................................................................. 11–8 11.4.6.4. Using Direct Generation to Create Rigid Target Elements .......................................... 11–9 11.4.6.5. Using ANSYS Meshing Tools to Create Rigid Target Elements .................................. 11–10 11.4.6.5.1. Some Modeling and Meshing Tips ................................................................. 11–12 11.4.6.5.2. Verifying Nodal Number Ordering (Contact Direction) of Target Surface ......... 11–13 11.4.7. Defining the Deformable Contact Surface ....................................................................... 11–14 11.4.7.1. Element Type ........................................................................................................ 11–14 11.4.7.2. Real Constants and Material Properties ................................................................... 11–15 11.4.7.3. Generating Contact Elements ................................................................................. 11–16 11.4.8. Set the Real Constants and Element KEYOPTS ................................................................. 11–17 11.4.8.1. Real Constants ....................................................................................................... 11–17 11.4.8.1.1. Positive and Negative Real Constant Values ................................................... 11–19
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xvii
Structural Analysis Guide 11.4.8.2. Element KEYOPTS .................................................................................................. 11–20 11.4.8.3. Selecting a Contact Algorithm (KEYOPT(2)) ............................................................. 11–21 11.4.8.3.1. Background .................................................................................................. 11–21 11.4.8.4. Determining Contact Stiffness and Allowable Penetration ...................................... 11–22 11.4.8.4.1. Background .................................................................................................. 11–22 11.4.8.4.2. Using FKN and FTOLN ................................................................................... 11–23 11.4.8.4.3. Using FKT and SLTO ...................................................................................... 11–23 11.4.8.4.4. Using KEYOPT(10) ......................................................................................... 11–24 11.4.8.4.5. Chattering Control Parameters ...................................................................... 11–25 11.4.8.5. Choosing a Friction Model ..................................................................................... 11–25 11.4.8.5.1. Background .................................................................................................. 11–25 11.4.8.5.2. Using TAUMAX, FACT, DC, and COHE ............................................................. 11–26 11.4.8.5.3. Static and Dynamic Friction Coefficients ........................................................ 11–26 11.4.8.6. Selecting Location of Contact Detection ................................................................. 11–28 11.4.8.6.1. Background .................................................................................................. 11–28 11.4.8.6.2. Using KEYOPT(4) and TOLS ............................................................................ 11–28 11.4.8.7. Adjusting Initial Contact Conditions ....................................................................... 11–30 11.4.8.7.1. Background .................................................................................................. 11–30 11.4.8.7.2. Using PMIN, PMAX, CNOF, ICONT, KEYOPT(5), and KEYOPT(9) ......................... 11–30 11.4.8.8. Physically Moving Contact Nodes Towards the Target Surface ................................ 11–37 11.4.8.9. Determining Contact Status and the Pinball Region ................................................ 11–38 11.4.8.9.1. Background .................................................................................................. 11–38 11.4.8.9.2. Using PINB .................................................................................................... 11–39 11.4.8.10. Avoiding Spurious Contact in Self Contact Problems ............................................. 11–39 11.4.8.11. Selecting Surface Interaction Models .................................................................... 11–40 11.4.8.11.1. Background ................................................................................................ 11–40 11.4.8.11.2. Using KEYOPT(12) and FKOP ........................................................................ 11–40 11.4.8.12. Modeling Contact with Superelements ................................................................. 11–41 11.4.8.12.1. Background ................................................................................................ 11–41 11.4.8.12.2. Using KEYOPT(3) ......................................................................................... 11–41 11.4.8.13. Accounting for Thickness Effect ............................................................................ 11–42 11.4.8.13.1. Background ................................................................................................ 11–42 11.4.8.13.2. Using KEYOPT(11) ....................................................................................... 11–42 11.4.8.14. Using Time Step Control ...................................................................................... 11–42 11.4.8.14.1. Background ................................................................................................ 11–42 11.4.8.14.2. Using KEYOPT(7) ......................................................................................... 11–42 11.4.8.15. Using the Birth and Death Option ......................................................................... 11–42 11.4.9. Controlling the Motion of the Rigid Target Surface (Rigid-to-Flexible Contact) ................. 11–43 11.4.10. Modeling Thermal Contact ........................................................................................... 11–44 11.4.10.1. Thermal Contact Behavior vs. Contact Status ........................................................ 11–44 11.4.10.2. Free Thermal Surface ........................................................................................... 11–44 11.4.10.3. Temperature on Target Surface ............................................................................ 11–45 11.4.10.4. Modeling Conduction .......................................................................................... 11–45 11.4.10.4.1. Using TCC ................................................................................................... 11–45 11.4.10.4.2. Using the Quasi Solver Option ..................................................................... 11–46 11.4.10.5. Modeling Convection ........................................................................................... 11–46 11.4.10.6. Modeling Radiation ............................................................................................. 11–46 11.4.10.6.1. Background ................................................................................................ 11–46 11.4.10.6.2. Using SBCT and RDVF .................................................................................. 11–47 11.4.10.7. Modeling Heat Generation Due to Friction ........................................................... 11–47 11.4.10.7.1. Background ................................................................................................ 11–47 11.4.10.7.2. Using FHTG and FWGT ................................................................................ 11–47
xviii
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 11.4.10.8. Modeling External Heat Flux ................................................................................. 11–48 11.4.11. Modeling Electric Contact ............................................................................................. 11–48 11.4.11.1. Modeling Surface Interaction ............................................................................... 11–48 11.4.11.1.1. Background ................................................................................................ 11–48 11.4.11.1.2. Using ECC ................................................................................................... 11–49 11.4.11.2. Modeling Heat Generation Due to Electric Current ................................................ 11–49 11.4.12. Modeling Magnetic Contact .......................................................................................... 11–50 11.4.12.1. Using MCC ........................................................................................................... 11–50 11.4.12.2. Modeling Perfect Magnetic Contact ..................................................................... 11–51 11.4.13. Applying Necessary Boundary Conditions to the Deformable Elements ......................... 11–51 11.4.14. Defining Solution and Load Step Options ...................................................................... 11–51 11.4.15. Solving the Problem ..................................................................................................... 11–52 11.4.16. Reviewing the Results ................................................................................................... 11–53 11.4.16.1. Points to Remember ............................................................................................ 11–53 11.4.16.2. Reviewing Results in POST1 .................................................................................. 11–53 11.4.16.3. Reviewing Results in POST26 ................................................................................ 11–54 11.5. GUI Aids for Contact Analyses .................................................................................................. 11–54 11.5.1. The Contact Manager ..................................................................................................... 11–54 11.5.2. The Contact Wizard ........................................................................................................ 11–55 11.5.3. Managing Contact Pairs .................................................................................................. 11–56 11.6. Performing a Node-to-Surface Contact Analysis ....................................................................... 11–57 11.6.1. Using the Node-to-Surface Contact Elements .................................................................. 11–57 11.6.1.1. CONTA175 KEYOPTS .............................................................................................. 11–59 11.6.1.1.1. KEYOPT(3) ..................................................................................................... 11–59 11.6.1.1.2. KEYOPT(4) ..................................................................................................... 11–59 11.6.1.2. CONTA175 Real Constants ..................................................................................... 11–60 11.6.1.3. Multiphysics Contact ............................................................................................. 11–60 11.7. Using the Internal MPC Approach for Assemblies and Kinematic Constraints ............................ 11–60 11.7.1. Modeling Solid-solid and Shell-shell Assemblies .............................................................. 11–61 11.7.2. Modeling a Shell-solid Assembly ..................................................................................... 11–62 11.7.3. Surface-based Constraints .............................................................................................. 11–66 11.7.3.1. Defining Surface-based Constraints ........................................................................ 11–67 11.7.3.2. Modeling a Beam-solid Assembly ........................................................................... 11–68 11.7.4. Restrictions and Recommendations for Internal MPC ....................................................... 11–69 11.8. Performing a Node-to-Node Contact Analysis .......................................................................... 11–70 11.8.1. Creating Geometry and Meshing the Model .................................................................... 11–71 11.8.2. Generating Contact Elements ......................................................................................... 11–71 11.8.2.1. Generating Contact Elements Automatically at Coincident Nodes ........................... 11–72 11.8.2.2. Generating Contact Elements Automatically at Offset Nodes .................................. 11–72 11.8.2.3. Node Ordering ...................................................................................................... 11–72 11.8.3. Defining the Contact Normal .......................................................................................... 11–73 11.8.4. Defining the Initial Interference or Gap ........................................................................... 11–74 11.8.5. Selecting the Contact Algorithm ..................................................................................... 11–74 11.8.6. Applying Necessary Boundary Conditions ....................................................................... 11–74 11.8.7. Defining the Solution Options ........................................................................................ 11–75 11.8.8. Solving the Problem ....................................................................................................... 11–76 11.8.9. Reviewing the Results ..................................................................................................... 11–76 12. Fracture Mechanics .......................................................................................................................... 12–1 12.1. Definition of Fracture Mechanics ............................................................................................... 12–1 12.2. Solving Fracture Mechanics Problems ....................................................................................... 12–1 12.2.1. Modeling the Crack Region ............................................................................................... 12–1 12.2.1.1. 2-D Fracture Models ................................................................................................ 12–3
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xix
Structural Analysis Guide 12.2.1.2. 3-D Fracture Models ................................................................................................ 12–4 12.2.2. Calculating Fracture Parameters ....................................................................................... 12–5 12.2.2.1. Stress Intensity Factors ............................................................................................ 12–5 12.2.2.2. J-Integral ................................................................................................................. 12–6 12.2.2.3. Energy Release Rate ................................................................................................. 12–8 13. Composites ...................................................................................................................................... 13–1 13.1. Definition of Composites ........................................................................................................... 13–1 13.2. Modeling Composites ............................................................................................................... 13–1 13.2.1. Choosing the Proper Element Type ................................................................................... 13–1 13.2.2. Defining the Layered Configuration .................................................................................. 13–2 13.2.2.1. Specifying Individual Layer Properties ...................................................................... 13–3 13.2.2.2. Defining the Constitutive Matrices ........................................................................... 13–4 13.2.2.3. Sandwich and Multiple-Layered Structures ............................................................... 13–4 13.2.2.4. Node Offset ............................................................................................................. 13–5 13.2.3. Specifying Failure Criteria ................................................................................................. 13–5 13.2.4. Additional Modeling and Postprocessing Guidelines ......................................................... 13–6 14. Fatigue ............................................................................................................................................. 14–1 14.1. Definition of Fatigue ................................................................................................................. 14–1 14.1.1. What the ANSYS Program Does ........................................................................................ 14–1 14.1.2. Basic Terminology ............................................................................................................ 14–1 14.2. Doing a Fatigue Evaluation ....................................................................................................... 14–2 14.2.1. Enter POST1 and Resume Your Database .......................................................................... 14–2 14.2.2. Establish the Size, Fatigue Material Properties, and Locations ............................................ 14–2 14.2.3. Store Stresses and Assign Event Repetitions and Scale Factors ........................................... 14–4 14.2.3.1. Storing Stresses ....................................................................................................... 14–4 14.2.3.1.1. Manually Stored Stresses ................................................................................. 14–4 14.2.3.1.2. Nodal Stresses from Jobname.RST ................................................................... 14–5 14.2.3.1.3. Stresses at a Cross-Section ............................................................................... 14–5 14.2.3.2. Listing, Plotting, or Deleting Stored Stresses ............................................................. 14–6 14.2.3.3. Assigning Event Repetitions and Scale Factors ......................................................... 14–6 14.2.3.4. Guidelines for Obtaining Accurate Usage Factors ..................................................... 14–7 14.2.4. Activate the Fatigue Calculations ...................................................................................... 14–9 14.2.5. Review the Results ........................................................................................................... 14–9 14.2.6. Other Approaches to Range Counting .............................................................................. 14–9 14.2.7. Sample Input ................................................................................................................... 14–9 15. p-Method Structural Static Analysis ................................................................................................ 15–1 15.1. Definition of p-Method Analysis ................................................................................................ 15–1 15.2. Benefits of Using the p-Method ................................................................................................. 15–1 15.3. Using the p-Method .................................................................................................................. 15–1 15.3.1. Select the p-Method Procedure ........................................................................................ 15–1 15.3.2. Build the Model ................................................................................................................ 15–2 15.3.2.1. Define the Element Types ........................................................................................ 15–2 15.3.2.1.1. Specifying a p-Level Range .............................................................................. 15–2 15.3.2.2. Specify Material Properties and/or Real Constants .................................................... 15–3 15.3.2.2.1. Material Properties .......................................................................................... 15–3 15.3.2.2.2. Real Constants ................................................................................................ 15–3 15.3.2.3. Define the Model Geometry ..................................................................................... 15–4 15.3.2.4. Mesh the Model into Solid or Shell Elements ............................................................ 15–4 15.3.2.4.1. Using Program Defaults .................................................................................. 15–4 15.3.2.4.2. Specifying Mesh Controls ................................................................................ 15–4 15.3.2.4.3. Guidelines for Creating a Good Mesh ............................................................... 15–5 15.3.3. Additional Information for Building Your Model ................................................................ 15–5
xx
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 15.3.3.1. Viewing your element model ................................................................................... 15–5 15.3.3.2. Coupling ................................................................................................................. 15–6 15.3.3.2.1. Coupling of Corner Nodes ............................................................................... 15–6 15.3.3.2.2. Midside Node Coupling ................................................................................... 15–7 15.3.4. Apply Loads and Obtain the Solution ................................................................................ 15–7 15.3.5. Helpful Hints for Common Problems ............................................................................... 15–12 15.3.6. Review the Results .......................................................................................................... 15–12 15.3.6.1. The p-Element Subgrid .......................................................................................... 15–13 15.3.7. Querying Subgrid Results ............................................................................................... 15–13 15.3.8. Printing and Plotting Node and Element Results ............................................................. 15–14 15.3.8.1. Specialized p-Method Displays and Listings ............................................................ 15–14 15.4. Sample p-Method Analysis (GUI Method) ................................................................................. 15–14 15.4.1. Problem Description ....................................................................................................... 15–15 15.4.2. Problem Specifications ................................................................................................... 15–15 15.4.3. Problem Diagram ........................................................................................................... 15–15 15.4.3.1. Set the Analysis Title .............................................................................................. 15–15 15.4.3.2. Select p-Method .................................................................................................... 15–15 15.4.3.3. Define the Element Type and Options .................................................................... 15–15 15.4.3.4. Define the Real Constants ...................................................................................... 15–16 15.4.3.5. Define Material Properties ...................................................................................... 15–16 15.4.3.6. Create Plate with Hole ............................................................................................ 15–16 15.4.3.7. Mesh the Areas ...................................................................................................... 15–16 15.4.3.8. Define Symmetry Boundary Conditions .................................................................. 15–17 15.4.3.9. Define Pressure Load along Right Edge. .................................................................. 15–17 15.4.3.10. Define Convergence Criteria ................................................................................ 15–17 15.4.3.11. Solve the Problem ................................................................................................ 15–17 15.4.3.12. Review the Results and Exit ANSYS ....................................................................... 15–18 15.5. Sample p-Method Analysis (Command or Batch Method) ......................................................... 15–18 16. Beam Analysis and Cross Sections .................................................................................................. 16–1 16.1. An Overview of Beams .............................................................................................................. 16–1 16.2. What Are Cross Sections? .......................................................................................................... 16–1 16.3. How to Create Cross Sections .................................................................................................... 16–2 16.3.1. Defining a Section and Associating a Section ID Number ................................................... 16–3 16.3.2. Defining Cross Section Geometry and Setting the Section Attribute Pointer ...................... 16–3 16.3.2.1. Determining the Number of Cells to Define .............................................................. 16–4 16.3.3. Meshing a Line Model with BEAM44, BEAM188, or BEAM189 Elements .............................. 16–4 16.4. Creating Cross Sections ............................................................................................................. 16–5 16.4.1. Using the Beam Tool to Create Common Cross Sections .................................................... 16–5 16.4.2. Creating Custom Cross Sections with a User-defined Mesh ................................................ 16–6 16.4.3. Creating Custom Cross Sections with Mesh Refinement and Multiple Materials .................. 16–7 16.4.4. Defining Composite Cross Sections ................................................................................... 16–8 16.4.5. Defining a Tapered Beam ................................................................................................. 16–8 16.5. Managing Cross Section and User Mesh Libraries ....................................................................... 16–9 16.6. Sample Lateral Torsional Buckling Analysis (GUI Method) ........................................................... 16–9 16.6.1. Problem Description ....................................................................................................... 16–10 16.6.2. Problem Specifications ................................................................................................... 16–10 16.6.3. Problem Sketch .............................................................................................................. 16–11 16.6.4. Eigenvalue Buckling and Nonlinear Collapse ................................................................... 16–11 16.6.5. Set the Analysis Title and Define Model Geometry ........................................................... 16–12 16.6.6. Define Element Type and Cross Section Information ....................................................... 16–12 16.6.7. Define the Material Properties and Orientation Node ...................................................... 16–12 16.6.8. Mesh the Line and Verify Beam Orientation ..................................................................... 16–13
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xxi
Structural Analysis Guide 16.6.9. Define the Boundary Conditions ..................................................................................... 16–13 16.6.10. Solve the Eigenvalue Buckling Analysis ......................................................................... 16–14 16.6.11. Solve the Nonlinear Buckling Analysis ........................................................................... 16–15 16.6.12. Plot and Review the Results .......................................................................................... 16–15 16.7. Sample Problem with Cantilever Beams, Command Method .................................................... 16–16 16.8. Where to Find Other Examples ................................................................................................ 16–17 17. Shell Analysis and Cross Sections .................................................................................................... 17–1 17.1. An Overview of Shells ................................................................................................................ 17–1 17.2. What Are Cross Sections? .......................................................................................................... 17–1 17.3. How to Create Cross Sections .................................................................................................... 17–1 17.3.1. Defining a Section and Associating a Section ID Number ................................................... 17–2 17.3.2. Defining Layer Data .......................................................................................................... 17–2 17.3.3. Overriding Program Calculated Section Properties ............................................................ 17–3 17.3.4. Specifying a Shell Thickness Variation (Tapered Shells) ...................................................... 17–3 17.3.5. Setting the Section Attribute Pointer ................................................................................ 17–3 17.3.6. Associating an Area with a Section .................................................................................... 17–3 17.3.7. Using the Shell Tool to Create Sections ............................................................................. 17–3 17.3.8. Managing Cross Section Libraries ..................................................................................... 17–5 Index ................................................................................................................................................. Index–1
List of Figures 2.1. Diagram of Allen Wrench .................................................................................................................. 2–14 3.1. Diagram of a Model Airplane Wing .................................................................................................... 3–12 3.2. Choose Master DOF .......................................................................................................................... 3–20 3.3. Choosing Master DOFs ...................................................................................................................... 3–20 3.4. Choosing Masters in an Axisymmetric Shell Model ............................................................................. 3–21 4.1. Harmonic Response Systems ............................................................................................................... 4–1 4.2. Relationship Between Real/Imaginary Components and Amplitude/Phase Angle ................................. 4–6 4.3. An Unbalanced Rotating Antenna ....................................................................................................... 4–7 4.4. Two-Mass-Spring-System .................................................................................................................. 4–14 5.1. Examples of Load-Versus-Time Curves ................................................................................................. 5–4 5.2. Examples of Gap Conditions .............................................................................................................. 5–21 5.3. Model of a Steel Beam Supporting a Concentrated Mass .................................................................... 5–27 5.4. Effect of Integration Time Step on Period Elongation ......................................................................... 5–34 5.5. Transient Input vs. Transient Response .............................................................................................. 5–35 5.6. Rayleigh Damping ............................................................................................................................ 5–38 6.1. Single-Point and Multi-Point Response Spectra ................................................................................... 6–2 6.2. Simply Supported Beam with Vertical Motion of Both Supports ......................................................... 6–11 7.1. Buckling Curves .................................................................................................................................. 7–1 7.2. Adjusting Variable Loads to Find an Eigenvalue of 1.0 .......................................................................... 7–4 7.3. Bar with Hinged Ends .......................................................................................................................... 7–9 8.1. Common Examples of Nonlinear Structural Behavior ........................................................................... 8–1 8.2. A Fishing Rod Demonstrates Geometric Nonlinearity ........................................................................... 8–2 8.3. Newton-Raphson Approach ................................................................................................................ 8–3 8.4. Traditional Newton-Raphson Method vs. Arc-Length Method .............................................................. 8–4 8.5. Load Steps, Substeps, and Time .......................................................................................................... 8–4 8.6. Nonconservative (Path-Dependent) Behavior ...................................................................................... 8–5 8.7. Load Directions Before and After Deflection ........................................................................................ 8–6 8.8. Stress-Stiffened Beams ........................................................................................................................ 8–8 8.9. Elastoplastic Stress-Strain Curve .......................................................................................................... 8–9 xxii
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide 8.10. Kinematic Hardening ...................................................................................................................... 8–10 8.11. Bauschinger Effect .......................................................................................................................... 8–11 8.12. NLISO Stress-Strain Curve ................................................................................................................ 8–14 8.13. Cast Iron Plasticity ........................................................................................................................... 8–16 8.14. Hyperelastic Structure ..................................................................................................................... 8–17 8.15. Typical Hyperelastic Stress-Strain Curves ......................................................................................... 8–23 8.16. Data Locations in Stress and Strain Input Arrays ............................................................................... 8–25 8.17. Typical Evaluated Hyperelastic Stress-Strain Curve ........................................................................... 8–27 8.18. Stress Relaxation and Creep ............................................................................................................ 8–29 8.19. Time Hardening Creep Analysis ....................................................................................................... 8–30 8.20. Shape Memory Alloy Phases ............................................................................................................ 8–32 8.21. Viscoplastic Behavior in a Rolling Operation .................................................................................... 8–33 8.22. Viscoelastic Behavior (Maxwell Model) ............................................................................................. 8–34 8.23. Linear Interpolation of Nonlinear Results Can Introduce Some Error ................................................. 8–58 8.24. Convergence Norms Displayed By the Graphical Solution Tracking (GST) Feature ............................. 8–67 8.25. Typical Nonlinear Output Listing ..................................................................................................... 8–70 8.26. Cyclic Point Load History ................................................................................................................. 8–73 10.1. Element Topology of a 3-D 8-Node Interface Element ...................................................................... 10–2 10.2. Pressure vs. Closure Behavior of a Gasket Material ............................................................................ 10–5 10.3. Gasket Material Input: Linear Unloading Curves ............................................................................... 10–7 10.4. Gasket Material Input: Nonlinear Unloading Curves ......................................................................... 10–8 10.5. Gasket Compression and Unloading Curves at Two Temperatures .................................................. 10–11 10.6. Gasket Finite Element Model Geometry ......................................................................................... 10–14 10.7. Whole Model Mesh with Brick Element .......................................................................................... 10–14 10.8. Interface Layer Mesh ..................................................................................................................... 10–15 10.9. Whole Model Tetrahedral Mesh ..................................................................................................... 10–15 10.10. Interface Layer Mesh with Degenerated Wedge Elements ............................................................ 10–16 11.1. Localized Contact Zones ................................................................................................................. 11–6 11.2. ANSYS Geometric Entities and Their Corresponding Rigid Target Elements .................................... 11–10 11.3. A Single Circular Target Segment Created From Arc Line Segments ................................................ 11–11 11.4. Meshing Patterns for Arbitrary Target Surfaces .............................................................................. 11–12 11.5. Smoothing Convex Corner ............................................................................................................ 11–13 11.6. Correct Node Ordering .................................................................................................................. 11–13 11.7. Contact Element Types .................................................................................................................. 11–15 11.8. Specification of the Contact Surface's Outward Normal .................................................................. 11–17 11.9. Depth of the Underlying Element .................................................................................................. 11–20 11.10. Sliding Contact Resistance ........................................................................................................... 11–26 11.11. Friction Decay ............................................................................................................................. 11–27 11.12. Contact Detection Located at Gauss Point ................................................................................... 11–28 11.13. Contact Detection Point Location at Nodal Point ......................................................................... 11–29 11.14. Node Slippage Using Nodal Integration KEYOPT(4) = 1 or 2 .......................................................... 11–29 11.15. Contact Surface Adjustment With ICONT ..................................................................................... 11–32 11.16. Contact Surface Adjustment (PMIN, PMAX) .................................................................................. 11–33 11.17. A Scenario in Which Initial Adjustment Will Fail ............................................................................ 11–34 11.18. Ignoring Initial Penetration, KEYOPT(9) = 1 .................................................................................. 11–35 11.19. Components of True Penetration ................................................................................................. 11–36 11.20. Ramping Initial Interference ........................................................................................................ 11–37 11.21. Effect of Moving Contact Nodes .................................................................................................. 11–38 11.22. Auto Spurious Prevention ............................................................................................................ 11–39 11.23. Target Temperature .................................................................................................................... 11–45 11.24. Contact Manager Toolbar ............................................................................................................ 11–54 11.25. Example of a Contact Wizard Dialog ............................................................................................ 11–56
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xxiii
Structural Analysis Guide 11.26. Node-to-Surface Contact Elements .............................................................................................. 11–58 11.27. Example of Shell-solid Assembly .................................................................................................. 11–62 11.28. Shell-solid Assembly (Original Mesh) ........................................................................................... 11–63 11.29. Shell-solid Assembly with Solid-solid Constraint Option ............................................................... 11–64 11.30. Shell-solid Assembly with Shell-shell Constraint Option ............................................................... 11–64 11.31. Shell-solid Assembly with Shell-solid Constraint Option ............................................................... 11–65 11.32. Rigid Constraint Surface .............................................................................................................. 11–66 11.33. Force-distributed Surface ............................................................................................................ 11–67 11.34. Beam-solid Assembly Defined by Rigid Constraint Surface ........................................................... 11–69 11.35. Beam-solid Assembly Defined by Force-distributed Surface ......................................................... 11–69 11.36. Node-to-Node Contact Elements ................................................................................................. 11–70 11.37. Contact Between Two Concentric Pipes ....................................................................................... 11–72 11.38. Two Concentric Pipes, Normals Rotated Properly ......................................................................... 11–73 11.39. Example of Overconstrained Contact Problem ............................................................................. 11–75 12.1. Crack Tip and Crack Front ................................................................................................................ 12–2 12.2. Examples of Singular Elements ........................................................................................................ 12–3 12.3. A Fracture Specimen and 2-D FE Model ........................................................................................... 12–4 12.4. Taking Advantage of Symmetry ...................................................................................................... 12–4 12.5. Crack Coordinate Systems ............................................................................................................... 12–5 12.6. Typical Path Definitions ................................................................................................................... 12–6 12.7. J-Integral Contour Path Surrounding a Crack-Tip ............................................................................. 12–7 12.8. Examples of Paths for J-integral Calculation ..................................................................................... 12–7 13.1. Layered Model Showing Dropped Layer .......................................................................................... 13–3 13.2. Sandwich Construction ................................................................................................................... 13–4 13.3. Layered Shell With Nodes at Midplane ............................................................................................. 13–5 13.4. Layered Shell With Nodes at Bottom Surface ................................................................................... 13–5 13.5. Example of an Element Display ........................................................................................................ 13–7 13.6. Sample LAYPLOT Display for [45/-45/ - 45/45] Sequence .................................................................. 13–8 14.1. Cylinder Wall with Stress Concentration Factors (SCFs) .................................................................... 14–4 14.2. Three Loadings in One Event ........................................................................................................... 14–5 14.3. Surface Nodes are Identified by PPATH Prior to Executing FSSECT .................................................... 14–6 15.1. Fan Model Showing p-Element vs. h-Element Meshes ...................................................................... 15–5 15.2. Coupled Nodes on One Element ...................................................................................................... 15–6 15.3. Nodes Coupled Between Adjacent Elements ................................................................................... 15–6 15.4. Both Corner Nodes are Coupled ...................................................................................................... 15–7 15.5. All Coupled Nodes are Midside Nodes ............................................................................................. 15–7 15.6. Constraints on Rotated Nodes ......................................................................................................... 15–9 15.7. p-Element Subgrids for Quadrilateral Elements .............................................................................. 15–13 15.8. Steel Plate With a Hole .................................................................................................................. 15–15 16.1. Plot of a Z Cross Section .................................................................................................................. 16–2 16.2. Types of Solid Section Cell Mesh ...................................................................................................... 16–4 16.3. BeamTool with Subtypes Drop Down List Displayed ........................................................................ 16–6 16.4. Lateral-Torsional Buckling of a Cantilever I-Beam ........................................................................... 16–10 16.5. Diagram of a Beam With Deformation Indicated ............................................................................ 16–11 17.1. Plot of a Shell Section ...................................................................................................................... 17–2 17.2. Shell Tool With Layup Page Displayed ............................................................................................. 17–4 17.3. Shell Tool With Section Controls Page Displayed .............................................................................. 17–4 17.4. Shell Tool With Summary Page Displayed ........................................................................................ 17–5
xxiv
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Structural Analysis Guide
List of Tables 1.1. Structural Element Types .................................................................................................................... 1–2 2.1. Basic Tab Options ............................................................................................................................... 2–3 2.2. Sol'n Options Tab Options ................................................................................................................... 2–4 2.3. Nonlinear Tab Options ........................................................................................................................ 2–4 2.4. Advanced NL Tab Options ................................................................................................................... 2–5 2.5. Loads Applicable in a Static Analysis ................................................................................................... 2–8 3.1. Analysis Types and Options ................................................................................................................. 3–2 3.2. Loads Applicable in a Modal Analysis .................................................................................................. 3–5 3.3. Load Commands for a Modal Analysis ................................................................................................. 3–5 3.4. Load Step Options .............................................................................................................................. 3–6 3.5. Expansion Pass Options ...................................................................................................................... 3–8 3.6. Symmetric System Eigensolver Choices ............................................................................................. 3–17 4.1. Analysis Types and Options ................................................................................................................. 4–4 4.2. Applicable Loads in a Harmonic Response Analysis .............................................................................. 4–7 4.3. Load Commands for a Harmonic Response Analysis ............................................................................ 4–8 4.4. Load Step Options .............................................................................................................................. 4–9 4.5. Expansion Pass Options .................................................................................................................... 4–22 5.1. Transient Tab Options ......................................................................................................................... 5–8 5.2. Options for the First Load Step-Mode Superposition Analysis ............................................................. 5–15 5.3. Options for the First Load Step-Reduced Analysis .............................................................................. 5–22 5.4. Expansion Pass Options .................................................................................................................... 5–24 5.5. Damping for Different Analysis Types ................................................................................................ 5–36 5.6. Damping Matrix Formulation with Different Damping Coefficients .................................................... 5–39 6.1. Analysis Types and Options ................................................................................................................. 6–4 6.2. Load Step Options .............................................................................................................................. 6–4 6.3. Solution Items Available in a PSD Analysis ......................................................................................... 6–21 6.4. Organization of Results Data from a PSD Analysis .............................................................................. 6–22 8.1. Suggested Mooney-Rivlin Constants ................................................................................................. 8–23 8.2. Data Locations in Stress and Strain Input Arrays ................................................................................. 8–24 9.1. Experimental Details for Case 1 and 2 Models and Blatz-Ko .................................................................. 9–2 9.2. Experimental Details for Case 3 Models ............................................................................................... 9–2 9.3. Hyperelastic Curve Fitting Model Types ............................................................................................... 9–3 9.4. Creep Data Types and Abbreviations ................................................................................................... 9–8 9.5. Creep Model and Data/Type Attribute ................................................................................................. 9–8 9.6. Creep Models and Abbreviations ....................................................................................................... 9–10 9.7. Viscoelastic Data Types and Abbreviations ........................................................................................ 9–15 11.1. ANSYS Contact Capabilities ............................................................................................................. 11–2 11.2. Summary of Real Constant Defaults in Different Environments ....................................................... 11–18 11.3. Summary of KEYOPT Defaults in Different Environments ................................................................ 11–21 16.1. ANSYS Cross Section Commands ..................................................................................................... 16–2 17.1. ANSYS Cross Section Commands ..................................................................................................... 17–1
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
xxv
xxvi
Chapter 1: Overview of Structural Analyses 1.1. Definition of Structural Analysis Structural analysis is probably the most common application of the finite element method. The term structural (or structure) implies not only civil engineering structures such as bridges and buildings, but also naval, aeronautical, and mechanical structures such as ship hulls, aircraft bodies, and machine housings, as well as mechanical components such as pistons, machine parts, and tools.
1.2. Types of Structural Analysis The seven types of structural analyses available in the ANSYS family of products are explained below. The primary unknowns (nodal degrees of freedom) calculated in a structural analysis are displacements. Other quantities, such as strains, stresses, and reaction forces, are then derived from the nodal displacements. Structural analyses are available in the ANSYS Multiphysics, ANSYS Mechanical, ANSYS Structural, and ANSYS Professional programs only. You can perform the following types of structural analyses. Each of these analysis types are discussed in detail in this manual. Static Analysis--Used to determine displacements, stresses, etc. under static loading conditions. Both linear and nonlinear static analyses. Nonlinearities can include plasticity, stress stiffening, large deflection, large strain, hyperelasticity, contact surfaces, and creep. Modal Analysis--Used to calculate the natural frequencies and mode shapes of a structure. Different mode extraction methods are available. Harmonic Analysis--Used to determine the response of a structure to harmonically time-varying loads. Transient Dynamic Analysis--Used to determine the response of a structure to arbitrarily time-varying loads. All nonlinearities mentioned under Static Analysis above are allowed. Spectrum Analysis--An extension of the modal analysis, used to calculate stresses and strains due to a response spectrum or a PSD input (random vibrations). Buckling Analysis--Used to calculate the buckling loads and determine the buckling mode shape. Both linear (eigenvalue) buckling and nonlinear buckling analyses are possible. Explicit Dynamic Analysis--This type of structural analysis is only available in the ANSYS LS-DYNA program. ANSYS LS-DYNA provides an interface to the LS-DYNA explicit finite element program. Explicit dynamic analysis is used to calculate fast solutions for large deformation dynamics and complex contact problems. Explicit dynamic analysis is described in the ANSYS LS-DYNA User's Guide. In addition to the above analysis types, several special-purpose features are available: •
Fracture mechanics
•
Composites
•
Fatigue
•
p-Method
•
Beam Analyses Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 1: Overview of Structural Analyses
1.3. Elements Used in Structural Analyses Most ANSYS element types are structural elements, ranging from simple spars and beams to more complex layered shells and large strain solids. Most types of structural analyses can use any of these elements. Note — Explicit dynamics analysis can use only the explicit dynamic elements (LINK160, BEAM161, PLANE162, SHELL163, SOLID164, COMBI165, MASS166, LINK167, and SOLID168).
Table 1.1 Structural Element Types Category
Element Name(s)
Spars
LINK1, LINK8, LINK10, LINK180
Beams
BEAM3, BEAM4, BEAM23, BEAM24, BEAM44, BEAM54, BEAM188, BEAM189
Pipes
PIPE16, PIPE17, PIPE18, PIPE20, PIPE59, PIPE60
2-D Solids
PLANE2, PLANE25, PLANE42, HYPER56, HYPER74, PLANE82, PLANE83, HYPER84, VISCO88, VISCO106, VISCO108, PLANE145, PLANE146, PLANE182, PLANE183
3-D Solids
SOLID45, SOLID46, HYPER58, SOLID64, SOLID65, HYPER86, VISCO89, SOLID92, SOLID95, VISCO107, SOLID147, SOLID148, HYPER158, SOLID185, SOLID186, SOLID187, SOLID191
Shells
SHELL28, SHELL41, SHELL43, SHELL51, SHELL61, SHELL63, SHELL91, SHELL93, SHELL99, SHELL150, SHELL181
Interface
INTER192, INTER193, INTER194, INTER195
Contact
CONTAC12, CONTAC52, TARGE169, TARGE170, CONTA171, CONTA172, CONTA173, CONTA174, CONTA175
Coupled-Field
SOLID5, PLANE13, FLUID29, FLUID30, FLUID38, SOLID62, FLUID79, FLUID80, FLUID81, SOLID98, FLUID129, INFIN110, INFIN111, FLUID116, FLUID130
Specialty
COMBIN7, LINK11, COMBIN14, MASS21, MATRIX27, COMBIN37, COMBIN39, COMBIN40, MATRIX50, SURF153, SURF154
Explicit Dynamics
LINK160, BEAM161, PLANE162, SHELL163, SOLID164, COMBI165, MASS166, LINK167, SOLID168
1.4. Material Model Interface For analyses described in this guide, if you are using the GUI, you must specify the material you will be simulating using an intuitive material model interface. This interface uses a hierarchical tree structure of material categories, which is intended to assist you in choosing the appropriate model for your analysis. See Section 1.2.4.4: Material Model Interface in the ANSYS Basic Analysis Guide for details on the material model interface.
1.5. Types of Solution Methods Two solution methods are available for solving structural problems in the ANSYS family of products: the hmethod and the p-method. The h-method can be used for any type of analysis, but the p-method can be used only for linear structural static analyses. Depending on the problem to be solved, the h-method usually requires a finer mesh than the p-method. The p-method provides an excellent way to solve a problem to a desired level of accuracy while using a coarse mesh. In general, the discussions in this manual focus on the procedures required for the h-method of solution. Chapter 15, “p-Method Structural Static Analysis” discusses procedures specific to the p-method.
1–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 2: Structural Static Analysis 2.1. Definition of Static Analysis A static analysis calculates the effects of steady loading conditions on a structure, while ignoring inertia and damping effects, such as those caused by time-varying loads. A static analysis can, however, include steady inertia loads (such as gravity and rotational velocity), and time-varying loads that can be approximated as static equivalent loads (such as the static equivalent wind and seismic loads commonly defined in many building codes). Static analysis is used to determine the displacements, stresses, strains, and forces in structures or components caused by loads that do not induce significant inertia and damping effects. Steady loading and response conditions are assumed; that is, the loads and the structure's response are assumed to vary slowly with respect to time. The kinds of loading that can be applied in a static analysis include: •
Externally applied forces and pressures
•
Steady-state inertial forces (such as gravity or rotational velocity)
•
Imposed (nonzero) displacements
•
Temperatures (for thermal strain)
•
Fluences (for nuclear swelling)
More information about the loads that you can apply in a static analysis appears in Section 2.3.4: Apply the Loads.
2.2. Linear vs. Nonlinear Static Analyses A static analysis can be either linear or nonlinear. All types of nonlinearities are allowed - large deformations, plasticity, creep, stress stiffening, contact (gap) elements, hyperelastic elements, and so on. This chapter focuses on linear static analyses, with brief references to nonlinearities. Details of how to handle nonlinearities are described in Chapter 8, “Nonlinear Structural Analysis”.
2.3. Performing a Static Analysis The procedure for a static analysis consists of these tasks: 1.
Section 2.3.1: Build the Model
2.
Section 2.3.2: Set Solution Controls
3.
Section 2.3.3: Set Additional Solution Options
4.
Section 2.3.4: Apply the Loads
5.
Section 2.3.5: Solve the Analysis
6.
Section 2.3.6: Review the Results
2.3.1. Build the Model See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details, see the ANSYS Modeling and Meshing Guide.
2.3.1.1. Points to Remember Keep the following points in mind when doing a static analysis: Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 2: Structural Static Analysis •
You can use both linear and nonlinear structural elements.
•
Material properties can be linear or nonlinear, isotropic or orthotropic, and constant or temperature-dependent. –
You must define stiffness in some form (for example, Young's modulus (EX), hyperelastic coefficients, and so on).
–
For inertia loads (such as gravity), you must define the data required for mass calculations, such as density (DENS).
–
For thermal loads (temperatures), you must define the coefficient of thermal expansion (ALPX).
Note the following information about mesh density: •
Regions where stresses or strains vary rapidly (usually areas of interest) require a relatively finer mesh than regions where stresses or strains are nearly constant (within an element).
•
While considering the influence of nonlinearities, remember that the mesh should be able to capture the effects of the nonlinearities. For example, plasticity requires a reasonable integration point density (and therefore a fine element mesh) in areas with high plastic deformation gradients.
2.3.2. Set Solution Controls Setting solution controls involves defining the analysis type and common analysis options for an analysis, as well as specifying load step options for it. When you are doing a structural static analysis, you can take advantage of a streamlined solution interface (called the Solution Controls dialog box) for setting these options. The Solution Controls dialog box provides default settings that will work well for many structural static analyses, which means that you may need to set only a few, if any, of the options. Because the streamlined solution interface is the recommended tool for setting solution controls in a structural static analysis, it is the method that is presented in this chapter. If you prefer not to use the Solution Controls dialog box (Main Menu> Solution> Analysis Type> Sol'n Controls), you can set solution controls for your analysis using the standard set of ANSYS solution commands and the standard corresponding menu paths (Main Menu> Solution> Unabridged Menu> option). For a general overview of the Solution Controls dialog box, see Section 3.11: Using Special Solution Controls for Certain Types of Structural Analyses in the ANSYS Basic Analysis Guide.
2.3.2.1. Access the Solution Controls Dialog Box To access the Solution Controls dialog box, choose menu path Main Menu> Solution> Analysis Type> Sol'n Controls. The following sections provide brief descriptions of the options that appear on each tab of the dialog box. For details about how to set these options, select the tab that you are interested in (from within the ANSYS program), and then click the Help button. Chapter 8, “Nonlinear Structural Analysis” also contains details about the nonlinear options introduced in this chapter.
2.3.2.2. Using the Basic Tab The Basic tab is active when you access the dialog box. The controls that appear on the Basic tab provide the minimum amount of data that ANSYS needs for the analysis. Once you are satisfied with the settings on the Basic tab, you do not need to progress through the remaining tabs unless you want to adjust the default settings for the more advanced controls. As soon as you click OK on any tab of the dialog box, the settings are applied to the ANSYS database and the dialog box closes.
2–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.3: Performing a Static Analysis You can use the Basic tab to set the options listed in Table 2.1: “Basic Tab Options”. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Basic tab, and click the Help button.
Table 2.1 Basic Tab Options Option
For more information on this option, see: •
Section 1.2.6.1: Defining the Analysis Type and Analysis Options in the ANSYS Basic Analysis Guide
•
Chapter 8, “Nonlinear Structural Analysis” in the ANSYS Structural Analysis Guide
•
Section 3.16: Restarting an Analysis in the ANSYS Basic Analysis Guide
Control time settings, including: time at end of load step [TIME], automatic time stepping [AUTOTS], and number of substeps to be taken in a load step [NSUBST or DELTIM]
•
Section 2.4: The Role of Time in Tracking in the ANSYS Basic Analysis Guide
•
Section 2.7.1: General Options in the ANSYS Basic Analysis Guide
Specify solution data to write to database [OUTRES]
•
Section 2.7.4: Output Controls in the ANSYS Basic Analysis Guide
Specify analysis type [ANTYPE, NLGEOM]
Special considerations for setting these options in a static analysis include: •
When setting ANTYPE and NLGEOM, choose Small Displacement Static if you are performing a new analysis and you want to ignore large deformation effects such as large deflection, large rotation, and large strain. Choose Large Displacement Static if you expect large deflections (as in the case of a long, slender bar under bending) or large strains (as in a metal-forming problem). Choose Restart Current Analysis if you want to restart a failed nonlinear analysis, or you have previously completed a static analysis, and you want to specify additional loads.
•
When setting TIME, remember that this load step option specifies time at the end of the load step. The default value is 1.0 for the first load step. For subsequent load steps, the default is 1.0 plus the time specified for the previous load step. Although time has no physical meaning in a static analysis (except in the case of creep, viscoplasticity, or other rate-dependent material behavior), it is used as a convenient way of referring to load steps and substeps (see Chapter 2, “Loading” in the ANSYS Basic Analysis Guide).
•
When setting OUTRES, keep this caution in mind: Caution: By default, only 1000 results sets can be written to the results file (Jobname.RST). If this number is exceeded (based on your OUTRES specification), the program will terminate with an error. Use the command /CONFIG,NRES to increase the limit (see Chapter 19, “Memory Management and Configuration” in the ANSYS Basic Analysis Guide).
2.3.2.3. The Transient Tab The Transient tab contains transient analysis controls; it is available only if you choose a transient analysis and remains grayed out when you choose a static analysis. For these reasons, it is not described here.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–3
Chapter 2: Structural Static Analysis
2.3.2.4. Using the Sol'n Options Tab You can use the Sol'n Options tab to set the options listed in Table 2.2: “Sol'n Options Tab Options”. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Sol'n Options tab, and click the Help button.
Table 2.2 Sol'n Options Tab Options Option
For more information about this option, see the following section(s) in the ANSYS Basic Analysis Guide:
Specify equation solver [EQSLV]
•
Section 3.2: Selecting a Solver through Section 3.10: Using the Automatic Iterative (Fast) Solver Option
Specify parameters for multiframe restart [RESCONTROL]
•
Section 3.16.2: Multiframe Restart
Special considerations for setting these options in a static analysis include: •
When setting EQSLV, specify one of these solvers: –
Program chosen solver (ANSYS selects a solver for you, based on the physics of the problem)
–
Sparse direct solver (default for linear and nonlinear, static and full transient analyses)
–
Preconditioned Conjugate Gradient (PCG) solver (recommended for large models/high wavefronts, bulky structures)
–
Algebraic Multigrid (AMG) solver (applicable in the same situations as the PCG solver, but provides parallel processing; for faster turnaround times when used in a multiprocessor environment)
–
Distributed Domain Solver (DDS) provides parallel processing on multiple systems across a network
–
Iterative solver (auto-select; for linear static/full transient structural or steady-state thermal analyses only; recommended)
–
Frontal direct solver
Note — The AMG and DDS solvers are part of Parallel Performance for ANSYS, which is a separately-licensed product. See Chapter 13, “Improving ANSYS Performance and Parallel Performance for ANSYS” in the ANSYS Advanced Analysis Techniques Guide for more information about these solvers.
2.3.2.5. Using the Nonlinear Tab You can use the Nonlinear tab to set the options listed in Table 2.3: “Nonlinear Tab Options”. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Nonlinear tab, and click the Help button.
Table 2.3 Nonlinear Tab Options Option Activate line search [LNSRCH]
2–4
For more information about this option, see the following section(s) in the ANSYS Structural Analysis Guide: •
Section 8.5.2.3.5: Line Search Option
•
Section 8.10.2.4: Using Line Search
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.3: Performing a Static Analysis Option
For more information about this option, see the following section(s) in the ANSYS Structural Analysis Guide:
Activate a predictor on the DOF solution [PRED]
•
Section 8.5.2.3.4: Predictor-Corrector Option
Specify the maximum number of iterations allowed per substep [NEQIT]
•
Section 8.5.2.3.3: Maximum Number of Equilibrium Iterations
Specify whether you want to include creep calculation [RATE]
•
Section 8.3.1.5: Creep
•
Section 8.5.3.2.1: Creep Criteria
Set convergence criteria [CNVTOL]
•
Section 8.5.2.3.2: Convergence Criteria
Control bisections [CUTCONTROL]
•
Section 8.5.2.3.6: Cutback Criteria
2.3.2.6. Using the Advanced NL Tab You can use the Advanced NL tab to set the options listed in Table 2.4: “Advanced NL Tab Options”. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Advanced NL tab, and click the Help button.
Table 2.4 Advanced NL Tab Options Option
For more information about this option, see the following section(s) in the ANSYS Structural Analysis Guide:
Specify analysis termination criteria [NCNV]
•
Section 8.5.2.3.3: Maximum Number of Equilibrium Iterations
Control activation and termination of the arc-length method [ARCLEN, ARCTRM]
•
Section 8.10.2.5: Using the Arc-Length Method
•
Chapter 2, “Loading” in the ANSYS Basic Analysis Guide
2.3.3. Set Additional Solution Options This section discusses additional options that you can set for the solution. These options do not appear on the Solution Controls dialog box because they are used very infrequently, and their default settings rarely need to be changed. ANSYS menu paths are provided in this section to help you access these options for those cases in which you choose to override the ANSYS-assigned defaults. Many of the options that appear in this section are nonlinear options, and are described further in Chapter 8, “Nonlinear Structural Analysis”.
2.3.3.1. Stress Stiffening Effects Some elements, including those in the 18x family of elements, include stress stiffening effects regardless of the SSTIF command setting. To determine whether an element includes stress stiffening, refer to the appropriate element description in the ANSYS Elements Reference. By default, stress stiffening effects are ON when NLGEOM is ON. Specific situations in which you can turn OFF stress stiffening effects include:
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–5
Chapter 2: Structural Static Analysis •
Stress stiffening is relevant only in nonlinear analyses. If you are performing a linear analysis [NLGEOM,OFF], you can turn stress stiffening OFF.
•
Prior to the analysis, you know that the structure is not likely to fail because of buckling (bifurcation, snap through).
Including stress stiffness terms, in general, accelerates nonlinear convergence characteristics. Keeping in mind the points listed above, you may choose to turn stress stiffening OFF for specific problems in which convergence difficulties are seen; for example, local failures. Command(s): SSTIF GUI: Main Menu> Solution> Unabridged Menu> Analysis Options
2.3.3.2. Newton-Raphson Option Use this analysis option only in a nonlinear analysis. This option specifies how often the tangent matrix is updated during solution. You can specify one of these values: •
Program-chosen (default)
•
Full
•
Modified
•
Initial stiffness
•
Full with unsymmetric matrix Command(s): NROPT GUI: Main Menu> Solution> Unabridged Menu> Analysis Options
2.3.3.3. Prestress Effects Calculation Use this analysis option to perform a prestressed analysis on the same model, such as a prestressed modal analysis. The default is OFF. Note — The stress stiffening effects and the prestress effect calculation both control the generation of the stress stiffness matrix, and therefore should not be used together in an analysis. If both are specified, the last option specified will override the previous setting. Command(s): PSTRES GUI: Main Menu> Solution> Unabridged Menu> Analysis Options
2.3.3.4. Mass Matrix Formulation Use this analysis option if you plan to apply inertial loads on the structure (such as gravity and spinning loads). You can specify one of these values: •
Default (depends on element type)
•
Lumped mass approximation Note — For a static analysis, the mass matrix formulation you use does not significantly affect the solution accuracy (assuming that the mesh is fine enough). However, if you want to do a prestressed dynamic analysis on the same model, the choice of mass matrix formulation may be important; see the appropriate dynamic analysis section for recommendations. Command(s): LUMPM GUI: Main Menu> Solution> Unabridged Menu> Analysis Options
2–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.3: Performing a Static Analysis
2.3.3.5. Reference Temperature This load step option is used for thermal strain calculations. Reference temperature can be made material-dependent with the MP,REFT command. Command(s): TREF GUI: Main Menu> Solution> Load Step Opts> Other> Reference Temp
2.3.3.6. Mode Number This load step option is used for axisymmetric harmonic elements. Command(s): MODE GUI: Main Menu> Solution> Load Step Opts> Other> For Harmonic Ele
2.3.3.7. Creep Criteria This nonlinear load step option specifies the creep criterion for automatic time stepping. Command(s): CRPLIM GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Creep Criterion
2.3.3.8. Printed Output Use this load step option to include any results data on the output file (Jobname.OUT). Command(s): OUTPR GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Output Ctrls> Solu Printout Caution: Proper use of multiple OUTPR commands can sometimes be a little tricky. See Section 2.7.4: Output Controls in the ANSYS Basic Analysis Guide for more information on how to use this command.
2.3.3.9. Extrapolation of Results Use this load step option to review element integration point results by copying them to the nodes instead of extrapolating them (default when no material nonlinearities are present). Command(s): ERESX GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Output Ctrls> Integration Pt
2.3.4. Apply the Loads After you set the desired solution options, you are ready to apply loads to the model.
2.3.4.1. Load Types All of the following load types are applicable in a static analysis.
2.3.4.1.1. Displacements (UX, UY, UZ, ROTX, ROTY, ROTZ) These are DOF constraints usually specified at model boundaries to define rigid support points. They can also indicate symmetry boundary conditions and points of known motion. The directions implied by the labels are in the nodal coordinate system.
2.3.4.1.2. Forces (FX, FY, FZ) and Moments (MX, MY, MZ) These are concentrated loads usually specified on the model exterior. The directions implied by the labels are in the nodal coordinate system. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–7
Chapter 2: Structural Static Analysis
2.3.4.1.3. Pressures (PRES) These are surface loads, also usually applied on the model exterior. Positive values of pressure act towards the element face (resulting in a compressive effect).
2.3.4.1.4. Temperatures (TEMP) These are applied to study the effects of thermal expansion or contraction (that is, thermal stresses). The coefficient of thermal expansion must be defined if thermal strains are to be calculated. You can read in temperatures from a thermal analysis [LDREAD], or you can specify temperatures directly, using the BF family of commands.
2.3.4.1.5. Fluences (FLUE) These are applied to study the effects of swelling (material enlargement due to neutron bombardment or other causes) or creep. They are used only if you input a swelling or creep equation.
2.3.4.1.6. Gravity, Spinning, Etc. These are inertia loads that affect the entire structure. Density (or mass in some form) must be defined if inertia effects are to be included.
2.3.4.2. Apply Loads to the Model Except for inertia loads, which are independent of the model, you can define loads either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). You can also apply boundary conditions via TABLE type array parameters (see Section 2.3.4.2.1: Applying Loads Using TABLE Type Array Parameters) or as function boundary conditions (see Section 2.6.15: Applying Loads Using Function Boundary Conditions). Table 2.5: “Loads Applicable in a Static Analysis” summarizes the loads applicable to a static analysis. In an analysis, loads can be applied, removed, operated on, or listed.
Table 2.5 Loads Applicable in a Static Analysis Load Type
Category
For details on commands and menu paths for defining these loads, see...
Displacement (UX, UY, UZ, ROTX, ROTY, Constraints ROTZ)
Section 2.6.3: DOF Constraints in the ANSYS Basic Analysis Guide
Force, Moment (FX, FY, FZ, MX, MY, MZ) Forces
Section 2.6.6: Forces (Concentrated Loads) in the ANSYS Basic Analysis Guide
Pressure (PRES)
Surface Loads
Section 2.6.7: Surface Loads in the ANSYS Basic Analysis Guide
Temperature (TEMP), Fluence (FLUE)
Body Loads
Section 2.6.8: Body Loads in the ANSYS Basic Analysis Guide
Gravity, Spinning, and so on
Inertia Loads
Section 2.6.9: Inertia Loads in the ANSYS Basic Analysis Guide
2.3.4.2.1. Applying Loads Using TABLE Type Array Parameters You can also apply loads using TABLE type array parameters. For details on using tabular boundary conditions, see Section 2.6.14: Applying Loads Using TABLE Type Array Parameters in the ANSYS Basic Analysis Guide. In a structural analysis, valid primary variables are TIME, TEMP, and location (X, Y, Z). 2–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.3: Performing a Static Analysis When defining the table, TIME must be in ascending order in the table index (as in any table array). You can define a table array parameter via command or interactively. For more information on defining table array parameters, see the ANSYS APDL Programmer's Guide.
2.3.4.3. Calculating Inertia Relief You can use a static analysis to perform inertia relief calculations, which calculate the accelerations that will counterbalance the applied loads. You can think of inertia relief as an equivalent free-body analysis. Issue this command before SOLVE as part of the inertia load commands. Your model should meet the following requirements: •
The model should not contain axisymmetric elements, substructures, or nonlinearities. Models with a mixture of 2-D and 3-D element types are not recommended.
•
The effects of offsets and tapering are ignored for beam elements (BEAM23, BEAM24, BEAM44, and BEAM54) as well as for layered elements (SHELL91, SHELL99, SOLID46, and SOLID191). The effects of unsymmetrical layups for layered elements are also ignored. (Breaking up each tapered element into several elements will give a more accurate solution.)
•
Data required for mass calculations (such as density) must be specified.
•
Specify only the minimum number of displacement constraints - those required to prevent rigid-body motion. Three constraints (or fewer, depending on the element type) are necessary for 2-D models and six (or fewer) are necessary for 3-D models. Additional constraints, such as those required to impose symmetry conditions, are permitted, but check for zero reaction forces at all the constraints to make sure that the model is not overconstrained for inertia relief.
•
The loads for which inertia relief calculations are desired should be applied. Command(s): IRLF,1 GUI: Main Menu> Solution> Load Step Opts> Other> Inertia Relief
2.3.4.3.1. Inertia Relief Output Use the IRLIST command to print the output from inertia relief calculations. This output consists of the translational and rotational accelerations required to balance the applied loads and can be used by other programs to perform kinematics studies. The summary listing of mass and moments of inertia (produced during solution) is accurate, not approximate. The reaction forces at the constraints will be zero because the calculated inertia forces balance the applied forces. Inertia relief output is stored in the database rather than in the results file (Jobname.RST). When you issue IRLIST, ANSYS pulls the information from the database, which contains the inertia relief output from the most recent solution [SOLVE or PSOLVE]. Command(s): IRLIST GUI: No GUI equivalent.
2.3.4.3.2. Partial Inertia Relief Calculations You can also do a partial inertia relief calculation. Use the partial solution method [PSOLVE], as shown in the command input below: /PREP7 ... ... MP,DENS,... ... ...
! Generate model, define density
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–9
Chapter 2: Structural Static Analysis FINISH /SOLU D,... F,... SF,... OUTPR,ALL,ALL IRLF,1 PSOLVE,ELFORM PSOLVE,ELPREP IRLIST FINISH
! Specify only minimum no. of constraints ! Other loads ! ! ! ! ! ! !
Activates printout of all items Can also be set to -1 for precise mass and load summary only, no inertia relief Calculates element matrices Modifies element matrices and calculates inertia relief terms Lists the mass summary and total load summary tables
See the ANSYS Commands Reference for discussions of the OUTPR, IRLF, IRLIST, and PSOLVE commands.
2.3.4.3.3. Using a Macro to Perform Inertia Relief Calculations If you need to do inertia relief calculations frequently, you can write a macro containing the above commands. Macros are described in the ANSYS APDL Programmer's Guide.
2.3.5. Solve the Analysis You are now ready to solve the analysis. 1.
Save a backup copy of the database to a named file. You can then retrieve your model by reentering the ANSYS program and issuing RESUME. Command(s): SAVE GUI: Utility Menu> File> Save as
2.
Start solution calculations. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
3.
If you want the analysis to include additional loading conditions (that is, multiple load steps), you will need to repeat the process of applying loads, specifying load step options, saving, and solving for each load step. (Other methods for handling multiple load steps are described in Chapter 2, “Loading” in the ANSYS Basic Analysis Guide.)
4.
Leave SOLUTION. Command(s): FINISH GUI: Close the Solution menu.
2.3.6. Review the Results Results from a static analysis are written to the structural results file, Jobname.RST. They consist of the following data: •
Primary data: –
•
2–10
Nodal displacements (UX, UY, UZ, ROTX, ROTY, ROTZ)
Derived data: –
Nodal and element stresses
–
Nodal and element strains
–
Element forces Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.3: Performing a Static Analysis –
Nodal reaction forces
–
and so on
2.3.6.1. Postprocessors You can review these results using POST1, the general postprocessor, and POST26, the time-history processor. •
POST1 is used to review results over the entire model at specific substeps (time-points). Some typical POST1 operations are explained below.
•
POST26 is used in nonlinear static analyses to track specific result items over the applied load history. See Chapter 8, “Nonlinear Structural Analysis” for the use of POST26 in a nonlinear static analysis. For a complete description of all postprocessing functions, see Chapter 4, “An Overview of Postprocessing” in the ANSYS Basic Analysis Guide.
2.3.6.2. Points to Remember •
To review results in POST1 or POST26, the database must contain the same model for which the solution was calculated.
•
The results file (Jobname.RST) must be available.
2.3.6.3. Reviewing Results Data 1.
Read in the database from the database file. Command(s): RESUME GUI: Utility Menu> File> Resume from
2.
Read in the desired set of results. Identify the data set by load step and substep numbers or by time. (If you specify a time value for which no results are available, the ANSYS program will perform linear interpolation on all the data to calculate the results at that time.) Command(s): SET GUI: Main Menu> General Postproc> Read Results> By Load Step
3.
Perform the necessary POST1 operations. Typical static analysis POST1 operations are explained below.
2.3.6.4. Typical Postprocessing Operations Option: Display Deformed Shape Use the PLDISP command to display a deformed shape (Main Menu> General Postproc> Plot Results> Deformed Shape). The KUND field on PLDISP gives you the option of overlaying the undeformed shape on the display. Option: List Reaction Forces and Moments The PRRSOL command lists reaction forces and moments at the constrained nodes (Main Menu> General Postproc> List Results> Reaction Solu). To display reaction forces, issue /PBC,RFOR,,1 and then request a node or element display [NPLOT or EPLOT]. (Use RMOM instead of RFOR for reaction moments.) Option: List Nodal Forces and Moments
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–11
Chapter 2: Structural Static Analysis Use the PRESOL,F (or M) command to list nodal forces and moments (Main Menu> General Postproc> List Results> Element Solution). You can list the sum of all nodal forces and moments for a selected set of nodes. Select a set of nodes and use this feature to find out the total force acting on those nodes: Command(s): FSUM GUI: Main Menu> General Postproc> Nodal Calcs> Total Force Sum You can also check the total force and total moment at each selected node. For a body in equilibrium, the total load is zero at all nodes except where an applied load or reaction load exists: Command(s): NFORCE GUI: Main Menu> General Postproc> Nodal Calcs> Sum @ Each Node The FORCE command (Main Menu> General Postproc> Options for Outp) dictates which component of the forces is being reviewed: •
Total (default)
•
Static component
•
Damping component
•
Inertia component
For a body in equilibrium, the total load (using all FORCE components) is zero at all nodes except where an applied load or reaction load exists. Option: Line Element Results For line elements, such as beams, spars, and pipes, use ETABLE to gain access to derived data (stresses, strains, and so on) (Main Menu> General Postproc> Element Table> Define Table). Results data are identified by a combination of a label and a sequence number or component name on the ETABLE command. See the ETABLE discussion in The General Postprocessor (POST1) in the ANSYS Basic Analysis Guide for details. Option: Error Estimation For linear static analyses using solid or shell elements, use the PRERR command to list the estimated solution error due to mesh discretization (Main Menu> General Postproc> List Results> Percent Error). This command calculates and lists the percent error in structural energy norm (SEPC), which represents the error relative to a particular mesh discretization. Option: Structural Energy Error Estimation Use PLESOL,SERR to contour the element-by-element structural energy error (SERR) (Main Menu> General Postproc> Plot Results> Contour Plot> Element Solu). Regions of high SERR on the contour display are good candidates for mesh refinement. (You can activate automatic mesh refinement by means of the ADAPT command - see the ANSYS Modeling and Meshing Guide for more information.) See Section 5.3.6: Estimating Solution Error in the ANSYS Basic Analysis Guide for more details about error estimation. Option: Contour Displays Use PLNSOL and PLESOL to contour almost any result item, such as stresses (SX, SY, SZ...), strains (EPELX, EPELY, EPELZ...), and displacements (UX, UY, UZ...) (Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu). The KUND field on PLNSOL and PLESOL gives you the option of overlaying the undeformed shape on the display. 2–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.4: A Sample Static Analysis (GUI Method) Use PLETAB and PLLS to contour element table data and line element data (Main Menu> General Postproc> Element Table> Plot Element Table and Main Menu> General Postproc> Plot Results> Contour Plot> Line Elem Res). Caution: Derived data, such as stresses and strains, are averaged at the nodes by the PLNSOL command. This averaging results in "smeared" values at nodes where elements of different materials, different shell thicknesses, or other discontinuities meet. To avoid the smearing effect, use selecting (described in Chapter 7, “Selecting and Components” in the ANSYS Basic Analysis Guide) to select elements of the same material, same shell thickness, and so on before issuing PLNSOL. Alternatively, use PowerGraphics with the AVRES command (Main Menu> General Postproc> Options for Outp) to not average results across different materials and/or different shell thicknesses. Option: Vector Displays Use PLVECT to view vector displays (Main Menu> General Postproc> Plot Results> Vector Plot> Predefined) and PRVECT to view vector listings (Main Menu> General Postproc> List Results> Vector Data). Vector displays (not to be confused with vector mode) are an effective way of viewing vector quantities, such as displacement (DISP), rotation (ROT), and principal stresses (S1, S2, S3). Option: Tabular Listings Use these commands to produce tabular listings: Command(s): PRNSOL (nodal results), PRESOL (element-by-element results) PRRSOL (reaction data), and so on GUI: Main Menu> General Postproc> List Results> solution option Use the NSORT and ESORT commands to sort the data before listing them (Main Menu> General Postproc> List Results> Sorted Listing> Sort Nodes or Sort Elems). Other Postprocessing Capabilities Many other postprocessing functions - mapping results onto a path, load case combinations, and so on - are available in POST1. See Chapter 4, “An Overview of Postprocessing” in the ANSYS Basic Analysis Guide for details.
2.4. A Sample Static Analysis (GUI Method) In this sample analysis, you will run a static analysis of an Allen wrench.
2.4.1. Problem Description An Allen wrench (10 mm across the flats) is torqued by means of a 100 N force at its end. Later, a 20 N downward force is applied at the same end, at the same time retaining the original 100 N torquing force. The objective is to determine the stress intensity in the wrench under these two loading conditions.
2.4.2. Problem Specifications The following dimensions are used for this problem: Width across flats = 10 mm Configuration = hexagonal Length of shank = 7.5 cm Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–13
Chapter 2: Structural Static Analysis Length of handle = 20 cm Bend radius = 1 cm Modulus of elasticity = 2.07 x 1011 Pa Applied torquing force = 100 N Applied downward force = 20 N
2.4.3. Problem Sketch Figure 2.1 Diagram of Allen Wrench
2.4.3.1. Set the Analysis Title 1.
Choose menu path Utility Menu> File> Change Title.
2.
Type the text "Static Analysis of an Allen Wrench" and click on OK.
2.4.3.2. Set the System of Units 1.
Click once in the Input Window to make it active for text entry.
2.
Type the command /UNITS,SI and press ENTER. Notice that the command is stored in the history buffer, which can be accessed by clicking on the down arrow at the right of the input window.
3.
Choose menu path Utility Menu> Parameters> Angular Units. The Angular Units for Parametric Functions dialog box appears.
4.
In the drop down menu for Units for angular parametric functions, select "Degrees DEG."
5.
Click on OK.
2.4.3.3. Define Parameters 1.
Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.
2.
Type the following parameters and their values in the Selection field. Click on Accept after you define each parameter. For example, first type “exx = 2.07e11” in the Selection field and then click on Accept. Continue entering the remaining parameters and values in the same way. Parameter EXX
2–14
Value 2.07E11
Description Young's modulus is 2.07E11 Pa
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.4: A Sample Static Analysis (GUI Method) Parameter
Value
Description
W_HEX
.01
Width of hex across flats = .01 m
W_FLAT
W_HEX* TAN(30)
Width of flat = .0058 m
L_SHANK
.075
Length of shank (short end) .075 m
L_HANDLE
.2
Length of handle (long end) .2 m
BENDRAD
.01
Bend radius .01 m
L_ELEM
.0075
Element length .0075 m
NO_D_HEX
2
Number of divisions along hex flat = 2
TOL
25E-6
Tolerance for selecting node = 25E-6 m
Note — You can type the labels in upper- or lowercase; ANSYS always displays the labels in uppercase. 3.
Click on Close.
4.
Click on SAVE_DB on the ANSYS Toolbar.
2.4.3.4. Define the Element Types 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
In the scroll box on the left, click once on "Structural Solid."
4.
In the scroll box on the right, click once on "Brick 8node 45."
5.
Click on Apply to define it as element type 1.
6.
Scroll up the list on the right to "Quad 4node 42." Click once to select it.
7.
Click on OK to define Quad 4node42 as element type 2. The Library of Element Types dialog box closes.
8.
Click on Close in the Element Types dialog box.
2.4.3.5. Define Material Properties 1.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
2.
In the Material Models Available window, double-click on the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
3.
Type the text EXX in the EX field (for Young's modulus), and .3 for PRXY. Click on OK. This sets Young's modulus to the parameter specified above. Material Model Number 1 appears in the Material Models Defined window on the left.
4.
Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
2.4.3.6. Create Hexagonal Area as Cross-Section 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Areas> Polygon> By Side Length. The Polygon by Side Length dialog box appears.
2.
Enter 6 for number of sides.
3.
Enter W_FLAT for length of each side. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–15
Chapter 2: Structural Static Analysis 4.
Click on OK. A hexagon appears in the ANSYS Graphics window.
2.4.3.7. Create Keypoints Along a Path 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Keypoints> In Active CS. The Create Keypoints in Active Coordinate System dialog box appears.
2.
Enter 7 for keypoint number. Type a 0 in each of the X, Y, Z location fields.
3.
Click on Apply.
4.
Enter 8 for keypoint number.
5.
Enter 0,0,-L_SHANK for the X, Y, Z location, and click on Apply.
6.
Enter 9 for keypoint number.
7.
Enter 0,L_HANDLE,-L_SHANK for the X, Y, Z location, and click on OK.
2.4.3.8. Create Lines Along a Path 1.
Choose menu path Utility Menu> PlotCtrls> Window Controls> Window Options. The Window Options dialog box appears.
2.
In the Location of triad drop down menu, select "At top left."
3.
Click on OK.
4.
Choose menu path Utility Menu> PlotCtrls> Pan/Zoom/Rotate. The Pan-Zoom-Rotate dialog box appears.
5.
Click on "Iso" to generate an isometric view and click on Close.
6.
Choose menu path Utility Menu> PlotCtrls> View Settings> Angle of Rotation. The Angle of Rotation dialog box appears.
7.
Enter 90 for angle in degrees.
8.
In the Axis of rotation drop down menu, select "Global Cartes X."
9.
Click on OK.
10. Choose menu path Utility Menu> PlotCtrls> Numbering. The Plot Numbering Controls dialog box appears. 11. Click the Keypoint numbers radio button to turn keypoint numbering on. 12. Click the Line numbers radio button to turn line numbering on. 13. Click on OK. 14. Choose menu path Main Menu> Preprocessor> Modeling> Create> Lines> Lines> Straight Line. The Create Straight Line picking menu appears. 15. Click once on keypoints 4 and 1 to create a line between keypoints 1 and 4. (If you have trouble reading the keypoint numbers in the ANSYS Graphics window, use the controls on the Pan-Zoom-Rotate dialog box (Utility Menu> PlotCtrls> Pan/Zoom/Rotate) to zoom in.) 16. Click once on keypoints 7 and 8 to create a line between keypoints 7 and 8. 17. Click once on keypoints 8 and 9 to create a line between keypoints 8 and 9. 18. Click on OK.
2–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.4: A Sample Static Analysis (GUI Method)
2.4.3.9. Create Line from Shank to Handle 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Lines> Line Fillet. The Line Fillet picking menu appears.
2.
Click once on lines 8 and 9.
3.
Click on OK in the picking menu. The Line Fillet dialog box appears.
4.
Enter BENDRAD for Fillet radius and click on OK.
5.
Click on SAVE_DB on the ANSYS Toolbar.
2.4.3.10. Cut Hex Section In this step, you cut the hex section into two quadrilaterals. This step is required to satisfy mapped meshing. 1.
Choose menu path Utility Menu> PlotCtrls> Numbering. The Plot Numbering Controls dialog box appears.
2.
Click the Keypoint numbers radio button to Off.
3.
Click on OK.
4.
Choose menu path Utility Menu> Plot> Areas.
5.
Choose menu path Main Menu> Preprocessor> Modeling> Operate> Booleans> Divide> With Options> Area by Line. The Divide Area by Line picking menu appears.
6.
Click once on the shaded area, and click on OK.
7.
Choose menu path Utility Menu> Plot> Lines.
8.
Click once on line 7. (If you have trouble reading the line numbers in the ANSYS Graphics window, use the controls on the Pan-Zoom-Rotate dialog box (Utility Menu> PlotCtrls> Pan/Zoom/Rotate) to zoom in.)
9.
Click on OK. The Divide Area by Line with Options dialog box appears. In the Subtracted lines will be drop down menu, select Kept. Click OK.
10. Choose menu path Utility Menu> Select> Comp/Assembly> Create Component. The Create Component dialog box appears. 11. Enter BOTAREA for component name. 12. In the Component is made of drop down menu, select "Areas." 13. Click on OK.
2.4.3.11. Set Meshing Density 1.
Choose menu path Main Menu> Preprocessor> Meshing> Size Cntrls> Lines> Picked Lines. The Element Size on Picked Lines picking menu appears.
2.
Enter 1,2,6 in the picker, then press ENTER.
3.
Click on OK in the picking menu. The Element Sizes on Picked Lines dialog box appears.
4.
Enter NO_D_HEX for number of element divisions and click on OK.
2.4.3.12. Set Element Type for Area Mesh In this step, set the element type to PLANE42, all quadrilaterals for the area mesh.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–17
Chapter 2: Structural Static Analysis 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes. The Element Attributes dialog box appears.
2.
In the Element type number drop down menu, select “2 PLANE42” and click on OK.
3.
Choose menu path Main Menu> Preprocessor> Meshing> Mesher Opts. The Mesher Options dialog box appears.
4.
In the Mesher Type field, click on the Mapped radio button and then click on OK. The Set Element Shape dialog box appears.
5.
Click on OK to accept the default of Quad for 2-D shape key.
6.
Click on SAVE_DB on the ANSYS Toolbar.
2.4.3.13. Generate Area Mesh In this step, generate the area mesh you will later drag. 1.
Choose menu path Main Menu> Preprocessor> Meshing> Mesh> Areas> Mapped> 3 or 4 sided. The Mesh Areas picking box appears.
2.
Click on Pick All.
3.
Choose menu path Utility Menu> Plot> Elements.
2.4.3.14. Drag the 2-D Mesh to Produce 3-D Elements 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes. The Element Attributes dialog box appears.
2.
In the Element type number drop down menu, select “1 SOLID45” and click on OK.
3.
Choose menu path Main Menu> Preprocessor> Meshing> Size Cntrls> Global> Size. The Global Element Sizes dialog box appears.
4.
Enter L_ELEM for element edge length and click on OK.
5.
Choose menu path Utility Menu> PlotCtrls> Numbering.
6.
Click the Line numbers radio button to on if it is not already selected.
7.
Click on OK.
8.
Choose menu path Utility Menu> Plot> Lines.
9.
Choose menu path Main Menu> Preprocessor> Modeling> Operate> Extrude> Areas> Along Lines. The Sweep Areas along Lines picking box appears.
10. Click on Pick All. A second picking box appears. 11. Click once on lines 8, 10, and 9 (in that order). 12. Click on OK. The 3-D model appears in the ANSYS Graphics window. 13. Choose menu path Utility Menu> Plot> Elements. 14. Click on SAVE_DB on the ANSYS Toolbar.
2.4.3.15. Select BOTAREA Component and Delete 2-D Elements 1.
Choose menu path Utility Menu> Select> Comp/Assembly> Select Comp/Assembly. The Select Component or Assembly dialog appears.
2.
Click on OK to accept the default of select BOTAREA component.
2–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.4: A Sample Static Analysis (GUI Method) 3.
Choose menu path Main Menu> Preprocessor> Meshing> Clear> Areas. The Clear Areas picking menu appears.
4.
Click on Pick All.
5.
Choose menu path Utility Menu> Select> Everything.
6.
Choose menu path Utility Menu> Plot> Elements.
2.4.3.16. Apply Displacement Boundary Condition at End of Wrench 1.
Choose menu path Utility Menu> Select> Comp/Assembly> Select Comp/Assembly. The Select Component or Assembly dialog appears.
2.
Click on OK to accept the default of select BOTAREA component.
3.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears.
4.
In the top drop down menu, select "Lines."
5.
In the second drop down menu, select "Exterior."
6.
Click on Apply.
7.
In the top drop down menu, select "Nodes."
8.
In the second drop down menu, select "Attached to."
9.
Click on the "Lines, all" radio button to select it.
10. Click on OK. 11. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears. 12. Click on Pick All. The Apply U,ROT on Nodes dialog box appears. 13. In the scroll list for DOFs to be constrained, click on "ALL DOF." 14. Click on OK. 15. Choose menu path Utility Menu> Select> Entities. 16. In the top drop down menu, select "Lines." 17. Click on the "Sele All" button, then click on Cancel.
2.4.3.17. Display Boundary Conditions 1.
Choose menu path Utility Menu> PlotCtrls> Symbols. The Symbols dialog box appears.
2.
Click on the "All Applied BCs" radio button for Boundary condition symbol.
3.
In the Surface Load Symbols drop down menu, select "Pressures."
4.
In the “Show pres and convect as” drop down menu, select "Arrows."
5.
Click on OK.
2.4.3.18. Apply Pressure on Handle In this step, apply pressure on the handle to represent 100 N finger force. 1.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog appears.
2.
In the top drop down menu, select "Areas."
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–19
Chapter 2: Structural Static Analysis 3.
In the second drop down menu, select "By Location."
4.
Click on the "Y coordinates" radio button to select it.
5.
Enter BENDRAD,L_HANDLE for Min, Max, and click on Apply.
6.
Click on "X coordinates" to select it.
7.
Click on Reselect.
8.
Enter W_FLAT/2,W_FLAT for Min, Max, and click on Apply.
9.
In the top drop down menu, select "Nodes."
10. In the second drop down menu, select "Attached to." 11. Click on the "Areas, all" radio button to select it. 12. Click on the "From Full" radio button to select it. 13. Click on Apply. 14. In the second drop down menu, select "By Location." 15. Click on the "Y coordinates" radio button to select it. 16. Click on the "Reselect" radio button. 17. Enter L_HANDLE+TOL,L_HANDLE-(3.0*L_ELEM)-TOL for Min, Max. 18. Click on OK. 19. Choose menu path Utility Menu> Parameters> Get Scalar Data. The Get Scalar Data dialog box appears. 20. In the scroll box on the left, scroll to "Model Data" and select it. 21. In the scroll box on the right, scroll to "For selected set" and select it. 22. Click on OK. The Get Data for Selected Entity Set dialog box appears. 23. Enter "minyval" for the name of the parameter to be defined. 24. In the scroll box on the left, click once on "Current node set" to select it. 25. In the scroll box on the right, click once on "Min Y coordinate" to select it. 26. Click on Apply. 27. Click on OK again to select the default settings. The Get Data for Selected Entity Set dialog box appears. 28. Enter "maxyval" for the name of the parameter to be defined. 29. In the scroll box on the left, click once on "Current node set" to select it. 30. In the scroll box on the right, click once on "Max Y coordinate" to select it. 31. Click on OK. 32. Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears. 33. Type the text PTORQ=100/(W_HEX*(MAXYVAL-MINYVAL)) in the Selection text box and click on Accept. 34. Click on Close. 35. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Pressure> On Nodes. The Apply PRES on Nodes picking menu appears. 36. Click on Pick All. The Apply PRES on Nodes dialog box appears. 37. Enter PTORQ for Load PRES value and click on OK. 38. Choose menu path Utility Menu> Select> Everything. 2–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.4: A Sample Static Analysis (GUI Method) 39. Choose menu path Utility Menu> Plot> Nodes. 40. Click on SAVE_DB on the ANSYS Toolbar.
2.4.3.19. Write the First Load Step 1.
Choose menu path Main Menu> Solution> Load Step Opts> Write LS File. The Write Load Step File dialog appears.
2.
Enter 1 for load step file number n.
3.
Click on OK.
2.4.3.20. Define Downward Pressure In this step, you define the downward pressure on top of the handle, representing 20N (4.5 lb) of force. 1.
Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.
2.
Type the text PDOWN=20/(W_FLAT*(MAXYVAL-MINYVAL)) in the Selection text box and click on Accept.
3.
Click on Close.
4.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog appears.
5.
In the top drop down menu, select "Areas."
6.
In the second drop down menu, select "By Location."
7.
Click on the "Z coordinates" radio button to select it.
8.
Click on the "From Full" radio button to select it.
9.
Enter -(L_SHANK+(W_HEX/2)) for Min, Max.
10. Click on Apply. 11. In the top drop down menu, select "Nodes." 12. In the second drop down menu, select "Attached to." 13. Click on the Areas, all radio button to select it, and click on Apply. 14. In the second drop down menu, select "By Location." 15. Click on the "Y coordinates" radio button to select it. 16. Click on the "Reselect" radio button. 17. Enter L_HANDLE+TOL,L_HANDLE-(3.0*L_ELEM)-TOL for Min, Max. 18. Click on OK. 19. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Pressure> On Nodes. The Apply PRES on Nodes picking menu appears. 20. Click on Pick All. The Apply PRES on Nodes dialog box appears. 21. Enter PDOWN for Load PRES value and click on OK. 22. Choose menu path Utility Menu> Select> Everything. 23. Choose menu path Utility Menu> Plot> Nodes.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–21
Chapter 2: Structural Static Analysis
2.4.3.21. Write Second Load Step 1.
Choose menu path Main Menu> Solution> Load Step Opts> Write LS File. The Write Load Step File dialog box appears.
2.
Enter 2 for Load step file number n, and click on OK.
3.
Click on SAVE_DB on the ANSYS Toolbar.
2.4.3.22. Solve from Load Step Files 1.
Choose menu path Main Menu> Solution> Solve> From LS Files. The Solve Load Step Files dialog box appears.
2.
Enter 1 for Starting LS file number.
3.
Enter 2 for Ending LS file number, and click on OK.
4.
Click on the Close button after the Solution is done! window appears.
2.4.3.23. Read First Load Step and Review Results 1.
Choose menu path Main Menu> General Postproc> Read Results> First Set.
2.
Choose menu path Main Menu> General Postproc> List Results> Reaction Solu. The List Reaction Solution dialog box appears.
3.
Click on OK to accept the default of All Items.
4.
Review the information in the status window, and click on Close.
5.
Choose menu path Utility Menu> PlotCtrls> Symbols. The Symbols dialog box appears.
6.
Click on the "None" radio button for Boundary condition symbol, and click on OK.
7.
Choose menu path Utility Menu> PlotCtrls> Style> Edge Options. The Edge Options dialog box appears.
8.
In the Element outlines for non-contour/contour plots drop down menu, select "Edge Only/All."
9.
Click on OK.
10. Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears. 11. Click on the "Def + undeformed" radio button and click on OK. 12. Choose menu path Utility Menu> PlotCtrls> Save Plot Ctrls. The Save Plot Controls dialog box appears. 13. Type "pldisp.gsa" in the Selection box, and click on OK. 14. Choose menu path Utility Menu> PlotCtrls> View Settings> Angle of Rotation. The Angle of Rotation dialog box appears. 15. Enter 120 for Angle in degrees. 16. In the Relative/absolute drop down menu, select "Relative angle." 17. In the Axis of rotation drop down menu, select "Global Cartes Y." 18. Click on OK. 19. Choose menu path Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu. The Contour Nodal Solution Data dialog box appears. 20. In the scroll box on the left, click on "Stress." In the scroll box on the right, click on "Intensity SINT." 21. Click on OK. 2–22
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.4: A Sample Static Analysis (GUI Method) 22. Choose menu path Utility Menu> PlotCtrls> Save Plot Ctrls. The Save Plot Controls dialog box appears. 23. Type "plnsol.gsa" in the Selection box, and click on OK.
2.4.3.24. Read the Next Load Step and Review Results 1.
Choose menu path Main Menu> General Postproc> Read Results> Next Set.
2.
Choose menu path Main Menu> General Postproc> List Results> Reaction Solu. The List Reaction Solution dialog box appears.
3.
Click on OK to accept the default of All Items.
4.
Review the information in the status window, and click on Close.
5.
Choose menu path Utility Menu> PlotCtrls> Restore Plot Ctrls.
6.
Type "pldisp.gsa" in the Selection box, and click on OK.
7.
Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears.
8.
Click on the "Def + undeformed" radio button if it is not already selected and click on OK.
9.
Choose menu path Utility Menu> PlotCtrls> Restore Plot Ctrls.
10. Type "plnsol.gsa" in the Selection box, and click on OK. 11. Choose menu path Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu. The Contour Nodal Solution Data dialog box appears. 12. In the scroll box on the left, click on "Stress." In the scroll box on the right, scroll to "Intensity SINT" and select it. 13. Click on OK.
2.4.3.25. Zoom in on Cross-Section 1.
Choose menu path Utility Menu> WorkPlane> Offset WP by Increments. The Offset WP tool box appears.
2.
Enter 0,0,-0.067 for X, Y, Z Offsets and click on OK.
3.
Choose menu path Utility Menu> PlotCtrls> Style> Hidden Line Options. The Hidden-Line Options dialog box appears.
4.
In the drop down menu for Type of Plot, select "Capped hidden."
5.
In the drop down menu for Cutting plane is, select "Working plane."
6.
Click on OK.
7.
Choose menu path Utility Menu> PlotCtrls> Pan-Zoom-Rotate. The Pan-Zoom-Rotate tool box appears.
8.
Click on "WP."
9.
Drag the Rate slider bar to 10.
10. On the Pan-Zoom-Rotate dialog box, click on the large round dot several times to zoom in on the cross section.
2.4.3.26. Exit ANSYS 1.
Choose QUIT from the ANSYS Toolbar.
2.
Choose Quit - No Save! Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–23
Chapter 2: Structural Static Analysis 3.
Click on OK.
2.5. A Sample Static Analysis (Command or Batch Method) You can perform the example static analysis of an Allen wrench using the ANSYS commands shown below instead of GUI choices. Items prefaced with an exclamation point (!) are comments. /FILNAME,pm02! Jobname to use for all subsequent files /TITLE,Static analysis of an Allen wrench /UNITS,SI ! Reminder that the SI system of units is used /SHOW ! Specify graphics driver for interactive run; for batch ! run plots are written to pm02.grph ! Define parameters for future use EXX=2.07E11 ! Young's modulus (2.07E11 Pa = 30E6 psi) W_HEX=.01 ! Width of hex across flats (.01m=.39in) *AFUN,DEG ! Units for angular parametric functions W_FLAT=W_HEX*TAN(30) ! Width of flat L_SHANK=.075 ! Length of shank (short end) (.075m=3.0in) L_HANDLE=.2 ! Length of handle (long end) (.2m=7.9 in) BENDRAD=.01 ! Bend radius of Allen wrench (.01m=.39 in) L_ELEM=.0075 ! Element length (.0075 m = .30 in) NO_D_HEX=2 ! Number of divisions on hex flat TOL=25E-6 ! Tolerance for selecting nodes (25e-6 m = .001 in) /PREP7 ET,1,SOLID45 ! Eight-node brick element ET,2,PLANE42 ! Four-node quadrilateral (for area mesh) MP,EX,1,EXX ! Young's modulus for material 1 MP,PRXY,1,0.3 ! Poisson's ratio for material 1 RPOLY,6,W_FLAT ! Hexagonal area K,7 ! Keypoint at (0,0,0) K,8,,,-L_SHANK ! Keypoint at shank-handle intersection K,9,,L_HANDLE,-L_SHANK ! Keypoint at end of handle L,4,1 ! Line through middle of hex shape L,7,8 ! Line along middle of shank L,8,9 ! Line along handle LFILLT,8,9,BENDRAD ! Line along bend radius between shank and handle /VIEW,,1,1,1 ! Isometric view in window 1 /ANGLE,,90,XM ! Rotates model 90 degrees about X /PNUM,LINE,1 ! Line numbers turned on LPLOT /PNUM,LINE,0 ! Line numbers off L,1,4 ! Hex section is cut into two quadrilaterals ASBL,1,7,,,KEEP ! to satisfy mapped meshing requirements for bricks CM,BOTAREA,AREA ! Component name BOTAREA for the two areas ! Generate area mesh for later drag LESIZE,1,,,NO_D_HEX ! Number of divisions along line 1 LESIZE,2,,,NO_D_HEX LESIZE,6,,,NO_D_HEX TYPE,2 ! PLANE42 elements to be meshed first MSHAPE,0,2D ! Mapped quad mesh MSHKEY,1 SAVE ! Save database before meshing AMESH,ALL /TITLE,Meshed hex wrench end to be used in vdrag EPLOT ! Now drag the 2-D mesh to produce 3-D elements TYPE,1 ! ESIZE,L_ELEM ! VDRAG,2,3,,,,,8,10,9 ! /TYPE,,HIDP ! /TITLE,Meshed hex wrench EPLOT CMSEL,,BOTAREA !
2–24
Type pointer set to SOLID45 Element size Drag operation to create 3-D mesh Precise hidden line display
Select BOTAREA component and
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.5: A Sample Static Analysis (Command or Batch Method) ACLEAR,ALL ASEL,ALL FINISH
!
delete the 2-D elements
! Apply loads and obtain the solution /SOLU ANTYPE,STATIC ! Static analysis (default) /TITLE,Allen wrench -- Load step 1 ! First fix all nodes around bottom of shank CMSEL,,BOTAREA ! Bottom areas of shank LSEL,,EXT ! Exterior lines of those areas NSLL,,1 ! Nodes on those lines D,ALL,ALL ! Displacement constraints LSEL,ALL /PBC,U,,1 ! Displacement symbols turned on /TITLE,Boundary conditions on end of wrench NPLOT !Now apply pressure on handle to represent 100-N (22.5-lb) finger force ASEL,,LOC,Y,BENDRAD,L_HANDLE ! Areas on handle ASEL,R,LOC,X,W_FLAT/2,W_FLAT ! Two areas on one side of handle... NSLA,,1 ! ...and all corresponding nodes NSEL,R,LOC,Y,L_HANDLE+TOL,L_HANDLE-(3.0*L_ELEM)-TOL ! Reselects nodes at ! back end of handle (3 element lengths) *GET,MINYVAL,NODE,,MNLOC,Y ! Get minimum Y value of selected nodes *GET,MAXYVAL,NODE,,MXLOC,Y ! Get maximum Y value of selected nodes PTORQ=100/(W_HEX*(MAXYVAL-MINYVAL)) ! Pressure equivalent to 100 N SF,ALL,PRES,PTORQ ! PTORQ pressure on all selected nodes ALLSEL ! Restores full set of all entities /PSF,PRES,,2 ! Pressure symbols turned on /TITLE,Boundary conditions on wrench for load step 1 NPLOT LSWRITE ! Writes first load step /TITLE, Allen wrench -- load step 2 ! Downward pressure on top of handle, representing 20-N (4.5 -lb) force PDOWN=20/(W_FLAT*(MAXYVAL-MINYVAL)) ASEL,,LOC,Z,-(L_SHANK+(W_HEX/2)) ! Area on top flat of handle... NSLA,,1 ! ...and all corresponding nodes NSEL,R,LOC,Y,L_HANDLE+TOL,L_HANDLE-(3.0*L_ELEM)-TOL ! Reselects nodes at ! back end of handle (3 element lengths) SF,ALL,PRES,PDOWN ! PDOWN pressure at all selected nodes ALLSEL /TITLE,Boundary conditions on wrench for load step 2 NPLOT LSWRITE ! Writes second load step SAVE ! Save database before solution LSSOLVE,1,2 ! Initiates solution for load step files 1 and 2 FINISH !Review the results /POST1 SET,1 ! Reads load step 1 results PRRSOL ! Reaction solution listing /PBC,DEFA ! No BC symbols /PSF,DEFA ! No surface load symbols /EDGE,,1 ! Edges only, no interior element outlines /TITLE,Deformed allen wrench caused by torque PLDISP,2 ! Deformed shape overlaid with undeformed edge plot /GSAVE,pldisp,gsav ! Saves graphics specifications on pldisp.gsav /PLOPTS,INFO,ON ! Turns on entire legend column /PLOPTS,LEG1,OFF ! Turns off legend header /ANGLE,,120,YM,1 ! Additional rotation about model Y (to see high stress areas) /TITLE,Stress intensity contours caused by torque PLNSOL,S,INT ! Stress intensity contours
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–25
Chapter 2: Structural Static Analysis /GSAVE,plnsol,gsav ! Saves graphics specifications to plnsol.gsav SET,2 ! Reads load step 2 results PRRSOL ! Reaction solution listing /GRESUME,pldisp,gsav ! Resumes graphics specifications from pldisp.gsav /TITLE,Deformed allen wrench caused by torque and force PLDISP,2 /GRESUME,plnsol,gsav ! Resumes graphics specifications from plnsol.gsav /TITLE,Stress intensity contours caused by torque and force PLNSOL,S,INT WPOF,,,-0.067 ! Offset the working plane for cross-section view /TYPE,1,5 ! Capped hidden display /CPLANE,1 ! Cutting plane defined to use the WP /VIEW, 1 ,WP ! View will be normal to the WP /DIST,1,.01 ! Zoom in on the cross section /TITLE,Cross section of the allen wrench under torque and force loading PLNSOL,S,INT FINISH /EXIT,ALL
2.6. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual and the ANSYS Tutorials, describe additional structural static analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS family of products. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual includes the following structural static analysis test cases: VM1 - Statically Indeterminate Reaction Force Analysis VM2 - Beam Stresses and Deflections VM4 - Deflection of a Hinged Support VM11 - Residual Stress Problem VM12 - Combined Bending and Torsion VM13 - Cylindrical Shell Under Pressure VM16 - Bending of a Solid Beam VM18 - Out-of-plane Bending of a Curved Bar VM20 - Cylindrical Membrane Under Pressure VM25 - Stresses in a Long Cylinder VM29 - Friction on a Support Block VM31 - Cable Supporting Hanging Loads VM36 - Limit Moment Analysis VM39 - Bending of a Circular Plate with a Center Hole VM41 - Small Deflection of a Rigid Beam VM44 - Bending of an Axisymmetric Thin Pipe Under Gravity Loading VM53 - Vibration of a String Under Tension VM59 - Lateral Vibration of an Axially Loaded Bar VM63 - Static Hertz Contact Problem VM78 - Transverse Shear Stresses in a Cantilever Beam VM82 - Simply Supported Laminated Plate Under Pressure VM127 - Buckling of a Bar with Hinged Ends VM135 - Bending of a Beam on an Elastic Foundation VM141 - Diametric Compression of a Disk VM148 - Bending of a Parabolic Beam VM183 - Harmonic Response of a Spring-Mass System 2–26
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 2.6: Where to Find Other Examples VM199 - Viscoplastic Analysis of a Body Undergoing Shear Deformation VM201 - Rubber Cylinder Pressed Between Two Plates VM206 - Stranded Coil with Voltage Excitation VM211 - Rubber Cylinder Pressed Between Two Plates VM216 - Lateral Buckling of a Right-Angle Frame
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
2–27
2–28
Chapter 3: Modal Analysis 3.1. Definition of Modal Analysis You use modal analysis to determine the vibration characteristics (natural frequencies and mode shapes) of a structure or a machine component while it is being designed. It also can be a starting point for another, more detailed, dynamic analysis, such as a transient dynamic analysis, a harmonic response analysis, or a spectrum analysis.
3.2. Uses for Modal Analysis You use modal analysis to determine the natural frequencies and mode shapes of a structure. The natural frequencies and mode shapes are important parameters in the design of a structure for dynamic loading conditions. They are also required if you want to do a spectrum analysis or a mode superposition harmonic or transient analysis. You can do modal analysis on a prestressed structure, such as a spinning turbine blade. Another useful feature is modal cyclic symmetry, which allows you to review the mode shapes of a cyclically symmetric structure by modeling just a sector of it. Modal analysis in the ANSYS family of products is a linear analysis. Any nonlinearities, such as plasticity and contact (gap) elements, are ignored even if they are defined. You can choose from several mode-extraction methods: Block Lanczos (default), subspace, PowerDynamics, reduced, unsymmetric, damped, and QR damped. The damped and QR damped methods allow you to include damping in the structure. Details about mode-extraction methods are covered later in this section.
3.3. Overview of Steps in a Modal Analysis The procedure for a modal analysis consists of four main steps: 1.
Build the model.
2.
Apply loads and obtain the solution.
3.
Expand the modes.
4.
Review the results.
3.4. Build the Model See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details, see the ANSYS Modeling and Meshing Guide. When building your model, remember these points: •
Only linear behavior is valid in a modal analysis. If you specify nonlinear elements, they are treated as linear. For example, if you include contact elements, their stiffnesses are calculated based on their initial status and never change.
•
Material properties can be linear, isotropic or orthotropic, and constant or temperature-dependent. You must define both Young's modulus (EX) (or stiffness in some form) and density (DENS) (or mass in some form) for a modal analysis. Nonlinear properties are ignored. If applying element damping, you must define the required real constants for the specific element type (COMBIN7, COMBIN14, COMBIN37, and so on). Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 3: Modal Analysis
3.5. Apply Loads and Obtain the Solution In this step you define the analysis type and options, apply loads, specify load step options, and begin the finite element solution for the natural frequencies.
3.5.1. Enter the Solution Processor 1.
Enter the ANSYS solution processor. Command(s): /SOLU GUI: Main Menu> Solution
3.5.2. Define Analysis Type and Options After you have entered the solution processor, you define the analysis type and analysis options. ANSYS offers the options listed in Table 3.1: “Analysis Types and Options” for a modal analysis. Each of the options is explained in detail below.
Table 3.1 Analysis Types and Options Option
Command
GUI Path
New Analysis
ANTYPE
Main Menu> Solution> Analysis Type> New Analysis
Analysis Type: Modal (see Note below)
ANTYPE
Main Menu> Solution> Analysis Type> New Analysis> Modal
mode-extraction Method
MODOPT
Main Menu> Solution> Analysis Type> Analysis Options
Number of Modes to Extract
MODOPT
Main Menu> Solution> Analysis Type> Analysis Options
No. of Modes to Expand (see Note below) MXPAND
Main Menu> Solution> Analysis Type> Analysis Options
Mass Matrix Formulation
LUMPM
Main Menu> Solution> Analysis Type> Analysis Options
Prestress Effects Calculation
PSTRES
Main Menu> Solution> Analysis Type> Analysis Options
Note — When you specify a modal analysis, a Solution menu that is appropriate for modal analyses appears. The Solution menu will be either “abridged” or “unabridged,” depending on the actions you took prior to this step in your ANSYS session. The abridged menu contains only those solution options that are valid and/or recommended for modal analyses. If you are on the abridged Solution menu and you want to access other solution options (that is, solution options that are valid for you to use, but their use may not be encouraged for this type of analysis), select the Unabridged Menu option. For details, see Section 3.11.1: Using Abridged Solution Menus in the ANSYS Basic Analysis Guide. Note — In the single point response spectrum (SPOPT,SPRS) and Dynamic Design analysis method (SPOPT,DDAM), the modal expansion can be performed after the spectrum analysis, based on the significance factor SIGNIF on the MXPAND command. If you want to perform modal expansion after the spectrum analysis, choose NO for mode expansion (MXPAND) on the dialog box for the modal analysis options (MODOPT).
3.5.2.1. Option: New Analysis [ANTYPE] Choose New Analysis. Note — Restarts are not valid in a modal analysis. If you need to apply different sets of boundary conditions, do a new analysis each time (or use the "partial solution" procedure described in Chapter 3, “Solution” in the ANSYS Basic Analysis Guide). 3–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.5: Apply Loads and Obtain the Solution
3.5.2.2. Option: Analysis Type: Modal [ANTYPE] Use this option to specify a modal analysis.
3.5.2.3. Option: Mode-Extraction Method [MODOPT] Choose one of the extraction methods listed below. (For more detailed information, see Section 3.13: Comparing Mode-Extraction Methods.) •
Block Lanczos method (default) The Block Lanczos method is used for large symmetric eigenvalue problems. You can use this method for the same types of problems for which you use the subspace method, but you achieve a faster convergence rate. The Block Lanczos method uses the sparse matrix solver, overriding any solver specified via the EQSLV command.
•
Subspace method The subspace method is used for large symmetric eigenvalue problems. Several solution controls are available to control the subspace iteration process. When doing a modal analysis with a large number of constraint equations, use the subspace method with the frontal solver instead of the JCG solver, or use the Block Lanczos mode-extraction method.
•
PowerDynamics method The PowerDynamics method is used for very large models (100,000+ DOFs), and is especially useful to obtain a solution for the first several modes to learn how the model will behave. You can then choose the most appropriate extraction method (subspace or Block Lanczos) for running the final solution. This method automatically uses the lumped mass approximation (LUMPM,ON) To use the PowerDynamics method when running in batch or command mode, you first issue MODOPT,SUBSPACE, followed by EQSLV,PCG. (The PCGOUT solver can also be used, but it is very slow.)
•
Reduced (Householder) method The reduced method is faster than the subspace method because it uses reduced (condensed) system matrices to calculate the solution. However, it is less accurate because the reduced mass matrix is approximate. (See Section 3.13: Comparing Mode-Extraction Methods.)
•
Unsymmetric method The unsymmetric method is used for problems with unsymmetric matrices, such as fluid-structure interaction problems.
•
Damped method The damped method is used for problems where damping cannot be ignored, such as bearing problems.
•
QR Damped method The QR damped method is faster and achieves better calculation efficiency than the damped method. It uses the reduced modal damped matrix to calculate complex damped frequencies in modal coordinates.
For most applications, you will use the Block Lanczos, subspace, reduced, or PowerDynamics method. The unsymmetric, damped, and QR damped methods are meant for special applications. When you specify a mode-extraction method, ANSYS automatically chooses the appropriate equation solver. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–3
Chapter 3: Modal Analysis Note — The damped, unsymmetric, and QR damped methods are not available in the ANSYS Professional program.
3.5.2.4. Option: Number of Modes to Extract [MODOPT] This option is required for all mode-extraction methods except the reduced method. For the unsymmetric and damped methods, requesting a larger number of modes than necessary reduces the possibility of missed modes, but results in more solution time.
3.5.2.5. Option: Number of Modes to Expand [MXPAND] This option is required for the reduced, unsymmetric, and damped methods only. However, if you want element results, you need to turn on the "Calculate elem results" option, regardless of the mode-extraction method. In the single point response spectrum (SPOPT,SPRS) and Dynamic Design analysis method (SPOPT,DDAM), the modal expansion can be performed after the spectrum analysis, based on the significance factor SIGNIF on the MXPAND command. If you want to perform modal expansion after the spectrum analysis, choose NO for mode expansion (MXPAND) on the dialog box for the modal analysis options (MODOPT). If you want the mode shapes normalized to unity for the Block Lanczos or subspace methods, you will need to expand the modes as well.
3.5.2.6. Option: Mass Matrix Formulation [LUMPM] Use this option to specify the default formulation (which is element-dependent) or lumped mass approximation. We recommend the default formulation for most applications. However, for some problems involving "skinny" structures such as slender beams or very thin shells, the lumped mass approximation often yields better results. Also, the lumped mass approximation can result in a shorter run time and lower memory requirements.
3.5.2.7. Option: Prestress Effects Calculation [PSTRES] Use this option to calculate the modes of a prestressed structure. By default, no prestress effects are included; that is, the structure is assumed to be stress-free. To include prestress effects, element files from a previous static (or transient) analysis must be available; see Section 3.11: Prestressed Modal Analysis. If prestress effects are turned on, the lumped mass setting [LUMPM] in this and subsequent solutions must be the same as it was in the prestress static analysis. Note — You can use only axisymmetric loads for prestressing harmonic elements such as PLANE25 and SHELL61.
3.5.2.8. Additional Modal Analysis Options After you complete the fields on the Modal Analysis Options dialog box, click OK. A dialog box specific to the selected extraction method appears. You see some combination of the following fields: FREQB, FREQE, PRMODE, Nrmkey, RIGID, SUBOPT. Refer to the MODOPT and RIGID command descriptions for the meaning of these fields.
3.5.3. Define Master Degrees of Freedom In a modal analysis, you also need to define master degrees of freedom. These are required only for the reduced mode-extraction method. Master degrees of freedom (MDOF) are significant degrees of freedom that characterize the dynamic behavior of the structure. You should choose at least twice as many MDOF as the number of modes of interest. We recommend that you define as many MDOF as you can based on your knowledge of the dynamic characteristics of the 3–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.5: Apply Loads and Obtain the Solution structure [M,MGEN], and also let the program choose a few additional masters based on stiffness-to-mass ratios [TOTAL]. You can list the defined MDOF [MLIST], and delete extraneous MDOF [MDELE]. For more details about master degrees of freedom, see Section 3.14: Matrix Reduction. Command(s): M GUI: Main Menu> Solution> Master DOFs> User Selected> Define
3.5.4. Apply Loads After defining master degrees of freedom, apply loads on the model. The only "loads" valid in a typical modal analysis are zero-value displacement constraints. (If you input a nonzero displacement constraint, the program assigns a zero-value constraint to that DOF instead.) Other loads can be specified, but are ignored (see Note below). For directions in which no constraints are specified, the program calculates rigid-body (zero-frequency) as well as higher (nonzero frequency) free body modes. Table 3.2: “Loads Applicable in a Modal Analysis” shows the commands to apply displacement constraints. Notice that you can apply them either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). For a general discussion of solid-model loads versus finite-element loads, see Chapter 2, “Loading” in the ANSYS Basic Analysis Guide. Note — Other loads - forces, pressures, temperatures, accelerations, and so on - can be specified in a modal analysis, but they are ignored for the mode-extraction. However, the program will calculate a load vector and write it to the mode shape file (Jobname.MODE) so that it can be used in a subsequent modesuperposition harmonic or transient analysis.
Table 3.2 Loads Applicable in a Modal Analysis Load Type
Category
Cmd Family
Displacement (UX, UY, UZ, ROTX, Constraints D ROTY, ROTZ)
GUI Path Main Menu> Solution> Define Loads> Apply> Structural> Displacement
In an analysis, loads can be applied, removed, operated on, or listed.
3.5.4.1. Applying Loads Using Commands Table 3.3: “Load Commands for a Modal Analysis” lists all the commands you can use to apply loads in a modal analysis.
Table 3.3 Load Commands for a Modal Analysis Load Type Displacement
Solid Model or FE
Entity
Apply
Delete
List
Operate
Apply Settings
Solid Model
Keypoints
DK
DKDELE
DKLIST
DTRAN
-
Solid Model
Lines
DL
DLDELE
DLLIST
DTRAN
-
Solid Model
Areas
DA
DADELE
DALIST
DTRAN
-
Finite Elem
Nodes
D
DDELE
DLIST
DSCALE
DSYM, DCUM
3.5.4.2. Applying Loads Using the GUI All loading operations (except List; see Section 3.5.4.3: Listing Loads) are accessed through a series of cascading menus. From the Solution menu, you select the operation (apply, delete, and so on), then the load type (displacement, force, and so on), and then the object to which you are applying the load (keypoint, line, node, and so on).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–5
Chapter 3: Modal Analysis For example, to apply a displacement load to a line, follow this GUI path: GUI: Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On lines
3.5.4.3. Listing Loads To list existing loads, follow this GUI path: GUI: Utility Menu> List>Loads> load type
3.5.5. Specify Load Step Options The only load step options available for a modal analysis are damping options.
Table 3.4 Load Step Options Option
Command
Damping (Dynamics) Options Alpha (mass) Damping
ALPHAD
Beta (stiffness) Damping
BETAD
Material-Dependent Damping Ratio
MP,DAMP
Element Damping (applied via element real constant) R Constant Material Damping Coefficient
MP,DMPR
Damping is valid only for the damped and QR damped mode-extraction methods. Damping is ignored for the other mode-extraction methods; see the Note below. If you include damping and specify the damped mode-extraction method, the calculated eigenvalues and eigenvectors are complex. If you include damping and specify the QR damped mode-extraction method, the eigenvalues are complex. However, the real eigenvectors are used for the mode superposition analysis. See Section 3.13: Comparing Mode-Extraction Methods for details. Also see the section Section 5.10.3: Damping in Chapter 5, “Transient Dynamic Analysis” for more information on damping. Only the QR damped method supports the constant material damping coefficient application in a downstream mode superposition harmonic analysis. The QR damped eigen analysis itself, however, does not include the effect of the constant material damping coefficient. The corresponding modal damping matrix is formulated during modal harmonic analysis. Note — Damping can be specified in a non-damped modal analysis if a single-point response spectrum analysis is to follow the modal analysis. Although the damping does not affect the eigenvalue solution, it is used to calculate an effective damping ratio for each mode, which is then used to calculate the response to the spectrum. Spectrum analyses are discussed in Chapter 6, “Spectrum Analysis”.
3.5.6. Participation Factor Table Output The participation factor table lists participation factors, mode coefficients, and mass distribution percentages for each mode extracted. The participation factors and mode coefficients are calculated based on an assumed unit displacement spectrum in each of the global Cartesian directions and rotation about each of these axes.
3–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.5: Apply Loads and Obtain the Solution The reduced mass distribution is also listed. Rotational participation factors will be calculated when a real eigensolver mode-extraction method (such as Block Lanczos, subspace, or QRDAMP) is used. Note — You can retrieve a participation factor or mode coefficient by issuing a *GET command. The factor or coefficient is valid for the excitation (assumed unit displacement spectrum) directed along the last of the applicable coordinates (rotation about the Z axis for a 3-D analysis). To retrieve a participation factor or mode coefficient for another direction, perform a spectrum analysis with the excitation set (SED) to the desired direction, then issue another *GET command.
3.5.7. Solve Before you solve, you should save (SAVE) a back-up copy of the database to a named file. You can then retrieve your model by reentering the ANSYS program and issuing RESUME. Now start the solution calculations. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
3.5.7.1. Output The output from the solution consists mainly of the natural frequencies, which are printed as part of the printed output (Jobname.OUT) and also written to the mode shape file (Jobname.MODE). The printed output may include reduced mode shapes and the participation factor table, depending on your analysis options and output controls. No mode shapes are written to the database or to the results file, so you cannot postprocess the results yet. To do this, you need to expand the modes (explained next).
3.5.7.1.1. Output From Subspace Mode-Extraction Method If you use the subspace mode-extraction method, you might see the following warning in the solution printout: "STURM number = n should be m," where n and m are integer numbers. This indicates that a mode has been missed, or that the mthand nth mode gave the same frequencies and only m modes were requested. There are two methods that you can use to investigate the missed mode: use more iteration vectors, or change the shift point used in the eigenvalue extraction. Both methods are briefly described below. (See the ANSYS, Inc. Theory Reference for more information.) To use more iteration vectors, you can issue the SUBOPT,,NPAD command. If you prefer to use the GUI to adjust the number of iteration vectors, follow these steps: 1.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Modal Analysis dialog box appears.
2.
Choose “Subspace” as the mode-extraction method and specify the number of modes to extract; then click OK. The Subspace Modal Analysis dialog box appears.
3.
Change the value of the NPAD field and click OK.
To change the shift point that was used in the eigenvalue extraction, you can issue the MODOPT,,,FREQB command. If you prefer to use the GUI to change the shift point, follow these steps: 1.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Modal Analysis dialog box appears.
2.
Choose “Subspace” as the mode-extraction method and specify the number of modes to extract; then click OK. The Subspace Modal Analysis dialog box appears. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–7
Chapter 3: Modal Analysis 3.
Change the value of the FREQB field and click OK.
If you use the damped mode-extraction method, the eigenvalues and eigenvectors are complex. The imaginary part of the eigenvalue represents the natural frequency, and the real part is a measure of the stability of the system. If you use the QR damped mode-extraction method, the eigenvalues are complex. However, the real eigenvectors are used for the mode superposition analysis.
3.5.8. Exit the Solution Processor You must now exit the solution processor. Command(s): FINISH GUI: Main Menu> Finish
3.6. Expand the Modes In its strictest sense, the term "expansion" means expanding the reduced solution to the full DOF set. The "reduced solution" is usually in terms of master DOF. In a modal analysis, however, we use the term "expansion" to mean writing mode shapes to the results file. That is, "expanding the modes" applies not just to reduced mode shapes from the reduced mode-extraction method, but to full mode shapes from the other mode-extraction methods as well. Thus, if you want to review mode shapes in the postprocessor, you must expand them (that is, write them to the results file). Expanded modes are also required for subsequent spectrum analyses. In the single point response spectrum (SPOPT,SPRS) and Dynamic Design analysis method (SPOPT,DDAM), the modal expansion can be performed after the spectrum analysis, based on the significance factor SIGNIF on the MXPAND command. If you want to perform modal expansion after the spectrum analysis, choose NO for mode expansion (MXPAND) on the dialog box for the modal analysis options (MODOPT). No expansion is necessary for subsequent mode superposition analyses.
3.6.1. Points to Remember •
The mode shape file (Jobname.MODE), Jobname.EMAT, Jobname.ESAV, and Jobname.TRI (if reduced method) must be available.
•
The database must contain the same model for which the modal solution was calculated.
3.6.2. Expanding the Modes 1.
Reenter the ANSYS solution processor. Command(s): /SOLU GUI: Main Menu> Solution Note — You must explicitly leave SOLUTION (using the FINISH command) and reenter (/SOLU) before performing the expansion pass.
2.
Activate the expansion pass and its options. ANSYS offers these options for the expansion pass:
Table 3.5 Expansion Pass Options Option Expansion Pass On/Off
Command EXPASS
No. of Modes to Expand MXPAND
3–8
GUI Path Main Menu> Solution> Analysis Type> ExpansionPass Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> Expand Modes
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.6: Expand the Modes Option
Command
GUI Path
Freq. Range for Expansion MXPAND
Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> Expand Modes
MXPAND
Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> Expand Modes
Stress Calc. On/Off
Each of these options is explained in detail below. Expansion Pass On/Off [EXPASS] Choose ON. Number of Modes to Expand [MXPAND, NMODE] Specify the number. Remember that only expanded modes can be reviewed in the postprocessor. Default is no modes expanded. Frequency Range for Expansion [MXPAND,, FREQB, FREQE] This is another way to control the number of modes expanded. If you specify a frequency range, only modes within that range are expanded. Stress Calculations On/Off [MXPAND,,,, Elcalc] Choose ON only if you plan to do a subsequent spectrum analysis and are interested in stresses or forces to do the spectrum. "Stresses" from a modal analysis do not represent actual stresses in the structure, but give you an idea of the relative stress distributions for each mode. Default is no stresses calculated. 3.
Specify load step options. The only options valid in a modal expansion pass are output controls: •
Printed output Use this option to include any results data (expanded mode shapes, stresses, and forces) on the printed output file (Jobname.OUT). Command(s): OUTPR GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout
•
Database and results file output Use this option to control the data on the results file (Jobname.RST). The FREQ field on OUTRES can be only ALL or NONE; that is, the data are written for all modes or no modes. For example, you cannot write information for every other mode. Command(s): OUTRES GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> DB/Results File
4.
Start expansion pass calculations. The output consists of expanded mode shapes and, if requested, relative stress distributions for each mode. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
5.
Repeat steps 2, 3, and 4 for additional modes to be expanded (in different frequency ranges, for example). Each expansion pass is stored as a separate load step on the results file.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–9
Chapter 3: Modal Analysis Caution: Spectrum analyses expect all expanded modes to be in one load step. In the single point response spectrum (SPOPT,SPRS) and Dynamic Design analysis method (SPOPT,DDAM), the modal expansion can be performed after the spectrum analysis, based on the significance factor SIGNIF on the MXPAND command. If you want to perform modal expansion after the spectrum analysis, choose NO for mode expansion (MXPAND) on the dialog box for the modal analysis options (MODOPT). 6.
Leave SOLUTION. You can now review results in the postprocessor. Command(s): FINISH GUI: Close the Solution menu.
Note — The expansion pass has been presented here as a separate step. However, if you include the MXPAND command in the modal solution step, the program not only extracts the eigenvalues and eigenvectors, but also expands the specified mode shapes.
3.7. Review the Results Results from a modal analysis (that is, the modal expansion pass) are written to the structural results file, Jobname.RST. Results consist of: •
Natural frequencies
•
Expanded mode shapes
•
Relative stress and force distributions (if requested).
You can review these results in POST1 [/POST1], the general postprocessor. Some typical postprocessing operations for a modal analysis are described below. For a complete description of all postprocessing functions, see Chapter 4, “An Overview of Postprocessing” in the ANSYS Basic Analysis Guide.
3.7.1. Points to Remember •
If you want to review results in POST1, the database must contain the same model for which the solution was calculated.
•
The results file (Jobname.RST) must be available.
3.7.2. Reviewing Results Data 1.
Read in results data from the appropriate substep. Each mode is stored on the results file as a separate substep. If you expand six modes, for instance, your results file will have one load step consisting of six substeps. Command(s): SET,SBSTEP GUI: Main Menu> General Postproc> Read Results> substep
2.
Perform any desired POST1 operations. Typical modal analysis POST1 operations are explained below:
3.7.3. Option: Listing All Frequencies You may want to list the frequencies of all modes expanded. A sample output from this command is shown below. ***** INDEX OF DATA SETS ON RESULTS FILE ***** SET TIME/FREQ LOAD STEP SUBSTEP CUMULATIVE 1 22.973 1 1 1 2 40.476 1 2 2
3–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.7: Review the Results 3 4
78.082 188.34
1 1
3 4
3 4
Command(s): SET,LIST GUI: Main Menu> General Postproc> List Results
3.7.4. Option: Display Deformed Shape Command(s): PLDISP GUI: Main Menu> General Postproc> Plot Results> Deformed Shape Use the KUND field on PLDISP to overlay the nondeformed shape on the display.
3.7.5. Option: List Master DOF Command(s): MLIST,ALL GUI: Main Menu> Solution> Master DOFs> User Selected> List All Note — To display the master DOFs graphically, plot the nodes (Utility Menu> Plot> Nodes or command NLIST).
3.7.6. Option: Line Element Results Command(s): ETABLE GUI: Main Menu> General Postproc> Element Table> Define Table For line elements, such as beams, spars, and pipes, use the ETABLE command to access derived data (stresses, strains, and so on). Results data are identified by a combination of a label and a sequence number or component name on the ETABLE command. See the ETABLE discussion in The General Postprocessor (POST1) in the ANSYS Basic Analysis Guide for details.
3.7.7. Option: Contour Displays Command(s): PLNSOL or PLESOL GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu Use these options to contour almost any result item, such as stresses (SX, SY, SZ...), strains (EPELX, EPELY, EPELZ...), and displacements (UX, UY, UZ...). The KUND field on PLNSOL and PLESOL gives you the option of overlaying the nondeformed shape on the display. You can also contour element table data and line element data: Command(s): PLETAB, PLLS GUI: Main Menu> General Postproc> Element Table> Plot Element Table Main Menu> General Postproc> Plot Results> Contour Plot> Line Elem Res Caution: Derived data, such as stresses and strains, are averaged at the nodes by the PLNSOL command. This averaging results in "smeared" values at nodes where elements of different materials, different shell thicknesses, or other discontinuities meet. To avoid the smearing effect, use selecting (described in Chapter 7, “Selecting and Components” in the ANSYS Basic Analysis Guide) to select elements of the same material, same shell thickness, and so on before issuing PLNSOL.
3.7.8. Option: Tabular Listings Command(s): PRNSOL (nodal results) PRESOL (element-by-element results) PRRSOL (reaction data), and so on NSORT, ESORT GUI: Main Menu> General Postproc> List Results> solution option Main Menu> General Postproc> List Results> Sorted Listing> Sort Nodes Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–11
Chapter 3: Modal Analysis Main Menu> General Postproc> List Results> Sorted Listing> Sort Elems Use the NSORT and ESORT commands to sort the data before listing them.
3.7.9. Other Capabilities Many other postprocessing functions - mapping results onto a path, load case combinations, and so on - are available in POST1. See The General Postprocessor (POST1) in the ANSYS Basic Analysis Guide for details. See the ANSYS Commands Reference for a discussion of the ANTYPE, MODOPT, M, TOTAL, EXPASS, MXPAND, SET, and PLDISP commands.
3.8. A Sample Modal Analysis (GUI Method) In this example, you perform a modal analysis on the wing of a model plane to demonstrate the wing's modal degrees of freedom.
3.8.1. Problem Description This is a modal analysis of a wing of a model plane. The wing is of uniform configuration along its length, and its cross-sectional area is defined to be a straight line and a spline, as shown. It is held fixed to the body on one end and hangs freely at the other. The objective of the problem is to demonstrate the wing's modal degrees of freedom.
3.8.2. Problem Specifications The dimensions of the wing are shown in the problem sketch. The wing is made of low density polyethylene with the following values: Young's modulus = 38x103 psi Poisson's ratio = .3 Density = 8.3e-5 lb-sec2/in4
3.8.3. Problem Sketch Figure 3.1 Diagram of a Model Airplane Wing
3–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.9: A Sample Modal Analysis (Command or Batch Method) The detailed step-by-step procedure for this example, Modal Analysis of a Model Airplane Wing, is included in the Modal Tutorial.
3.9. A Sample Modal Analysis (Command or Batch Method) You can perform the example modal analysis of a model airplane wing using the ANSYS commands shown below instead of GUI choices. Items prefaced with an exclamation point (!) are comments. You may receive warning messages when you run this problem. The version of the problem that appears in the Modal Tutorial contains an explanation of the warnings. /FILNAM,MODAL /TITLE,Modal Analysis of a Model Airplane Wing /PREP7 ET,1,PLANE42 ! Define PLANE42 as element type ET,2,SOLID45 ! Define SOLID45 as element type MP,EX,1,38000 MP,DENS,1,8.3E-5 MP,NUXY,1,.3 K,1 ! Define keypoint 1 at 0,0,0 K,2,2 ! Define keypoint 2 at 2,0,0 K,3,2.3,.2 ! Define keypoint 3 at 2.3,.2,0 K,4,1.9,.45 ! Define keypoint 4 at 1.9,.45,0 K,5,1,.25 ! Define keypoint 5 at 1,.25,0 LSTR,1,2 ! Create a straight line between LSTR,5,1 ! Create a straight line between BSPLIN,2,3,4,5,,,-1,,,-1,-.25 ! Create a B-spline AL,1,3,2 ESIZE,.25 AMESH,1 ESIZE,,10 TYPE,2 VEXT,ALL,,,,,10 /VIEW,,1,1,1 /ANG,1 /REP EPLOT FINISH /SOLU ANTYPE,MODAL MODOPT,SUBSP,5 ESEL,U,TYPE,,1 NSEL,S,LOC,Z,0 D,ALL,ALL NSEL,ALL MXPAND,5 SOLVE FINISH
! ! ! !
1 2
keypoints 1 and 2 keypoints 5 and 1
Choose modal analysis type Choose the subspace mode-extraction method, extracting 5 modes Unselect element type 1
/POST1 SET,LIST,2 SET,FIRST PLDISP,0 ANMODE,10,.5E-1 SET,NEXT PLDISP,0 ANMODE,10,.5E-1 SET,NEXT PLDISP,0 ANMODE,10,.5E-1 SET,NEXT PLDISP,0 ANMODE,10,.5E-1 SET,NEXT PLDISP,0 ANMODE,10,.5E-1 Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–13
Chapter 3: Modal Analysis FINISH /EXIT
3.10. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional modal analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS family of products. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual includes variety of modal analysis test cases: VM45 - Natural Frequency of a Spring-mass System VM47 - Torsional Frequency of a Suspended Disk VM48 - Natural Frequency of a Motor-generator VM50 - Fundamental Frequency of a Simply Supported Beam VM52 - Automobile Suspension System Vibrations VM53 - Vibration of a String Under Tension VM54 - Vibration of a Rotating Cantilever Blade VM55 - Vibration of a Stretched Circular Membrane VM57 - Torsional Frequencies of a Drill Pipe VM59 - Lateral Vibration of an Axially-loaded Bar VM60 - Natural Frequency of a Cross-ply Laminated Spherical Shell VM61 - Longitudinal Vibration of a Free-free Rod VM62 - Vibration of a Wedge VM66 - Vibration of a Flat Plate VM67 - Radial Vibrations of a Circular Ring from an Axisymmetric Model VM68 - PSD Response of a Two DOF Spring-mass System VM69 - Seismic Response VM70 - Seismic Response of a Beam Structure VM76 - Harmonic Response of a Guitar String VM89 - Natural Frequencies of a Two-mass-spring System VM151 - Nonaxisymmetric Vibration of a Circular Plate VM152 - Nonaxisymmetric Vibration of a Stretched Circular Membrane (Harmonic Els) VM153 - Nonaxisymmetric Vibration of a Stretched Circular Membrane (Modal) VM154 - Vibration of a Fluid Coupling VM175 - Natural Frequency of a Piezoelectric Transducer VM181 - Natural Frequency of a Flat Circular Plate with a Clamped Edge VM182 - Transient Response of a Spring-mass System VM183 - Harmonic Response of a Spring-mass System VM202 - Transverse Vibrations of a Shear Beam VM203 - Dynamic Load Effect on Simply-supported Thick Square Plate VM212 - Modal Analysis of a Rectangular Cavity
3.11. Prestressed Modal Analysis Use a prestressed modal analysis to calculate the frequencies and mode shapes of a prestressed structure, such as a spinning turbine blade. The procedure to do a prestressed modal analysis is essentially the same as a regular modal analysis, except that you first need to prestress the structure by doing a static analysis:
3–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.12: Prestressed Modal Analysis of a Large-Deflection Solution 1.
Build the model and obtain a static solution with prestress effects turned on [PSTRES,ON]. The same lumped mass setting [LUMPM] used here must also be used in the later prestress modal analysis. Chapter 2, “Structural Static Analysis” describes the procedure to obtain a static solution.
2.
Reenter SOLUTION and obtain the modal solution, also with prestress effects turned on (reissue PSTRES,ON). Files Jobname.EMAT (if ANSYS creates it) and Jobname.ESAV from the static analysis must be available. If the model is spinning, include spin-softening effects (via the OMEGA command's KSPIN option) if necessary.
3.
Expand the modes and review them in the postprocessor.
Step 1 above can also be a transient analysis. In such a case, save the EMAT and ESAV files at the desired time point. If the deformed shape from the static solution differs significantly from its nondeformed shape, you can perform a prestressed modal analysis of a large-deflection solution instead.
3.12. Prestressed Modal Analysis of a Large-Deflection Solution You can also perform a prestressed modal analysis following a large deflection (NLGEOM,ON) static analysis in order to calculate the frequencies and mode shapes of a highly deformed structure. Use the prestressed modal analysis procedure, but use the PSOLVE command (rather than the SOLVE command) to obtain the modal solution, as shown in the sample input listing below. Along with the PSOLVE command, you must issue the UPCOORD command to update the coordinates necessary for obtaining the correct stresses. This procedure uses the element matrices and element load vectors (for example, from pressures, temperature or acceleration loads) from a previous static analysis. These loads will be passed through to a subsequent mode superposition analysis if specified (LVSCALE command). Prestress must be applied (PSTRES,ON) during the static portion of the analysis. However, in cases where stressstiffening helps convergence: •
Stress-stiffening (SSTIF,ON) must be applied instead. (This requirement applies to elements outside of the 18x family of elements only.)
•
The EMATWRITE,YES command is also necessary to write the element matrices to File.EMAT.
Issuing either a PSTRES,OFF or SSTIF,OFF command prevents all previously specified prestressing from being applied. If the model is spinning, include spin-softening effects (via the OMEGA command's KSPIN option) in the modal solution if necessary. ! Initial, large deflection static analysis ! /PREP7 ... FINISH /SOLU ANTYPE,STATIC ! Static analysis NLGEOM,ON ! Large deflection analysis PSTRES,ON ! Flag to calculate the prestress matrix ... SOLVE FINISH ! ! Prestressed modal analysis ! Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–15
Chapter 3: Modal Analysis /SOLU ANTYPE,MODAL UPCOORD,1.0,ON PSTRES,ON MODOPT,... MXPAND,... PSOLVE,EIGxxxx FINISH /SOLU EXPASS,ON PSOLVE,EIGEXP
! ! ! ! ! ! ! !
Modal analysis Display mode shapes relative to deformed geometry in the postprocessor. Prestress effects ON Select eigensolver Specify the number of modes to expand, if desired. Calculate the eigenvalues and eigenvectors. Use EIGLANB or EIGFULL to match MODOPT command.
!Additional solution step for expansion. ! Expand the eigenvector solution. (Required if you ! want to review mode shapes in the postprocessor.)
FINISH
Note — You may also use one of the other eigensolvers (PSOLVE,EIGSYM, PSOLVE,EIGUNSY, PSOLVE,EIGDAMP or PSOLVE,EIGREDUC). In such a case, a PSOLVE,TRIANG command must precede the PSOLVE,EIGxxx command.
3.13. Comparing Mode-Extraction Methods The basic equation solved in a typical undamped modal analysis is the classical eigenvalue problem:
[K ]{φ i} = ω2i [M]{φ i} where: [K] = stiffness matrix {Φi} = mode shape vector (eigenvector) of mode i ω2 Ωi = natural circular frequency of mode i ( i is the eigenvalue) [M] = mass matrix Many numerical methods are available to solve the above equation. ANSYS offers these methods: •
Block Lanczos method (default)
•
Subspace method
•
PowerDynamics method
•
Reduced (Householder) method
•
Unsymmetric method
•
Damped method (The damped method solves a different equation; see the ANSYS, Inc. Theory Reference for more information.)
•
QR damped method (The QR damped method solves a different equation; see the ANSYS, Inc. Theory Reference for more information.) Note — The damped, unsymmetric, and QR damped methods are not available in the ANSYS Professional program.
The first four methods (Block Lanczos, subspace, PowerDynamics, and reduced) are the most commonly used. Table 3.6: “Symmetric System Eigensolver Choices” compares these four mode-extraction methods. Following the table is a brief description of each mode-extraction method.
3–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.13: Comparing Mode-Extraction Methods
Table 3.6 Symmetric System Eigensolver Choices Eigensolver
Application
Memory Required
Disk Required
Block Lanczos
Default. To find many modes (about 40+) of large models. Recommended when the model consists of poorly shaped solid and shell elements. This solver performs well when the model consists of shells or a combination of shells and solids. Works faster but requires about 50% more memory than subspace.
Medium
Low
Subspace
To find few modes (up to about 40) of large models. Recommended when the model consists of well-shaped solid and shell elements. Works well if memory availability is limited.
Low
High
Power Dynamics To find few modes (up to about 20) of large models. Recommended for fast computation of eigenvalues of over 100K DOF models. On coarse mesh models, the frequencies are approximate. Missed modes are possible when repeated frequencies are present.
High
Low
Reduced
Low
Low
To find all modes of small to medium models (less than 10K DOF). Can be used to find few modes (up to about 40) of large models with proper selection of master DOF, but accuracy of frequencies depends on the master DOF selected.
3.13.1. Block Lanczos Method The Block Lanczos eigenvalue solver is the default. It uses the Lanczos algorithm where the Lanczos recursion is performed with a block of vectors. This method is as accurate as the subspace method, but faster. The Block Lanczos method uses the sparse matrix solver, overriding any solver specified via the EQSLV command. The Block Lanczos method is especially powerful when searching for eigenfrequencies in a given part of the eigenvalue spectrum of a given system. The convergence rate of the eigenfrequencies will be about the same when extracting modes in the midrange and higher end of the spectrum as when extracting the lowest modes. Therefore, when you use a shift frequency (FREQB) to extract n modes beyond the starting value of FREQB, the algorithm extracts the n modes beyond FREQB at about the same speed as it extracts the lowest n modes.
3.13.2. Subspace Method The subspace method uses the subspace iteration technique, which internally uses the generalized Jacobi iteration algorithm. It is highly accurate because it uses the full [K] and [M] matrices. For the same reason, however, the subspace method is slower than the reduced method. This method is typically used in cases where high accuracy is required or where selecting master DOF is not practical. When doing a modal analysis with a large number of constraint equations, use the subspace method with the frontal solver instead of the JCG solver, or use the Block Lanczos mode-extraction method. Using the JCG solver when your analysis has many constraint equations could result in an internal element stiffness assembly that requires large amounts of memory.
3.13.3. PowerDynamics Method The PowerDynamics method internally uses the subspace iterations, but uses the PCG iterative solver. This method may be significantly faster than either the subspace or the Block Lanczos methods, but may not converge if the model contains poorly-shaped elements, or if the matrix is ill-conditioned. This method is especially useful in very large models (100,000+ DOFs) to obtain a solution for the first few modes. Do not use this method if you will be running a subsequent spectrum analysis.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–17
Chapter 3: Modal Analysis The PowerDynamics method does not perform a Sturm sequence check (that is, it does not check for missing modes), which might affect problems with multiple repeated frequencies. This method always uses lumped mass approximation. Note — If you use PowerDynamics to solve a model that includes rigid body modes, be sure to issue the RIGID command or choose one of its GUI equivalents (Main Menu> Solution> Analysis Options or Main Menu> Preprocessor> Loads> Analysis Options).
3.13.4. Reduced Method The reduced method uses the HBI algorithm (Householder-Bisection-Inverse iteration) to calculate the eigenvalues and eigenvectors. It is relatively fast because it works with a small subset of degrees of freedom called master DOF. Using master DOF leads to an exact [K] matrix but an approximate [M] matrix (usually with some loss in mass). The accuracy of the results, therefore, depends on how well [M] is approximated, which in turn depends on the number and location of masters. Section 3.14: Matrix Reduction presents guidelines to select master DOFs.
3.13.5. Unsymmetric Method The unsymmetric method, which also uses the full [K] and [M] matrices, is meant for problems where the stiffness and mass matrices are unsymmetric (for example, acoustic fluid-structure interaction problems). It uses the Lanczos algorithm which calculates complex eigenvalues and eigenvectors if the system is non-conservative (for example, a shaft mounted on bearings). The real part of the eigenvalue represents the natural frequency and the imaginary part is a measure of the stability of the system - a negative value means the system is stable, whereas a positive value means the system is unstable. Sturm sequence checking is not available for this method. Therefore, missed modes are a possibility at the higher end of the frequencies extracted.
3.13.6. Damped Method The damped method is meant for problems where damping cannot be ignored, such as rotor dynamics applications. It uses full matrices ([K], [M], and the damping matrix [C]). It uses the Lanczos algorithm and calculates complex eigenvalues and eigenvectors (as described below). Sturm sequence checking is not available for this method. Therefore, missed modes are a possibility at the higher end of the frequencies extracted.
3.13.6.1. Damped Method-Real and Imaginary Parts of the Eigenvalue The imaginary part of the eigenvalue, Ω, represents the steady-state circular frequency of the system. The real part of the eigenvalue, σ, represents the stability of the system. If σ is less than zero, then the displacement amplitude will decay exponentially, in accordance with EXP(σ). If σ is greater than zero, then the amplitude will increase exponentially. (Or, in other words, negative σ gives an exponentially decreasing, or stable, response; and positive σ gives an exponentially increasing, or unstable, response.) If there is no damping, the real component of the eigenvalue will be zero. Note — The eigenvalue results reported by ANSYS are actually divided by 2* π. This gives the frequency in Hz (cycles/second). In other words: Imaginary part of eigenvalue, as reported = Ω/(2* π) Real part of eigenvalue, as reported = σ/(2* π)
3.13.6.2. Damped Method-Real and Imaginary Parts of the Eigenvector In a damped system, the response at different nodes can be out of phase. At any given node, the amplitude will be the vector sum of the real and imaginary components of the eigenvector.
3–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.14: Matrix Reduction
3.13.7. QR Damped Method The QR damped method combines the advantages of the Block Lanczos method with the complex Hessenberg method. The key concept is to approximately represent the first few complex damped eigenvalues by a linear combination of a small number of eigenvectors of the undamped system. After the undamped mode shapes are evaluated by using the real eigensolution (Block Lanczos method), the equations of motion are transformed to these modal coordinates. Using the QR algorithm, a smaller eigenvalue problem is then solved in the modal subspace. This approach gives good results for lightly damped systems and can also be applicable to any arbitrary damping type (proportional or non-proportional symmetric damping or unsymmetric gyroscopic damping matrix). Because the accuracy of this method is dependent on the number of modes used in the calculations, a sufficient number of fundamental modes are recommended, especially for highly damped systems to provide good results. This method is not recommended for critically damped or overdamped systems. This method outputs both the real and imaginary eigenvalues (frequencies), but outputs only the real eigenvectors (mode shapes).
3.14. Matrix Reduction Matrix reduction is a way to reduce the size of the matrices of a model and perform a quicker and cheaper analysis. It is mainly used in dynamic analyses such as modal, harmonic, and transient analyses. Matrix reduction is also used in substructure analyses to generate a superelement. Matrix reduction allows you to build a detailed model, as you would for a static stress analysis, and use only a "dynamic" portion of it for a dynamic analysis. You choose the "dynamic" portion by identifying key degrees of freedom, called master degrees of freedom, that characterize the dynamic behavior of the model. The ANSYS program then calculates reduced matrices and the reduced DOF solution in terms of the master DOF. You can then expand the solution to the full DOF set by performing an expansion pass. The main advantage of this procedure is the savings in CPU time to obtain the reduced solution, especially for dynamic analyses of large problems.
3.14.1. Theoretical Basis of Matrix Reduction The ANSYS program uses the Guyan Reduction procedure to calculate the reduced matrices. The key assumption in this procedure is that for the lower frequencies, inertia forces on the slave DOF (those DOF being reduced out) are negligible compared to elastic forces transmitted by the master DOF. Therefore, the total mass of the structure is apportioned among only the master DOF. The net result is that the reduced stiffness matrix is exact, whereas the reduced mass and damping matrices are approximate. For details about how the reduced matrices are calculated, refer to the ANSYS, Inc. Theory Reference.
3.14.1.1. Guidelines for Selecting Master DOF Choosing master DOF is an important step in a reduced analysis. The accuracy of the reduced mass matrix (and hence the accuracy of the solution) depends on the number and location of masters. For a given problem, you can choose many different sets of master DOF and will probably obtain acceptable results in all cases. You can choose masters using M and MGEN commands, or you can have the program choose masters during solution using the TOTAL command. We recommend that you do both: choose a few masters yourself, and also have the ANSYS program choose masters. This way, the program can pick up any modes that you may have missed. The following list summarizes the guidelines for selecting master DOF: •
The total number of master DOF should be at least twice the number of modes of interest.
•
Choose master DOF in directions in which you expect the structure or component to vibrate. For a flat plate, for example, you should choose at least a few masters in the out-of-plane direction (see Fig-
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–19
Chapter 3: Modal Analysis ure 3.2: “Choose Master DOF” (a)). In cases where motion in one direction induces a significant motion in another direction, choose master DOF in both directions (see Figure 3.2: “Choose Master DOF” (b)).
Figure 3.2 Choose Master DOF
(a) Possible out-of-plane masters for a flat plate(b) Motion in X induces motion in Y •
Choose masters at locations having relatively large mass or rotary inertia and relatively low stiffness (see Figure 3.3: “Choosing Master DOFs”). Examples of such locations are overhangs and "loosely" connected structures. Conversely, do not choose masters at locations with relatively small mass, or at locations with high stiffness (such as DOF close to constraints).
Figure 3.3 Choosing Master DOFs
Choose masters at locations with (a) large rotary inertia, (b) large mass •
If your primary interest is in bending modes, you can neglect rotational and "stretching" DOF.
•
If the degree of freedom to be chosen belongs to a coupled set, choose only the first (primary) DOF of the coupled set.
•
Choose master DOF at locations where forces or nonzero displacements are to be applied.
•
For axisymmetric shell models (SHELL51 or SHELL61), choose as masters the global UX degree of freedom at all nodes on those sections of the model that are parallel to or nearly parallel to the center line, so oscillatory motions between master DOF can be avoided (see Figure 3.4: “Choosing Masters in an Axisymmetric Shell Model”). This recommendation can be relaxed if the motion is primarily parallel to the centerline. For axisymmetric harmonic elements with MODE = 2 or greater, choose as masters both UX and UZ degrees of freedom.
3–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 3.14: Matrix Reduction
Figure 3.4 Choosing Masters in an Axisymmetric Shell Model
The best way to check the validity of the master DOF set is to rerun the analysis with twice (or half) the number of masters and to compare the results. Another way is to review the reduced mass distribution printed during a modal solution. The reduced mass should be, at least in the dominant direction of motion, within 10-15 percent of the total mass of the structure.
3.14.1.2. A Note About Program-Selected Masters If you let the ANSYS program select masters [TOTAL], the distribution of masters selected will depend on the order in which elements are processed during the solution. For example, different master DOF sets may be selected depending on whether the elements are processed from left to right or from right to left. However, this difference usually yields insignificant differences in the results. For meshes with uniform element sizes and properties (for example, a flat plate), the distribution of masters will, in general, not be uniform. In such cases, you should specify some master DOF of your own [M, MGEN]. The same recommendation applies to structures with an irregular mass distribution, where the program-selected master DOF may be concentrated in the higher-mass regions.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
3–21
3–22
Chapter 4: Harmonic Response Analysis 4.1. Definition of Harmonic Response Analysis Any sustained cyclic load will produce a sustained cyclic response (a harmonic response) in a structural system. Harmonic response analysis gives you the ability to predict the sustained dynamic behavior of your structures, thus enabling you to verify whether or not your designs will successfully overcome resonance, fatigue, and other harmful effects of forced vibrations.
4.2. Uses for Harmonic Response Analysis Harmonic response analysis is a technique used to determine the steady-state response of a linear structure to loads that vary sinusoidally (harmonically) with time. The idea is to calculate the structure's response at several frequencies and obtain a graph of some response quantity (usually displacements) versus frequency. "Peak" responses are then identified on the graph and stresses reviewed at those peak frequencies. This analysis technique calculates only the steady-state, forced vibrations of a structure. The transient vibrations, which occur at the beginning of the excitation, are not accounted for in a harmonic response analysis (see Figure 4.1: “Harmonic Response Systems”).
Figure 4.1 Harmonic Response Systems
!#" %$
34 ! 2!!*
"56#7 ' % $
ω
&
"' $
& ' ( )'!!*
+-,.+ /0 -" ω21 φ $ <= @ =>?
;<
, 0 '9!!*
8"5: ' ( (# 7 ' % $
% "6!$
Typical harmonic response system. Fo and Ω are known. uo and Φ are unknown (a). Transient and steady-state dynamic response of a structural system (b). Harmonic response analysis is a linear analysis. Some nonlinearities, such as plasticity will be ignored, even if they are defined. You can, however, have unsymmetric system matrices such as those encountered in a fluidstructure interaction problem (see Chapter 15, “Acoustics” in the ANSYS Coupled-Field Analysis Guide). Harmonic analysis can also be performed on a prestressed structure, such as a violin string (assuming the harmonic stresses are much smaller than the pretension stress). See Section 4.11.1.1: Prestressed Full Harmonic Response Analysis for more information on prestressed harmonic analyses.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 4: Harmonic Response Analysis
4.3. Commands Used in a Harmonic Response Analysis You use the same set of commands to build a model and perform a harmonic response analysis that you use to do any other type of finite element analysis. Likewise, you choose similar options from the graphical user interface (GUI) to build and solve models no matter what type of analysis you are doing. Section 4.6: Sample Harmonic Response Analysis (GUI Method) and Section 4.7: Sample Harmonic Response Analysis (Command or Batch Method) show a sample harmonic response analysis done via the GUI and via commands, respectively. For detailed, alphabetized descriptions of the ANSYS commands, see the ANSYS Commands Reference.
4.4. The Three Solution Methods Three harmonic response analysis methods are available: full, reduced, and mode superposition. (A fourth, relatively expensive method is to do a transient dynamic analysis with the harmonic loads specified as time-history loading functions; see Chapter 5, “Transient Dynamic Analysis” for details.) The ANSYS Professional program allows only the mode superposition method. Before we study the details of how to implement each of these methods, let's explore the advantages and disadvantages of each method.
4.4.1. The Full Method The full method is the easiest of the three methods. It uses the full system matrices to calculate the harmonic response (no matrix reduction). The matrices may be symmetric or unsymmetric. The advantages of the full method are: •
It is easy to use, because you don't have to worry about choosing master degrees of freedom or mode shapes.
•
It uses full matrices, so no mass matrix approximation is involved.
•
It allows unsymmetric matrices, which are typical of such applications as acoustics and bearing problems.
•
It calculates all displacements and stresses in a single pass.
•
It accepts all types of loads: nodal forces, imposed (nonzero) displacements, and element loads (pressures and temperatures).
•
It allows effective use of solid-model loads.
A disadvantage is that this method usually is more expensive than either of the other methods when you use the frontal solver. However, when you use the JCG solver or the ICCG solver, the full method can be very efficient.
4.4.2. The Reduced Method The reduced method enables you to condense the problem size by using master degrees of freedom and reduced matrices. After the displacements at the master DOF have been calculated, the solution can be expanded to the original full DOF set. (See Section 3.14: Matrix Reduction, for a more detailed discussion of the reduction procedure.) The advantages of this method are: •
It is faster and less expensive compared to the full method when you are using the frontal solver.
•
Prestressing effects can be included.
The disadvantages of the reduced method are:
4–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.5: How to Do Harmonic Response Analysis •
The initial solution calculates only the displacements at the master DOF. A second step, known as the expansion pass, is required for a complete displacement, stress, and force solution. (However, the expansion pass might be optional for some applications.)
•
Element loads (pressures, temperatures, etc.) cannot be applied.
•
All loads must be applied at user-defined master degrees of freedom. (This limits the use of solid-model loads.)
4.4.3. The Mode Superposition Method The mode superposition method sums factored mode shapes (eigenvectors) from a modal analysis to calculate the structure's response. Its advantages are: •
It is faster and less expensive than either the reduced or the full method for many problems.
•
Element loads applied in the preceding modal analysis can be applied in the harmonic response analysis via the LVSCALE command, unless the modal analysis was done using PowerDynamics.
•
It allows solutions to be clustered about the structure's natural frequencies. This results in a smoother, more accurate tracing of the response curve.
•
Prestressing effects can be included.
•
It accepts modal damping (damping ratio as a function of frequency).
Disadvantages of the mode superposition method are: •
Imposed (nonzero) displacements cannot be applied.
•
When you are using PowerDynamics for the modal analysis, initial conditions cannot have previouslyapplied loads.
4.4.4. Restrictions Common to All Three Methods All three methods are subject to certain common restrictions: •
All loads must be sinusoidally time-varying.
•
All loads must have the same frequency.
•
No nonlinearities are permitted.
•
Transient effects are not calculated.
You can overcome any of these restrictions by performing a transient dynamic analysis, with harmonic loads expressed as time-history loading functions. Chapter 5, “Transient Dynamic Analysis” describes the procedure for a transient dynamic analysis.
4.5. How to Do Harmonic Response Analysis We will first describe how to do a harmonic response analysis using the full method, and then list the steps that are different for the reduced and mode superposition methods.
4.5.1. Full Harmonic Response Analysis The procedure for a full harmonic response analysis consists of three main steps: 1.
Build the model. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–3
Chapter 4: Harmonic Response Analysis 2.
Apply loads and obtain the solution.
3.
Review the results.
4.5.2. Build the Model See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details, see the ANSYS Modeling and Meshing Guide.
4.5.2.1. Points to Remember •
Only linear behavior is valid in a harmonic response analysis. Nonlinear elements, if any, will be treated as linear elements. If you include contact elements, for example, their stiffnesses are calculated based on their initial status and are never changed.
•
Both Young's modulus (EX) (or stiffness in some form) and density (DENS) (or mass in some form) must be defined. Material properties may be linear, isotropic or orthotropic, and constant or temperature-dependent. Nonlinear material properties, if any, are ignored.
4.5.3. Apply Loads and Obtain the Solution In this step, you define the analysis type and options, apply loads, specify load step options, and initiate the finite element solution. Details of how to do these tasks are explained below. Note — Peak harmonic response occurs at forcing frequencies that match the natural frequencies of your structure. Before obtaining the harmonic solution, you should first determine the natural frequencies of your structure by obtaining a modal solution (as explained in Chapter 3, “Modal Analysis”).
4.5.3.1. Enter the ANSYS Solution Processor Command(s): /SOLU GUI: Main Menu> Solution
4.5.3.2. Define the Analysis Type and Options ANSYS offers these options for a harmonic response analysis:
Table 4.1 Analysis Types and Options Option
Command
GUI Path
New Analysis
ANTYPE
Main Menu> Solution> Analysis Type> New Analysis
Analysis Type: Harmonic Response ANTYPE
Main Menu> Solution> Analysis Type> New Analysis> Harmonic
Solution Method
HROPT
Main Menu> Solution> Analysis Type> Analysis Options
Solution Listing Format
HROUT
Main Menu> Solution> Analysis Type> Analysis Options
Mass Matrix Formulation
LUMPM
Main Menu> Solution> Analysis Type> Analysis Options
Equation Solver
EQSLV
Main Menu> Solution> Analysis Type> Analysis Options
4–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.5: How to Do Harmonic Response Analysis Each of these options is explained in detail below. •
Option: New Analysis (ANTYPE) Choose New Analysis. Restarts are not valid in a harmonic response analysis; if you need to apply additional harmonic loads, do a new analysis each time.
•
Option: Analysis Type: Harmonic Response (ANTYPE) Choose Harmonic Response as the analysis type.
•
Option: Solution Method (HROPT) Choose one of the following solution methods: – Full method – Reduced method – Mode superposition method
•
Option: Solution Listing Format (HROUT) This option determines how the harmonic displacement solution is listed in the printed output (Jobname.OUT). You can choose between real and imaginary parts (default), and amplitudes and phase angles.
•
Option: Mass Matrix Formulation (LUMPM) Use this option to specify the default formulation (which is element dependent) or lumped mass approximation. We recommend the default formulation for most applications. However, for some problems involving "skinny" structures such as slender beams or very thin shells, the lumped mass approximation often yields better results. Also, the lumped mass approximation can result in a shorter run time and lower memory requirements. After you complete the fields on the Harmonic Analysis Options dialog box, click on OK to reach a second Harmonic Analysis dialog box, where you choose an equation solver.
•
Option: Equation Solver (EQSLV) You can choose the frontal solver (default), the sparse direct solver (SPARSE), the Jacobi Conjugate Gradient (JCG) solver, or the Incomplete Cholesky Conjugate Gradient (ICCG) solver. The frontal direct solver or sparse direct solver is recommended for most structural models. When using a direct solver to solve a relatively large problem, choose the sparse solver over the frontal solver.
4.5.3.3. Apply Loads on the Model A harmonic analysis, by definition, assumes that any applied load varies harmonically (sinusoidally) with time. To completely specify a harmonic load, three pieces of information are usually required: the amplitude, the phase angle, and the forcing frequency range (see Figure 4.2: “Relationship Between Real/Imaginary Components and Amplitude/Phase Angle”).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–5
Chapter 4: Harmonic Response Analysis
Figure 4.2 Relationship Between Real/Imaginary Components and Amplitude/Phase Angle
2
* /.10 2 +-, 1 2 +@0
!#"$&% ACB10D% %
'( !)"$% 5 !
34% 6!79 >:? 8: ;< =
2
The amplitude is the maximum value of the load, which you specify using the commands shown in Table 4.2: “ Applicable Loads in a Harmonic Response Analysis”. The phase angle is a measure of the time by which the load lags (or leads) a frame of reference. On the complex plane (see Figure 4.2: “Relationship Between Real/Imaginary Components and Amplitude/Phase Angle”), it is the angle measured from the real axis. The phase angle is required only if you have multiple loads that are out of phase with each other. For example, the unbalanced rotating antenna shown in Figure 4.3: “An Unbalanced Rotating Antenna” will produce out-of-phase vertical loads at its four support points. The phase angle cannot be specified directly; instead, you specify the real and imaginary components of the out-of-phase loads using the VALUE and VALUE2 fields of the appropriate displacement and force commands. Pressures and other surface and body loads can only be specified with a phase angle of 0 (no imaginary component) with the following exceptions: nonzero imaginary components of pressures can be applied using the SURF153 and SURF154 elements in a full harmonic response analysis, or using a mode superposition harmonic response analysis if the mode-extraction method is Block Lanczos (see the SF and SFE commands). Figure 4.2: “Relationship Between Real/Imaginary Components and Amplitude/Phase Angle” shows how to calculate the real and imaginary components. The forcing frequency range is the frequency range of the harmonic load (in cycles/time). It is specified later as a load step option with the HARFRQ command.
4–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.5: How to Do Harmonic Response Analysis
Figure 4.3 An Unbalanced Rotating Antenna !
" # $&% "$& '$$("
,
)( # $ (*) )( +
+ "./'0 (1 ! '(1 '+ '$( '
+ "./'0 (1 ! '(1 '+ '$( '
: 6 "$
2"$(342 .5# '3/1 +(6 "+ # 7& 8 9
An unbalanced rotating antenna will produce out-of-phase vertical loads at its four support points. Note — A harmonic analysis cannot calculate the response to multiple forcing functions acting simultaneously with different frequencies (for example, two machines with different rotating speeds running at the same time). However, POST1 can superimpose multiple load cases to obtain the total response. Table 4.2: “ Applicable Loads in a Harmonic Response Analysis” summarizes the loads applicable to a to a harmonic response analysis. Except for inertia loads, you can define loads either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). For a general discussion of solid-model loads versus finite element loads, see Chapter 2, “Loading” in the ANSYS Basic Analysis Guide.
Table 4.2 Applicable Loads in a Harmonic Response Analysis Load Type
Category
Cmd Family
GUI Path
Displacement (UX, UY, Constraints UZ, ROTX, ROTY, ROTZ)
D
Main Menu> Solution> Define Loads> Apply> Structural> Displacement
Force, Moment (FX, FY, Forces FZ, MX, MY, MZ)
F
Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment
Pressure (PRES)
SF
Main Menu> Solution> Define Loads> Apply> Structural> Pressure
Surface Loads
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–7
Chapter 4: Harmonic Response Analysis Load Type Temperature (TEMP), Fluence (FLUE)
Category Body Loads
Gravity, Spinning, etc. Inertia Loads
Cmd Family
GUI Path
BF
Main Menu> Solution> Define Loads> Apply> Structural> Temperature
-
Main Menu> Solution> Define Loads> Apply> Structural> Other
In an analysis, loads can be applied, removed, operated on, or listed.
4.5.3.3.1. Applying Loads Using Commands Table 4.3: “Load Commands for a Harmonic Response Analysis” lists all the commands you can use to apply loads in a harmonic response analysis.
Table 4.3 Load Commands for a Harmonic Response Analysis Load Type Solid Model or FE Displacement
Force
Pressure
Temperature, Fluence
4–8
Entity
Apply
Delete
List
Operate
Apply Settings
Solid Mod- Keypoints el
DK
DKDELE
DKLIST
DTRAN
-
Solid Mod- Lines el
DL
DLDELE
DLLIST
DTRAN
-
Solid Mod- Areas el
DA
DADELE
DALIST
DTRAN
-
Finite Elem Nodes
D
DDELE
DLIST
DSCALE
Solid Mod- Keypoints el
FK
FKDELE
FKLIST
FTRAN
Finite Elem Nodes
F
FDELE
FLIST
FSCALE
FCUM
Solid Mod- Lines el
SFL
SFLDELE
SFLLIST
SFTRAN
SFGRAD
Solid Mod- Areas el
SFA
SFADELE
SFALIST
SFTRAN
SFGRAD
Finite Elem Nodes
SF
SFDELE
SFLIST
SFSCALE
SFGRAD, SFCUM
Finite Elem Elements
SFE
SFEDELE
SFELIST
SFSCALE
SFGRAD, SFBEAM, SFFUN, SFCUM
Solid Mod- Keypoints el
BFK
BFKDELE
BFKLIST
BFTRAN
-
Solid Mod- Lines el
BFL
BFLDELE
BFLLIST
BFTRAN
-
Solid Mod- Areas el
BFA
BFADELE
BFALIST
BFTRAN
-
Solid Mod- Volumes el
BFV
BFVDELE
BFVLIST
BFTRAN
-
Finite Elem Nodes
BF
BFDELE
BFLIST
BFSCALE
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
DSYM, DCUM -
BFCUM , BFUNIF , TBUNIF
Section 4.5: How to Do Harmonic Response Analysis Finite Elem Elements Load Type Solid Model or FE Inertia
-
BFE
BFEDELE
BFELIST
BFSCALE
BFCUM
Entity
Apply
Delete
List
Operate
Apply Settings
-
ACEL, OMEGA, DOMEGA, CGLOC, CGOMGA, DCGOMG
-
-
-
-
4.5.3.3.2. Applying Loads and Listing Loads Using the GUI These steps for a harmonic analysis are the same as those for most other analyses. See Section 3.5.4.2: Applying Loads Using the GUI and Section 3.5.4.3: Listing Loads for more information.
4.5.3.4. Specify Load Step Options The following options are available for a harmonic response analysis:
Table 4.4 Load Step Options Option
Command
GUI Path
General Options Number of Harmonic Solutions NSUBST
Main Menu> Solution> Load Step Opts> Time/Frequenc> Freq and Substeps
Stepped or Ramped Loads
KBC
Main Menu> Solution> Load Step Opts> Time/Frequenc> Time - Time Step or Freq and Substeps
Forcing Frequency Range
HARFRQ
Main Menu> Solution> Load Step Opts> Time/Frequenc> Freq and Substeps
Damping
ALPHAD, BETAD, DMPRAT
Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
Dynamics Options
MP,DAMP, MP,DM- Main Menu> Solution> Load Step Opts> Other> PR Change Mat Props> Material Models> Structural> Damping Output Control Options Printed Output
OUTPR
Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout
Database and Results File Output OUTRES
Main Menu> Solution> Load Step Opts> Output Ctrls> DB/ Results File
Extrapolation of Results
Main Menu> Solution> Load Step Opts> Output Ctrls> Integration Pt
ERESX
4.5.3.4.1. General Options General options include the following: •
Number of Harmonic Solutions (NSUBST)
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–9
Chapter 4: Harmonic Response Analysis You can request any number of harmonic solutions to be calculated. The solutions (or substeps) will be evenly spaced within the specified frequency range (HARFRQ). For example, if you specify 10 solutions in the range 30 to 40 Hz, the program will calculate the response at 31, 32, 33, ..., 39, and 40 Hz. No response is calculated at the lower end of the frequency range. •
Stepped or Ramped Loads (KBC) The loads may be stepped or ramped. By default, they are ramped, that is, the load amplitude is gradually increased with each substep. By stepping the loads (KBC,1), the same load amplitude will be maintained for all substeps in the frequency range. Note — Surface and body loads do not ramp from their previous load step values, except for those applied to PLANE2, SOLID45, SOLID92, and SOLID95 element types. The remaining element types always ramp from zero or from the value specified via BFUNIF.
4.5.3.4.2. Dynamics Options Dynamics options include the following: •
Forcing Frequency Range (HARFRQ) The forcing frequency range must be defined (in cycles/time) for a harmonic analysis. Within this range, you then specify the number of solutions to be calculated.
•
Damping Damping in some form should be specified; otherwise, the response will be infinity at the resonant frequencies. ALPHAD and BETAD result in a frequency-dependent damping ratio, whereas DMPRAT specifies a constant damping ratio to be used at all frequencies. Damping can also be specified for individual materials using MP,DAMP and MP,DMPR. See Section 5.10.3: Damping for further details. Note — If no damping is specified in a direct harmonic analysis (full or reduced), the program uses zero damping by default.
•
Alpha (Mass) Damping (ALPHAD)
•
Beta (Stiffness) Damping (BETAD)
•
Constant Damping Ratio (DMPRAT)
•
Material Dependent Damping Multiplier (MP,DAMP)
•
Constant Material Damping Coefficient (MP,DMPR)
4.5.3.4.3. Output Controls Output control options include the following: •
Printed Output (OUTPR) Use this option to include any results data on the output file (Jobname.OUT).
•
Database and Results File Output (OUTRES) This option controls the data on the results file (Jobname.RST).
• 4–10
Extrapolation of Results (ERESX) Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.5: How to Do Harmonic Response Analysis Use this option to review element integration point results by copying them to the nodes instead of extrapolating them (default).
4.5.3.5. Save a Backup Copy of the Database to a Named File You can then retrieve your model by reentering the ANSYS program and issuing RESUME. Command(s): SAVE GUI: Utility Menu> File> Save as
4.5.3.6. Start Solution Calculations Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
4.5.3.7. Repeat for Additional Load Steps Repeat the process for any additional loads and frequency ranges (that is, for additional load steps). If you plan to do time-history postprocessing (POST26), the frequency ranges should not overlap from one load step to the next. Another method for multiple load steps, which allows you to store the load steps on files and then solve them at once using a macro, is described in the ANSYS Basic Analysis Guide.
4.5.3.8. Leave SOLUTION Command(s): FINISH GUI: Close the Solution menu.
4.5.4. Review the Results The results data for a harmonic analysis are the same as the data for a basic structural analysis with the following additions: If you defined damping in the structure, the response will be out-of-phase with the loads. All results are then complex in nature and are stored in terms of real and imaginary parts. Complex results will also be produced if out-of-phase loads were applied. See Section 2.3.6: Review the Results in Chapter 2, “Structural Static Analysis”.
4.5.4.1. Postprocessors You can review these results using either POST26 or POST1. The normal procedure is to first use POST26 to identify critical forcing frequencies - frequencies at which the highest displacements (or stresses) occur at points of interest in the model - and to then use POST1 to postprocess the entire model at these critical forcing frequencies. •
POST1 is used to review results over the entire model at specific frequencies.
•
POST26 allows you to review results at specific points in the model over the entire frequency range.
Some typical postprocessing operations for a harmonic response analysis are explained below. For a complete description of all postprocessing functions, see Chapter 4, “An Overview of Postprocessing” in the ANSYS Basic Analysis Guide.
4.5.4.2. Points to Remember The points to remember for a harmonic analysis are the same as those for most structural analyses. See Section 2.3.6.2: Points to Remember in Chapter 2, “Structural Static Analysis”. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–11
Chapter 4: Harmonic Response Analysis
4.5.4.3. Using POST26 POST26 works with tables of result item versus frequency, known as variables. Each variable is assigned a reference number, with variable number 1 reserved for frequency. 1.
Define the variables using these options: Command(s): NSOL, ESOL, RFORCE GUI: Main Menu> TimeHist Postpro> Define Variables Note — The NSOL command is for primary data (nodal displacements), the ESOL command for derived data (element solution data, such as stresses), and the RFORCE command for reaction force data. To specify the total force, static component of the total force, damping component, or the inertia component, use the FORCE command.
2.
Graph the variables (versus frequency or any other variable). Then use PLCPLX to work with just the amplitude, phase angle, real part, or imaginary part. Command(s): PLVAR, PLCPLX GUI: Main Menu> TimeHist Postpro> Graph Variables Main Menu> TimeHist Postpro> Settings> Graph
3.
Get a listing of the variable. To list just the extreme values, use the EXTREM command. Then use the PRCPLX command to work with amplitude and phase angle or real and imaginary part. Command(s): PRVAR, EXTREM, PRCPLX GUI: Main Menu> TimeHist Postpro> List Variables> List Extremes Main Menu> TimeHist Postpro> List Extremes Main Menu> TimeHist Postpro> Settings> List
Many other functions, such as performing math operations among variables (in complex arithmetic), moving variables into array parameters, moving array parameters into variables, etc., are available in POST26; see Chapter 6, “The Time-History Postprocessor (POST26)” in the ANSYS Basic Analysis Guide for details. By reviewing the time-history results at strategic points throughout the model, you can identify the critical frequencies for further POST1 postprocessing.
4.5.4.4. Using POST1 1.
Read in results for the desired harmonic solution. You can use the SET command for this purpose, but it will read in either the real component or the imaginary component, not both at the same time. The true magnitude of the results is given by an SRSS (square-root-of-sum-of-squares) combination of the real and imaginary components (see Figure 4.2: “Relationship Between Real/Imaginary Components and Amplitude/Phase Angle”) and can be done for specific points in the model in POST26.
2.
Display the deformed shape of the structure, contours of stresses, strains, etc., or vector plots of vector items (PLVECT). To obtain tabular listings of data, use PRNSOL, PRESOL, PRRSOL, etc.
4–12
•
Option: Display Deformed Shape Command(s): PLDISP GUI: Main Menu> General Postproc> Plot Results> Deformed Shape
•
Option: Contour Displays Command(s): PLNSOL or PLESOL GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.6: Sample Harmonic Response Analysis (GUI Method) Use these options to contour almost any result item, such as stresses (SX, SY, SZ...), strains (EPELX, EPELY, EPELZ...), and displacements (UX, UY, UZ...). The KUND field on PLNSOL and PLESOL gives you the option of overlaying the undeformed shape on the display. •
Option: Vector Plots Command(s): PLVECT GUI: Main Menu> General Postproc> Plot Results> Vector Plot> Predefined Use PLNSOL or PLESOL to contour almost any result item, such as stresses (SX, SY, SZ...), strains (EPELX, EPELY, EPELZ...), and displacements (UX, UY, UZ...).
•
Option: Tabular Listings Command(s): PRNSOL (nodal results) PRESOL (element-by-element results) PRRSOL (reaction data) etc. NSORT, ESORT GUI: Main Menu> General Postproc> List Results> Nodal Solution Main Menu> General Postproc> List Results> Element Solution Main Menu> General Postproc> List Results> Reaction Solution Use the NSORT and ESORT commands to sort the data before listing them.
Many other functions, such as mapping results on to a path, transforming results to different coordinate systems, load case combinations, etc., are available in POST1; see Chapter 3, “Solution” in the ANSYS Basic Analysis Guide for details. See the ANSYS Commands Reference for a discussion of the ANTYPE, HROPT, HROUT, HARFRQ, DMPRAT, NSUBST, KBC, NSOL, ESOL, RFORCE, PLCPLX, PLVAR, PRCPLX, PRVAR, PLDISP, PRRSOL, and PLNSOL commands.
4.6. Sample Harmonic Response Analysis (GUI Method) In this sample problem, you will determine the harmonic response of a two-mass-spring system.
4.6.1. Problem Description Determine the response amplitude (Xi) and phase angle (Φi) for each mass (mi) of the system shown below when excited by a harmonic force (F1sin Ωt) acting on mass m1.
4.6.2. Problem Specifications Material properties for this problem are: m1 = m2 = 0.5 lb-sec2/in k1 = k2 = kc = 200 lb/in Loading for this problem is: F1 = 200 lb The spring lengths are arbitrarily selected and are used only to define the spring direction. Two master degrees of freedom are selected at the masses in the spring direction. A frequency range from zero to 7.5 Hz with a Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–13
Chapter 4: Harmonic Response Analysis solution at 7.5/30 = 0.25 Hz intervals is chosen to give an adequate response curve. POST26 is used to get an amplitude versus frequency display.
4.6.3. Problem Diagram Figure 4.4 Two-Mass-Spring-System
4.6.3.1. Set the Analysis Title 1.
Choose menu path Utility Menu> File> Change Title.
2.
Type the text "Harmonic Response of Two-Mass-Spring System" and click on OK.
4.6.3.2. Define the Element Types 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
Scroll down the list on the left to "Combination" and select it.
4.
Click once on "Spring-damper 14" in the list on the right.
5.
Click on Apply.
4–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.6: Sample Harmonic Response Analysis (GUI Method) 6.
Scroll up the list on the left to "Structural Mass" and select it.
7.
Click once on "3D mass 21" in the list on the right.
8.
Click on OK. The Library of Element Types dialog box closes.
9.
Click on Close in the Element Types dialog box.
4.6.3.3. Define the Real Constants 1.
Choose menu path Main Menu> Preprocessor> Real Constants.
2.
Click on Add. The Element Type for Real Constants dialog box appears.
3.
Click once on Type 1 to highlight it.
4.
Click on OK. The Real Constants for COMBIN14 dialog box appears.
5.
Enter 200 for the spring constant (K) and 0.1 for the damping coefficient (CV1). Click on OK.
6.
Repeat steps 2-4 for Type 2, MASS21.
7.
Enter .5 for mass in X direction and click on OK.
8.
Click on Close to close the Real Constants dialog box.
4.6.3.4. Create the Nodes 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Nodes> In Active CS.
2.
Enter 1 for node number.
3.
Enter 0, 0, 0 for the X, Y, and Z coordinates, respectively.
4.
Click on Apply.
5.
Enter 4 for node number.
6.
Enter 1, 0, 0 for the X, Y, and Z coordinates, respectively.
7.
Click on OK.
8.
Choose menu path Utility Menu> PlotCtrls> Numbering. The Plot Numbering Controls dialog box appears.
9.
Click once on "Node numbers" to turn node numbers on.
10. Click on OK. 11. Choose menu path Main Menu> Preprocessor> Modeling> Create> Nodes> Fill between Nds. A picking menu appears. 12. In the ANSYS Graphics window, click once on nodes 1 and 4 (on the left and right sides of the screen). A small box appears around each node. 13. Click on OK on the picking menu. The Create Nodes Between 2 Nodes dialog box appears. 14. Click on OK to accept the default of 2 nodes to fill. Nodes 2 and 3 appear in the graphics window.
4.6.3.5. Create the Spring Elements 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Thru Nodes. A picking menu appears.
2.
In the graphics window, click once on nodes 1 and 2.
3.
Click on Apply. A line appears between the selected nodes. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–15
Chapter 4: Harmonic Response Analysis 4.
Click once on nodes 2 and 3.
5.
Click on Apply. A line appears between the selected nodes.
6.
Click once on nodes 3 and 4.
7.
Click on OK. A line appears between the selected nodes.
4.6.3.6. Create the Mass Elements 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes.
2.
Enter 2 for element type number.
3.
Enter 2 for real constant set number and click on OK.
4.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Thru Nodes. A picking menu appears.
5.
In the graphics window, click once on node 2.
6.
Click on Apply.
7.
Click once on node 3 and click on OK.
4.6.3.7. Specify the Analysis Type, MDOF, and Load Step Specifications 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis.
2.
Click once on "Harmonic" and click on OK.
3.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options.
4.
Click once on "Full" to select the solution method.
5.
Click once on "Amplitud + phase" to select the DOF printout format and click on OK.
6.
Click OK in the Full Harmonic Analysis dialog box.
7.
Choose menu path Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout.
8.
Click on "Last substep" to set the print frequency and click on OK.
9.
Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Freq and Substeps.
10. Enter 0 and 7.5 for the harmonic frequency range. 11. Enter 30 for the number of substeps. 12. Click once on "Stepped" to specify stepped boundary conditions. 13. Click on OK.
4.6.3.8. Define Loads and Boundary Conditions 1.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. A picking menu appears.
2.
Click on Pick All. The Apply U, ROT on Nodes dialog box appears.
3.
In the scroll box for DOFs to be constrained, click once on "UY" to highlight it (make sure no other selections are highlighted).
4.
Click on OK.
5.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. A picking menu appears.
4–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.6: Sample Harmonic Response Analysis (GUI Method) 6.
In the graphics window, click once on nodes 1 and 4.
7.
Click on OK. The Apply U, ROT on Nodes dialog box appears.
8.
In the scroll box for DOFs to be constrained, click once on "UX" to highlight it and click once on "UY" to deselect it.
9.
Click on OK.
10. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Force/ Moment> On Nodes. A picking menu appears. 11. In the graphics window, click once on node 2. 12. Click on OK. The Apply F/M on Nodes dialog box appears. 13. In the scroll box for direction of force/moment, click once on "FX." 14. Enter 200 for the real part of force/moment and click on OK.
4.6.3.9. Solve the Model 1.
Choose menu path Main Menu> Solution> Solve> Current LS.
2.
Review the information in the status window and click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to begin the solution.
4.
When the solution is finished, a dialog box stating "Solution is done!" appears. Click on Close.
4.6.3.10. Review the Results For this sample, you will review the time-history results of nodes 2 and 3. 1.
Choose menu path Main Menu> TimeHist Postpro> Define Variables. The Defined Time-History Variables dialog box appears.
2.
Click on Add. The Add Time-History Variable dialog box appears.
3.
Click on OK to accept the default of Nodal DOF result. The Define Nodal Data dialog box appears.
4.
Enter 2 for reference number of variable.
5.
Enter 2 for node number.
6.
Enter 2UX for the user-specified label.
7.
In the scroll box on the right, click once on "Translation UX" to highlight it.
8.
Click on OK.
9.
Click on Add in the Defined Time-History Variables dialog box. The Add Time-History Variable dialog box appears.
10. Click on OK to accept the default of Nodal DOF result. The Define Nodal Data dialog box appears. 11. Enter 3 for reference number of variable. 12. Enter 3 for node number. 13. Enter 3UX for the user-specified label. 14. In the scroll box on the right, click once on "Translation UX" to highlight it. 15. Click on OK. 16. Click on Close.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–17
Chapter 4: Harmonic Response Analysis 17. Choose menu path Utility Menu> PlotCtrls> Style> Graphs. The Graph Controls dialog box appears. 18. In the scroll box for type of grid, scroll to "X and Y lines" to select it. 19. Click on OK. 20. Choose menu path Main Menu> TimeHist Postpro> Graph Variables. The Graph Time-History Variables dialog box appears. Your graph should look like this:
21. Enter 2 for 1st variable to graph. 22. Enter 3 for 2nd variable to graph. 23. Click on OK. A graph appears in the graphic window.
4.6.3.11. Exit ANSYS You are now finished with this sample problem. 1.
In the ANSYS Toolbar, click on Quit.
2.
Choose the save option you want and click on OK.
4.7. Sample Harmonic Response Analysis (Command or Batch Method) You can perform the example harmonic response analysis of a two-mass-spring system by using the following ANSYS commands instead of the GUI. /PREP7 /TITLE, Harmonic response of a two-mass-spring system ET,1,COMBIN14,,,2
4–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.8: Where to Find Other Examples ET,2,MASS21,,,4 R,1,200 R,2,.5 N,1 N,4,1 FILL E,1,2 E,2,3 E,3,4 TYPE,2 REAL,2 E,2 E,3 FINISH /SOLU ANTYPE,HARMIC HROPT,FULL HROUT,OFF OUTPR,BASIC,1 NSUBST,30 HARFRQ,,7.5 KBC,1 D,1,UY,,,4 D,1,UX,,,4,3 F,2,FX,200 SOLVE FINISH /POST26 NSOL,2,2,U,X,2UX NSOL,3,3,U,X,3UX /GRID,1 /AXLAB,Y,DISP PLVAR,2,3 FINISH
! Spring constant = 200 ! Mass = 0.5
! Spring element ! Spring element
! Mass element ! Mass element
! Harmonic response analysis ! Full harmonic response ! Print results as amplitudes and phase angles ! ! ! ! !
30 Intervals within freq. range Frequency range from 0 to 7.5 HZ Step boundary condition Constrain all 44 DOF Constrain nodes 1 and 4 in UX
! Store UX Displacements ! Turn grid on ! Y-axis label disp ! Display variables 2 and 3
4.8. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional harmonic analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS family of products. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual includes a variety of harmonic analysis test cases: VM19 - Random Vibration Analysis of a Deep Simply-Supported Beam VM76 - Harmonic Response of a Guitar String VM86 - Harmonic Response of a Dynamic System VM87 - Equivalent Structural Damping VM88 - Response of an Eccentric Weight Exciter VM90 - Harmonic Response of a Two-Mass-Spring System VM176 - Frequency Response of Electrical Input Admittance for a Piezoelectric Transducer VM177 - Natural Frequency of a Submerged Ring VM183 - Harmonic Response of a Spring-Mass System VM203 - Dynamic Load Effect on Simply-Supported Thick Square Plate
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–19
Chapter 4: Harmonic Response Analysis
4.9. Reduced Harmonic Response Analysis The reduced method, as its name implies, uses reduced matrices to calculate the harmonic solution. The procedure for a reduced harmonic analysis consists of five main steps: 1.
Build the model.
2.
Apply the loads and obtain the reduced solution.
3.
Review the results of the reduced solution.
4.
Expand the solution (expansion pass).
5.
Review the results of the expanded solution.
Of these, the first step is the same as for the full method. Details of the other steps are explained below.
4.9.1. Apply Loads and Obtain the Reduced Solution By reduced solution, we mean the degree of freedom solution calculated at the master DOF. The tasks required to obtain the reduced solution are as follows: 1.
Enter the ANSYS solution processor. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define the analysis type and options. Options for the reduced solution are the same as described for the full method except for the following differences: •
Choose the reduced solution method.
•
You can include prestress effects (PSTRES). This requires element files from a previous static (or transient) analysis that also included prestress effects. See Section 4.11.1: Prestressed Harmonic Response Analysis for details.
3.
Define master degrees of freedom. Master DOF are essential or dynamic degrees of freedom that characterize the dynamic behavior of the structure. For a reduced harmonic response dynamic analysis, master DOF are also required at locations where you want to apply forces or nonzero displacements. See Section 3.14: Matrix Reduction for guidelines to choose master DOF.
4.
Apply loads on the model. Harmonic loading is the same as described for the full method, except for the following restrictions: •
Only displacements and forces are valid. Element loads such as pressures, temperatures, and accelerations are not allowed.
•
Forces and nonzero displacements must be applied only at master DOF.
5.
Specify load step options. These are the same as described for the full method except that the OUTRES and ERESX commands are not available, and the constant material damping coefficient (MP,DMPR) is not applicable for the reduced method. The OUTPR command controls the printout of the nodal solution at the master DOF (OUTPR,NSOL,ALL (or NONE)).
6.
Save a copy of the database. Command(s): SAVE GUI: Utility Menu> File> Save as
7.
Start solution calculations.
4–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.9: Reduced Harmonic Response Analysis Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS 8.
Repeat steps 4 through 7 for any additional loads and frequency ranges (that is, for additional load steps). If you plan to do time-history postprocessing (POST26), the frequency ranges should not overlap from one load step to the next. Another method for multiple load steps, which allows you to store the load steps on files and then solve them at once using a macro, is described in the ANSYS Basic Analysis Guide.
9.
Leave SOLUTION. Command(s): FINISH GUI: Close the Solution menu.
4.9.2. Review the Results of the Reduced Solution Results from the reduced harmonic solution are written to the reduced harmonic displacement file, Jobname.RFRQ. They consist of displacements at the master DOF, which vary harmonically at each forcing frequency for which the solution was calculated. As with the full method, these displacements will be complex in nature if damping was defined or if out-of-phase loads were applied. You can review the master DOF displacements as a function of frequency using POST26. (POST1 cannot be used, because the complete solution at all DOF is not available.) The procedure to use POST26 is the same as described for the full method, except for the following differences: •
Before defining the POST26 variables, use the FILE command to specify that data are to be read from Jobname.RFRQ. For example, if HARMONIC is the jobname, the FILE command would be: FILE,HARMONIC,RFRQ. (By default, POST26 looks for a results file, which is not written by a reduced harmonic solution.)
•
Only nodal degree of freedom data (at master DOF) are available for processing, so you can use only the NSOL command to define variables.
4.9.3. Expand the Solution (Expansion Pass) The expansion pass starts with the reduced solution and calculates the complete displacement, stress, and force solution at all degrees of freedom. These calculations are done only at frequencies and phase angles that you specify. Therefore, before you begin the expansion pass, you should review the results of the reduced solution (using POST26) and identify the critical frequencies and phase angles. An expansion pass is not always required. For instance, if you are interested mainly in displacements at specific points on the structure, then the reduced solution could satisfy your requirements. However, if you want to determine displacements at non-master DOF, or if you are interested in the stress solution, then you must perform an expansion pass.
4.9.3.1. Points to Remember •
The .RFRQ, .TRI, .EMAT, and .ESAV files from the reduced solution must be available.
•
The database must contain the same model for which the reduced solution was calculated.
4.9.3.2. Expanding the Modes 1.
Reenter the ANSYS solution processor. Command(s): /SOLU GUI: Main Menu> Solution
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–21
Chapter 4: Harmonic Response Analysis Note — You must explicitly leave SOLUTION (using the FINISH command) and reenter (/SOLU) before performing the expansion pass. 2.
Activate the expansion pass and its options. ANSYS offers these options for the expansion pass:
Table 4.5 Expansion Pass Options Option
Command
GUI Path
Expansion Pass On/Off
EXPASS
Main Menu> Solution> Analysis Type> ExpansionPass
No. of Solutions to Expand
NUMEXP
Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> Range of Solu's
Freq. Range for Expansion
NUMEXP
Main Menu> Solution> Load Step Opts> ExpansionPass> Singe Expand> Range of Solu's
Phase Angle for Expansion
HREXP
Main Menu> Solution> Load Step Opts> ExpansionPass> Singe Expand> Range of Solu's
Stress Calculations On/Off
NUMEXP, EXPSOL
Main Menu> Solution> Load Step Opts> ExpansionPass> Singe Expand> Range of Solu's
Nodal Solution Listing Format
HROUT
Main Menu> Solution> Analysis Type> Analysis Options
Each of these options is explained in detail below. •
Option: Expansion Pass On/Off (EXPASS) Choose ON.
•
Option: Number of Solutions to Expand (NUMEXP,NUM) Specify the number. This number of evenly spaced solutions will be expanded over a frequency range (specified next). For example, NUMEXP,4,1000,2000 specifies four solutions in the frequency range 1000 to 2000 (that is, expanded solutions at 1250, 1500, 1750, and 2000).
•
Option: Frequency Range for Expansion (NUMEXP, BEGRNG, ENDRNG) Specify the frequency range. See the example above. If you do not need to expand multiple solutions, you can use EXPSOL to identify a single solution for expansion (either by its load step and substep numbers or by its frequency value).
•
Option: Phase Angle for Expansion (HREXP) If multiple solutions are to be expanded over a frequency range (NUMEXP), we suggest that you request both the real and imaginary parts to be expanded (HREXP,ALL). This way, you can easily combine the two parts in POST26 to review the peak values of displacements, stresses, and other results. If, on the other hand, a single solution is to be expanded (EXPSOL), you can specify the phase angle at which peak displacements occurred using HREXP,angle.
•
Option: Stress Calculations On/Off (NUMEXP or EXPSOL) You can turn off stress and force calculations if you are not interested in them. Default is to calculate stresses and forces.
• 4–22
Option: Nodal Solution Listing Format (HROUT) Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.9: Reduced Harmonic Response Analysis Determines how the harmonic displacement solution is listed in the printed output (Jobname.OUT). You can choose between real and imaginary parts (default), and amplitudes and phase angles. 3.
Specify load step options. The only options valid for a harmonic expansion pass are output controls: •
Printed Output Use this option to include any results data on the printed output file (Jobname.OUT). Command(s): OUTPR GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout
•
Database and Results File Output Use this option to control the data on the results file (Jobname.RST). Command(s): OUTRES GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> DB/Results File
•
Extrapolation of Results Use this option to review element integration point results by copying them to the nodes instead of extrapolating them (default). Note — The FREQ field on OUTPR and OUTRES can be only ALL or NONE. Command(s): ERESX GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> Integration Pt
4.
Start expansion pass calculations. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
5.
Repeat steps 2, 3, and 4 for additional solutions to be expanded. Each expansion pass is stored as a separate load step on the results file. Caution: Subsequent spectrum analyses expect all expanded modes to be in one load step.
6.
Leave SOLUTION. You can now review results in the postprocessor. Command(s): FINISH GUI: Close the Solution menu.
4.9.4. Review the Results of the Expanded Solution This step is the same as the corresponding step in a basic structural analysis with the following additions: You can review the results using POST1. (If you expanded solutions at several frequencies, you can also use POST26 to obtain graphs of stress versus frequency, strain versus frequency, etc.) The procedure to use POST1 (or POST26) is the same as described for the full method, except for one difference: if you requested expansion at a specific phase angle (HREXP,angle), there is only one solution available for each frequency. Use the SET command to read in the results. See Section 2.3.6: Review the Results in Chapter 2, “Structural Static Analysis”.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–23
Chapter 4: Harmonic Response Analysis
4.9.5. Sample Input A sample input listing for a reduced harmonic response analysis is shown below: ! Build the Model /FILNAM,... ! Jobname /TITLE,... ! Title /PREP7 ! Enter PREP7 -----! Generate model --FINISH ! Apply Loads and Obtain the Reduced Solution /SOLU ! Enter SOLUTION ANTYPE,HARMIC ! Harmonic analysis HROPT,REDU ! Reduced method HROUT,... ! Harmonic analysis output options M,... ! Master DOF TOTAL,... D,... ! Constraints F,... ! Loads (real and imaginary components) HARFRQ,... ! Forcing frequency range DMPRAT,... ! Damping ratio NSUBST,... ! Number of harmonic solutions KBC,... ! Ramped or stepped loads SAVE SOLVE ! Initiate multiple load step solution FINISH ! Review the Results of the Reduced Solution /POST26 FILE,,RFRQ ! Postprocessing file is Jobname.RFRQ NSOL,... ! Store nodal result as a variable PLCPLX,... ! Define how to plot complex variables PLVAR,... ! Plot variables PRCPLX,... ! Define how to list complex variables PRVAR,... ! List variables FINISH ! Expand the Solution /SOLU EXPASS,ON EXPSOL,... HREXP,... OUTRES,... SOLVE FINISH
! ! ! !
Reenter SOLUTION Expansion pass Expand a single solution Phase angle for expanded solution
! Review the Results of the Expanded Solution /POST1 SET,... ! Read results for desired frequency PLDISP,... ! Deformed shape PRRSOL,... ! List reactions PLNSOL,... ! Contour plot of nodal results -----! Other postprocessing as desired --FINISH
See the ANSYS Commands Reference for a discussion of the ANTYPE, HROPT, HROUT, M, TOTAL, HARFRQ, DMPRAT, NSUBST, KBC, FILE, NSOL, PLCPLX, PLVAR, PRCPLX, PRVAR, EXPASS, EXPSOL, HREXP, PLDISP, PRRSOL, and PLNSOL commands.
4–24
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.10: Mode Superposition Harmonic Response Analysis
4.10. Mode Superposition Harmonic Response Analysis The mode superposition method sums factored mode shapes (obtained from a modal analysis) to calculate the harmonic response. It is the only method allowed in the ANSYS Professional program. The procedure to use the method consists of five main steps: 1.
Build the model.
2.
Obtain the modal solution.
3.
Obtain the mode superposition harmonic solution.
4.
Expand the mode superposition solution.
5.
Review the results.
Of these, the first step is the same as described for the full method. The remaining steps are described below.
4.10.1. Obtain the Modal Solution Chapter 3, “Modal Analysis” describes how to obtain a modal solution. Following are some additional hints: •
The mode-extraction method should be Block Lanczos (default), subspace, reduced, PowerDynamics, or QR damped. (The other methods, unsymmetric and damped, do not apply to mode superposition.)
•
Be sure to extract all modes that may contribute to the harmonic response.
•
If PowerDynamics was used for the modal solution, no nonzero loads or displacements are allowed (that is, only u = 0 is valid as the initial condition). PowerDynamics does not create a load vector; therefore, the LVSCALE command is not valid unless the scale factor is set to zero.
•
For the reduced mode-extraction method, include those master degrees of freedom at which harmonic loads will be applied.
•
If you use the QR damped mode-extraction method, you must specify any damping (ALPHAD, BETAD, MP,DAMP, or element damping including gyroscopic) that you want to include during preprocessing or in the modal analysis. (ANSYS ignores damping specified during the mode superposition harmonic analysis.) You can set a constant damping ratio (DMPRAT), define constant material damping coefficients (MP,DMPR), or define the damping ratio as a function of mode (MDAMP) in a modal superposition harmonic analysis.
•
If you need to apply harmonically varying element loads (pressures, temperatures, accelerations, and so on), specify them in the modal analysis. ANSYS ignores the loads for the modal solution, but calculates a load vector and writes it to the mode shape file (Jobname.MODE). You can then use the load vector for the harmonic solution. The imaginary component of the load vector calculated from element loads will always be zero with only one exception: in a full harmonic response analysis or a mode superposition harmonic response analysis with the Block Lanczos mode-extraction method, you can apply imaginary pressures via SURF153 or SURF154.
•
The modes need not be expanded for the mode superposition solution. (If you want to review mode shapes, however, you must expand the mode shapes.)
•
Do not change the model data (for example, nodal rotations) between the modal and harmonic analyses.
4.10.2. Obtain the Mode Superposition Harmonic Solution In this step, the program uses mode shapes extracted by the modal solution to calculate the harmonic response. The mode shape file (Jobname.MODE) must be available, and the database must contain the same model for which the modal solution was obtained. If the modal solution was performed using the subspace or Block Lanczos Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–25
Chapter 4: Harmonic Response Analysis method using the default mass formulation (not the lumped mass approximation), the full file (Jobname.FULL) must also be available. The following tasks are involved: 1.
Enter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define the analysis type and analysis options. These are the same as described for the full method, except for the following differences:
3.
4.
•
Choose the mode superposition method of solution (HROPT).
•
Specify the modes you want to use for the solution (HROPT). This determines the accuracy of the harmonic solution. Generally, the number of modes specified should cover about 50 percent more than the frequency range of the harmonic loads.
•
Optionally, cluster the solutions about the structure's natural frequencies (HROUT) for a smoother and more accurate tracing of the response curve.
•
Optionally, at each frequency, print a summary table that lists the contributions of each mode to the response (HROUT). Note, OUTPR,NSOL must be specified to print mode contributions at each frequency.
Apply loads on the model. Harmonic loading is the same as described for the full method, except for the following restrictions: •
Only forces, accelerations, and the load vector created in the modal analysis are valid. Use the LVSCALE command to apply the load vector from the modal solution. Note that ALL loads from the modal analysis are scaled, including forces and accelerations. To avoid load duplication, delete any loads that were applied in the modal analysis.
•
If mode shapes from a reduced modal solution are being used, forces may be applied only at master DOF.
Specify load step options. These are the same as described for the reduced method except that you can also specify modal damping (MDAMP). In addition, if the QR damped method is specified, constant material damping coefficients (MP,DMPR) can be defined. The NSUBST command specifies the number of solutions on each side of a natural frequency if the clustering option (HROUT) is chosen. The default is to calculate four solutions, but you can specify any number of solutions from 2 through 20. (Any value over this range defaults to 10 and any value below this range defaults to 4.)
5.
If you used either the Block Lanczos (default) or the subspace option for the modal analysis (MODOPT,LANB or SUBSP), you may use a nodal component with the OUTRES,NSOL command to limit the displacement data written to the reduced displacement file Jobname.RFRQ. The expansion pass will only produce valid results for those nodes and for those elements in which all of the nodes of the elements have been written to the .RFRQ file. To use this option, first suppress all writing by invoking OUTRES,NSOL,NONE, then specify the item(s) of interest by invoking OUTRES,NSOL,ALL,component. Repeat the OUTRES command for any additional nodal components that you want to write to the .RFRQ file.
6.
Save a copy of the database. Command(s): SAVE GUI: Utility Menu> File> Save as
7.
Start solution calculations.
4–26
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.10: Mode Superposition Harmonic Response Analysis Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS 8.
Repeat steps 3 to 7 for any additional loads and frequency ranges (that is, for additional load steps). If you plan to do time-history postprocessing (POST26), the frequency ranges should not overlap from one load step to the next.
9.
Leave SOLUTION. Command(s): FINISH GUI: Close the Solution menu.
The mode superposition harmonic solution is written to the reduced displacement file, Jobname.RFRQ, regardless of whether the subspace, Block Lanczos, reduced, PowerDynamics, or QR damped method was used for the modal solution. You will therefore need to expand the solution if you are interested in stress results.
4.10.3. Expand the Mode Superposition Solution The procedure for the expansion pass is the same as described for the reduced method. Jobname.TRI from the modal analysis is needed only if the reduced eigenvalue extraction method was used. The output from the expansion pass includes the structural results file, Jobname.RST, containing expanded results. See Section 4.9.3: Expand the Solution (Expansion Pass).
4.10.4. Review the Results Results consist of harmonically varying displacements, stresses, and reaction forces at each forcing frequency for which the solution was calculated. You can review these results using POST26 or POST1, as explained for the reduced method.
4.10.5. Sample Input A sample input listing for a mode superposition harmonic response analysis is shown below: ! Build the Model /FILNAM,... /TITLE,... /PREP7 ------FINISH
! Jobname ! Title ! Enter PREP7 ! Generate model
! Obtain the Modal Solution /SOLU ! Enter SOLUTION ANTYPE,MODAL ! Modal analysis MODOPT,REDU ! Reduced method M,... ! Masters TOTAL,.. D,... ! Constraints SF,... ! Element loads SAVE SOLVE ! Initiate modal solution FINISH ! Obtain the Mode Superposition Harmonic Solution /SOLU ! Enter SOLUTION ANTYPE,HARMIC HROPT,MSUP,... HROUT,... LVSCALE,... F,... HARFRQ,...
! ! ! ! ! !
Harmonic analysis Mode superposition method; number of modes to use Harmonic analysis output options; cluster option Scale factor for loads from modal analysis Nodal loads Forcing frequency range
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–27
Chapter 4: Harmonic Response Analysis DMPRAT,... MDAMP,... NSUBST,... KBC,... SAVE SOLVE FINISH
! ! ! !
Damping ratio Modal damping ratios Number of harmonic solutions Ramped or stepped loads
! Initiate solution
! Review the Results of the Mode Superposition Solution /POST26 FILE,,RFRQ ! Postprocessing file is Jobname.RFRQ NSOL,... ! Store nodal result as a variable PLCPLX,... ! Define how to plot complex variables PLVAR,... ! Plot variables FINISH ! Expand the Solution (for Stress Results) /SOLU! Re-enter SOLUTION EXPASS,ON ! Expansion pass EXPSOL,... ! Expand a single solution HREXP,... ! Phase angle for expanded solution SOLVE FINISH ! Review the Results of the Expanded Solution /POST1 SET,... ! Read results for desired frequency PLDISP,... ! Deformed shape PLNSOL,... ! Contour plot of nodal results --FINISH
See the ANSYS Commands Reference for a discussion of the ANTYPE, MODOPT, M, TOTAL, HROPT, HROUT, LVSCALE, F, HARFRQ, DMPRAT, MDAMP, NSUBST, KBC, FILE, NSOL, PLCPLX, PLVAR, EXPASS, EXPSOL, HREXP, SET, and PLNSOL commands.
4.11. Other Analysis Details 4.11.1. Prestressed Harmonic Response Analysis A prestressed harmonic response analysis calculates the dynamic response of a prestressed structure, such as a violin string. It is assumed that the harmonically varying stresses (which are superimposed on the prestress) are much smaller than the prestress itself.
4.11.1.1. Prestressed Full Harmonic Response Analysis The procedure to do a prestressed full harmonic analysis is essentially the same as that for any other full harmonic analysis except that you first need to prestress the structure by doing a static analysis: 1.
Build the model and obtain a static solution with prestress effects turned on (PSTRES,ON). The procedure to obtain the static solution is explained in Chapter 2, “Structural Static Analysis”.
2.
Reenter SOLUTION and obtain the full harmonic solution, also with prestress effects turned on (reissue PSTRES,ON). Files Jobname.EMAT and Jobname.ESAV from the static analysis must be available. If thermal body forces were present during the static prestress analysis, these thermal body forces must not be deleted during the full harmonic analysis or else the thermal prestress will vanish. Hence, any temperature loads used to define the thermal prestress must also be used in the full harmonic response analysis as sinusoidally time-varying temperature loads. You should be aware of this limitation and exercise some judgement about whether or not to include temperature loads in their static prestress analysis.
4–28
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 4.11: Other Analysis Details
4.11.1.2. Prestressed Reduced Harmonic Response Analysis The procedure to do a prestressed reduced harmonic analysis is essentially the same as that for any other reduced harmonic analysis except that you first need to prestress the structure by doing a static analysis: 1.
Build the model and obtain a static solution with prestress effects turned on (PSTRES,ON). The procedure to obtain the static solution is explained in Chapter 2, “Structural Static Analysis”.
2.
Reenter SOLUTION and obtain the reduced harmonic solution, also with prestress effects turned on (reissue PSTRES,ON). Files Jobname.EMAT and Jobname.ESAV from the static analysis must be available.
4.11.1.3. Prestressed Mode Superposition Harmonic Response Analysis To include prestress effects in a mode superposition analysis, you must first perform a prestressed modal analysis. See Chapter 3, “Modal Analysis” for details. Once prestressed modal analysis results are available, proceed as for any other mode superposition analysis.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
4–29
4–30
Chapter 5: Transient Dynamic Analysis 5.1. Definition of Transient Dynamic Analysis Transient dynamic analysis (sometimes called time-history analysis) is a technique used to determine the dynamic response of a structure under the action of any general time-dependent loads. You can use this type of analysis to determine the time-varying displacements, strains, stresses, and forces in a structure as it responds to any combination of static, transient, and harmonic loads. The time scale of the loading is such that the inertia or damping effects are considered to be important. If the inertia and damping effects are not important, you might be able to use a static analysis instead (see Chapter 2, “Structural Static Analysis”). The basic equation of motion solved by a transient dynamic analysis is && } + (C){ u& } + (K){u} = {F(t)} (M){ u where: (M) = mass matrix (C) = damping matrix (K) = stiffness matrix && } = nodal acceleration vector {u { u& } = nodal velocity vector {u} = nodal displacement vector {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 && }) and damping forces ((C){ u& }). The ANSYS program uses the Newmark time into account inertia forces ((M){ u integration method or an improved method called HHT to solve these equations at discrete time points. The time increment between successive time points is called the integration time step.
5.2. Preparing for a Transient Dynamic Analysis A transient dynamic analysis is more involved than a static analysis because it generally requires more computer resources and more of your resources, in terms of the “engineering” time involved. You can save a significant amount of these resources by doing some preliminary work to understand the physics of the problem. For example, you can: 1.
Analyze a simpler model first. A model of beams, masses, and springs can provide good insight into the problem at minimal cost. This simpler model may be all you need to determine the dynamic response of the structure.
2.
If you are including nonlinearities, try to understand how they affect the structure's response by doing a static analysis first. In some cases, nonlinearities need not be included in the dynamic analysis.
3.
Understand the dynamics of the problem. By doing a modal analysis, which calculates the natural frequencies and mode shapes, you can learn how the structure responds when those modes are excited. The natural frequencies are also useful for calculating the correct integration time step.
4.
For a nonlinear problem, consider substructuring the linear portions of the model to reduce analysis costs. Substructuring is described in the ANSYS Advanced Analysis Techniques Guide.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 5: Transient Dynamic Analysis
5.3. Three Solution Methods Three methods are available to do a transient dynamic analysis: full, mode superposition, and reduced. The ANSYS Professional program allows only the mode superposition method. Before we study the details of how to implement each of these methods, we will examine the advantages and disadvantages of each.
5.3.1. Full Method The full method uses the full system matrices to calculate the transient response (no matrix reduction). It is the most general of the three methods because it allows all types of nonlinearities to be included (plasticity, large deflections, large strain, and so on). Note — If you do not want to include any nonlinearities, you should consider using one of the other methods because the full method is also the most expensive method of the three. The advantages of the full method are: •
It is easy to use, because you do not have to worry about choosing master degrees of freedom or mode shapes.
•
It allows all types of nonlinearities.
•
It uses full matrices, so no mass matrix approximation is involved.
•
All displacements and stresses are calculated in a single pass.
•
It accepts all types of loads: nodal forces, imposed (nonzero) displacements (although not recommended), and element loads (pressures and temperatures) and allows tabular boundary condition specification via TABLE type array parameters.
•
It allows effective use of solid-model loads.
The main disadvantage of the full method is that it is more expensive than either of the other methods. For procedural information about using the full method, see Section 5.4: Performing a Full Transient Dynamic Analysis.
5.3.2. Mode Superposition Method The mode superposition method sums factored mode shapes (eigenvectors) from a modal analysis to calculate the structure's response. This is the only method available in the ANSYS Professional program. Its advantages are: •
It is faster and less expensive than the reduced or the full method for many problems.
•
Element loads applied in the preceding modal analysis can be applied in the transient dynamic analysis via the LVSCALE command, unless the modal analysis was done using PowerDynamics.
•
It accepts modal damping (damping ratio as a function of mode number).
The disadvantages of the mode superposition method are: •
The time step must remain constant throughout the transient, so automatic time stepping is not allowed.
•
The only nonlinearity allowed is simple node-to-node contact (gap condition).
•
It does not accept imposed (nonzero) displacements.
5–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.4: Performing a Full Transient Dynamic Analysis For procedural information about using the mode superposition method, see Section 5.5: Performing a Mode Superposition Transient Dynamic Analysis.
5.3.3. Reduced Method The reduced method condenses the problem size by using master degrees of freedom and reduced matrices. After the displacements at the master DOF have been calculated, ANSYS expands the solution to the original full DOF set. (See Section 3.14: Matrix Reduction for a more detailed discussion of the reduction procedure.) The advantage of the reduced method is: •
It is faster and less expensive than the full method.
The disadvantages of the reduced method are: •
The initial solution calculates only the displacements at the master DOF. A second step, known as the expansion pass, is required for a complete displacement, stress, and force solution. (However, the expansion pass might not be needed for some applications.)
•
Element loads (pressures, temperatures, and so on) cannot be applied. Accelerations, however, are allowed.
•
All loads must be applied at user-defined master degrees of freedom. (This limits the use of solid-model loads.)
•
The time step must remain constant throughout the transient, so automatic time stepping is not allowed.
•
The only nonlinearity allowed is simple node-to-node contact (gap condition).
For procedural information about using the reduced method, see Section 5.6: Performing a Reduced Transient Dynamic Analysis.
5.4. Performing a Full Transient Dynamic Analysis Note - Before reading this section, you are encouraged to become familiar with the concepts presented in Chapter 2, “Structural Static Analysis”. We will first describe how to do a transient dynamic analysis using the full method. We will then list the steps that are different for the mode superposition and reduced methods. The procedure for a full transient dynamic analysis (available in the ANSYS Multiphysics, ANSYS Mechanical, and ANSYS Structural products) consists of these steps: 1.
Section 5.4.1: Build the Model
2.
Section 5.4.2: Establish Initial Conditions
3.
Section 5.4.3: Set Solution Controls
4.
Section 5.4.4: Set Additional Solution Options
5.
Section 5.4.5: Apply the Loads
6.
Section 5.4.6: Save the Load Configuration for the Current Load Step
7.
Section 5.4.7: Repeat Steps 3-6 for Each Load Step
8.
Section 5.4.8: Save a Backup Copy of the Database
9.
Section 5.4.9: Start the Transient Solution
10. Section 5.4.10: Exit the Solution Processor 11. Section 5.4.11: Review the Results Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–3
Chapter 5: Transient Dynamic Analysis
5.4.1. Build the Model See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details, see the ANSYS Modeling and Meshing Guide.
5.4.1.1. Points to Remember Keep the following points in mind when building a model for a full transient dynamic analysis: •
You can use both linear and nonlinear elements.
•
Both Young's modulus (EX) (or stiffness in some form) and density (DENS) (or mass in some form) must be defined. Material properties may be linear or nonlinear, isotropic or orthotropic, and constant or temperature-dependent.
Some comments on mesh density: •
The mesh should be fine enough to resolve the highest mode shape of interest.
•
Regions where stresses or strains are of interest require a relatively finer mesh than regions where only displacements are of interest.
•
If you want to include nonlinearities, the mesh should be able to capture the effects of the nonlinearities. For example, plasticity requires a reasonable integration point density (and therefore a fine element mesh) in areas with high plastic deformation gradients.
•
If you are interested in wave propagation effects (for example, a bar dropped exactly on its end), the mesh should be fine enough to resolve the wave. A general guideline is to have at least 20 elements per wavelength along the direction of the wave.
5.4.2. Establish Initial Conditions Before you can perform a full transient dynamic analysis on a model, you need to understand how to establish initial conditions and use load steps. A transient analysis, by definition, involves loads that are functions of time. To specify such loads, you need to divide the load-versus-time curve into suitable load steps. Each "corner" on the load-time curve may be one load step, as shown in Figure 5.1: “Examples of Load-Versus-Time Curves”.
Figure 5.1 Examples of Load-Versus-Time Curves
5–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.4: Performing a Full Transient Dynamic Analysis The first load step you apply is usually to establish initial conditions. You then specify the loads and load step options for the second and subsequent transient load steps. For each load step, you need to specify both load values and time values, along with other load step options such as whether to step or ramp the loads, use automatic time stepping, and so on. You then write each load step to a file and solve all load steps together. Establishing initial conditions is described below; the remaining tasks are described later in this chapter. The first step in applying transient loads is to establish initial conditions (that is, the condition at Time = 0). A transient dynamic analysis requires two sets of initial conditions (because the equations being solved are of
u& u& second order): initial displacement (uo) and initial velocity ( o ). If no special action is taken, both uo and o are && u
assumed to be zero. Initial accelerations ( o ) are always assumed to be zero, but you can specify nonzero initial accelerations by applying appropriate acceleration loads over a small time interval. The following paragraphs describe how to apply different combinations of initial conditions.
u&
Zero initial displacement and zero initial velocity - These are the default conditions, that is, if uo = o = 0, you do not need to specify anything. You may apply the loads corresponding to the first corner of the load-versus-time curve in the first load step. Nonzero initial displacement and/or nonzero initial velocity - You can set these initial conditions with the IC command. Command(s): IC GUI: Main Menu> Solution> Define Loads> Apply> Initial Condit'n> Define Caution: Be careful not to define inconsistent initial conditions. For instance, if you define an initial velocity at a single DOF, the initial velocity at every other DOF will be 0.0, potentially leading to conflicting initial conditions. In most cases, you will want to define initial conditions at every unconstrained DOF in your model. If these conditions are not the same at every DOF, it is usually much easier to define initial conditions explicitly, as documented below (rather than by using the IC command). See the ANSYS Commands Reference for a discussion of the TIMINT and IC commands. Zero initial displacement and nonzero initial velocity - The nonzero velocity is established by applying small displacements over a small time interval on the part of the structure where velocity is to be specified. For example if
u& o = 0.25, you can apply a displacement of 0.001 over a time interval of 0.004, as shown below. ... TIMINT,OFF D,ALL,UY,.001 TIME,.004 LSWRITE DDEL,ALL,UY TIMINT,ON ...
! ! ! ! ! !
Time integration effects off Small UY displ. (assuming Y-direction velocity) Initial velocity = 0.001/0.004 = 0.25 Write load data to load step file (Jobname.S01) Remove imposed displacements Time integration effects on
Nonzero initial displacement and nonzero initial velocity - This is similar to the above case, except that the imposed displacements are actual values instead of "small" values. For example, if uo = 1.0 and a displacement of 1.0 over a time interval of 0.4: ... TIMINT,OFF D,ALL,UY,1.0 TIME,.4 LSWRITE DDELE,ALL,UY
! ! ! ! !
u& o = 2.5, you would apply
Time integration effects off Initial displacement = 1.0 Initial velocity = 1.0/0.4 = 2.5 Write load data to load step file (Jobname.S01) Remove imposed displacements
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–5
Chapter 5: Transient Dynamic Analysis TIMINT,ON ...
! Time integration effects on
Nonzero initial displacement and zero initial velocity - This requires the use of two substeps (NSUBST,2) with a step change in imposed displacements (KBC,1). Without the step change (or with just one substep), the imposed displacements would vary directly with time, leading to a nonzero initial velocity. The example below shows how
u& to apply uo = 1.0 and o = 0.0: ... TIMINT,OFF ! Time integration effects off for static solution D,ALL,UY,1.0 ! Initial displacement = 1.0 TIME,.001 ! Small time interval NSUBST,2 ! Two substeps KBC,1 ! Stepped loads LSWRITE ! Write load data to load step file (Jobname.S01) ! Transient solution TIMINT,ON ! Time-integration effects on for transient solution TIME,... ! Realistic time interval DDELE,ALL,UY ! Remove displacement constraints KBC,0 ! Ramped loads (if appropriate) ! Continue with normal transient solution procedures ...
Nonzero initial acceleration - This can be approximated by specifying the required acceleration (ACEL) over a small interval of time. For example, the commands to apply an initial acceleration of 9.81 would look like this: ... ACEL,,9.81 ! Initial Y-direction acceleration TIME,.001 ! Small time interval NSUBST,2 ! Two substeps KBC,1 ! Stepped loads ! The structure must be unconstrained in the initial load step, or ! else the initial acceleration specification will have no effect. DDELE, ... ! Remove displacement constraints (if appropriate) LSWRITE ! Write load data to load step file (Jobname.S01) ! Transient solution TIME, ... ! Realistic time interval NSUBST, ... ! Use appropriate time step KBC,0 ! Ramped loads (if appropriate) D, ... ! Constrain structure as desired ! Continue with normal transient solution procedures LSWRITE ! Write load data to load step file (Jobname.S02) ...
See the ANSYS Commands Reference for discussions of the ACEL, TIME, NSUBST, KBC, LSWRITE, DDELE, and KBC commands.
5.4.3. Set Solution Controls This step for a transient dynamic analysis is the same as for a basic structural analysis (see Section 2.3.2: Set Solution Controls in Chapter 2, “Structural Static Analysis”) with the following additions: If you need to establish initial conditions for the full transient dynamic analysis (as described in Section 5.4.2: Establish Initial Conditions), you must do so for the first load step of the analysis. You can then cycle through the Solution Controls dialog box additional times to set individual load step options for the second and subsequent load steps (as described in Section 5.4.7: Repeat Steps 3-6 for Each Load Step).
5.4.3.1. Access the Solution Controls Dialog Box To access the Solution Controls dialog box, choose menu path Main Menu> Solution> Analysis Type> Sol'n Control. The following sections provide brief descriptions of the options that appear on each tab of the dialog 5–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.4: Performing a Full Transient Dynamic Analysis box. For details about how to set these options, select the tab that you are interested in (from within the ANSYS program), and then click the Help button. Chapter 8, “Nonlinear Structural Analysis” also contains details about the nonlinear options introduced in this chapter.
5.4.3.2. Using the Basic Tab The Basic tab is active when you access the dialog box. The controls that appear on the Basic tab provide the minimum amount of data that ANSYS needs for the analysis. Once you are satisfied with the settings on the Basic tab, you do not need to progress through the remaining tabs unless you want to adjust the default settings for the more advanced controls. As soon as you click OK on any tab of the dialog box, the settings are applied to the ANSYS database and the dialog box closes. You can use the Basic tab to set the options listed in Table 2.1: “Basic Tab Options”. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Basic tab, and click the Help button. Special considerations for setting these options in a full transient analysis include: •
When setting ANTYPE and NLGEOM, choose Small Displacement Transient if you are performing a new analysis and you want to ignore large deformation effects such as large deflection, large rotation, and large strain. Choose Large Displacement Transient if you expect large deflections (as in the case of a long, slender bar under bending) or large strains (as in a metal-forming problem). Choose Restart Current Analysis if you want to restart a failed nonlinear analysis, or you have previously completed a static prestress or a full transient dynamic analysis, and you want to extend the time-history.
•
When setting AUTOTS, remember that this load step option (which is also known as time-step optimization in a transient analysis) increases or decreases the integration time step based on the response of the structure. For most problems, we recommend that you turn on automatic time stepping, with upper and lower limits for the integration time step. These limits, specified using DELTIM or NSUBST, help to limit the range of variation of the time step; see Section 5.10.2: Automatic Time Stepping for more information. The default is ON.
•
NSUBST and DELTIM are load step options that specify the integration time step for a transient analysis. The integration time step is the time increment used in the time integration of the equations of motion. You can specify the time increment directly or indirectly (that is, in terms of the number of substeps). The time step size determines the accuracy of the solution: the smaller its value, the higher the accuracy. You should consider several factors in order to calculate a "good" integration time step; see Section 5.10.1: Guidelines for Integration Time Step for details.
•
When setting OUTRES, keep this caution in mind: Caution: By default, only the last substep (time-point) is written to the results file (Jobname.RST) in a full transient dynamic analysis. To write all substeps, set the Frequency so that it writes all of the substeps. Also, by default, only 1000 results sets can be written to the results file. If this number is exceeded (based on your OUTRES specification), the program will terminate with an error. Use the command /CONFIG,NRES to increase the limit (see Chapter 19, “Memory Management and Configuration” in the ANSYS Basic Analysis Guide).
5.4.3.3. Using the Transient Tab You can use the Transient tab to set the options listed in Table 5.1: “Transient Tab Options”. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Transient tab, and click the Help button. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–7
Chapter 5: Transient Dynamic Analysis
Table 5.1 Transient Tab Options Option
For more information about this option, see:
Specify whether time integration effects are on or off (TIMINT)
•
Section 8.6: Performing a Nonlinear Transient Analysis in the ANSYS Structural Analysis Guide
Specify whether to ramp the load change over the load step or to step-apply the load change (KBC)
•
Section 2.5: Stepped Versus Ramped Loads in the ANSYS Basic Analysis Guide
•
Section 2.7.1.5: Stepping or Ramping Loads in the ANSYS Basic Analysis Guide
Specify mass and stiffness damping (ALPHAD, BETAD)
•
Section 5.10.3: Damping in the ANSYS Structural Analysis Guide
Choose the time integration method, Newmark or HHT (TRNOPT)
•
Section 17.2: Transient Analysis in the ANSYS, Inc. Theory Reference
Define integration parameters (TINTP)
•
ANSYS, Inc. Theory Reference
Special considerations for setting these options in a full transient analysis include: •
TIMINT is a dynamic load step option that specifies whether time integration effects are on or off. Time integration effects must be turned on for inertia and damping effects to be included in the analysis (otherwise a static solution is performed), so the default is to include time integration effects. This option is useful when beginning a transient analysis from an initial static solution; that is, the first load steps are solved with the time integration effects off.
•
ALPHAD (alpha, or mass, damping) and BETAD (beta, or stiffness, damping) are dynamic load step options for specifying damping options. Damping in some form is present in most structures and should be included in your analysis. See Section 5.4.4.2: Damping Option for other damping options.
•
TRNOPT (TINTOPT) specifies the time integration method to be used. The default is Newmark method.
•
TINTP is a dynamic load step option that specifies transient integration parameters. Transient integration parameters control the nature of the Newmark and HHT time integration techniques.
5.4.3.4. Using the Remaining Solution Controls Tabs The options on the remaining tabs in the Solution Controls dialog box for a full transient analysis are the same as the ones you can set for a static structural analysis. See the following sections of Chapter 2, “Structural Static Analysis” for a list of these options: •
Section 2.3.2.4: Using the Sol'n Options Tab
•
Section 2.3.2.5: Using the Nonlinear Tab
•
Section 2.3.2.6: Using the Advanced NL Tab. Exception: You cannot use arc-length options in a full transient analysis.
5.4.4. Set Additional Solution Options The additional solution options that you can set for a full transient analysis are mostly the same as the ones you can set for a static structural analysis. For a general description of what additional solution options are, along with descriptions of those options that are the same, see the following sections of Chapter 2, “Structural Static Analysis”: 5–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.4: Performing a Full Transient Dynamic Analysis •
Section 2.3.3: Set Additional Solution Options
•
Section 2.3.3.1: Stress Stiffening Effects
•
Section 2.3.3.2: Newton-Raphson Option
•
Section 2.3.3.7: Creep Criteria
•
Section 2.3.3.8: Printed Output
•
Section 2.3.3.9: Extrapolation of Results
Additional solution options for a full transient analysis that differ from those for a static analysis, or have different descriptions are presented in the following sections.
5.4.4.1. Prestress Effects You may include prestress effects in your analysis. This requires element files from a previous static (or transient) analysis; see Section 5.9: Performing a Prestressed Transient Dynamic Analysis for details. Command(s): PSTRES GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options
5.4.4.2. Damping Option Use this load step option to include damping. Damping in some form is present in most structures and should be included in your analysis. In addition to setting ALPHAD and BETAD on the Solution Controls dialog box (as described in Section 5.4.3.3: Using the Transient Tab), you can specify the following additional forms of damping for a full transient dynamic analysis: •
Material-dependent beta damping (MP,DAMP)
•
Element damping (COMBIN7, and so on)
To use the MP form of damping: Command(s): MP,DAMP GUI: Main Menu> Solution> Load Step Opts> Other> Change Mat Props> Material Models> Structural> Damping Note that constant material damping coefficient (MP,DMPR) is not applicable in transient analysis. See Section 5.10.3: Damping for further details.
5.4.4.3. Mass Matrix Formulation Use this analysis option to specify a lumped mass matrix formulation. We recommend the default formulation for most applications. However, for some problems involving "skinny" structures, such as slender beams or very thin shells, the lumped mass approximation might provide better results. Also, the lumped mass approximation can result in a shorter run time and lower memory requirements. To use this option: Command(s): LUMPM GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options
5.4.5. Apply the Loads You are now ready to apply loads for the analysis. Table 2.5: “Loads Applicable in a Static Analysis” summarizes the loads applicable to a transient dynamic analysis. Except for inertia loads, you can define loads either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). Section 2.3.4: Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–9
Chapter 5: Transient Dynamic Analysis Apply the Loads describes the types of loads that are applicable. In an analysis, loads can be applied, removed, operated on, or deleted. For a general discussion of solid-model loads versus finite-element loads, see Chapter 2, “Loading” in the ANSYS Basic Analysis Guide. You can also apply time-dependent boundary conditions by defining a one-dimensional table (TABLE type array parameter). See Section 2.3.4.2.1: Applying Loads Using TABLE Type Array Parameters.
5.4.6. Save the Load Configuration for the Current Load Step As described in Section 5.4.2: Establish Initial Conditions, you need to apply loads and save the load configuration to a load step file for each corner of the load-versus-time curve. You may also want to have an additional load step that extends past the last time point on the curve to capture the response of the structure after the transient loading. Command(s): LSWRITE GUI: Main Menu> Solution> Load Step Opts> Write LS File
5.4.7. Repeat Steps 3-6 for Each Load Step For each load step that you want to define for a full transient dynamic analysis, you need to repeat steps 3-6. That is, for each load step, reset any desired solution controls and options, apply loads, and write the load configuration to a file. For each load step, you can reset any of these load step options: TIMINT, TINTP, ALPHAD, BETAD, MP,DAMP, TIME, KBC, NSUBST, DELTIM, AUTOTS, NEQIT, CNVTOL, PRED, LNSRCH, CRPLIM, NCNV, CUTCONTROL, OUTPR, OUTRES, ERESX, and RESCONTROL. An example load step file is shown below: TIME, ... Loads ... KBC, ... LSWRITE TIME, ... Loads ... KBC, ... LSWRITE TIME, ... Loads ... KBC, ... LSWRITE Etc.
! Time at the end of 1st transient load step ! Load values at above time ! Stepped or ramped loads ! Write load data to load step file ! Time at the end of 2nd transient load step ! Load values at above time ! Stepped or ramped loads ! Write load data to load step file ! Time at the end of 3rd transient load step ! Load values at above time ! Stepped or ramped loads ! Write load data to load step file
5.4.8. Save a Backup Copy of the Database Save a copy of the database to a named file. You can then retrieve your model by reentering the ANSYS program and issuing RESUME. Command(s): SAVE GUI: Utility Menu> File> Save as
5.4.9. Start the Transient Solution Use one of these methods to start the transient solution: Command(s): LSSOLVE GUI: Main Menu> Solution> Solve> From LS Files For additional ways to create and solve multiple load steps (the array parameter method and the multiple SOLVE method), see Section 3.14: Solving Multiple Load Steps in the ANSYS Basic Analysis Guide. 5–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.4: Performing a Full Transient Dynamic Analysis
5.4.10. Exit the Solution Processor Use one of these methods to exit the solution processor: Command(s): FINISH GUI: Close the Solution menu.
5.4.11. Review the Results You review results for a full transient analysis in the same way that you review results for most structural analyses. See Section 2.3.6: Review the Results in Chapter 2, “Structural Static Analysis”.
5.4.11.1. Postprocessors You can review these results using either POST26, which is the time-history postprocessor, or POST1, which is the general postprocessor. •
POST26 is used to review results at specific points in the model as functions of time.
•
POST1 is used to review results over the entire model at specific time points.
Some typical postprocessing operations for a transient dynamic analysis are explained below. For a complete description of all postprocessing functions, see Section 4.1: What Is Postprocessing? in the ANSYS Basic Analysis Guide.
5.4.11.2. Points to Remember The points to remember for a full transient analysis are the same as those for most structural analyses. See Section 2.3.6.2: Points to Remember in Chapter 2, “Structural Static Analysis”.
5.4.11.3. Using POST26 POST26 works with tables of result item versus time, known as variables. Each variable is assigned a reference number, with variable number 1 reserved for time. 1.
Define the variables. Command(s): NSOL (primary data, that is, nodal displacements) ESOL (derived data, that is, element solution data, such as stresses) RFORCE (reaction force data) FORCE (total force, or static, damping, or inertia component of total force) SOLU (time step size, number of equilibrium iterations, response frequency, and so on) GUI: Main Menu> TimeHist Postpro> Define Variables Note — In the mode superposition or reduced methods, only static force is available with the FORCE command.
2.
Graph or list the variables. By reviewing the time-history results at strategic points throughout the model, you can identify the critical time points for further POST1 postprocessing. Command(s): PLVAR (graph variables) PRVAR, EXTREM (list variables) GUI: Main Menu> TimeHist Postpro> Graph Variables Main Menu> TimeHist Postpro> List Variables Main Menu> TimeHist Postpro> List Extremes
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–11
Chapter 5: Transient Dynamic Analysis
5.4.11.4. Other Capabilities Many other postprocessing functions, such as performing math operations among variables, moving variables into array parameters, and moving array parameters into variables, are available in POST26. See Chapter 6, “The Time-History Postprocessor (POST26)” in the ANSYS Basic Analysis Guide for details.
5.4.11.5. Using POST1 1.
Read in model data from the database file. Command(s): RESUME GUI: Utility Menu> File> Resume from
2.
Read in the desired set of results. Use the SET command to identify the data set by load step and substep numbers or by time. Command(s): SET GUI: Main Menu> General Postproc> Read Results> By Time/Freq
3.
Perform the necessary POST1 operations. The typical POST1 operations that you perform for a transient dynamic analysis are the same as those that you perform for a static analysis. See Section 2.3.6.4: Typical Postprocessing Operations for a list of these operations. Note — If you specify a time for which no results are available, the results that are stored will be a linear interpolation between the two nearest time points.
5.4.12. Sample Input for a Full Transient Dynamic Analysis A sample input listing for a full transient analysis is shown below: ! Build the Model /FILNAM,... /TITLE,... /PREP7 -----! Generate model --FINISH
! Jobname ! Title ! Enter PREP7
! Apply Loads and Obtain the Solution /SOLU ! Enter SOLUTION ANTYPE,TRANS ! Transient analysis TRNOPT,FULL ! Full method D,... ! Constraints F,... ! Loads SF,... ALPHAD,... ! Mass damping BETAD,... ! Stiffness damping KBC,... ! Ramped or stepped loads TIME,... ! Time at end of load step AUTOTS,ON ! Auto time stepping DELTIM,... ! Time step size OUTRES,... ! Results file data options LSWRITE ! Write first load step -----! Loads, time, etc. for 2nd load step --LSWRITE ! Write 2nd load step SAVE LSSOLVE,1,2 ! Initiate multiple load step solution FINISH ! ! Review the Results /POST26 SOLU,... ! Store solution summary data
5–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.5: Performing a Mode Superposition Transient Dynamic Analysis NSOL,... ESOL,,,, RFORCE,... PLVAR,... PRVAR,... FINISH
! ! ! ! !
/POST1 SET,... ! PLDISP,... ! PRRSOL,... ! PLNSOL,... ! PRERR ! -----! Other postprocessing as --FINISH
Store nodal result as a variable Store element result as a variable Store reaction as a variable Plot variables List variables
Read desired set of results into database Deformed shape Reaction loads Contour plot of nodal results Global percent error (a measure of mesh adequacy) desired
See the ANSYS Commands Reference for discussions of the ANTYPE, TRNOPT, ALPHAD, BETAD, KBC, TIME, AUTOTS, DELTIM, OUTRES, LSWRITE, LSSOLVE, SOLU, NSOL, ESOL, RFORCE, PLVAR, PRVAR, PLDISP, PRRSOL, PLNSOL, and PRERR commands.
5.5. Performing a Mode Superposition Transient Dynamic Analysis The mode superposition method sums factored mode shapes (obtained from a modal analysis) to calculate the dynamic response. This method is available in the ANSYS Multiphysics, ANSYS Mechanical, ANSYS Structural, and ANSYS Professional products. The procedure to use the method consists of five main steps: 1.
Build the model.
2.
Obtain the modal solution.
3.
Obtain the mode superposition transient solution.
4.
Expand the mode superposition solution.
5.
Review the results.
5.5.1. Build the Model Building the model for a mode superposition transient dynamic analysis is the same as that described for the full method. See Section 5.4.1: Build the Model for more information.
5.5.2. Obtain the Modal Solution Chapter 3, “Modal Analysis” describes how to obtain a modal solution. Following are some additional hints: •
The mode-extraction method should be Block Lanczos (default), reduced, subspace, PowerDynamics, or QR damped. (The other methods, unsymmetric and damped, do not apply to mode superposition.) PowerDynamics does not create a load vector.
•
Be sure to extract all modes that may contribute to the dynamic response.
•
If PowerDynamics was used for the modal solution, no nonzero loads or displacements are allowed (that is, only u = 0 is valid as the initial condition). PowerDynamics does not create a load vector; therefore, the LVSCALE command is not valid unless the scale factor is set to zero.
•
For the reduced mode-extraction method, include those master degrees of freedom at those nodes at which forces and gap conditions are to be defined.
•
If you use the QR damped mode-extraction method, you must specify any damping (ALPHAD, BETAD, MP,DAMP, or element damping including gyroscopic) that you want to include during preprocessing or Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–13
Chapter 5: Transient Dynamic Analysis in the modal analysis. (ANSYS ignores damping specified during the mode superposition harmonic analysis.) You can set a constant damping ratio (DMPRAT) or define the damping ratio as a function of mode (MDAMP) in a modal superposition harmonic analysis. Note that constant material damping coefficient (MP,DMPR) is not applicable in transient analysis. •
Specify displacement constraints, if any. These constraints will be ignored if they are specified in the mode superposition transient solution instead of in the modal solution.
•
If you need to apply element loads (pressures, temperatures, accelerations, and so on) in the transient dynamic analysis, you must specify them in the modal analysis. The loads are ignored for the modal solution, but a load vector will be calculated and written to the mode shape file (Jobname.MODE). You can then use this load vector for the transient solution.
•
The modes need not be expanded for the mode superposition solution. (If you want to review mode shapes from a reduced modal solution, however, you must expand the mode shapes.)
•
The model data (for example, nodal rotations) should not be changed between the modal and transient analyses.
5.5.3. Obtain the Mode Superposition Transient Solution In this step, the program uses mode shapes extracted by the modal solution to calculate the transient response.
5.5.3.1. Points to Remember •
The mode shape file (Jobname.MODE) must be available.
•
The database must contain the same model for which the modal solution was obtained.
5.5.3.2. Obtaining the Solution The procedure to obtain the mode superposition transient solution is described below: 1.
Enter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define the analysis type and analysis options. These are the same as the analysis options that are described for the full method (in Section 5.4.3: Set Solution Controls and Section 5.4.4: Set Additional Solution Options), except for the following differences:
5–14
•
You cannot use the Solution Controls dialog box to define analysis type and analysis options for a mode superposition transient analysis. Instead, you must set them using the standard set of ANSYS solution commands (which are listed in Section 5.4.3: Set Solution Controls and Section 5.4.4: Set Additional Solution Options) and the standard corresponding menu paths.
•
Restarts are not available (ANTYPE).
•
Choose the mode superposition method of solution (TRNOPT).
•
When you specify a mode superposition transient analysis, a Solution menu that is appropriate for that specific type of analysis appears. The Solution menu will be either “abridged” or “unabridged,” depending on the actions you took prior to this step in your ANSYS session. The abridged menu contains only those solution options that are valid and/or recommended for mode superposition transient analyses. If you are on the abridged Solution menu and you want to access other solution options (that is, solution options that are valid for you to use, but their use may not be encouraged for this type of analysis), select the Unabridged Menu option from the Solution menu. For details, see Section 3.11.1: Using Abridged Solution Menus in the ANSYS Basic Analysis Guide. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.5: Performing a Mode Superposition Transient Dynamic Analysis •
Specify the number of modes you want to use for the solution (TRNOPT). This determines the accuracy of the transient solution. At a minimum, you should use all modes that you think will contribute to the dynamic response. If you expect higher frequencies to be excited, for example, the number of modes specified should include the higher modes. The default is to use all modes calculated in the modal solution.
•
If you do not want to use rigid body (0 frequency) modes, use MINMODE on the TRNOPT command to skip over them.
•
Nonlinear options (NLGEOM, SSTIF, NROPT) are not available.
3.
Define gap conditions, if any. They can only be defined between two master degree of freedom (DOF) nodes or between master DOF nodes and ground. When a non-reduced mode-extraction method is used, a master DOF implies an unconstrained, active DOF. If you used the QR damped mode-extraction method, gap conditions are not supported. More details about gap conditions are presented in Section 5.6.1.3.1: Gap Conditions. Command(s): GP GUI: Main Menu> Solution> Dynamic Gap Cond> Define
4.
Apply loads to the model. The following loading restrictions apply in a mode superposition transient dynamic analysis: •
Only forces, accelerations, and a load vector created in the modal analysis are valid. Imposed nonzero displacements are ignored. Use the LVSCALE command (Main Menu> Solution> Define Loads> Apply> Load Vector> For Mode Super) to apply the load vector from the modal solution.
•
If mode shapes from a reduced modal solution are being used, forces may be applied only at master DOF.
Multiple load steps are usually required to specify the load history in a transient analysis. The first load step is used to establish initial conditions, and second and subsequent load steps are used for the transient loading, as explained next. 5.
Establish initial conditions. In modal superposition transient analyses, a first solution is done at TIME = 0. This establishes the initial condition and time step size for the entire transient analysis. Generally, the only load applicable for the first load step is initializing nodal forces. For this pseudo-static analysis, the mode superposition method may yield poor results at TIME = 0 if nonzero loads are applied. The following load step options are available for the first load step:
Table 5.2 Options for the First Load Step-Mode Superposition Analysis Option
Command
GUI Path
Dynamics Options Transient Integration Paramet- TINTP ers
Main Menu> Solution> Load Step Opts> Time/Frequenc> Time Integration
Load Vector
LVSCALE
Main Menu> Solution> Define Loads> Apply> Load Vector> For Mode Super
Damping
ALPHAD, BETAD, DMPRAT, MP, MDAMP
Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping Main Menu> Solution> Load Step Opts> Other> Change Mat Props> Material Models> Structural> Damping
General Options
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–15
Chapter 5: Transient Dynamic Analysis Option Integration Time Step
Command
GUI Path
DELTIM
Main Menu> Solution> Load Step Opts> Time/Frequenc> Time-Time Step
OUTPR
Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout
Output Control Options Printed Output
•
Dynamics options include the following: – Transient Integration Parameters (TINTP) Transient integration parameters control the nature of the Newmark time integration technique. The default is to use the constant average acceleration scheme; see your ANSYS, Inc. Theory Reference for further details. –
Load Vector (LVSCALE) The load vector option allows you to apply a load vector created by the modal solution as one of the loads. You can use such a load vector to apply element loads (pressures, temperatures, and so on) on the model.
–
Damping Damping in some form is present in most structures and should be included in your analysis. You can specify five forms of damping in a mode superposition transient dynamic analysis: → Alpha (mass) damping (ALPHAD) → Beta (stiffness) damping (BETAD) → Constant damping ratio (DMPRAT) → Material-dependent beta damping (MP,DAMP) → Modal damping (MDAMP) Remember that, as described earlier in Section 5.5.2: Obtain the Modal Solution, any damping that you specify in the mode superposition transient analysis is ignored if you used the QR damped mode-extraction method. Constant material damping coefficient (MP,DMPR) is not applicable in transient analysis. See Section 5.10.3: Damping for further details.
•
The only valid general option for the first load step is integration time step (DELTIM), which is assumed to be constant throughout the transient. By default, the integration time step is assumed to be 1/(20f), where f is the highest frequency chosen for the solution. The DELTIM command is valid only in the first load step and is ignored in subsequent load steps. Note — If you do issue the TIME command in the first load step, it will be ignored. The first solution is always a static solution at TIME = 0.
•
6.
5–16
The output control option for the first load step is printed output (OUTPR). Use this option to control printout of the displacement solution at the master DOF.
Write the first load step to a load step file (Jobname.S01) by issuing the LSWRITE command. Command(s): LSWRITE Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.5: Performing a Mode Superposition Transient Dynamic Analysis GUI: Main Menu> Solution> Load Step Opts> Write LS File 7.
Specify loads and load step options for the transient loading portion, writing each load step to a load step file (LSWRITE). •
General options include the following: –
Time Option (TIME) This option specifies time at the end of the load step.
–
Load Vector (LVSCALE) The load vector option allows you to apply a load vector created by the modal solution as one of the loads.
–
Stepped or Ramped Loads (KBC) This option indicates whether to ramp the load change over the load step (KBC) or to step-apply the load change (KBC,1). The default is ramped.
•
Output control options include the following: –
Printed Output (OUTPR) Use this option to control printed output.
–
Database and Results File Output (OUTRES) This option controls the data on the reduced displacement file.
The only valid label on these commands is NSOL (nodal solution). The default for OUTRES is to write the solution for every fourth time-point to the reduced displacement file (unless there are gap conditions defined, in which case the default is to write every solution). 8.
If you used either the Block Lanczos (default) or subspace option for the modal analysis (MODOPT,LANB or MODOPT,SUBSP), you may use a nodal component with the OUTRES,NSOL command to limit the displacement data written to the reduced displacement file Jobname.RDSP. The expansion pass will only produce valid results for those nodes and for those elements in which all of the nodes of the elements have been written to the .RDSP file. To use this option, first suppress all writing by invoking OUTRES,NSOL,NONE, then specify the item(s) of interest by invoking OUTRES,NSOL,FREQ,COMP. Repeat the OUTRES command for any additional nodal components that you want to write to the .RDSP file. Only one output frequency is allowed - ANSYS uses the last frequency specified by OUTRES.
9.
Save a backup copy of the database to a named file. Command(s): SAVE GUI: Utility Menu> File> Save as
10. Start the transient solution. Command(s): LSSOLVE GUI: Main Menu> Solution> Solve> From LS Files 11. Leave SOLUTION. Command(s): FINISH GUI: Close the Solution menu.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–17
Chapter 5: Transient Dynamic Analysis The mode superposition transient solution is written to the reduced displacement file, Jobname.RDSP, regardless of whether the subspace, Block Lanczos, reduced, PowerDynamics, or QR damped method was used for the modal solution. You will therefore need to expand the solution if you are interested in stress results.
5.5.4. Expand the Mode Superposition Solution The procedure for the expansion pass is the same as described for the reduced method (see Section 5.6.3: Expand the Solution (Expansion Pass)). Jobname.TRI is needed only if the reduced method was used for the modal solution. The output from the expansion pass includes the structural results file, Jobname.RST, containing expanded results.
5.5.5. Review the Results Results consist of displacements, stresses, and reaction forces at each time-point for which the solution was expanded. You can review these results using POST26 or POST1, as explained for the full method (see Section 5.4.11: Review the Results). Note — In the mode superposition or reduced methods, only static force is available with the FORCE command.
5.5.6. Sample Input for a Mode Superposition Transient Dynamic Analysis A sample input listing for a mode superposition transient analysis is shown below: ! Build the Model /FILNAM,... /TITLE,... /PREP7 -----! Generate model --FINISH
! Jobname ! Title ! Enter PREP7
! Obtain the Modal Solution /SOLU ! Enter SOLUTION ANTYPE,MODAL ! Modal analysis MODOPT,REDU ! Reduced method M,... ! Master DOF TOTAL,... D,... ! Constraints SF,... ! Element loads ACEL,... SAVE SOLVE FINISH ! Obtain the Mode Superposition Transient Solution /SOLU ! Reenter SOLUTION ANTYPE,TRANS ! Transient analysis TRNOPT,MSUP,... ! Mode superposition method LVSCALE,... ! Scale factor for element loads F,... ! Nodal Loads MDAMP,... ! Modal damping ratios DELTIM,... ! Integration time step sizes LSWRITE ! Write first load step (Remember: the first load step --! is solved statically at time=0.) -----! Loads, etc. for 2nd load step TIME,... ! Time at end of second load step KBC,... ! Ramped or stepped loads OUTRES,... ! Results-file data controls --LSWRITE ! Write 2nd load step (first transient load step) SAVE
5–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.6: Performing a Reduced Transient Dynamic Analysis LSSOLVE FINISH
! Initiate multiple load step solution
! Review results of the mode superposition solution /POST26 ! Enter POST26 FILE,,RDSP ! Results file is Jobname.RDSP SOLU,... ! Store solution summary data NSOL,... ! Store nodal result as a variable PLVAR,... ! Plot variables PRVAR,... ! List variables FINISH ! Expand the Solution /SOLU ! Reenter SOLUTION EXPASS,ON ! Expansion pass NUMEXP,... ! No. of solutions to expand; time range OUTRES,... ! Results-file data controls SOLVE FINISH ! Review the Results of the Expanded Solution /POST1 SET,... ! Read desired set of results into database PLDISP,... ! Deformed shape PRRSOL,... ! Reaction loads PLNSOL,... ! Contour plot of nodal results PRERR ! Global percent error (a measure of mesh adequacy) -----! Other postprocessing as desired --FINISH
See the ANSYS Commands Reference for discussions of the ANTYPE, MODOPT, M, TOTAL, ACEL, TRNOPT, LVSCALE, MDAMP, DELTIM, TIME, KBC, OUTRES, LSSOLVE, FILE, SOLU, NSOL, PLVAR, PRVAR, EXPASS, NUMEXP, OUTRES, PLDISP, PRRSOL, PLNSOL, and PRERR commands.
5.6. Performing a Reduced Transient Dynamic Analysis The reduced method, as its name implies, uses reduced matrices to calculate the dynamic response. It is available in the ANSYS Multiphysics, ANSYS Mechanical, and ANSYS Structural products. You should consider using this method if you do not want to include nonlinearities (other than simple node-to-node contact) in the analysis. The procedure for a reduced transient dynamic analysis consists of these main steps: 1.
Build the model.
2.
Obtain the reduced solution.
3.
Review the results of the reduced solution.
4.
Expand the solution (expansion pass).
5.
Review the results of the expanded solution.
Of these, the first step is the same as for the full method, except that no nonlinearities are allowed (other than simple node-to-node contact, which is specified in the form of a gap condition instead of an element type). Details of the other steps are explained below.
5.6.1. Obtain the Reduced Solution By reduced solution, we mean the degree of freedom solution calculated at the master DOF. The tasks required to obtain the reduced solution are explained in the following sections. For the following tasks, you need to first enter the SOLUTION processor. Command(s): /SOLU Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–19
Chapter 5: Transient Dynamic Analysis GUI: Main Menu> Solution
5.6.1.1. Define the Analysis Type and Options These are the same as the analysis options that are described for the full method (in Section 5.4.3: Set Solution Controls and Section 5.4.4: Set Additional Solution Options) except for the following differences: •
You cannot use the Solution Controls dialog box to define analysis type and analysis options for a reduced transient dynamic analysis. Instead, you must set them using the standard set of ANSYS solution commands (which are listed in Section 5.4.3: Set Solution Controls and Section 5.4.4: Set Additional Solution Options) and the standard corresponding menu paths.
•
Restarts are not available (ANTYPE).
•
Choose the reduced method of solution (TRNOPT).
•
When you specify a reduced transient analysis, a Solution menu that is appropriate for that specific type of analysis appears. The Solution menu will be either “abridged” or “unabridged,” depending on the actions you took prior to this step in your ANSYS session. The abridged menu contains only those solution options that are valid and/or recommended for reduced transient analyses. If you are on the abridged Solution menu and you want to access other solution options (that is, solution options that are valid for you to use, but their use may not be encouraged for this type of analysis), select the Unabridged Menu option from the Solution menu. For details, see Section 3.11.1: Using Abridged Solution Menus in the ANSYS Basic Analysis Guide.
•
Nonlinear options (NLGEOM, SSTIF, NROPT) are not available.
5.6.1.2. Define Master Degrees of Freedom Master DOF are essential degrees of freedom that characterize the dynamic behavior of the structure. For a reduced transient dynamic analysis, master DOF are also required at locations where you want to define gap conditions, forces, or nonzero displacements. You can list the defined master DOF or delete master DOF as well. See Section 3.14: Matrix Reduction for guidelines to choose master DOF. Command(s): M, MGEN, TOTAL, MLIST, MDELE GUI: Main Menu> Solution> Master DOFs> User Selected> Define Main Menu> Solution> Master DOFs> User Selected> Copy Main Menu> Solution> Master DOFs> Program Selected Main Menu> Solution> Master DOFs> User Selected> List All Main Menu> Solution> Master DOFs> User Selected> Delete
5.6.1.3. Define Gap Conditions Define any gap conditions. Command(s): GP GUI: Main Menu> Solution> Dynamic Gap Cond> Define You can also list the defined gaps and delete gaps. Command(s): GPLIST, GPDELE GUI: Main Menu> Solution> Dynamic Gap Cond> List All Main Menu> Solution> Dynamic Gap Cond> Delete
5.6.1.3.1. Gap Conditions Gap conditions can only be defined between two master degree of freedom (DOF) nodes or between master DOF nodes and ground, as shown in the following figure. 5–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.6: Performing a Reduced Transient Dynamic Analysis
Figure 5.2 Examples of Gap Conditions
Gap conditions are similar to gap elements and are specified between surfaces that are expected to contact (impact) each other during the transient. The ANSYS program accounts for the gap force, which develops when the gap closes, by using an equivalent nodal load vector. Some guidelines to define gap conditions are presented below: •
Use enough gap conditions to obtain a smooth contact stress distribution between the contacting surfaces.
•
Define a reasonable gap stiffness. If the stiffness is too low, the contacting surfaces may overlap too much. If the stiffness is too high, a very small time step will be required during impact. A general recommendation is to specify a gap stiffness that is one or two orders of magnitude higher than the adjacent element stiffness. You can estimate the adjacent element stiffness using AE/L, where A is the contributing area around the gap condition, E is the elastic modulus of the softer material at the interface, and L is the depth of the first layer of elements at the interface.
•
The nonlinear gap damping provided through the DAMP field of the GP command runs faster than a full transient analysis using a gap element COMBIN40. Only TRNOPT = MSUP allows the nonlinear gap damping action. Damping conditions are ignored for the reduced transient analysis method.
5.6.1.4. Apply Initial Conditions to the Model The following loading restrictions apply in a reduced transient dynamic analysis: •
Only displacements, forces, and translational accelerations (such as gravity) are valid. Acceleration loading is not allowed if the model contains any master DOF at any nodes with rotated nodal coordinate systems.
•
Forces and nonzero displacements must be applied only at master DOF.
As mentioned for the full method, multiple load steps are usually required to specify the load history in a transient analysis. The first load step is used to establish initial conditions, and second and subsequent load steps are used for the transient loading, as explained next. •
Establish initial conditions. The only initial condition that may be explicitly established is the initial dis-
u&
&& u
placement (uo); that is, initial velocity and acceleration must be zero ( o = 0, o = 0). Displacements cannot be deleted in subsequent load steps, therefore they cannot be used to specify an initial velocity. In a reduced transient analysis, a static solution is always performed as the first solution, using the loads given, to determine uo. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–21
Chapter 5: Transient Dynamic Analysis •
Specify load step options for the first load step. Valid options appear in Table 5.3: “Options for the First Load Step-Reduced Analysis”.
Table 5.3 Options for the First Load Step-Reduced Analysis Option
Command
GUI Path
Dynamics Options Transient Integration Parameters
TINTP
Main Menu> Solution> Load Step Opts> Time/Frequenc> Time Integration
Damping
ALPHAD, BETAD, MP,DAMP
Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping Main Menu> Solution> Load Step Opts> Other> Change Mat Props> Material Models> Structural> Damping
DELTIM
Main Menu> Solution> Load Step Opts> Time/Frequenc> Time- Time Step
OUTPR
Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout
General Options Integration Time Step Output Control Options Printed Output
5.6.1.4.1. Dynamics Options Dynamic options include the following: •
Transient Integration Parameters (TINTP) Transient integration parameters control the nature of the Newmark time integration technique. The default is to use the constant average acceleration scheme; see the ANSYS, Inc. Theory Reference for further details.
•
Damping Damping in some form is present in most structures and should be included in your analysis. You can specify four forms of damping in a reduced transient dynamic analysis: –
Alpha (mass) damping (ALPHAD)
–
Beta (stiffness) damping (BETAD)
–
Material-dependent beta damping (MP,DAMP)
–
Element damping (COMBIN7, and so on)
See Section 5.10.3: Damping for further details.
5.6.1.4.2. General Options The only valid general option is Integration Time Step (DELTIM). The integration time step is assumed to be constant throughout the transient. Note — If you do issue the TIME command for the first load step, it will be ignored. The first solution is always a static solution at TIME = 0.
5–22
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.6: Performing a Reduced Transient Dynamic Analysis
5.6.1.4.3. Output Control Options Use the Printed Output (OUTPR) option to output the displacement solution at the master DOF.
5.6.1.5. Write the First Load Step to a Load Step File Write the first load step to a load step file (Jobname.S01). Command(s): LSWRITE GUI: Main Menu> Solution> Load Step Opts> Write LS File
5.6.1.6. Specify Loads and Load Step Options Specify loads and load step options for the transient loading portion, writing each load step to a load step file (LSWRITE). The following load step options are valid for the transient load steps: •
•
General Options –
Time (specifies the time at the end of the load step) (TIME)
–
Stepped (KBC,1) or ramped loads (KBC)
Output Controls – Printed output (OUTPR) – Reduced displacement file (OUTRES) The only valid label on these commands is NSOL (nodal solution). The default for OUTRES is to write the solution for every fourth time-point to the reduced displacement file (unless there are gap conditions defined, in which case the default is to write every solution).
5.6.1.7. Obtaining the Solution Solving a reduced transient dynamic analysis involves the same steps as those involved in solving a full transient analysis. See the following sections for a description of those steps: •
Section 5.4.8: Save a Backup Copy of the Database
•
Section 5.4.9: Start the Transient Solution
•
Section 5.4.10: Exit the Solution Processor
5.6.2. Review the Results of the Reduced Solution Results from the reduced transient dynamic solution are written to the reduced displacement file, Jobname.RDSP. They consist of time-varying displacements at the master DOF. You can review the master DOF displacements as a function of time using POST26. (POST1 cannot be used, because the complete solution at all DOF is not available.) The procedure to use POST26 is the same as described for the full method, except for the following differences: •
Before defining the POST26 variables, use the FILE command (Main Menu> TimeHist Postpro> Settings> File) to specify that data are to be read from Jobname.RDSP. For example, if the jobname is TRANS, the
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–23
Chapter 5: Transient Dynamic Analysis FILE command would be: FILE,TRANS,RDSP. (By default, POST26 looks for a results file, which is not written by a reduced transient solution.) •
Only nodal degree of freedom data (at master DOF) are available for processing, so you can use only the NSOL command to define variables.
5.6.3. Expand the Solution (Expansion Pass) The expansion pass starts with the reduced solution and calculates the complete displacement, stress, and force solution at all degrees of freedom. These calculations are done only at time points that you specify. Before you begin the expansion pass, therefore, you should review the results of the reduced solution (using POST26) and identify the critical time points. Note — An expansion pass is not always required. For instance, if you are interested mainly in displacements at specific points on the structure, then the reduced solution could satisfy your requirements. However, if you want to determine displacements at non-master DOF, or if you are interested in the stress or force solution, then you must perform an expansion pass.
5.6.3.1. Points to Remember •
The .RDSP, .EMAT, .ESAV, .DB, and .TRI files from the reduced solution must be available.
•
The database must contain the same model for which the reduced solution was calculated.
The procedure for the expansion pass is explained below.
5.6.3.2. Expanding the Solution 1.
Reenter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution Note — You must explicitly leave SOLUTION (using the FINISH command) and reenter (/SOLU) before performing the expansion pass.
2.
Activate the expansion pass and its options.
Table 5.4 Expansion Pass Options Option Expansion Pass On/Off
Command EXPASS
GUI Path Main Menu> Solution> Analysis Type> ExpansionPass
No. of Solutions to be Expan- NUMEXP ded
Main Menu> Solution> Load Step Opts> ExpansionPass> Range of Solu's
Single Solution to Expand
Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> By Time/Freq
•
EXPSOL
Option: Expansion Pass On/Off (EXPASS) Choose ON.
•
5–24
Option: Number of Solutions to be Expanded (NUMEXP)
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.6: Performing a Reduced Transient Dynamic Analysis Specify the number. This number of evenly spaced solutions will be expanded over the specified time range. The solutions nearest these times will be expanded. Also specify whether to calculate stresses and forces (default is to calculate both). •
Option: Single Solution to Expand (EXPSOL) Use this option to identify a single solution for expansion if you do not need to expand multiple solutions in a range. You can specify it either by load step and substep number or by time. Also specify whether to calculate stresses and forces (default is to calculate both).
3.
Specify load step options. The only options valid for a transient dynamic expansion pass are output controls: •
Output Controls –
Printed Output (OUTPR) Use this option to include any results data on the output file (Jobname.OUT).
–
Database and Results File Output (OUTRES) This option controls the data on the results file (Jobname.RST).
–
Extrapolation of Results (ERESX) Use this option to review element integration point results by copying them to the nodes instead of extrapolating them (default). Note — The FREQ field on OUTPR and OUTRES can only be ALL or NONE. ERESX allows you to review element integration point results by copying them to the nodes instead of extrapolating them (default).
4.
Start expansion pass calculations. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
5.
Repeat steps 2, 3, and 4 for additional solutions to be expanded. Each expansion pass is stored as a separate load step on the results file.
6.
Leave SOLUTION. Command(s): FINISH GUI: Close the Solution window.
5.6.4. Review the Results of the Expanded Solution You review results for an expansion pass in the same way that you review results for most structural analyses. See Section 2.3.6: Review the Results in Chapter 2, “Structural Static Analysis”. You can review these results using POST1. (If you expanded solutions at several time points, you can also use POST26 to obtain graphs of stress versus time, strain versus time, and so on.) The procedure to use POST1 (or POST26) is the same as described for the full method.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–25
Chapter 5: Transient Dynamic Analysis
5.7. Sample Reduced Transient Dynamic Analysis (GUI Method) In this example, you will perform a transient dynamic analysis using the reduced method to determine the transient response to a constant force with a finite rise in time. In this problem, a steel beam supporting a concentrated mass is subjected to a dynamic load.
5.7.1. Problem Description A steel beam of length l and geometric properties shown in Problem Specifications is supporting a concentrated mass, m. The beam is subjected to a dynamic load F(t) with a rise time tr and a maximum value F1. If the weight of the beam is considered to be negligible, determine the time of maximum displacement response tmax and the response ymax. Also determine the maximum bending stress σbend in the beam. The beam is not used in this solution and its area is arbitrarily input as unity. The final time of 0.1 sec allows the mass to reach its largest deflection. One master degree of freedom is selected at the mass in the lateral direction. A static solution is done at the first load step. Symmetry could have been used in this model. The time of maximum response (0.092 sec) is selected for the expansion pass calculation.
5.7.2. Problem Specifications The following material properties are used for this problem: E = 30 x 103 ksi m = 0.0259067 kips-sec2/in The following geometric properties are used for this problem: l = 800.6 in4 h = 18 in l = 20 ft = 240 in. Loading for this problem is: F1 = 20 kips tr = 0.075 sec
5–26
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.7: Sample Reduced Transient Dynamic Analysis (GUI Method)
5.7.3. Problem Sketch Figure 5.3 Model of a Steel Beam Supporting a Concentrated Mass
5.7.3.1. Specify the Title 1.
Choose menu path Utility Menu> File> Change Title.
2.
Enter the text "Transient response to a constant force with a finite rise time."
3.
Click on OK.
5.7.3.2. Define Element Types 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete. The Element Types dialog box appears.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
In the left scroll box, click on "Structural Beam."
4.
In the right scroll box, click on "2D elastic 3," and click on Apply.
5.
In the left scroll box, click on "Structural Mass."
6.
In the right scroll box, click on "3D mass 21," and click on OK.
7.
In the Element Types dialog box, click once on "Type 2," and click on Options.
8.
In the scroll box for Rotary inertia options, scroll to "2D w/o rot iner" and select it.
9.
Click on OK and click on Close in the Element Types dialog box.
5.7.3.3. Define Real Constants 1.
Choose menu path Main Menu> Preprocessor> Real Constants> Add/Edit/Delete. The Real Constants dialog box appears.
2.
Click on Add. The Element Type for Real Constants dialog box appears.
3.
Click on Type1 BEAM3 then Click on OK. The Real Constants for BEAM3 dialog box appears.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–27
Chapter 5: Transient Dynamic Analysis 4.
Enter 1 for Area, 800.6 for IZZ, and 18 for Height.
5.
Click on OK.
6.
In the Real Constants dialog box, click on Add.
7.
Click on Type 2 MASS21 and click on OK. The Real Constant Set Number 2, for MASS21 dialog box appears.
8.
Enter .0259067 in the 2-D mass field and click on OK.
9.
Click on Close in the Real Constants dialog box.
5.7.3.4. Define Material Properties 1.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
2.
In the Material Models Available window, double-click on the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
3.
Enter 30e3 for EX (Young's modulus), enter 0.3 for PRXY, and click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
4.
Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
5.7.3.5. Define Nodes 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Nodes> In Active CS. The Create Nodes in Active Coordinate System dialog box appears.
2.
Enter 1 for node number and click on Apply to define node 1 at 0,0,0.
3.
Enter 3 for node number.
4.
Enter 240,0,0 for X, Y, Z coordinates and click on OK.
5.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Nodes> Fill between Nds. The Fill between Nds picking menu appears.
6.
Click once on nodes 1 and 3 in the ANSYS Graphics window, and click on OK in the picking menu. The Create Nodes Between 2 Nodes dialog box appears.
7.
Click on OK to accept the default settings.
5.7.3.6. Define Elements 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Thru Nodes. The Elements from Nodes picking menu appears.
2.
Click once on nodes 1 and 2, and click on Apply.
3.
Click once on nodes 2 and 3, and click on OK.
4.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes. The Element Attributes dialog box appears.
5.
In the Element type number drop down menu, select “2 MASS21.”
6.
In the Real constant set number drop down menu, select 2 and click OK.
7.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Thru Nodes. The Elements from Nodes picking menu appears.
8.
Click once on node 2 and click OK.
5–28
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.7: Sample Reduced Transient Dynamic Analysis (GUI Method) 9.
Click on SAVE_DB on the ANSYS Toolbar.
5.7.3.7. Define Analysis Type and Analysis Options 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis.
2.
Click on "Transient" to select it, and click on OK. The Transient Analysis dialog box appears.
3.
Click on "Reduced" and click on OK.
4.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Reduced Transient Analysis dialog box appears.
5.
In the drop down menu for Damping effects, select "Ignore."
6.
Click on OK.
5.7.3.8. Define Master Degrees of Freedom 1.
Choose menu path Main Menu> Solution> Master DOFs> User Selected> Define. The Define Master DOFs picking menu appears.
2.
Click on node 2 and click on OK. The Define Master DOFs dialog box appears.
3.
In the drop down menu for 1st degree of freedom, select "UY."
4.
Click on OK.
5.7.3.9. Set Load Step Options 1.
Choose the menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Time-Time Step. The Time and Time Step Options dialog box appears.
2.
Enter .004 for Time step size and click on OK.
5.7.3.10. Apply Loads for the First Load Step 1.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears.
2.
Click on node 1 and click on Apply. The Apply U,ROT on Nodes dialog box appears.
3.
Click on "UY" to select it and click on Apply. The Apply U,ROT on Nodes picking menu appears.
4.
Click on node 3, and click on OK. The Apply U,ROT on Nodes dialog box appears.
5.
Click on "UX" to select it. "UY" should remain selected. Click on OK.
6.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment> On Nodes. The Apply F/M on Nodes picking menu appears.
7.
Click on node 2 and click on OK. The Apply F/M on Nodes dialog box appears.
8.
In the drop down menu for Direction of force/mom, select "FY." Leave the value as blank (zero) for the initial static solution.
9.
Click on OK, and click on SAVE_DB on the ANSYS Toolbar.
5.7.3.11. Specify Output 1.
Choose menu path Main Menu> Solution> Load Step Opts> Output Ctrls> DB/Results File. The Controls for Database and Results File Writing dialog box appears.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–29
Chapter 5: Transient Dynamic Analysis 2.
Click on the "Every substep" radio button and click on OK.
5.7.3.12. Solve the First Load Step 1.
Choose menu path Main Menu> Solution> Solve> Current LS.
2.
Review the information in the status window, and click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to begin the solution.
4.
Click on Close when the Solution is done! window appears.
5.7.3.13. Apply Loads for the Next Load Step 1.
Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc>Time-Time Step. The Time and Time Step Options dialog box appears.
2.
Enter .075 for Time at end of load step and click on OK.
3.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment> On Nodes. The Apply F/M on Nodes picking menu appears.
4.
Click on node 2 and click on OK. The Apply F/M on Nodes dialog box appears.
5.
Enter 20 for Force/moment value and click on OK.
5.7.4. Solve the Next Load Step 1.
Choose menu path Main Menu> Solution> Solve> Current LS.
2.
Review the information in the status window, and click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to begin the solution.
4.
Click on Close when the Solution is done! window appears
5.7.4.1. Set the Next Time Step and Solve 1.
Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Time-Time Step. The Time and Time Step Options dialog box appears.
2.
Enter .1 for Time at end of load step and click on OK.
3.
Choose menu path Main Menu> Solution> Solve> Current LS.
4.
Review the information in the status window, and click on Close.
5.
Click on OK on the Solve Current Load Step dialog box to begin the solution.
6.
Click on Close when the Solution is done! window appears.
7.
Choose menu path Main Menu> Finish.
5.7.4.2. Run the Expansion Pass and Solve 1.
Choose menu path Main Menu> Solution> Analysis Type> ExpansionPass. Set the Expansion pass radio button to On and click on OK.
2.
Choose menu path Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> By Time/Freq. The Expand Single Solution by Time/Frequency dialog box appears.
3.
Enter 0.092 for Time-point/Frequency and click on OK.
4.
Choose menu path Main Menu >Solution> Solve> Current LS.
5–30
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.8: Sample Reduced Transient Dynamic Analysis (Command or Batch Method) 5.
Review the information in the status window, and click on Close.
6.
Click on OK on the Solve Current Load Step dialog box to begin the solution.
7.
Click on Close when the Solution is done! window appears.
5.7.4.3. Review the Results in POST26 1.
Choose menu path Main Menu> TimeHist Postpro> Settings> File. The File Settings dialog box appears.
2.
Click browse and select "file.rdsp" and click on open then OK.
3.
Choose menu path Main Menu> TimeHist Postpro> Define Variables. The Defined Time-History Variables dialog box appears.
4.
Click on Add. The Add Time-History Variable dialog box appears.
5.
Click on OK to accept the default of Nodal DOF result. The Define Nodal Data picking menu appears. Pick node 2 and click OK.
6.
Accept the default of 2 for the reference number of the variable.
7.
Make sure that 2 is entered for node number.
8.
Enter NSOL for user-specified label.
9.
In the right scroll box, click on "Translation UY" to select it.
10. Click on OK, then click on Close in the Defined Time-History Variables dialog box. 11. Choose menu path Main Menu> TimeHist Postpro> Graph Variables. 12. Enter 2 for 1st variable to graph and click on OK. The graph appears in the ANSYS Graphics window. 13. Choose menu path Main Menu> TimeHist Postpro> List Variables. 14. Enter 2 for 1st variable to list and click on OK. 15. Review the information in the status window and click on Close.
5.7.4.4. Review the Results in POST1 1.
Choose menu path Main Menu> General Postproc> Read Results> First Set.
2.
Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears.
3.
Click on "Def + undeformed" and click on OK.
5.7.4.5. Exit ANSYS 1.
Choose QUIT from the ANSYS Toolbar.
2.
Click on the save option you want, and click on OK.
5.8. Sample Reduced Transient Dynamic Analysis (Command or Batch Method) You can perform the example transient dynamic analysis of a bracket using the ANSYS commands shown below instead of GUI choices. Items prefaced with an exclamation point (!) are comments. /PREP7 /TITLE, Transient Response to a Constant Force with a Finite Rise Time ET,1,BEAM3 ! 2-D beam
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–31
Chapter 5: Transient Dynamic Analysis ET,2,MASS21,,,4 R,1,1,800.6,18 R,2,.0259067 MP,EX,1,30e3 N,1 N,3,240 FILL E,1,2! Beam elements EGEN,2,1,1 TYPE,2 REAL,2 E,2 M,2,UY FINISH /SOLU ANTYPE,TRANS TRNOPT,REDUC,,NODAMP DELTIM,.004 D,1,UY D,3,UX,,,,,UY OUTPR,BASIC,1 OUTRES,ALL,1 F,2,FY,0 SOLVE TIME,.075 F,2,FY,20 SOLVE TIME,.1 SOLVE FINISH
! 2-D mass ! Beam area = 1, I = 800.6, h = 18 ! Mass
! Type 2 element with real constant 2 ! Master DOF in Y direction at middle of beam
! Transient dynamic analysis ! Reduced transient analysis, ignore damping ! Integration time step size
! Force = 0 at Time = 0 ! Time at end of load step ! Force is ramped to 20 ! Constant force until time = 0.1
/SOLU ! The following is the expansion pass using BEAM3 and MASS21 elements EXPASS,ON ! Expansion pass on EXPSOL,,,0.092 ! Time of maximum response SOLVE FINISH /POST26 NUMVAR,0 FILE,file,rdsp NSOL,2,2,U,Y,NSOL PLVAR,2 PRVAR,2 FINISH /POST1 SET,FIRST PLDISP,1 FINISH
! Define the variables ! Graph the variables ! List the variables
! Read in results ! Display deformed and undeformed shape
5.9. Performing a Prestressed Transient Dynamic Analysis A prestressed transient dynamic analysis calculates the dynamic response of a prestressed structure, such as a heat-treated part with residual thermal stresses. Prestressed-analysis procedures vary, depending on the type of transient dynamic analysis being performed.
5.9.1. Prestressed Full Transient Dynamic Analysis You can include prestressing effects in a full transient dynamic analysis by applying the prestressing loads in a preliminary static load step. (Do not remove these loads in subsequent load steps.) The procedure consists of two steps: 1.
5–32
Build your model, enter SOLUTION, and define a transient analysis type (ANTYPE,TRANS).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.10: Other Analysis Details •
Apply all prestressing loads.
•
Turn time integration effects off (TIMINT,OFF).
•
Turn stress stiffening effects on (SSTIF,ON).
•
Set time equal to some small dummy value (TIME).
•
Write your first load step to Jobname.S01 (LSWRITE).
If prestressing effects develop because of nonlinear behavior (as in the case of residual thermal stresses in a casting), several load steps might be required to complete the static prestressing phase of your analysis. In the case of geometric nonlinearities (large deformation effects), you can capture the prestressing effect by issuing NLGEOM,ON. 2.
For all subsequent load steps, turn time integration effects on (TIMINT,ON), and proceed using the full transient dynamic analysis procedures described previously. Once all load steps are written to files (LSWRITE), you can initiate the multiple load step solution (LSSOLVE).
Note — The static prestress solution must be done as a separate solution if initial conditions are to be defined with the IC command. (Main Menu> Solution> Define Loads> Apply> Initial Condit'n> Define) The IC command is valid only in the first load step.
5.9.2. Prestressed Mode Superposition Transient Dynamic Analysis In order to include prestress effects in a mode superposition analysis, you must first do a prestressed modal analysis. See Chapter 3, “Modal Analysis” for details. Once prestressed modal analysis results are available, proceed as for any other mode superposition analysis.
5.9.3. Prestressed Reduced Transient Dynamic Analysis The procedure to do a prestressed reduced transient dynamic analysis requires that you first prestress the structure in a separate static analysis, as explained below. It is assumed that the transient (time-varying) stresses (which are superimposed on the prestress) are much smaller than the prestress itself. If they are not, you should use the full transient dynamic analysis. 1.
Build the model and obtain a static solution with prestress effects turned on (PSTRES,ON). The procedure to obtain a static solution is explained in Chapter 2, “Structural Static Analysis”.
2.
Reenter SOLUTION (/SOLU) and obtain the reduced transient solution, also with prestress effects turned on (PSTRES,ON). Files Jobname.DB, Jobname.EMAT, and Jobname.ESAV from the static analysis must be available.
5.10. Other Analysis Details The following sections provide additional details about defining integration time step, automatic time stepping, and damping.
5.10.1. Guidelines for Integration Time Step As mentioned earlier, the accuracy of the transient dynamic solution depends on the integration time step: the smaller the time step, the higher the accuracy. A time step that is too large will introduce error that affects the response of the higher modes (and hence the overall response). A time step that is too small will waste computer resources. To calculate an optimum time step, you should consider the following guidelines: Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–33
Chapter 5: Transient Dynamic Analysis 1.
Resolve the response frequency. The time step should be small enough to resolve the motion (response) of the structure. Since the dynamic response of a structure can be thought of as a combination of modes, the time step should be able to resolve the highest mode that contributes to the response. For the Newmark time integration scheme, it has been found that using approximately twenty points per cycle of the highest frequency of interest results in a reasonably accurate solution. That is, if f is the frequency (in cycles/time), the integration time step (ITS) is given by ITS = 1/20f Smaller ITS values may be required if acceleration results are needed. The following figure shows the effect of ITS on the period elongation of a single-DOF spring-mass system. Notice that 20 or more points per cycle result in a period elongation of less than 1 percent.
Figure 5.4 Effect of Integration Time Step on Period Elongation
For the HHT time integration method, the same guidelines for time step should be applied. Note that if the same time step and time integration parameters are used, the HHT method will be more accurate compared to the Newmark method. 2.
5–34
Resolve the applied load-versus-time curve(s). The time step should be small enough to “follow” the loading function. The response tends to lag the applied loads, especially for stepped loads, as shown in Figure 5.5: “Transient Input vs. Transient Response”. Stepped loads require a small ITS at the time of the step change so that the step change can be closely followed. ITS values as small as 1/180f may be needed to follow stepped loads.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.10: Other Analysis Details
Figure 5.5 Transient Input vs. Transient Response
3.
Resolve the contact frequency. In problems involving contact (impact), the time step should be small enough to capture the momentum transfer between the two contacting surfaces. Otherwise, an apparent energy loss will occur and the impact will not be perfectly elastic. The integration time step can be determined from the contact frequency (fc) as:
ITS =1/Nfc
fc =(1/ 2π) k /m
where k is the gap stiffness, m is the effective mass acting at the gap, and N is the number of points per cycle. To minimize the energy loss, at least thirty points per cycle of (N = 30) are needed. Larger values of N may be required if acceleration results are needed. For the reduced and mode superposition methods, N must be at least 7 to ensure stability. You can use fewer than thirty points per cycle during impact if the contact period and contact mass are much less than the overall transient time and system mass, because the effect of any energy loss on the total response would be small. 4.
Resolve the wave propagation. If you are interested in wave propagation effects, the time step should be small enough to capture the wave as it travels through the elements. See Section 5.4.1: Build the Model for a discussion of element size.
5.
Resolve the nonlinearities. For most nonlinear problems, a time step that satisfies the preceding guidelines is sufficient to resolve the nonlinearities. There are a few exceptions, however: if the structure tends to stiffen under the loading (for example, large deflection problems that change from bending to membrane load-carrying behavior), the higher frequency modes that are excited will have to be resolved.
After calculating the time step using the appropriate guidelines, use the minimum value for your analysis. By using automatic time stepping, you can let the ANSYS program decide when to increase or decrease the time step during the solution. Automatic time stepping is discussed next. Caution: Avoid using exceedingly small time steps, especially when establishing initial conditions. Exceedingly small numbers can cause numerical difficulties. Based on a problem time scale of unity, for example, time steps smaller than 10-10 could cause numerical difficulties.
5.10.2. Automatic Time Stepping Automatic time stepping, also known as time step optimization, attempts to adjust the integration time step during solution based on the response frequency and on the effects of nonlinearities. The main benefit of this feature is that the total number of substeps can be reduced, resulting in computer resource savings. Also, the Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–35
Chapter 5: Transient Dynamic Analysis number of times that you might have to rerun the analysis (adjusting the time step size, nonlinearities, and so on) is greatly reduced. If nonlinearities are present, automatic time stepping gives the added advantage of incrementing the loads appropriately and retreating to the previous converged solution (bisection) if convergence is not obtained. You can activate automatic time stepping with the AUTOTS command. (For more information on automatic time stepping in the context of nonlinearities, see Chapter 8, “Nonlinear Structural Analysis”.) Although it seems like a good idea to activate automatic time stepping for all analyses, there are some cases where it may not be beneficial (and may even be harmful): •
Problems that have only localized dynamic behavior (for example, turbine blade and hub assemblies), where the low-frequency energy content of part of the system may dominate the high-frequency areas
•
Problems that are constantly excited (for example, seismic loading), where the time step tends to change continually as different frequencies are excited
•
Kinematics (rigid-body motion) problems, where the rigid-body contribution to the response frequency term may dominate
5.10.3. Damping Damping is present in most systems and should be specified in a dynamic analysis. The following forms of damping are available in the ANSYS program: •
Alpha and Beta Damping (Rayleigh Damping)
•
Material-Dependent Damping
•
Constant Material Damping Coefficient
•
Constant Damping Ratio
•
Modal Damping
•
Element Damping
Only the constant damping ratio and modal damping are available in the ANSYS Professional program. You can specify more than one form of damping in a model. The program will formulate the damping matrix (C) as the sum of all the specified forms of damping. The constant material damping coefficient is only applicable in full and modal harmonic analyses. Table 5.5: “Damping for Different Analysis Types” shows the types of damping available for different structural analyses.
Table 5.5 Damping for Different Analysis Types Alpha, Beta Damping ALAnalysis Type PHAD, BETAD Static
Material- Dependent Constant Damping Damping Ratio MP,DAMP DMPRAT
Modal Damping MDAMP
Element Constant MaDamping(3) terial Damping COMBIN7, and Coefficient so on MP,DMPR
N/A
N/A
N/A
N/A
N/A
N/A
No(5)
No(5)
No(5)
No
No
No
Yes
Yes
No
No
Yes
No(7)
Full
Yes
Yes
Yes
No
Yes
Yes
Reduced
Yes
Yes
Yes
No
Yes
No
Modal Undamped Damped Harmonic
5–36
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.10: Other Analysis Details
Alpha, Beta Damping ALAnalysis Type PHAD, BETAD Mode Sup
Material- Dependent Constant Damping Damping Ratio MP,DAMP DMPRAT
Modal Damping MDAMP
Element Constant MaDamping(3) terial Damping COMBIN7, and Coefficient so on MP,DMPR
Yes(6)
Yes(4,6)
Yes
Yes
Yes(6)
Yes(7)
Full
Yes
Yes
No
No
Yes
No
Reduced
Yes
Yes
No
No
Yes
No
Mode Sup
Yes(6)
Yes(4,6)
Yes
Yes
Yes(6)
No
SPRS, MPRS(2)
Yes(1)
Yes
Yes
Yes
No
No
DDAM(2)
Yes(1)
Yes
Yes
Yes
No
No
PSD(2)
Yes
No
Yes
Yes
No
No
Buckling
N/A
N/A
N/A
N/A
N/A
N/A
Substructure
Yes
Yes
No
No
Yes
No
Transient
Spectrum
N/A Not applicable 1.
β damping only, no α damping
2.
Damping is used only for mode combination and not for computation of mode coefficients
3.
Includes superelement damping matrix
4.
If converted to modal damping by expansion of modes
5.
If specified, an effective damping ratio is calculated for subsequent spectrum analyses
6.
If you use the QR damped mode-extraction method (MODOPT,QRDAMP), and you specify any kind of damping during preprocessing or in the modal analysis, ANSYS ignores damping specified during the mode superposition analysis
7.
Only the QR damped method supports the constant material damping coefficient application in a downstream mode superposition harmonic analysis
Alpha damping and Beta damping are used to define Rayleigh damping constants α and β. The damping matrix (C) is calculated by using these constants to multiply the mass matrix (M) and stiffness matrix (K): (C) = α(M) + β(K) The ALPHAD and BETAD commands are used to specify α and β, respectively, as decimal numbers. The values of α and β are not generally known directly, but are calculated from modal damping ratios, ξi. ξi is the ratio of actual damping to critical damping for a particular mode of vibration, i. If ωi is the natural circular frequency of mode i, α and β satisfy the relation ξi = α/2ωi + βωi/2 In many practical structural problems, alpha damping (or mass damping) may be ignored (α = 0). In such cases, you can evaluate β from known values of ξi and ωi, as β = 2 ξi/ωi Only one value of β can be input in a load step, so choose the most dominant frequency active in that load step to calculate β. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–37
Chapter 5: Transient Dynamic Analysis To specify both α and β for a given damping ratio ξ, it is commonly assumed that the sum of the α and β terms is nearly constant over a range of frequencies (see Figure 5.6: “Rayleigh Damping”). Therefore, given ξ and a frequency range ωi to ωj, two simultaneous equations can be solved for α and β.
Figure 5.6 Rayleigh Damping
Alpha damping can lead to undesirable results if an artificially large mass has been introduced into the model. One common example is when an artificially large mass is added to the base of a structure to facilitate acceleration spectrum input. (You can use the large mass to convert an acceleration spectrum to a force spectrum.) The alpha damping coefficient, which is multiplied by the mass matrix, will produce artificially large damping forces in such a system, leading to inaccuracies in the spectrum input, as well as in the system response. Beta damping and material damping can lead to undesirable results in a nonlinear analysis. These damping coefficients are multiplied by the stiffness matrix, which is constantly changing in a nonlinear analysis. The resulting change in damping can sometimes be opposite to the actual change in damping that can occur in physical structures. For example, whereas physical systems that experience softening due to plastic response will usually experience a corresponding increase in damping, an ANSYS model that has beta damping will experience a decrease in damping as plastic softening response develops. Material-dependent damping allows you to specify beta damping (β) as a material property (MP,DAMP). Note, however, that MP,DAMP in a spectrum analysis (ANTYPE,SPECTR) specifies a material-dependent damping ratio ξ, not β. Also note that for multi-material elements such as SOLID46, SOLID65, SHELL91, and SHELL99, β can only be specified for the element as a whole, not for each material in the element. In these cases, β is determined from the material pointer for the element (set with the MAT command), rather than the material pointed to by any real constant MAT for the element. MP,DAMP is not assumed to be temperature-dependent, and is always evaluated at T = 0.0. The constant material damping coefficient is available only for full and modal harmonic analyses. The constant damping ratio is the simplest way of specifying damping in the structure. It represents the ratio of actual damping to critical damping, and is specified as a decimal number with the DMPRAT command. DMPRAT is available only for spectrum, harmonic response, and mode superposition transient dynamic analyses. Modal damping gives you the ability to specify different damping ratios for different modes of vibration. It is specified with the MDAMP command and is available only for the spectrum and mode superposition method of solution (transient dynamic and harmonic response analyses). Element damping involves using element types having viscous damping characteristics, such as COMBIN7, COMBIN14, COMBIN37, COMBIN40, and so on.
5–38
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 5.10: Other Analysis Details If you are running a mode superposition analysis and used the QR damping solution method for the modal solution, alpha (ALPHAD), beta (BETAD), material-dependent, and element damping must be defined in the QR damping modal solution for the damping to be available in a subsequent mode superposition analysis. For more information about damping, see the ANSYS, Inc. Theory Reference. The explicit mathematical expressions that form the damping matrix in different analysis options are shown in Table 5.6: “Damping Matrix Formulation with Different Damping Coefficients”. These expressions define how each of the damping options in Table 5.5: “Damping for Different Analysis Types” is handled in a dynamic analysis.
Table 5.6 Damping Matrix Formulation with Different Damping Coefficients Analysis Type Full Harmonic & Modal Analysis Mode Superposi- Mode Superposi- Spectrum AnaTransient AnaLANB(1) tion Harmonic Ana- tion Transient Ana- lysis(1) (modal lysis lysis(1) lysis(1) damping ratio) Modal Analysis QRDA(1) ALPHAD α
α[M]
No
ΦTα[M]Φ = α
ΦTα[M]Φ = α
No
Φ Tβ[K ]Φ = βω2i
Φ Tβ[K ]Φ = βω2i
βωi 2
α[M] BETAD β
β[K]
No
β[K] MP,DAMP
βm j
No
No
Nm
m ∑ β j [K j ]
No
No
j =1
Nm
m s ∑ βj Ej
j =1 Nm
s ∑ Ej j =1
See Equation 17–104 in the ANSYS, Inc. Theory Reference m ∑ β j [K j ]
Nm Φ T ∑ βm j [K j ]Φ
Nm Φ T ∑ βm j [K j ]Φ
No
No
2ξωi
2ξωi
ξ
Nm
j =1
DMPRAT ξ
Harmonic
j =1
j =1
2ξ [K ] Ω MDAMP
No
No
ξm i
No
2ξm i ωi
2ξm i ωi
ξm i No
Element Damping
No
No
∑ [Ck ]
Φ T ∑ [Ck ]Φ
Φ T ∑ [Ck ]Φ
No
No
No
Ne
∑ [Ck ]
k =1
Ne
k =1
MP,DMPR
βξj
Harmonic Nm
2βξj [K j ]
j =1
Ω
∑
Ne
k =1
No
No
Ne
k =1
No
2βξj [K j ] Φ ∑ Φ Ω j =1 N T m
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
5–39
Chapter 5: Transient Dynamic Analysis Note — 1.
For modal, mode superposition, and spectrum analyses the boxes are split where applicable with the top indicating the Lanczos method and the bottom indicating the QR damped method.
5.11. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional transient dynamic analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS program. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual includes a variety of transient dynamic analysis test cases: VM9 - Large Lateral Deflection of Unequal Stiffness Springs VM40 - Large Deflection and Rotation of a Beam Pinned at One End VM65 - Transient Response of a Ball Impacting a Flexible Surface VM71 - Transient Response of a Spring, Mass, Damping System VM72 - Logarithmic Decrement VM73 - Free Vibration with Coulomb Damping VM74 - Transient Response to an Impulsive Excitation VM75 - Transient Response to a Step Excitation VM77 - Transient Response to a Constant Force with a Finite Rise Time VM79 - Transient Response of a Bilinear Spring Assembly VM80 - Plastic Response to a Suddenly Applied Constant Force VM81 - Transient Response of a Drop Container VM84 - Displacement Propagation along a Bar with Free Ends VM85 - Transient Displacements in a Suddenly Stopped Moving Bar VM91 - Large Rotation of a Swinging Pendulum VM156 - Natural Frequency of Nonlinear Spring-Mass System VM158 - Motion of a Bobbing Buoy VM179 - Dynamic Double Rotation of a Jointed Beam VM182 - Transient Response of a Spring-Mass System
5–40
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 6: Spectrum Analysis 6.1. Definition of Spectrum Analysis A spectrum analysis is one in which the results of a modal analysis are used with a known spectrum to calculate displacements and stresses in the model. It is mainly used in place of a time-history analysis to determine the response of structures to random or time-dependent loading conditions such as earthquakes, wind loads, ocean wave loads, jet engine thrust, rocket motor vibrations, and so on.
6.2. What is a Spectrum? The spectrum is a graph of spectral value versus frequency that captures the intensity and frequency content of time-history loads. Three types of spectra are available for a spectrum analysis: •
Response Spectrum –
Single-point Response Spectrum (SPRS)
–
Multi-point Response Spectrum (MPRS)
•
Dynamic Design Analysis Method (DDAM)
•
Power Spectral Density (PSD)
The only method available in the ANSYS Professional program is the single-point response spectrum.
6.2.1. Response Spectrum A response spectrum represents the response of single-DOF systems to a time-history loading function. It is a graph of response versus frequency, where the response might be displacement, velocity, acceleration, or force. Two types of response spectrum analysis are possible: single-point response spectrum and multi-point response spectrum.
6.2.1.1. Single-Point Response Spectrum (SPRS) In a single-point response spectrum (SPRS) analysis, you specify one response spectrum curve (or a family of curves) at a set of points in the model, such as at all supports, as shown in Figure 6.1: “Single-Point and Multi-Point Response Spectra” (a).
6.2.1.2. Multi-Point Response Spectrum (MPRS) In a multi-point response spectrum (MPRS) analysis, you specify different spectrum curves at different sets of points, as shown in Figure 6.1: “Single-Point and Multi-Point Response Spectra” (b).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 6: Spectrum Analysis
Figure 6.1 Single-Point and Multi-Point Response Spectra
6.2.2. Dynamic Design Analysis Method (DDAM) The Dynamic Design Analysis Method (DDAM) is a technique used to evaluate the shock resistance of shipboard equipment. The technique is essentially a response spectrum analysis in which the spectrum is obtained from a series of empirical equations and shock design tables provided in the U.S. Naval Research Laboratory Report NRL-1396.
6.2.3. Power Spectral Density Power spectral density (PSD) is a statistical measure defined as the limiting mean-square value of a random variable. It is used in random vibration analyses in which the instantaneous magnitudes of the response can be specified only by probability distribution functions that show the probability of the magnitude taking a particular value. A PSD is a statistical measure of the response of a structure to random dynamic loading conditions. It is a graph of the PSD value versus frequency, where the PSD may be a displacement PSD, velocity PSD, acceleration PSD, or force PSD. Mathematically, the area under a PSD-versus-frequency curve is equal to the variance (square of the standard deviation of the response). Similar to response spectrum analysis, a random vibration analysis may be single-point or multi-point. In a singlepoint random vibration analysis, you specify one PSD spectrum at a set of points in the model. In a multi-point random vibration analysis, you specify different PSD spectra at different points in the model.
6.2.4. Deterministic vs. Probabilistic Analyses Response spectrum and DDAM analyses are deterministic analyses because both the input to the analyses and output from the analyses are actual maximum values. Random vibration analysis, on the other hand, is probabilistic in nature, because both input and output quantities represent only the probability that they take on certain values.
6.3. Steps in a Single-Point Response Spectrum (SPRS) Analysis The procedure for a single-point response spectrum analysis consists of six main steps: 1.
6–2
Build the model.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.3: Steps in a Single-Point Response Spectrum (SPRS) Analysis 2.
Obtain the modal solution.
3.
Obtain the spectrum solution.
4.
Expand the modes.
5.
Combine the modes.
6.
Review the results.
The modal solution is required because the structure's mode shapes and frequencies must be available to calculate the spectrum solution. Also, by performing the spectrum solution ahead of mode expansion, you can expand only the significant modes that contribute to the final solution.
6.3.1. Build the Model See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details, see the ANSYS Modeling and Meshing Guide.
6.3.1.1. Points to Remember •
Only linear behavior is valid in a spectrum analysis. Nonlinear elements, if any, are treated as linear. If you include contact elements, for example, their stiffnesses are calculated based on their initial status and are never changed.
•
Both Young's modulus (EX) (or stiffness in some form) and density (DENS) (or mass in some form) must be defined. Material properties can be linear, isotropic or orthotropic, and constant or temperature-dependent. Nonlinear properties, if any, are ignored.
6.3.2. Obtain the Modal Solution The modal solution - natural frequencies and mode shapes - is needed to calculate the spectrum solution. The procedure to obtain the modal solution is described in Chapter 3, “Modal Analysis”, but you should keep in mind the following additional points: •
Use the Block Lanczos (default), subspace, or reduced method to extract the modes. The other methods - unsymmetric, damped, QR damped, and PowerDynamics - are not valid for subsequent spectrum analysis.
•
The number of modes extracted should be enough to characterize the structure's response in the frequency range of interest.
•
If you are using GUI method, choose NO for mode expansion on the dialog box for the modal analysis options [MODOPT], so that modes are not expanded at this time, but can be expanded selectively in a separate solution pass. (See the use of the SIGNIF field on the MXPAND command.) Otherwise, choose YES to expand all the modes at this phase.
•
If material-dependent damping is to be included in the spectrum analysis, it must be specified in the modal analysis.
•
Be sure to constrain those DOF where you want to apply a base excitation spectrum.
•
At the end of the solution, leave the SOLUTION processor.
6.3.3. Obtain the Spectrum Solution The procedure to obtain the spectrum solution is explained below. The mode file and the full file (jobname.MODE, jobname.FULL) from the modal analysis must be available, and the database must contain the model data.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–3
Chapter 6: Spectrum Analysis 1.
Enter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define the analysis type and analysis options. ANSYS offers the following analysis options for a spectrum analysis. Not all modal analysis options and not all eigenvalue extraction techniques work with all spectrum analysis options.
Table 6.1 Analysis Types and Options Option New Analysis
Command ANTYPE
Analysis Type: Spec- ANTYPE trum
GUI Path Main Menu> Solution> Analysis Type> New Analysis Main Menu> Solution> Analysis Type> New Analysis> Spectrum
SPOPT
Main Menu> Solution> Analysis Type> Analysis Options
No. of Modes to Use SPOPT for Solution
Main Menu> Solution> Analysis Type> Analysis Options
Spectrum Type: SPRS
•
Option: New Analysis [ANTYPE] Choose New Analysis.
•
Option: Analysis Type: Spectrum [ANTYPE] Choose analysis type spectrum.
•
Option: Spectrum Type: Single-point Response Spectrum [SPOPT] Choose Single-point Response Spectrum (SPRS).
•
Option: Number of Modes to Use for Solution [SPOPT] Choose enough modes to cover the frequency range spanned by the spectrum and to characterize the structure's response. The accuracy of the solution depends on the number of modes used: the larger the number, the higher the accuracy. Make sure to choose YES on the SPOPT command if you want to calculate element stresses.
3.
Specify load step options. The following options are available for single-point response spectrum analysis:
Table 6.2 Load Step Options Option
Command
GUI Path
Spectrum Options Type of Response Spectrum
SVTYP
Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Settings
Excitation Direction SED
Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Settings
Spectral-value- vs- FREQ, SV frequency Curve
Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Freq Table or Spectr Values
Damping (Dynamics Options) Beta (Stiffness) Damping
6–4
BETAD
Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.3: Steps in a Single-Point Response Spectrum (SPRS) Analysis Option
Command
GUI Path
Constant Damping DMPRAT Ratio
Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
MDAMP
Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
Modal Damping
•
Spectrum Options These data include the following: –
Type of Response Spectrum [SVTYP] The spectrum type can be displacement, velocity, acceleration, force, or PSD. All except the force spectrum represent seismic spectra; that is, they are assumed to be specified at the base. The force spectrum is specified at non-base nodes with the F or FK command, and the direction is implied by labels FX, FY, FZ. The PSD spectrum [SVTYP,4] is internally converted to a displacement response spectrum and is limited to flat, narrowband spectra; a more robust random vibration analysis procedure is described in Section 6.7: How to Do a Random Vibration (PSD) Analysis.
–
Excitation Direction [SED]
–
Spectral-Value-Versus-Frequency Curve [FREQ, SV] SV and FREQ commands are used to define the spectral curve. You can define a family of spectral curves, each curve for a different damping ratio. Use the STAT command to list current spectrum curve values. Another command, ROCK, allows you to specify a rocking spectrum.
•
Damping (Dynamics Options) If you specify more than one form of damping, the ANSYS program calculates an effective damping ratio at each frequency. The spectral value at this effective damping ratio is then calculated by loglog interpolation of the spectral curves. If no damping is specified, the spectral curve with the lowest damping is used. For further details about the different forms of damping, see Section 5.10.3: Damping in Chapter 5, “Transient Dynamic Analysis”. The following forms of damping are available: –
Beta (stiffness) Damping [BETAD] This option results in a frequency-dependent damping ratio.
–
Constant Damping Ratio [DMPRAT] This option specifies a constant damping ratio to be used at all frequencies.
–
Modal Damping [MDAMP] Note — Material-dependent damping ratio [MP,DAMP] is also available but only if specified in the modal analysis. MP,DAMP also specifies a material-dependent constant damping ratio (and not material-dependent beta damping, as used in other analyses).
4.
Start solution calculations. Command(s): SOLVE Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–5
Chapter 6: Spectrum Analysis GUI: Main Menu> Solution> Solve> Current LS The output from the solution includes the participation factor table. The participation factor table, which is part of the printed output, lists the participation factors, mode coefficients (based on lowest damping ratio), and the mass distribution for each mode. To obtain the maximum response of each mode (modal response), multiply the mode shape by the mode coefficient. You do this by retrieving the mode coefficient with the *GET command and using it as a scale factor in the SET command. 5.
Repeat steps 3 and 4 for additional response spectra, if any. Note that solutions are not written to the file.rst at this time.
6.
Leave the SOLUTION processor. Command(s): FINISH GUI: Close the Solution menu.
6.3.4. Expand the Modes 1.
Click on the expansion pass option button on the Expansion Pass dialog box to signify YES for an expansion pass. Command(s): MXPAND GUI: Main Menu> Solution> Analysis Type> New Analysis> Modal Main Menu> Solution> Analysis Type> Expansion Pass Main Menu> Solution> Load Step Opts> Expansion Pass> Expand Modes
2.
You must expand modes regardless of whether you used the Block Lanczos, subspace, or reduced extraction method. Details of how to expand the modes are explained in Chapter 3, “Modal Analysis” under "Expand the Modes" as a separate solution pass, but you should keep in mind the following points: •
Only significant modes can be selectively expanded. (See the use of the SIGNIF field on the MXPAND command.) If you are using the GUI method and want to selectively expand modes, choose NO for mode expansion on the dialog box for the modal analysis options [MODOPT] in the modal analysis phase. You then perform mode expansion as a separate solution pass after performing the spectrum solution.
•
Only expanded modes are used for the mode combination operation in the subsequent mode combination pass.
•
If you are interested in stresses caused by the spectrum, be sure to request stress calculations here. By default, no stresses are calculated in the expansion pass, which means no stresses are available for the spectrum analysis.
•
If you want to expand all the modes, you can include the mode expansion steps in the modal solution pass by issuing the MXPAND command. If you are using the GUI method and want to expand all the modes, choose YES for mode expansion on the dialog box for the modal analysis options [MODOPT] in the modal solution step. But if you want to expand only the significant modes, you must perform mode expansion as a separate solution pass after performing the spectrum solution.
Note that modal analysis solutions are written to the results file (Jobname.RST) only if the mode expansion is performed.
6.3.5. Combine the Modes Combine the modes in a separate solution phase. The procedure is as follows: 1.
6–6
Enter SOLUTION. Command(s): /SOLU Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.3: Steps in a Single-Point Response Spectrum (SPRS) Analysis GUI: Main Menu> Solution 2.
Define analysis type. Command(s): ANTYPE GUI: Main Menu> Solution> Analysis Type> New Analysis •
Option: New Analysis [ANTYPE] Choose New Analysis.
•
Option: Analysis Type: Spectrum [ANTYPE] Choose analysis type spectrum.
3.
Choose one of the mode combination methods. ANSYS offers five different mode combination methods for the single-point response spectrum analysis: •
Square Root of Sum of Squares (SRSS)
•
Complete Quadratic Combination (CQC)
•
Double Sum (DSUM)
•
Grouping (GRP)
•
Naval Research Laboratory Sum (NRLSUM)
The NRLSUM method is typically used in the context of the Dynamic Design and Analysis Method (DDAM) spectrum analysis. The following commands are used to invoke different methods of mode combinations: Command(s): SRSS, CQC, DSUM, GRP, NRLSUM GUI: Main Menu> Solution> Analysis Type> New Analysis> Spectrum Main Menu> Solution> Analysis Type> Analysis Opts> Single-pt resp Main Menu> Load Step Opts> Spectrum> Spectrum-Single Point-Mode Combine These commands allow computation of three different types of responses: •
Displacement (label = DISP)
Displacement response refers to displacements, stresses, forces, etc. •
Velocity (label = VELO)
Velocity response refers to velocities, "stress velocities," "force velocities," etc. •
Acceleration (label = ACEL)
Acceleration response refers to accelerations, "stress accelerations," "force accelerations," etc. The DSUM method also allows the input of time duration for earthquake or shock spectrum. Note — You must specify damping if you use the Complete Quadratic Combination method of mode combination (CQC). In addition, if you use material-dependent damping [MP,DAMP,...], you must request that element results be calculated in the modal expansion. (Elcalc = YES on the MXPAND command.)
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–7
Chapter 6: Spectrum Analysis 4.
Start solution. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS The mode combination phase writes a file of POST1 commands (Jobname.MCOM). Read in this file in POST1 to do the mode combinations, using the results file (Jobname.RST) from the modal expansion pass. The file Jobname.MCOM contains POST1 commands that combine the maximum modal responses by using the specified mode combination method to calculate the overall response of the structure. The mode combination method determines how the structure's modal responses are to be combined:
5.
•
If you selected displacement as the response type (label = DISP), displacements and stresses are combined for each mode on the mode combination command.
•
If you selected velocity as the response type (label = VELO), velocities and stress velocities are combined for each mode on the mode combination command.
•
If you selected acceleration as the response type (label = ACEL), accelerations and stress accelerations are combined for each mode on the mode combination command.
Leave the SOLUTION processor. Command(s): FINISH GUI: Close the Solution menu. Note — If you want to compute velocity or acceleration in addition to displacement, repeat the mode combination step after postprocessing the displacement solution by using the VELO or ACEL label on the mode combination commands (SRSS, CQC, GRP, DSUM, NRLSUM). Remember that the existing Jobname.MCOM file is overwritten by the additional mode combination step(s).
6.3.6. Review the Results Results from a single-point response spectrum analysis are written to the mode combination file, Jobname.MCOM, in the form of POST1 commands. These commands calculate the overall response of the structure by combining the maximum modal responses in some fashion (specified by one of the mode combination methods). The overall response consists of the overall displacements (or velocities or accelerations) and, if placed on the results file during the expansion pass, the overall stresses (or stress velocities or stress accelerations), strains (or strain velocities or strain accelerations), and reaction forces (or reaction force velocities or reaction force accelerations). You can use POST1, the general postprocessor, to review the results. Note — If you want a direct combination of the derived stresses (S1, S2, S3, SEQV, SI) from the results file, issue the SUMTYPE,PRIN command before reading in the Jobname.MCOM file. With the PRIN option, component stresses are not available. Note that the command default (SUMTYPE,COMP) is to directly operate only on the unaveraged element component stresses and compute the derived quantities from these. Refer to Section 5.5.3: Creating and Combining Load Cases in the ANSYS Basic Analysis Guide. Also, see the ANSYS Commands Reference for a description of the SUMTYPE command. 1.
6–8
Read the commands on Jobname.MCOM. Command(s): /INPUT
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.3: Steps in a Single-Point Response Spectrum (SPRS) Analysis GUI: Utility Menu> File> Read Input From For example, issue /INPUT with the following arguments: /INPUT,FILE,MCOM!Assumes the default jobname FILE
2.
Display results. •
Option: Display Deformed Shape Command(s): PLDISP GUI: Main Menu> General Postproc> Plot Results> Deformed Shape
•
Option: Contour Displays Command(s): PLNSOL or PLESOL GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu Use PLNSOL or PLESOL to contour almost any result item, such as stresses (SX, SY, SZ ...), strains (EPELX, EPELY, EPELZ ...), and displacements (UX, UY, UZ ...). If you previously issued the SUMTYPE command, the results of the PLNSOL or PLESOL command are affected by the particular SUMTYPE command option (SUMTYPE,COMP or SUMTYPE,PRIN) that you selected. Use the PLETAB command to contour element table data and PLLS to contour line element data. Caution: Derived data, such as stresses and strains, are averaged at the nodes by the PLNSOL command. This averaging results in "smeared" values at nodes where elements of different materials, different shell thicknesses, or other discontinuities meet. To avoid the smearing effect, use selecting (described in Chapter 7, “Selecting and Components” in the ANSYS Basic Analysis Guide) to select elements of the same material, same shell thickness, etc. before issuing PLNSOL. You can view correct membrane results for shells (SHELL, MID) by using KEYOPT(8) = 2 (for SHELL181 or SHELL93) or KEYOPT(11) = 2 (SHELL63). These KEYOPTS write the mid-surface node results directly to the results file, and allow the membrane results to be directly operated on during squaring operations. The default method of averaging the TOP and BOTsquared values to obtain a MID value can possibly yield incorrect MID values.
•
Option: Vector Displays Command(s): PLVECT GUI: Main Menu> General Postproc> Plot Results> Vector Plot> Predefined
•
Option: Tabular Listings Command(s): PRNSOL (nodal results) PRESOL (element-by-element results) PRRSOL (reaction data) GUI: Main Menu> General Postproc> List Results> Nodal Solution Main Menu> General Postproc> List Results> Element Solution Main Menu> General Postproc> List Results> Reaction Solution
•
Other Capabilities Many other postprocessing functions, such as mapping results onto a path, transforming results to different coordinate systems, and load case combinations, are available in POST1. See The General Postprocessor (POST1) in the ANSYS Basic Analysis Guide for details.
If you are using batch mode, note the following: Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–9
Chapter 6: Spectrum Analysis •
The modal solution and spectrum solution passes can be combined into a single modal analysis [ANTYPE,MODAL] solution pass, with spectrum loads [SV, SVTYP, SED, FREQ].
•
The mode expansion and mode combination solution passes can be combined into a single modal analysis [ANTYPE,MODAL and EXPASS,ON] solution pass with a mode combination command.
6.4. Sample Spectrum Analysis (GUI Method) In this sample problem, you determine the seismic response of a beam structure.
6.4.1. Problem Description A simply supported beam of length l , mass per unit length m, and section properties shown in Problem Specifications, is subjected to a vertical motion of both supports. The motion is defined in terms of a seismic displacement response spectrum. Determine the nodal displacements, reactions forces, and the element solutions.
6.4.2. Problem Specifications The following material properties are used for this problem: E = 30 x 106 psi m = 0.2 lb-sec2/in2 The following geometric properties are used for this problem: I = (1000/3) in4 A = 273.9726 in2 l = 240 in h = 14 in
6–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.4: Sample Spectrum Analysis (GUI Method)
6.4.3. Problem Sketch Figure 6.2 Simply Supported Beam with Vertical Motion of Both Supports
6.4.4. Procedure 6.4.4.1. Set the Analysis Title 1.
Choose menu path Utility Menu> File> Change Title.
2.
Type the text "Seismic Response of a Beam Structure" and click on OK.
6.4.4.2. Define the Element Type 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete. The Element Types dialog box appears.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
Scroll down the list on the left to "Structural Beam" and select it.
4.
Click on "2D elastic 3" in the list on the right.
5.
Click on OK. The Library of Element Types dialog box closes.
6.
Click on Close in the Element Types dialog box.
6.4.4.3. Define the Real Constants 1.
Choose menu path Main Menu> Preprocessor> Real Constants. The Real Constants dialog box appears.
2.
Click on Add. The Element Type for Real Constants dialog box appears.
3.
Click on OK. The Real Constants for BEAM3 dialog box appears. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–11
Chapter 6: Spectrum Analysis 4.
Enter 273.9726 for cross-sectional area.
5.
Enter (1000/3) for area moment of inertia.
6.
Enter 14 for total beam height and click on OK.
7.
Click on Close to close the Real Constants dialog box.
6.4.4.4. Define Material Properties 1.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
2.
In the Material Models Available window, double-click on the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
3.
Enter 30e3 for EX (Young's modulus), and click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
4.
Double-click on Density. A dialog box appears.
5.
Enter 73E-5 for DENS (density), and click on OK.
6.
Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
6.4.4.5. Define Keypoints and Line 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Keypoints> In Active CS. The Create Keypoints in Active Coordinate System dialog box appears.
2.
Enter 1 for keypoint number.
3.
Click on Apply to accept the default X, Y, Z coordinates of 0,0,0.
4.
Enter 2 for keypoint number.
5.
Enter 240,0,0 for X, Y, and Z coordinates, respectively.
6.
Click on OK.
7.
Choose menu path Utility Menu> PlotCtrls> Numbering. The Plot Numbering Controls dialog box appears.
8.
Click on "keypoint numbers" to turn keypoint numbering on.
9.
Click on OK.
10. Choose menu path Main Menu> Preprocessor> Modeling> Create> Lines> Lines> Straight Line. A picking menu appears. 11. Click on keypoint 1, and then on keypoint 2. A straight line appears between the two keypoints. 12. Click on OK. The picking menu closes.
6.4.4.6. Set Global Element Density and Mesh Line 1.
Choose menu path Main Menu> Preprocessor> Meshing> Size Cntrls> Global> Size. The Global Element Sizes dialog box appears.
2.
Enter 8 for the number of element divisions and click on OK. The Global Element Sizes dialog box closes.
3.
Choose menu path Main Menu> Preprocessor> Meshing> Mesh> Lines. A picking menu appears.
4.
Click on Pick All. The picking menu closes.
6–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.4: Sample Spectrum Analysis (GUI Method)
6.4.4.7. Set Boundary Conditions 1.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. A picking menu appears.
2.
In the graphics window, click once on the node at the left end of the beam.
3.
Click on OK. The Apply U,ROT on Nodes dialog box appears.
4.
In the scroll box of DOFs to be constrained, click once on "UY" to highlight it.
5.
Click on OK.
6.
Repeat steps 1-3 and select the node at the right end of the beam.
7.
In the scroll box of DOFs to be constrained, click once on "UX." Both "UX" and "UY" should be highlighted.
8.
Click on OK. The Apply U,ROT on Nodes dialog box closes.
6.4.4.8. Specify Analysis Type and Options 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis. The New Analysis dialog box appears.
2.
Click on "Modal" to select it and click on OK. The New Analysis dialog box closes.
3.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Modal Analysis dialog box appears.
4.
Click on "Reduced" as the mode extraction method [MODOPT].
5.
Enter 1 for the number of modes to expand.
6.
Click on the Calculate elem. results dialog button [MXPAND] to specify YES.
7.
Click on OK. The Modal Analysis dialog box closes, and the Reduced Modal Analysis dialog box appears.
8.
Enter 3 for the No. of modes to print and click on OK. The Reduced Modal Analysis dialog box closes.
9.
Choose menu path Main Menu> Solution> Master DOFs> User Selected> Define. The picking menu appears.
10. Choose Pick All. The Define Master DOFs dialog box appears. 11. Select UY for the 1st degree of freedom and click on OK. The Define Master DOFs dialog box closes.
6.4.4.9. Solve the Modal Analysis 1.
Choose menu path Main Menu> Solution> Solve> Current LS. The Solve Current Load Step dialog box appears, along with a status window.
2.
Carefully review the information in the status window, and then click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to start the solution.
4.
When the solution is finished, a dialog box stating "Solution is done!" appears. Click on Close.
6.4.4.10. Set Up the Spectrum Analysis 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis. The New Analysis dialog box appears, along with a warning message that states: "Changing the analysis type is only valid within the first load step. Pressing OK will cause you to exit and reenter SOLUTION. This will reset load step count to 1." Click on CLOSE to close the warning message box.
2.
Click on "Spectrum" to select it, and click on OK. The New Analysis dialog box closes. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–13
Chapter 6: Spectrum Analysis 3.
Choose menu path Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Settings. The Settings for Single-point Response Spectrum dialog box appears.
4.
Select "Seismic displac" in the scroll box as the type of response spectrum.
5.
Enter 0,1,0 for excitation direction into the excitation direction input windows and click on OK.
6.4.4.11. Define Spectrum Value vs. Frequency Table 1.
Choose menu path Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Freq Table. The Frequency Table dialog box appears.
2.
Enter 0.1 for FREQ1, enter 10 for FREQ2, and click on OK.
3.
Choose menu path Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Spectr Values. The Spectrum Values - Damping Ratio dialog box appears.
4.
Click on OK to accept the default of no damping. The Spectrum Values dialog box appears.
5.
Enter 0.44 and 0.44 for FREQ1 and FREQ2, respectively.
6.
Click on OK. The Spectrum Values dialog box closes.
6.4.4.12. Solve Spectrum Analysis 1.
Choose menu path Main Menu> Solution> Solve> Current LS. The Solve Current Load Step dialog box appears, along with a status window.
2.
Carefully review the information in the status window, and then click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to start the solution.
4.
When the solution is finished, a dialog box stating "Solution is done!" appears. Click on Close.
6.4.4.13. Set up the Expansion Pass 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis. The New Analysis dialog box appears, along with a warning message that states: "Changing the analysis type is only valid within the first load step. Pressing OK will cause you to exit and reenter SOLUTION. This will reset load step count to 1." Click on CLOSE to close the warning message box.
2.
Click on "Modal" to select it, and click on OK. The New Analysis dialog box closes.
3.
Choose menu path Main Menu> Solution> Analysis Type> Expansion Pass. The Expansion Pass dialog box appears.
4.
Click on the expansion pass dialog button to turn it ON and click on OK. The Expansion Pass dialog box closes.
6.4.4.14. Expand the Modes 1.
Choose menu path Main Menu> Solution> Load Step Opts> ExpansionPass> Expand Modes. The Expand Modes dialog box appears.
2.
Enter 10 for the number of modes to expand and enter 0.005 for the significant threshold.
3.
Click on the calculate element results dialog button to specify YES for element results calculation.
4.
Click on OK. The Expand Modes dialog box closes.
6–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.4: Sample Spectrum Analysis (GUI Method)
6.4.4.15. Start Expansion Pass Calculation 1.
Choose menu path Main Menu> Solution> Solve> Current LS. The Solve Current Load Step dialog box appears, along with a status window.
2.
Carefully review the information in the status window, and then click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to start the solution.
4.
When the solution is finished, a dialog box stating "Solution is done!" appears. Click on Close.
6.4.4.16. Set Up Mode Combination for Spectrum Analysis 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis. The New Analysis dialog box appears, along with a warning message that states: "Changing the analysis type is only valid within the first load step. Pressing OK will cause you to exit and reenter SOLUTION. This will reset load step count to 1." Click on CLOSE to close the warning message box.
2.
Click on "Spectrum" to select it, and click on OK. The New Analysis dialog box closes.
3.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Spectrum Analysis dialog box appears.
4.
Accept the default spectrum type single-point response. Click on OK. The Spectrum Analysis dialog box closes.
6.4.4.17. Select Mode Combination Method 1.
Choose menu path Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Mode Combine. The Mode Combination Methods dialog box appears.
2.
Select SRSS as the mode combination method.
3.
Enter 0.15 for the significant threshold.
4.
Select displacement for the type of output. Click OK. The Mode Combination Methods dialog box closes.
6.4.4.18. Combine the Modes 1.
Choose menu path Main Menu> Solution> Solve> Current LS. The Solve Current Load Step dialog box appears, along with a status window.
2.
Carefully review the information in the status window, and then click on Close.
3.
Click on OK on the Solve Current Load Step dialog box to start the solution.
4.
When the solution is finished, a dialog box stating "Solution is done!" appears. Click on Close.
6.4.4.19. Postprocessing: Print Out Nodal, Element, and Reaction Solutions 1.
Choose menu path Main Menu> General Postproc> List Results> Results Summary. The SET Command listing window appears.
2.
Review the information in the listing window, and click on Close. The SET Command listing window closes.
3.
Choose menu path Utility Menu> File> Read Input From. The Read File dialog box appears.
4.
From the left side of the Read File dialog box, select the directory containing your results from the scroll box.
5.
From the right side of the Read File dialog box, select the jobname.mcom file from the scroll box. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–15
Chapter 6: Spectrum Analysis 6.
Click on OK. The Read File dialog box closes.
7.
Choose menu path Main Menu> General Postproc> List Results> Nodal Solution. The List Nodal Solution dialog box appears.
8.
Click on OK to accept the default settings of "DOF solution" in the scroll box on the left and "All DOFs DOF" in the scroll box on the right. The List Nodal Solution dialog box closes.
9.
The PRNSOL Command listing window appears. Review the results and click on Close to close the PRNSOL Command listing window.
10. Choose menu path Main Menu> General Postproc> List Results> Element Solution. The List Element Solution dialog box appears. 11. Scroll down the list on the left to select "Line Elem results" and select "Structural ELEM" on the scroll box on the right. Click on OK. The List Element Solution dialog box closes. 12. The PRESOL Command listing window appears. Review the results and click on Close to close the PRESOL Command listing window. 13. Choose menu path Main Menu> General Postproc> List Results> Reaction Solu. The List Reaction Solution dialog box appears. 14. Scroll down the list to "All struc forc F" to select it and click on OK. The List Reaction Solution dialog box closes. 15. The PRRSOL Command listing window appears. Review the results in the listing window and click on Close to close the PRRSOL Command listing window.
6.4.4.20. Exit ANSYS 1.
In the ANSYS Toolbar, click on Quit.
2.
Choose the save option you want and click on OK.
You are now finished with this sample problem.
6.5. Sample Spectrum Analysis (Command or Batch Method) You can perform the example spectrum analysis using the ANSYS commands shown below instead of GUI choices. Items prefaced by an exclamation point (!) are comments. /PREP7 /TITLE Seismic Response of a Beam Structure ET,1,BEAM3 R,1,273.9726,(1000/3),14 ! A = 273.9726, I = (1000/3), H = 14 MP,EX,1,30E6 MP,DENS,1,73E-5 K,1 K,2,240 L,1,2 ESIZE,,8 LMESH,1 NSEL,S,LOC,X,0 D,ALL,UY NSEL,S,LOC,X,240 D,ALL,UX,,,,,UY NSEL,ALL FINISH /SOLU ANTYPE,MODAL
6–16
! Mode-frequency analysis
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.6: Where to Find Other Examples MODOPT,REDUC,,,,3 MXPAND,1,,,YES M,ALL,UY OUTPR,BASIC,1 SOLVE FINISH
! Householder, print first 3 reduced mode shapes ! Expand first mode shape, calculate element stresses
/SOLU ANTYPE,SPECTR SPOPT,SPRS SED,,1 SVTYPE,3 FREQ,.1,10 SV,,.44,.44 SOLVE FINISH
! ! ! ! ! !
/SOLU ANTYPE,MODAL EXPASS,ON MXPAND,10,,,YES,0.005
Spectrum analysis Single point spectrum Global Y-axis as spectrum direction Seismic displacement spectrum Frequency points for SV vs. freq. table Spectrum values associated with frequency points
! Mode-frequency analysis ! Expand 10 mode shapes, calculate element stresses ! set signif=0.005
SOLVE FINISH /SOLU ANTYPE,SPECTR SRSS,0.15,DISP
! Square Root of Sum of Squares Mode combination ! with signif=0.15 and displacement solution requested
SOLVE FINISH /POST1 SET,LIST /INP,,mcom PRNSOL,DOF PRESOL,ELEM PRRSOL,F FINISH
! Print nodal solution ! Print element solution in element format ! Print reaction solution
6.6. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional spectrum analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS program. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual includes a variety of spectrum analysis test cases: VM19 - Random Vibration Analysis of a Deep Simply-Supported Beam VM68 - PSD Response of a Two DOF Spring-Mass System VM69 - Seismic Response VM70 - Seismic Response of a Beam Structure VM203 - Dynamic Load Effect on Simply-Supported Thick Square Plate See the ANSYS Commands Reference for a discussion of the ANTYPE, MODOPT, D, EXPASS, MXPAND, SPOPT, SVTYP, SED, FREQ, SV, SRSS, CQC, DSUM, GRP, NRLSUM, and DMPRAT commands.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–17
Chapter 6: Spectrum Analysis
6.7. How to Do a Random Vibration (PSD) Analysis The procedure for a PSD analysis consists of six main steps: 1.
Build the model.
2.
Obtain the modal solution.
3.
Expand the modes.
4.
Obtain the spectrum solution.
5.
Combine the modes.
6.
Review the results.
Of these, the first two steps are the same as described for a single-point response spectrum analysis. The procedure for the remaining four steps is explained below. Random vibration analysis is not available in the ANSYS Professional program. In the GUI method, the dialog box for the modal analysis options [MODOPT] contains an option for mode expansion [MXPAND]. Choose YES for mode expansion. You then follow the instructions in Section 6.7.1: Expand the Modes. The procedures for obtaining the modal solution and expanding the nodes are combined into a single step.
6.7.1. Expand the Modes You must expand modes regardless of whether you used the subspace, Block Lanczos, or reduced extraction method. Details about expanding the modes are explained in Section 3.6: Expand the Modes, but keep in mind the following additional points: •
Only expanded modes are used for the mode combination step.
•
If you are interested in stresses caused by the spectrum, be sure to request stress calculations here. By default, no stresses are calculated in the expansion pass, which means no stresses are available at the end of the spectrum solution.
•
The mode expansion can be performed as a separate step, or can be included in the modal analysis phase.
•
At the end of the expansion pass, leave SOLUTION with the FINISH command. If you want to exit ANSYS after running the modal analysis, you must save the database at this point.
As explained in Chapter 3, “Modal Analysis”, you can combine the modal solution and mode expansion steps by including the MXPAND command in the modal analysis step (GUI and batch modes).
6.7.2. Obtain the Spectrum Solution To obtain the PSD spectrum solution, the database must contain the model data as well as the modal solution data. If you leave ANSYS after running the modal analysis, you must save the database. In addition, the following files from the modal solution must be available: Jobname.MODE, .ESAV, .EMAT, .FULL (only for subspace and Block Lanczos methods), .RST. 1.
Enter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define the analysis type and analysis options:
6–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.7: How to Do a Random Vibration (PSD) Analysis
3.
•
For spectrum type [SPOPT], choose Power Spectral Density (PSD).
•
Specify stress calculations ON [SPOPT] if you are interested in stress results. Stresses caused by the spectrum are calculated only if they were also requested during the modal expansion pass.
Specify load step options. The following options are available for a random vibration analysis: •
Spectrum Data –
Type of PSD Command(s): PSDUNIT GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> Settings The PSD type can be displacement, velocity, force, pressure, or acceleration. Whether it is a base excitation or a nodal excitation is specified in Steps 4 and 5. If a pressure PSD is to be applied, the pressures should be applied in the modal analysis itself.
–
PSD-versus-frequency table Define a piecewise-linear (in log-log scale) PSD versus frequency table. Since a curve-fitting polynomial is used for the closed-form integration of the curve, you should graph the input, which is overlaid with the fitted curve, to ensure a good fit. If the fit is not good, you should add one or more intermediate points to the table until you obtain a good fit. Command(s): PSDFRQ, PSDVAL, PSDGRAPH GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> PSD vs Freq Main Menu> Solution> Load Step Opts> Spectrum> PSD> Graph PSD Tables PSDFRQ and PSDVAL are used to define the PSD-versus-frequency table. Step 6 describes how to apply additional PSD excitations (if any). You can issue STAT to list PSD tables and issue PSDGRAPH to graph them.
•
Damping (Dynamics Options) The following forms of damping are available: ALPHAD, BETAD, and MDAMP result in a frequencydependent damping ratio, whereas DMPRAT specifies a constant damping ratio to be used at all frequencies. If you specify more than one form of damping, ANSYS calculates an effective damping ratio at each frequency. Note — If no damping is specified in a PSD analysis, a default DMPRAT of 1 percent is used. –
Alpha (Mass) Damping Command(s): ALPHAD GUI: Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
–
Beta (Stiffness) Damping Command(s): BETAD GUI: Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
–
Constant Damping Ratio Command(s): DMPRAT GUI: Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping
–
Frequency-Dependent Damping Ratio Command(s): MDAMP GUI: Main Menu> Solution> Load Step Opts> Time/Frequenc> Damping Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–19
Chapter 6: Spectrum Analysis
The remaining steps are specific to a random vibration analysis: 4.
Apply the PSD excitation at the desired nodes. Use a value of 1.0 to indicate points where the PSD excitation applies. A value of 0.0 (or blank) can be used to remove a specification. The excitation direction is implied by the UX, UY, UZ labels on the D command (for base excitation), and by FX, FY, FZ on the F command (for nodal excitation). For nodal excitation, values other than 1.0 can be used to scale the participation factors. For pressure PSD, bring in the load vector from the modal analysis (LVSCALE). You can use the scale factor. Note — You can apply base excitations only at nodes that were constrained in the modal analysis. Command(s): D (or DK, DL, or DA) for base excitation F (or FK) for nodal excitation LVSCALE for pressure PSD GUI: Main Menu> Solution> Define Loads> Apply> Structural> Spectrum> Base PSD Excit> On Nodes
5.
Begin participation factor calculations for the above PSD excitation. Use the TBLNO field to indicate which PSD table to use, and Excit to specify whether the calculations are for a base or nodal excitation. Command(s): PFACT GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> Calculate PF
6.
If you need to apply multiple PSD excitations on the same model, repeat steps 3, 4, and 5 for each additional PSD table. Then define, as necessary, the degree of correlation between the excitations, using any of the following commands: Command(s): COVAL for cospectral values QDVAL for quadspectral values PSDSPL for a spatial relationship PSDWAV for a wave propagation relationship PSDGRAPH to graph the data overlaid with the fitted curve GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> Correlation Main Menu> Solution> Load Step Opts> Spectrum> PSD> Graph Tables When you use the PSDSPL or PSDWAV command, you must use SPATIAL or WAVE, respectively, for Parcor on the PFACT command. PSDSPL and PSDWAV relationships might be quite CPU intensive for multi-point base excitations. Nodal excitation and base excitation input must be consistent when using PSDWAV and PSDSPL (for example, FY cannot be applied to one node and FZ be applied to another). The PSDSPL and PSDWAV commands are not available for a pressure PSD analysis.
7.
Specify the output controls. The only valid output control command for this analysis is PSDRES, which specifies the amount and form of output written to the results file. Up to three sets of solution quantities can be calculated: displacement solution, velocity solution, or acceleration solution. Each of these can be relative to the base or absolute. Command(s): PSDRES GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> Calc Controls Table 6.3: “Solution Items Available in a PSD Analysis” shows a summary of the possible solution sets. To limit the amount of data written to the results file, use OUTRES at the mode expansion step. Using OUTPR,NSOL,ALL provides a summary table of the significant modal covariance terms.
6–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.7: How to Do a Random Vibration (PSD) Analysis
Table 6.3 Solution Items Available in a PSD Analysis Solution
Items
Displacement Solution (label DISP Displacements, stresses, strains, forces on PSDRES) Velocity Solution (label VELO on PSDRES)
Form Relative, absolute, or neither
Velocities, stress velocities, force Relative, absolute, or neither velocities, etc.
Acceleration Solution (label ACEL Accelerations, stress accl's, force accl's, etc. on PSDRES)
8.
Start solution calculations. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
9.
Leave the SOLUTION processor. Command(s): FINISH GUI: Close the Solution menu.
Relative, absolute, or neither
6.7.3. Combine the Modes The modes can be combined in a separate solution phase. The procedure is as follows: 1.
Enter Solution. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define analysis type. •
Option: New Analysis [ANTYPE] Choose New Analysis.
•
Option: Analysis Type: Spectrum [ANTYPE] Choose analysis type spectrum.
3.
Only the PSD mode combination method is valid in a random vibration analysis. This method triggers calculation of the one-sigma displacements, stresses, etc., in the structure. If you do not issue the PSDCOM command, the program does not calculate the one-sigma response of the structure. Command(s): PSDCOM GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> Mode Combin The SIGNIF and COMODE fields on the PSD mode combination method [PSDCOM] offer options to reduce the number of modes to be combined (see the description of PSDCOM command). If you want to exercise these options, it is prudent to print the modal covariance matrices in Section 6.7.2: Obtain the Spectrum Solution to first investigate the relative contributions of the modes toward the final solution.
4.
Start the solution. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
5.
Leave the SOLUTION processor. Command(s): FINISH GUI: Close the Solution menu.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–21
Chapter 6: Spectrum Analysis
6.7.4. Review the Results Results from a random vibration analysis are written to the structural results file, Jobname.RST. They consist of the following quantities: 1.
Expanded mode shapes from the modal analysis
2.
Static solution for base excitation [PFACT,,BASE]
3.
The following output, if mode combinations are requested [PSDCOM] and based on the PSDRES setting: •
1 σ displacement solution (displacements, stresses, strains, and forces)
•
1 σ velocity solution (velocities, stress velocities, strain velocities, and force velocities)
•
1 σ acceleration solution (accelerations, stress accelerations, strain accelerations, and force accelerations)
You can review these results in POST1, the general postprocessor, and then calculate response PSDs in POST26, the time-history postprocessor.
6.7.4.1. Reviewing the Results in POST1 To review results in POST1, you first need to understand how the results data are organized on the results file. Table 6.4: “Organization of Results Data from a PSD Analysis” shows the organization. Note — Load step 2 is left blank if you specify only nodal PSD excitation. Also, if you suppress the displacement, velocity, or acceleration solution using the PSDRES command, the corresponding load step is left blank. Also, the superelement displacement file (.DSUB) is not written for load steps 3, 4, or 5 in a PSD analysis.
Table 6.4 Organization of Results Data from a PSD Analysis Load Step
Substep
1
1
Expanded modal solution for 1st mode
2
Expanded modal solution for 2nd mode
3
Expanded modal solution for 3rd mode
Etc. 2 (Base excit. only)
Contents
Etc.
1
Unit static solution for PSD table 1
2
Unit static solution for PSD table 2
Etc.
Etc.
3
1
1 sigma displacement solution
4
1
1 sigma velocity solution (if requested)
5
1
1 sigma acceleration solution (if requested)
6.7.4.1.1. Read the Desired Set of Results into the Database For example, to read in the 1 σ displacement solution, issue the command: SET,3,1
Command(s): SET GUI: Main Menu> General Postproc> Read Results> First Set 6–22
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.7: How to Do a Random Vibration (PSD) Analysis
6.7.4.1.2. Display the Results Use the same options available for the SPRS analysis. Note — Nodal stress averaging performed by the PLNSOL command may not be appropriate in a random vibration analysis because the "stresses" are not actual stresses but stress statistics.
6.7.4.2. Calculating Response PSDs in POST26 You can calculate and display response PSDs for any results quantity available on the results file (displacements, velocities, and/or accelerations) if the Jobname.RST and Jobname.PSD files are available. The procedure to calculate the response PSD is as follows: 1.
Enter POST26, the time-history postprocessor. Command(s): /POST26 GUI: Main Menu> TimeHist PostPro
2.
Store the frequency vector. NPTS is the number of frequency points to be added on either side of natural frequencies in order to "smooth" the frequency vector (defaults to 5). The frequency vector is stored as variable 1. Command(s): STORE,PSD,NPTS GUI: Main Menu> TimeHist Postpro> Store Data
3.
Define the variables in which the result items of interest (displacements, stresses, reaction forces, etc.) are to be stored. Command(s): NSOL, ESOL, and/or RFORCE GUI: Main Menu> TimeHist Postpro> Define Variables
4.
Calculate the response PSD and store it in the desired variable. The PLVAR command can then be used to plot the response PSD. Command(s): RPSD GUI: Main Menu> TimeHist Postpro> Calc Resp PSD
6.7.4.3. Calculating Covariance in POST26 You can compute the covariance between two quantities available on the results file (displacements, velocities, and/or accelerations), if the Jobname.RST and Jobname.PSD files are available. The procedure to calculate the covariance between two quantities is as follows: 1.
Enter POST26, the time-history postprocessor. Command(s): /POST26 GUI: Main Menu> TimeHist PostPro
2.
Define the variables in which the result items of interest (displacements, stresses, reaction forces, etc.) are to be stored. Command(s): NSOL, ESOL, and/or RFORCE GUI: Main Menu> TimeHist Postpro> Define Variables
3.
Calculate the contributions of each response component (relative or absolute response) and store them in the desired variable. The PLVAR command can then be used to plot the modal contributions (relative response) followed by the contributions of pseudo-static and mixed part responses to the total covariance. Command(s): CVAR GUI: Main Menu> TimeHist Postpro> Calc Covariance
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–23
Chapter 6: Spectrum Analysis 4.
Obtain the covariance. Command(s): *GET,NameVARI,n,EXTREM,CVAR GUI: Utility Menu> Parameters> Get Scalar Data
6.7.5. Sample Input A sample input listing for a random vibration (PSD) analysis is shown below: ! Build the Model /FILNAM, /TITLE, /PREP7 ... ... ... FINISH ! ! Obtain the Modal Solution /SOLU ANTYPE,MODAL MODOPT,REDU M, ... TOTAL, ... D, ... SAVE SOLVE FINISH ! Expand the Modes /SOLU EXPASS,ON MXPAND, ... SOLVE FINISH ! ! Obtain the Spectrum Solution /SOLU! Reenter SOLUTION ANTYPE,SPECTR SPOPT,PSD, ... PSDUNIT, ... PSDFRQ, ...
! Jobname ! Title ! Enter PREP7 ! Generate model
! ! ! !
Enter SOLUTION Modal analysis Reduced method Master DOF
! Constraints ! Initiates solution
! Reenter SOLUTION ! Expansion pass ! Number of modes to expand
! ! ! ! ! ! ! ! ! ! !
Spectrum analysis Power Spectral Density; No. of modes; Stress calcs. on/off Type of spectrum Frequency pts. (for spectrum values vs. frequency tables) Spectrum values Damping ratio Base excitation Calculate participation factors Output controls
PSDVAL, ... DMPRAT, ... D,0 PFACT, ... PSDRES, ... SAVE SOLVE FINISH ! ! Combine modes using PSD method /SOLU ! Re-enter SOLUTION ANTYPE,SPECTR ! Spectrum analysis PSDCOM,SIGNIF,COMODE ! PSD mode combinations with significance factor and ! option for selecting a subset of modes for ! combination SOLVE FINISH ! ! Review the Results /POST1 ! Enter POST1 SET, ... ! Read results from appropriate load step, substep ...! Postprocess as desired ...! (PLDISP; PLNSOL; NSORT; PRNSOL; etc.) ... FINISH ! ! Calculate Response PSD /POST26 ! Enter POST26
6–24
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 6.9: How to Do Multi-Point Response Spectrum (MPRS) Analysis STORE,PSD NSOL,2,... RPSD,3,2,,... PLVAR,3 ... ! Calculate Covariance RESET NSOL,2 NSOL,3 CVAR,4,2,3,1,1
! ! ! !
! ! ! ! ! *GET,CVAR23U,VARI,4,EXREME,CVAR ! FINISH
Store frequency vector (variable 1) Define variable 2 (nodal data) Calculate response PSD (variable 3) Plot the response PSD
Reset all POST26 specifications to initial defaults. Define variable 2 (nodal data). Define variable 3 (nodal data). Calculate covariance between displacement at nodes 2 and 3. Obtain covariance.
See the ANSYS Commands Reference for a discussion of the ANTYPE, MODOPT, M, TOTAL, D, EXPASS, MXPAND, SPOPT, PSDUNIT, PSDFRQ, PSDVAL, DMPRAT, PFACT, PSDCOM, SUMTYPE, and PSDRES commands.
6.8. How to Do DDAM Spectrum Analysis The procedure for a DDAM spectrum analysis is the same as that for a single-point response spectrum (SPRS) analysis (including file requirements), with the following exceptions: •
Use the British system of units [inches (not feet), pounds, etc.] for all input data - model geometry, material properties, element real constants, etc.
•
Choose DDAM instead of SPRS as the spectrum type [SPOPT command].
•
Use the ADDAM and VDDAM commands instead of SVTYP, SV, and FREQ to specify the spectrum values and types. Specify the global direction of excitation using the SED command. Based on the coefficients specified in the ADDAM and VDDAM commands, the program computes the mode coefficients according to the empirical equations given in the ANSYS, Inc. Theory Reference.
•
The most applicable mode combination method is the NRL sum method [NRLSUM]. Mode combinations are done in the same manner as for a single-point response spectrum. Mode combinations require damping.
•
No damping needs to be specified for solution because it is implied by the ADDAM and VDDAM commands. If damping is specified, it is used for mode combinations but ignored for solution. Note — As in the Single-point Response Spectrum analysis, DDAM spectrum analysis requires six steps to systematically perform the analysis.
If you are using batch mode, note the following: •
The modal solution and DDAM spectrum solution passes can be combined into a single modal analysis [ANTYPE,MODAL] solution pass with DDAM spectrum loads [ADDAM, VDDAM, SED].
•
The mode expansion and mode combination solution passes can be combined into a single modal analysis [ANTYPE,MODAL and EXPASS,ON] solution pass with a mode combination command.
DDAM spectrum analysis is not available in the ANSYS Professional program.
6.9. How to Do Multi-Point Response Spectrum (MPRS) Analysis The procedure for a multi-point response spectrum analysis is the same as that for random vibration (PSD) analysis (including file requirements), with the following exceptions: •
Choose MPRS instead of PSD as the type of spectrum [SPOPT command].
•
The "PSD-versus-frequency" tables now represent spectral values versus frequency. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
6–25
Chapter 6: Spectrum Analysis •
You cannot specify any degree of correlation between the spectra (i.e., they are assumed to be uncorrelated).
•
Only relative results (relative to the base excitation) not absolute values, are calculated.
•
All mode combination methods are available except PSDCOM.
•
Results from a multi-point response spectrum analysis are written to the mode combination file, Jobname.MCOM, in the form of POST1 commands. The commands calculate the overall response of the structure by combining the maximum modal responses in some fashion (specified by the mode combination command in SOLUTION). The overall response consists of the overall displacements and, if placed on the results file during the modal expansion pass, the overall stresses, strains, and reaction forces. If Label = VELO or ACEL on the mode combination command (SRSS, CQC, GRP, DSUM, or NRLSUM) during SOLUTION, the corresponding velocity or acceleration responses are written to the mode combination file.
Multi-point response spectrum analysis is not available in the ANSYS Professional program.
6–26
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 7: Buckling Analysis 7.1. Definition of Buckling Analysis Buckling analysis is a technique used to determine buckling loads - critical loads at which a structure becomes unstable - and buckled mode shapes - the characteristic shape associated with a structure's buckled response.
7.2. Types of Buckling Analyses Two techniques are available in the ANSYS Multiphysics, ANSYS Mechanical, ANSYS Structural, and ANSYS Professional programs for predicting the buckling load and buckling mode shape of a structure: nonlinear buckling analysis, and eigenvalue (or linear) buckling analysis. Since these two methods frequently yield quite different results, let's examine the differences between them before discussing the details of their implementation.
7.2.1. Nonlinear Buckling Analysis Nonlinear buckling analysis is usually the more accurate approach and is therefore recommended for design or evaluation of actual structures. This technique employs a nonlinear static analysis with gradually increasing loads to seek the load level at which your structure becomes unstable, as depicted in Figure 7.1: “Buckling Curves” (a). Using the nonlinear technique, your model can include features such as initial imperfections, plastic behavior, gaps, and large-deflection response. In addition, using deflection-controlled loading, you can even track the post-buckled performance of your structure (which can be useful in cases where the structure buckles into a stable configuration, such as "snap-through" buckling of a shallow dome).
7.2.2. Eigenvalue Buckling Analysis Eigenvalue buckling analysis predicts the theoretical buckling strength (the bifurcation point) of an ideal linear elastic structure. (See Figure 7.1: “Buckling Curves” (b).) This method corresponds to the textbook approach to elastic buckling analysis: for instance, an eigenvalue buckling analysis of a column will match the classical Euler solution. However, imperfections and nonlinearities prevent most real-world structures from achieving their theoretical elastic buckling strength. Thus, eigenvalue buckling analysis often yields unconservative results, and should generally not be used in actual day-to-day engineering analyses.
Figure 7.1 Buckling Curves
(a) Nonlinear load-deflection curve, (b) Linear (Eigenvalue) buckling curve Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 7: Buckling Analysis
7.3. Commands Used in a Buckling Analysis You use the same set of commands to build a model and perform a buckling analysis that you use to do any other type of finite element analysis. Likewise, you choose similar options from the graphical user interface (GUI) to build and solve models no matter what type of analysis you are doing. Section 7.6: Sample Buckling Analysis (GUI Method) and Section 7.7: Sample Buckling Analysis (Command or Batch Method) show you how to perform an example eigenvalue buckling analysis via the GUI or via commands, respectively. For detailed, alphabetized descriptions of the ANSYS commands, see the ANSYS Commands Reference.
7.4. Procedure for Nonlinear Buckling Analysis A nonlinear buckling analysis is a static analysis with large deflections turned on [NLGEOM,ON], extended to a point where the structure reaches its limit load or maximum load. Other nonlinearities such as plasticity may be included in the analysis. The procedure for a static analysis is described in Chapter 2, “Structural Static Analysis”, and nonlinearities are described in Chapter 8, “Nonlinear Structural Analysis”.
7.4.1. Applying Load Increments The basic approach in a nonlinear buckling analysis is to constantly increment the applied loads until the solution begins to diverge. Be sure to use a sufficiently fine load increment as your loads approach the expected critical buckling load. If the load increment is too coarse, the buckling load predicted may not be accurate. Turn on bisection and automatic time stepping [AUTOTS,ON] to help avoid this problem.
7.4.2. Automatic Time Stepping With automatic time stepping on, the program automatically seeks out the buckling load. If automatic time stepping is ON in a static analysis having ramped loading and the solution does not converge at a given load, the program bisects the load step increment and attempts a new solution at a smaller load. In a buckling analysis, each such convergence failure is typically accompanied by a "negative pivot" message indicating that the attempted load equals or exceeds the buckling load. You can usually ignore these messages if the program successfully obtains a converged solution at the next, reduced load. If stress stiffness is active [SSTIF,ON], you should run without adaptive descent active [NROPT,FULL,,OFF] to ensure that a lower bound to the buckling load is attained. The program normally converges to the limiting load as the process of bisection and resolution continues to the point at which the minimum time step increment (specified by DELTIM or NSUBST) is achieved. The minimum time step will directly affect the precision of your results.
7.4.3. Important Remember that an unconverged solution does not necessarily mean that the structure has reached its maximum load. It could also be caused by numerical instability, which might be corrected by refining your modeling technique. Track the load-deflection history of your structure's response to decide whether an unconverged load step represents actual structural buckling, or whether it reflects some other problem. Perform a preliminary analysis using the arc-length method [ARCLEN] to predict an approximate value of buckling load. Compare this approximate value to the more precise value calculated using bisection to help determine if the structure has indeed reached its maximum load. You can also use the arc-length method itself to obtain a precise buckling load, but this method requires you to adjust the arc-length radius by trial-and-error in a series of manually directed reanalyses.
7–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 7.5: Procedure for Eigenvalue Buckling Analysis
7.4.4. Points to Remember •
If the loading on the structure is perfectly in-plane (that is, membrane or axial stresses only), the out-ofplane deflections necessary to initiate buckling will not develop, and the analysis will fail to predict buckling behavior. To overcome this problem, apply a small out-of-plane perturbation, such as a modest temporary force or specified displacement, to begin the buckling response. (A preliminary eigenvalue buckling analysis of your structure may be useful as a predictor of the buckling mode shape, allowing you to choose appropriate locations for applying perturbations to stimulate the desired buckling response.) The imperfection (perturbation) induced should match the location and size of that in the real structure. The failure load is very sensitive to these parameters.
•
In a large-deflection analysis, forces (and displacements) will maintain their original orientation, but surface loads will "follow" the changing geometry of the structure as it deflects. Therefore, be sure to apply the proper type of loads.
•
You should carry your stability analysis through to the point of identifying the critical load in order to calculate the structure's factor of safety with respect to nonlinear buckling. (Merely establishing the fact that a structure is stable at a given load level is generally insufficient for most design practice; you will usually be required to provide a specified safety factor, which can only be determined by establishing the actual limit load.)
•
You can extend your analysis into the post-buckled range by activating the arc-length method [ARCLEN]. Use this feature to trace the load-deflection curve through regions of "snap-through" and "snap-back" response.
•
For those elements that support the consistent tangent stiffness matrix (BEAM4, SHELL63, and SHELL143), activate the consistent tangent stiffness matrix (KEYOPT(2) = 1 and NLGEOM,ON) to enhance the convergence behavior of your nonlinear buckling analyses and improve the accuracy of your results. This element KEYOPT must be defined before the first load step of the solution and cannot be changed once the solution has started.
•
Many other elements (such as BEAM188, BEAM189, and SHELL181) will provide consistent tangent stiffness matrix with NLGEOM,ON.
7.5. Procedure for Eigenvalue Buckling Analysis Again, remember that eigenvalue buckling analysis generally yields unconservative results, and should usually not be used for design of actual structures. If you decide that eigenvalue buckling analysis is appropriate for your application, follow this procedure: 1.
Build the model.
2.
Obtain the static solution.
3.
Obtain the eigenvalue buckling solution.
4.
Expand the solution.
5.
Review the results.
7.5.1. Build the Model See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details, see the ANSYS Modeling and Meshing Guide.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
7–3
Chapter 7: Buckling Analysis
7.5.1.1. Points to Remember •
Only linear behavior is valid. Nonlinear elements, if any, are treated as linear. If you include contact elements, for example, their stiffnesses are calculated based on their status after the static prestress run and are never changed.
•
Young's modulus (EX) (or stiffness in some form) must be defined. Material properties may be linear, isotropic or orthotropic, and constant or temperature-dependent. Nonlinear properties, if any, are ignored.
7.5.2. Obtain the Static Solution The procedure to obtain a static solution is the same as described in Chapter 2, “Structural Static Analysis”, with the following exceptions: •
Prestress effects [PSTRES] must be activated. Eigenvalue buckling analysis requires the stress stiffness matrix to be calculated.
•
Unit loads are usually sufficient (that is, actual load values need not be specified). The eigenvalues calculated by the buckling analysis represent buckling load factors. Therefore, if a unit load is specified, the load factors represent the buckling loads. All loads are scaled. (Also, the maximum permissible eigenvalue is 1,000,000 - you must use larger applied loads if your eigenvalue exceeds this limit.)
•
Note that eigenvalues represent scaling factors for all loads. If certain loads are constant (for example, self-weight gravity loads) while other loads are variable (for example, externally applied loads), you need to ensure that the stress stiffness matrix from the constant loads is not factored by the eigenvalue solution. One strategy that you can use to achieve this end is to iterate on the eigensolution, adjusting the variable loads until the eigenvalue becomes 1.0 (or nearly 1.0, within some convergence tolerance). Design optimization could be useful in driving this iterative procedure to a final answer. Consider, for example, a pole having a self-weight W0, which supports an externally-applied load, A. To determine the limiting value of A in an eigenvalue buckling solution, you could solve repetitively, using different values of A, until by iteration you find an eigenvalue acceptably close to 1.0.
Figure 7.2 Adjusting Variable Loads to Find an Eigenvalue of 1.0
•
You can apply a nonzero constraint in the prestressing pass as the static load. The eigenvalues found in the buckling solution will be the load factors applied to these nonzero constraint values. However, the mode shapes will have a zero value at these degrees of freedom (and not the nonzero value specified).
•
At the end of the solution, leave SOLUTION [FINISH].
7–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 7.5: Procedure for Eigenvalue Buckling Analysis
7.5.3. Obtain the Eigenvalue Buckling Solution This step requires files Jobname.EMAT and Jobname.ESAV from the static analysis. Also, the database must contain the model data (issue RESUME if necessary). Follow the steps below to obtain the eigenvalue buckling solution. 1.
Enter the ANSYS solution processor. Command(s): /SOLU GUI: Main Menu> Solution
2.
Specify the analysis type. Command(s): ANTYPE,BUCKLE GUI: Main Menu> Solution> Analysis Type> New Analysis Note — Restarts are not valid in an eigenvalue buckling analysis. Note — When you specify an eigenvalue buckling analysis, a Solution menu that is appropriate for buckling analyses appears. The Solution menu will be either "abridged" or "unabridged", depending on the actions you took prior to this step in your ANSYS session. The abridged menu contains only those solution options that are valid and/or recommended for buckling analyses. If you are on the abridged Solution menu and you want to access other solution options (that is, solution options that are valid for you to use, but their use may not be encouraged for this type of analysis), select the Unabridged Menu option from the Solution menu. For details, see Section 3.11.1: Using Abridged Solution Menus in the ANSYS Basic Analysis Guide.
3.
Specify analysis options. Command(s): BUCOPT, Method, NMODE, SHIFT GUI: Main Menu> Solution> Analysis Type> Analysis Options Regardless of whether you use the command or GUI method, you can specify values for these options:
4.
•
For Method, specify the eigenvalue extraction method. You can choose subspace iteration or Block Lanczos. The Block Lanczos and subspace iteration methods use the full system matrices. See Section 3.5.2.3: Option: Mode-Extraction Method [MODOPT] in this manual for more information about these solution methods.
•
For NMODE, specify the number of eigenvalues to be extracted. This argument defaults to one, which is usually sufficient for eigenvalue buckling.
•
For SHIFT, specify the point (load factor) about which eigenvalues are calculated. The shift point is helpful when numerical problems are encountered (due to negative eigenvalues, for example). Defaults to 0.0.
Specify load step options. The only load step options valid for eigenvalue buckling are output controls and expansion pass options. Command(s): OUTPR,NSOL,ALL GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout You can make the expansion pass a part of the eigenvalue buckling solution or perform it as a separate step. In this document, we treat the expansion pass as a separate step. See Section 7.5.4: Expand the Solution for details.
5.
Save a backup copy of the database to a named file. Command(s): SAVE Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
7–5
Chapter 7: Buckling Analysis GUI: Utility Menu> File> Save As 6.
Start solution calculations. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS The output from the solution mainly consists of the eigenvalues, which are printed as part of the printed output (Jobname.OUT). The eigenvalues represent the buckling load factors; if unit loads were applied in the static analysis, they are the buckling loads. No buckling mode shapes are written to the database or the results file, so you cannot postprocess the results yet. To do this, you need to expand the solution (explained next). Sometimes you may see both positive and negative eigenvalues calculated. Negative eigenvalues indicate that buckling occurs when the loads are applied in an opposite sense.
7.
Exit the SOLUTION processor. Command(s): FINISH GUI: Close the Solution menu.
7.5.4. Expand the Solution If you want to review the buckled mode shape(s), you must expand the solution regardless of which eigenvalue extraction method is used. In the case of the subspace iteration method, which uses full system matrices, you may think of "expansion" to simply mean writing buckled mode shapes to the results file.
7.5.4.1. Points to Remember •
The mode shape file (Jobname.MODE) from the eigenvalue buckling solution must be available.
•
The database must contain the same model for which the solution was calculated.
7.5.4.2. Expanding the Solution The procedure to expand the mode shapes is explained below. 1.
Reenter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution Note — You must explicitly leave SOLUTION (using the FINISH command) and reenter (/SOLU) before performing the expansion pass.
2.
Specify that this is an expansion pass. Command(s): EXPASS,ON GUI: Main Menu> Solution> Analysis Type> ExpansionPass
3.
Specify expansion pass options. Command(s): MXPAND, NMODE, , , Elcalc GUI: Main Menu> Solution> Load Step Opts> ExpansionPass> Expand Modes Regardless of whether you use the command or GUI method, the following options are required for the expansion pass: •
7–6
For NMODE, specify the number of modes to expand. This argument defaults to the total number of modes that were extracted. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 7.5: Procedure for Eigenvalue Buckling Analysis •
4.
For Elcalc, indicate whether you want ANSYS to calculate stresses. "Stresses" in an eigenvalue analysis do not represent actual stresses, but give you an idea of the relative stress or force distribution for each mode. By default, no stresses are calculated.
Specify load step options. The only options valid in a buckling expansion pass are the following output controls: •
Printed Output Use this option to include any results data on the output file (Jobname.OUT). Command(s): OUTPR GUI: Main Menu> Solution> Load Step Opts> Output Ctrl> Solu Printout
•
Database and Results File Output This option controls the data on the results file (Jobname.RST). Command(s): OUTRES GUI: Main Menu> Solution> Load Step Opts> Output Ctrl> DB/Results File Note — The FREQ field on OUTPR and OUTRES can only be ALL or NONE, that is, the data can be requested for all modes or no modes - you cannot write information for every other mode, for instance.
5.
Start expansion pass calculations. The output consists of expanded mode shapes and, if requested, relative stress distributions for each mode. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
6.
Leave the SOLUTION processor. You can now review results in the postprocessor. Command(s): FINISH GUI: Close the Solution menu. Note — The expansion pass has been presented here as a separate step. You can make it part of the eigenvalue buckling solution by including the MXPAND command (Main Menu> Solution> Load Step Opts> ExpansionPass> Expand Modes) as one of the analysis options.
7.5.5. Review the Results Results from a buckling expansion pass are written to the structural results file, Jobname.RST. They consist of buckling load factors, buckling mode shapes, and relative stress distributions. You can review them in POST1, the general postprocessor. Note — To review results in POST1, the database must contain the same model for which the buckling solution was calculated (issue RESUME if necessary). Also, the results file (Jobname.RST) from the expansion pass must be available. 1.
List all buckling load factors. Command(s): SET,LIST GUI: Main Menu> General Postproc> Results Summary Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
7–7
Chapter 7: Buckling Analysis 2.
Read in data for the desired mode to display buckling mode shapes. (Each mode is stored on the results file as a separate substep.) Command(s): SET,SBSTEP GUI: Main Menu> General Postproc> Read Results> load step
3.
Display the mode shape. Command(s): PLDISP GUI: Main Menu> General Postproc> Plot Results> Deformed Shape
4.
Contour the relative stress distributions. Command(s): PLNSOL or PLESOL GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solution Main Menu> General Postproc> Plot Results> Contour Plot> Element Solution
See the ANSYS Commands Reference for a discussion of the ANTYPE, PSTRES, D, F, SF, BUCOPT, EXPASS, MXPAND, OUTRES, SET, PLDISP, and PLNSOL commands.
7.6. Sample Buckling Analysis (GUI Method) In this sample problem, you will analyze the buckling of a bar with hinged ends.
7.6.1. Problem Description Determine the critical buckling load of an axially loaded long slender bar of length l with hinged ends. The bar has a cross-sectional height h, and area A. Only the upper half of the bar is modeled because of symmetry. The boundary conditions become free-fixed for the half-symmetry model. The moment of inertia of the bar is calculated as I = Ah2/12 = 0.0052083 in4.
7.6.2. Problem Specifications The following material properties are used for this problem: E = 30 x 106 psi The following geometric properties are used for this problem: l = 200 in A = 0.25 in2 h = 0.5 in Loading for this problem is: F = 1 lb.
7–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 7.6: Sample Buckling Analysis (GUI Method)
7.6.3. Problem Sketch Figure 7.3 Bar with Hinged Ends
7.6.3.1. Set the Analysis Title After you enter the ANSYS program, follow these steps to set the title. 1.
Choose menu path Utility Menu> File> Change Title.
2.
Enter the text "Buckling of a Bar with Hinged Ends" and click on OK.
7.6.3.2. Define the Element Type In this step, you define BEAM3 as the element type. 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete. The Element Types dialog box appears.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
In the scroll box on the left, click on "Structural Beam" to select it.
4.
In the scroll box on the right, click on "2D elastic 3" to select it.
5.
Click on OK, and then click on Close in the Element Types dialog box.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
7–9
Chapter 7: Buckling Analysis
7.6.3.3. Define the Real Constants and Material Properties 1.
Choose menu path Main Menu> Preprocessor> Real Constants> Add/Edit/Delete. The Real Constants dialog box appears.
2.
Click on Add. The Element Type for Real Constants dialog box appears.
3.
Click on OK. The Real Constants for BEAM3 dialog box appears.
4.
Enter .25 for area, 52083e-7 for IZZ, and .5 for height.
5.
Click on OK.
6.
Click on Close in the Real Constants dialog box.
7.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
8.
In the Material Models Available window, double-click on the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
9.
Enter 30e6 for EX (Young's modulus), and click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
10. Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
7.6.3.4. Define Nodes and Elements 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Nodes> In Active CS. The Create Nodes in Active Coordinate System dialog box appears.
2.
Enter 1 for node number.
3.
Click on Apply. Node location defaults to 0,0,0.
4.
Enter 11 for node number.
5.
Enter 0,100,0 for the X, Y, Z coordinates.
6.
Click on OK. The two nodes appear in the ANSYS Graphics window. Note — The triad, by default, hides the node number for node 1. To turn the triad off, choose menu path Utility Menu> PlotCtrls> Window Controls> Window Options and select the "Not Shown" option for Location of triad. Then click OK to close the dialog box.
7.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Nodes> Fill between Nds. The Fill between Nds picking menu appears.
8.
Click on node 1, then 11, and click on OK. The Create Nodes Between 2 Nodes dialog box appears.
9.
Click on OK to accept the settings (fill between nodes 1 and 11, and number of nodes to fill 9).
10. Choose menu path Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Thru Nodes. The Elements from Nodes picking menu appears. 11. Click on nodes 1 and 2, then click on OK. 12. Choose menu path Main Menu> Preprocessor> Modeling> Copy> Elements> Auto Numbered. The Copy Elems Auto-Num picking menu appears. 13. Click on Pick All. The Copy Elements (Automatically-Numbered) dialog box appears. 14. Enter 10 for total number of copies and enter 1 for node number increment. 15. Click on OK. The remaining elements appear in the ANSYS Graphics window. 7–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 7.6: Sample Buckling Analysis (GUI Method)
7.6.3.5. Define the Boundary Conditions 1.
Choose menu path Main Menu> Solution> Unabridged Menu> Analysis Type> New Analysis. The New Analysis dialog box appears.
2.
Click OK to accept the default of "Static."
3.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Static or SteadyState Analysis dialog box appears.
4.
In the scroll box for stress stiffness or prestress, scroll to "Prestress ON" to select it.
5.
Click on OK.
6.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears.
7.
Click on node 1 in the ANSYS Graphics window, then click on OK in the picking menu. The Apply U,ROT on Nodes dialog box appears.
8.
Click on "All DOF" to select it, and click on OK.
9.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment> On Nodes. The Apply F/M on Nodes picking menu appears.
10. Click on node 11, then click OK. The Apply F/M on Nodes dialog box appears. 11. In the scroll box for Direction of force/mom, scroll to "FY" to select it. 12. Enter -1 for the force/moment value, and click on OK. The force symbol appears in the ANSYS Graphics window.
7.6.3.6. Solve the Static Analysis 1.
Choose menu path Main Menu> Solution> Solve> Current LS.
2.
Carefully review the information in the status window, and click on Close.
3.
Click on OK in the Solve Current Load Step dialog box to begin the solution.
4.
Click on Close in the Information window when the solution is finished.
7.6.3.7. Solve the Buckling Analysis 1.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis. Note — Click on Close in the Warning window if the following warning appears: Changing the analysis type is only valid within the first load step. Pressing OK will cause you to exit and reenter SOLUTION. This will reset the load step count to 1.
2.
In the New Analysis dialog box, click the "Eigen Buckling" option on, then click on OK.
3.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Eigenvalue Buckling Options dialog box appears.
4.
Click on the "Block Lanczos" option, and enter 1 for number of modes to extract.
5.
Click on OK.
6.
Choose menu path Main Menu> Solution> Load Step Opts> ExpansionPass> Expand Modes.
7.
Enter 1 for number of modes to expand, and click on OK.
8.
Choose menu path Main Menu> Solution> Solve> Current LS. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
7–11
Chapter 7: Buckling Analysis 9.
Carefully review the information in the status window, and click on Close.
10. Click on OK in the Solve Current Load Step dialog box to begin the solution. 11. Click on Close in the Information window when the solution is finished.
7.6.3.8. Review the Results 1.
Choose menu path Main Menu> General Postproc> Read Results> First Set.
2.
Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears.
3.
Click the "Def + undeformed" option on. Click on OK. The deformed and undeformed shapes appear in the ANSYS graphics window.
7.6.3.9. Exit ANSYS 1.
In the ANSYS Toolbar, click on Quit.
2.
Choose the save option you want and click on OK.
7.7. Sample Buckling Analysis (Command or Batch Method) You can perform the example buckling analysis of a bar with hinged ends using the ANSYS commands shown below instead of GUI choices. Items prefaced by an exclamation point (!) are comments. /PREP7 /TITLE, BUCKLING OF A BAR WITH HINGED SOLVES ET,1,BEAM3 ! Beam element R,1,.25,52083E-7,.5 ! Area,IZZ, height MP,EX,1,30E6 ! Define material properties N,1 N,11,,100 FILL E,1,2 EGEN,10,1,1 FINISH /SOLU ANTYPE,STATIC PSTRES,ON D,1,ALL F,11,FY,-1 SOLVE FINISH /SOLU ANTYPE,BUCKLE BUCOPT,LANB,1 MXPAND,1 SOLVE FINISH /POST1 SET,FIRST PLDISP,1 FINISH
! ! ! !
Static analysis Calculate prestress effects Fix symmetry ends Unit load at free end
! Buckling analysis ! Use Block Lanczos solution method, extract 1 mode ! Expand 1 mode shape
7.8. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional buckling analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS program. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification 7–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 7.8: Where to Find Other Examples Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual contains a variety of buckling analysis test cases: VM17 - Snap-Through Buckling of a Hinged Shell VM127 - Buckling of a Bar with Hinged Ends (Line Elements) VM128 - Buckling of a Bar with Hinged Ends (Area Elements)
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
7–13
7–14
Chapter 8: Nonlinear Structural Analysis 8.1. What is Structural Nonlinearity? You encounter structural nonlinearities on a routine basis. For instance, whenever you staple two pieces of paper together, the metal staples are permanently bent into a different shape. (See Figure 8.1: “Common Examples of Nonlinear Structural Behavior” (a).) If you heavily load a wooden shelf, it will sag more and more as time passes. (See Figure (b).) As weight is added to a car or truck, the contact surfaces between its pneumatic tires and the underlying pavement change in response to the added load. (See Figure (c).) If you were to plot the load-deflection curve for each of these examples, you would discover that they all exhibit the fundamental characteristic of nonlinear structural behavior - a changing structural stiffness.
Figure 8.1 Common Examples of Nonlinear Structural Behavior
8.1.1. Causes of Nonlinear Behavior Nonlinear structural behavior arises from a number of causes, which can be grouped into these principal categories: •
Changing status
•
Geometric nonlinearities
•
Material nonlinearities
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 8: Nonlinear Structural Analysis
8.1.1.1. Changing Status (Including Contact) Many common structural features exhibit nonlinear behavior that is status-dependent. For example, a tensiononly cable is either slack or taut; a roller support is either in contact or not in contact. Status changes might be directly related to load (as in the case of the cable), or they might be determined by some external cause. Situations in which contact occurs are common to many different nonlinear applications. Contact forms a distinctive and important subset to the category of changing-status nonlinearities. See Chapter 11, “Contact” for detailed information on performing contact analyses using ANSYS.
8.1.1.2. Geometric Nonlinearities If a structure experiences large deformations, its changing geometric configuration can cause the structure to respond nonlinearly. An example would be the fishing rod shown in Figure 8.2: “A Fishing Rod Demonstrates Geometric Nonlinearity”. Geometric nonlinearity is characterized by "large" displacements and/or rotations.
Figure 8.2 A Fishing Rod Demonstrates Geometric Nonlinearity
8.1.1.3. Material Nonlinearities Nonlinear stress-strain relationships are a common cause of nonlinear structural behavior. Many factors can influence a material's stress-strain properties, including load history (as in elastoplastic response), environmental conditions (such as temperature), and the amount of time that a load is applied (as in creep response).
8.1.2. Basic Information About Nonlinear Analyses ANSYS employs the "Newton-Raphson" approach to solve nonlinear problems. In this approach, the load is subdivided into a series of load increments. The load increments can be applied over several load steps. Figure 8.3: “Newton-Raphson Approach” illustrates the use of Newton-Raphson equilibrium iterations in a single DOF nonlinear analysis.
8–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.1: What is Structural Nonlinearity?
Figure 8.3 Newton-Raphson Approach
Before each solution, the Newton-Raphson method evaluates the out-of-balance load vector, which is the difference between the restoring forces (the loads corresponding to the element stresses) and the applied loads. The program then performs a linear solution, using the out-of-balance loads, and checks for convergence. If convergence criteria are not satisfied, the out-of-balance load vector is reevaluated, the stiffness matrix is updated, and a new solution is obtained. This iterative procedure continues until the problem converges. A number of convergence-enhancement and recovery features, such as line search, automatic load stepping, and bisection, can be activated to help the problem to converge. If convergence cannot be achieved, then the program attempts to solve with a smaller load increment. In some nonlinear static analyses, if you use the Newton-Raphson method alone, the tangent stiffness matrix may become singular (or non-unique), causing severe convergence difficulties. Such occurrences include nonlinear buckling analyses in which the structure either collapses completely or "snaps through" to another stable configuration. For such situations, you can activate an alternative iteration scheme, the arc-length method, to help avoid bifurcation points and track unloading. The arc-length method causes the Newton-Raphson equilibrium iterations to converge along an arc, thereby often preventing divergence, even when the slope of the load vs. deflection curve becomes zero or negative. This iteration method is represented schematically in Figure 8.4: “Traditional Newton-Raphson Method vs. ArcLength Method”.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–3
Chapter 8: Nonlinear Structural Analysis
Figure 8.4 Traditional Newton-Raphson Method vs. Arc-Length Method
To summarize, a nonlinear analysis is organized into three levels of operation: •
The "top" level consists of the load steps that you define explicitly over a "time" span (see the discussion of "time" in Chapter 2, “Loading” in the ANSYS Basic Analysis Guide). Loads are assumed to vary linearly within load steps (for static analyses).
•
Within each load step, you can direct the program to perform several solutions (substeps or time steps) to apply the load gradually.
•
At each substep, the program will perform a number of equilibrium iterations to obtain a converged solution.
Figure 8.5: “Load Steps, Substeps, and Time” illustrates a typical load history for a nonlinear analysis. Also see the discussion of load steps, substeps, and equilibrium iterations in Chapter 2, “Loading” in the ANSYS Basic Analysis Guide.
Figure 8.5 Load Steps, Substeps, and Time
8–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.1: What is Structural Nonlinearity? The ANSYS program gives you a number of choices when you designate convergence criteria: you can base convergence checking on forces, moments, displacements, or rotations, or on any combination of these items. Additionally, each item can have a different convergence tolerance value. For multiple-degree-of-freedom problems, you also have a choice of convergence norms. You should almost always employ a force-based (and, when applicable, moment-based) convergence tolerance. Displacement-based (and, when applicable, rotation-based) convergence checking can be added, if desired, but should usually not be used alone.
8.1.2.1. Conservative versus Nonconservative Behavior; Path Dependency If all energy put into a system by external loads is recovered when the loads are removed, the system is said to be conservative. If energy is dissipated by the system (such as by plastic deformation or sliding friction), the system is said to be nonconservative. An example of a nonconservative system is shown in Figure 8.6: “Nonconservative (Path-Dependent) Behavior”. An analysis of a conservative system is path independent: loads can usually be applied in any order and in any number of increments without affecting the end results. Conversely, an analysis of a nonconservative system is path dependent: the actual load-response history of the system must be followed closely to obtain accurate results. An analysis can also be path dependent if more than one solution could be valid for a given load level (as in a snap-through analysis). Path dependent problems usually require that loads be applied slowly (that is, using many substeps) to the final load value.
Figure 8.6 Nonconservative (Path-Dependent) Behavior
8.1.2.2. Substeps When using multiple substeps, you need to achieve a balance between accuracy and economy: more substeps (that is, small time step sizes) usually result in better accuracy, but at a cost of increased run times. ANSYS provides automatic time stepping that is designed for this purpose. Automatic time stepping adjusts the time step size as needed, gaining a better balance between accuracy and economy. Automatic time stepping activates the ANSYS program's bisection feature. Bisection provides a means of automatically recovering from a convergence failure. This feature will cut a time step size in half whenever equilibrium iterations fail to converge and automatically restart from the last converged
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–5
Chapter 8: Nonlinear Structural Analysis substep. If the halved time step again fails to converge, bisection will again cut the time step size and restart, continuing the process until convergence is achieved or until the minimum time step size (specified by you) is reached.
8.1.2.3. Load Direction in a Large-Deflection Analysis Consider what happens to loads when your structure experiences large deflections. In many instances, the loads applied to your system maintain constant direction no matter how the structure deflects. In other cases, forces will change direction, "following" the elements as they undergo large rotations. The ANSYS program can model both situations, depending on the type of load applied. Accelerations and concentrated forces maintain their original orientation, regardless of the element orientation. Pressure loads always act normal to the deflected element surface, and can be used to model "following" forces. Figure 8.7: “Load Directions Before and After Deflection” illustrates constant-direction and following forces. Note — Nodal coordinate system orientations are not updated in a large deflection analysis. Calculated displacements are therefore output in the original directions.
Figure 8.7 Load Directions Before and After Deflection
8.1.2.4. Nonlinear Transient Analyses The procedure for analyzing nonlinear transient behavior is similar to that used for nonlinear static behavior: you apply the load in incremental steps, and the program performs equilibrium iterations at each step. The main difference between the static and transient procedures is that time-integration effects can be activated in the transient analysis. Thus, "time" always represents actual chronology in a transient analysis. The automatic time stepping and bisection feature is also applicable for transient analyses.
8.2. Using Geometric Nonlinearities Small deflection and small strain analyses assume that displacements are small enough that the resulting stiffness changes are insignificant.
8–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.2: Using Geometric Nonlinearities In contrast, large strain analyses account for the stiffness changes that result from changes in an element's shape and orientation. By issuing NLGEOM,ON (GUI path Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) or Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options), you activate large strain effects in those element types that support this feature. The large strain feature is available in most of the solid elements (including all of the large strain and hyperelastic elements), as well as in most of the shell and beam elements. Large strain effects are not available in the ANSYS Professional program. The large strain procedure places no theoretical limit on the total rotation or strain experienced by an element. (Certain ANSYS element types will be subject to practical limitations on total strain - see below.) However, the procedure requires that strain increments must be restricted to maintain accuracy. Thus, the total load should be broken into smaller steps.
8.2.1. Stress-Strain In large strain solutions, all stress-strain input and results will be in terms of true stress and true (or logarithmic) strain. (In one dimension, true strain would be expressed as ε = ln ( l / l 0). For small-strain regions of response, true strain and engineering strain are essentially identical.) To convert strain from small (engineering) strain to logarithmic strain, use εln = ln (1 + εeng). To convert from engineering stress to true stress, use σtrue = σeng (1 + εeng). (This stress conversion is valid only for incompressible plasticity stress-strain data.)
8.2.1.1. Large Deflections with Small Strain This feature is available in all beam and most shell elements, as well as in a number of the nonlinear elements. Issue NLGEOM,ON (Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) or Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options) to activate large deflection effects for those elements that are designed for small strain analysis types that support this feature.
8.2.2. Stress Stiffening The out-of-plane stiffness of a structure can be significantly affected by the state of in-plane stress in that structure. This coupling between in-plane stress and transverse stiffness, known as stress stiffening, is most pronounced in thin, highly stressed structures, such as cables or membranes. A drumhead, which gains lateral stiffness as it is tightened, would be a common example of a stress-stiffened structure. Even though stress stiffening theory assumes that an element's rotations and strains are small, in some structural systems (such as in Figure 8.8: “Stress-Stiffened Beams” (a)), the stiffening stress is only obtainable by performing a large deflection analysis. In other systems (such as in Figure 8.8: “Stress-Stiffened Beams” (b)), the stiffening stress is obtainable using small deflection, or linear, theory.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–7
Chapter 8: Nonlinear Structural Analysis
Figure 8.8 Stress-Stiffened Beams
To use stress stiffening in the second category of systems, you must issue PSTRES,ON (GUI path Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options) in your first load step. Large strain and large deflection procedures include initial stress effects as a subset of their theory. For most elements, initial stiffness effects are automatically included when large deformation effects are activated [NLGEOM,ON] (GUI path Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) or Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options).
8.2.3. Spin Softening Spin softening adjusts (softens) the stiffness matrix of a rotating body for dynamic mass effects. The adjustment approximates the effects of geometry changes due to large deflection circumferential motion in a small deflection analysis. It is usually used in conjunction with prestressing [PSTRES] (GUI path Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options), which is caused by centrifugal force in the rotating body. It should not be used with the other deformation nonlinearities, large deflection, or large strain. Spin softening is activated by the KSPIN field on the OMEGA and CMOMEGA commands (GUI path Main Menu> Preprocessor> Loads> Define Loads> Apply> Structural> Inertiav Angular Velocity).
8.3. Modeling Material Nonlinearities A number of material-related factors can cause your structure's stiffness to change during the course of an analysis. Nonlinear stress-strain relationships of plastic, multilinear elastic, and hyperelastic materials will cause a structure's stiffness to change at different load levels (and, typically, at different temperatures). Creep, viscoplasticity, and viscoelasticity will give rise to nonlinearities that can be time-, rate-, temperature-, and stress-related. Swelling will induce strains that can be a function of temperature, time, neutron flux level (or some analogous quantity), and stress. Any of these kinds of material properties can be incorporated into an ANSYS analysis if you use appropriate element types.
8.3.1. Nonlinear Materials If a material displays nonlinear or rate-dependent stress-strain behavior, then you must use the TB family of commands [TB, TBTEMP, TBDATA, TBPT, TBCOPY, TBLIST, TBPLOT, TBDELE] (GUI path Main Menu> Preprocessor> Material Props> Material Models> Structural> Nonlinear) to define the nonlinear material property relationships in terms of a data table. The exact form of these commands varies depending on the type of non8–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities linear material behavior being defined. The different material behavior options are described briefly below. See Data Tables - Implicit Analysis in the ANSYS Elements Reference for specific details for each material behavior type.
8.3.1.1. Plasticity Most common engineering materials exhibit a linear stress-strain relationship up to a stress level known as the proportional limit. Beyond this limit, the stress-strain relationship will become nonlinear, but will not necessarily become inelastic. Plastic behavior, characterized by nonrecoverable strain, begins when stresses exceed the material's yield point. Because there is usually little difference between the yield point and the proportional limit, the ANSYS program assumes that these two points are coincident in plasticity analyses (see Figure 8.9: “Elastoplastic Stress-Strain Curve”). Plasticity is a nonconservative, path-dependent phenomenon. In other words, the sequence in which loads are applied and in which plastic responses occur affects the final solution results. If you anticipate plastic response in your analysis, you should apply loads as a series of small incremental load steps or time steps, so that your model will follow the load-response path as closely as possible. The maximum plastic strain is printed with the substep summary information in your output (Jobname.OUT).
Figure 8.9 Elastoplastic Stress-Strain Curve
The automatic time stepping feature [AUTOTS] (GUI path Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) or Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc>Time and Substps) will respond to plasticity after the fact, by reducing the load step size after a load step in which a large number of equilibrium iterations was performed or in which a plastic strain increment greater than 15% was encountered. If too large a step was taken, the program will bisect and resolve using a smaller step size. Other kinds of nonlinear behavior might also occur along with plasticity. In particular, large deflection and large strain geometric nonlinearities will often be associated with plastic material response. If you expect large deformations in your structure, you must activate these effects in your analysis with the NLGEOM command (GUI path Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) or Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options). For large strain analyses, material stress-strain properties must be input in terms of true stress and logarithmic strain.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–9
Chapter 8: Nonlinear Structural Analysis
8.3.1.1.1. Plastic Material Options Several options are available for describing plasticity behavior. You may incorporate other options into the program by using User Programmable Features (see the Guide to ANSYS User Programmable Features). The Bilinear Kinematic Hardening (BKIN) option assumes the total stress range is equal to twice the yield stress, so that the Bauschinger effect is included (see Figure 8.11: “Bauschinger Effect”). This option is recommended for general small-strain use for materials that obey von Mises yield criteria (which includes most metals). It is not recommended for large-strain applications. You can combine the BKIN option with creep and Hill anisotropy options to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. Stress-strain-temperature data are demonstrated in the following example. Figure 8.10: “Kinematic Hardening”(a) illustrates a typical display [TBPLOT] of bilinear kinematic hardening properties. MPTEMP,1,0,500 MP,EX,1,12E6,-8E3 TB,BKIN,1,2 TBTEMP,0.0 TBDATA,1,44E3,1.2E6 TBTEMP,500 TBDATA,1,29.33E3,0.8E6 TBLIST,BKIN,1 /XRANGE,0,0.01 TBPLOT,BKIN,1
! ! ! ! ! ! ! ! ! !
Define temperatures for Young's modulus C0 and C1 terms for Young's modulus Activate a data table Temperature = 0.0 Yield = 44,000; Tangent modulus = 1.2E6 Temperature = 500 Yield = 29,330; Tangent modulus = 0.8E6 List the data table X-axis of TBPLOT to extend from varepsilon=0 to 0.01 Display the data table
See the MPTEMP, MP, TB, TBTEMP, TBDATA, TBLIST, /XRANGE, and TBPLOT command descriptions for more information.
Figure 8.10 Kinematic Hardening
(a) Bilinear kinematic hardening, (b) Multilinear kinematic hardening
8–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
Figure 8.11 Bauschinger Effect
The Multilinear Kinematic Hardening (KINH and MKIN) options use the Besseling model, also called the sublayer or overlay model, so that the Bauschinger effect is included. KINH is preferred for use over MKIN because it uses Rice's model where the total plastic strains remain constant by scaling the sublayers. KINH allows you to define more stress-strain curves (40 vs. 5), and more points per curve (20 vs. 5). Also, when KINH is used with LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189, you can use TBOPT = 4 (or PLASTIC) to define the stress vs. plastic strain curve. For either option, if you define more than one stressstrain curve for temperature dependent properties, then each curve should contain the same number of points. The assumption is that the corresponding points on the different stress-strain curves represent the temperature dependent yield behavior of a particular sublayer. These options are not recommended for large-strain analyses. You can combine either of these options with the Hill anisotropy option to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. Figure 8.10: “Kinematic Hardening”(b) illustrates typical stress-strain curves for the MKIN option. A typical stress-strain temperature data input using KINH is demonstrated by this example. TB,KINH,1,2,3 TBTEMP,20.0 TBPT,,0.001,1.0 TBPT,,0.1012,1.2 TBPT,,0.2013,1.3 TBTEMP,40.0 TBPT,,0.008,0.9 TBPT,,0.09088,1.0 TBPT,,0.12926,1.05
! ! ! ! ! ! ! ! !
Activate a data table Temperature = 20.0 Strain = 0.001, Stress = 1.0 Strain = 0.1012, Stress = 1.2 Strain = 0.2013, Stress = 1.3 Temperature = 40.0 Strain = 0.008, Stress = 0.9 Strain = 0.09088, Stress = 1.0 Strain = 0.12926, Stress = 1.05
In this example, the third point in the two stress-strain curves defines the temperature-dependent yield behavior of the third sublayer. A typical stress- plastic strain temperature data input using KINH is demonstrated by this example. TB,KINH,1,2,3,PLASTIC TBTEMP,20.0 TBPT,,0.000,1.0 TBPT,,0.1012,1.2 TBPT,,0.2013,1.3 TBTEMP,40.0 TBPT,,0.008,0.9 TBPT,,0.09088,1.0 TBPT,,0.12926,1.05
! Activate a data table ! Temperature = 20.0 ! Plastic Strain = 0.0000, ! Plastic Strain = 0.1000, ! Plastic Strain = 0.2000, ! Temperature = 40.0 ! Plastic Strain = 0.0000, ! Plastic Strain = 0.0900, ! Plastic Strain = 0.1290,
Stress = 1.0 Stress = 1.2 Stress = 1.3 Stress = 0.9 Stress = 1.0 Stress = 1.05
In this example, the stress - strain behavior is the same as the previous sample, except now the strain value is the plastic strain. The plastic strain can be converted from total strain as follows:
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–11
Chapter 8: Nonlinear Structural Analysis Plastic Stain = (total strain - stress)/Young's Modulus. A typical stress-strain temperature data input using MKIN is demonstrated by this example. MPTEMP,1,0,500 ! Define temperature-dependent EX, MP,EX,1,12E6,-8E3 ! as in BKIN example TB,MKIN,1,2 ! Activate a data table TBTEMP,,STRAIN ! Next TBDATA values are strains TBDATA,1,3.67E-3,5E-3,7E-3,10E-3,15E-3 ! Strains for all temps TBTEMP,0.0 ! Temperature = 0.0 TBDATA,1,44E3,50E3,55E3,60E3,65E3 ! Stresses at temperature = 0.0 TBTEMP,500 ! Temperature = 500 TBDATA,1,29.33E3,37E3,40.3E3,43.7E3,47E3 ! Stresses at temperature = 500 /XRANGE,0,0.02 TBPLOT,MKIN,1
Please see the MPTEMP, MP, TB, TBPT, TBTEMP, TBDATA, /XRANGE, and TBPLOT command descriptions for more information. The Nonlinear Kinematic Hardening (CHABOCHE) option uses the Chaboche model, which is a multi-component nonlinear kinematic hardening model that allows you to superpose several kinematic models. See the ANSYS, Inc. Theory Reference for details. Like the BKIN and MKIN options, you can use the CHABOCHE option to simulate monotonic hardening and the Bauschinger effect. This option also allows you to simulate the ratcheting and shakedown effect of materials. By combining the CHABOCHE option with isotropic hardening model options BISO, MISO, and NLISO, you have the further capability of simulating cyclic hardening or softening. You can also combine this option with the Hill anisotropy option to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. The model has 1 + 2 x n constants, where n is the number of kinematic models, and is defined by NPTS in the TB command. See the ANSYS, Inc. Theory Reference for details. You define the material constants using the TBTEMP and TBDATA commands. This model is suitable for large strain analysis. The following example is a typical data table with no temperature dependency and one kinematic model: TB,CHABOCHE,1 TBDATA,1,C1,C2,C3
! Activate CHABOCHE data table ! Values for constants C1, C2, and C3
The following example illustrates a data table of temperature dependent constants with two kinematic models at two temperature points: TB,CHABOCHE,1,2,2 TBTEMP,100 TBDATA,1,C11,C12,C13,C14,C15 TBTEMP,200 TBDATA,1,C21,C22,C23,C24,C25
! ! ! ! ! ! !
Activate CHABOCHE data table Define first temperature Values for constants C11, C12, C13, C14, and C15 at first temperature Define second temperature Values for constants C21, C22, C23, C24, and C25 at second temperature
Please see the TB, TBTEMP, and TBDATA command descriptions for more information. The Bilinear Isotropic Hardening (BISO) option uses the von Mises yield criteria coupled with an isotropic work hardening assumption. This option is often preferred for large strain analyses. You can combine BISO with Chaboche, creep, viscoplastic, and Hill anisotropy options to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. The Multilinear Isotropic Hardening (MISO) option is like the bilinear isotropic hardening option, except that a multilinear curve is used instead of a bilinear curve. This option is not recommended for cyclic or highly nonproportional load histories in small-strain analyses. It is, however, recommended for large strain analyses. The MISO option can contain up to 20 different temperature curves, with up to 100 different stress-strain points allowed 8–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities per curve. Strain points can differ from curve to curve. You can combine this option with nonlinear kinematic hardening (CHABOCHE) for simulating cyclic hardening or softening. You can also combine the MISO option with creep, viscoplastic, and Hill anisotropy options to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. The stress-straintemperature curves from the MKIN example would be input for a multilinear isotropic hardening material as follows: /prep7 MPTEMP,1,0,500 ! Define temperature-dependent EX, MPDATA,EX,1,,14.665E6,12.423e6 MPDATA,PRXY,1,,0.3 TB,MISO,1,2,5 TBTEMP,0.0 TBPT,DEFI,2E-3,29.33E3 TBPT,DEFI,5E-3,50E3 TBPT,DEFI,7E-3,55E3 TBPT,DEFI,10E-3,60E3 TBPT,DEFI,15E-3,65E3 TBTEMP,500 TBPT,DEFI,2.2E-3,27.33E3 TBPT,DEFI,5E-3,37E3 TBPT,DEFI,7E-3,40.3E3 TBPT,DEFI,10E-3,43.7E3 TBPT,DEFI,15E-3,47E3 /XRANGE,0,0.02 TBPLOT,MISO,1
! Activate a data table ! Temperature = 0.0 ! Strain, stress at temperature = 0
! Temperature = 500 ! Strain, stress at temperature = 500
See the MPTEMP, MP, TB, TBTEMP, TBPT, /XRANGE, and TBPLOT command descriptions for more information. The Nonlinear Isotropic Hardening (NLISO) option is based on the Voce hardening law (see the ANSYS, Inc. Theory Reference for details). The NLISO option is a variation of BISO where an exponential saturation hardening term is appended to the linear term (see Figure 8.12: “NLISO Stress-Strain Curve”).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–13
Chapter 8: Nonlinear Structural Analysis
Figure 8.12 NLISO Stress-Strain Curve
The advantage of this model is that the material behavior is defined as a specified function which has four material constants that you define through the TBDATA command. You can obtain the material constants by fitting material tension stress-strain curves. Unlike MISO, there is no need to be concerned about how to appropriately define the pairs of the material stress-strain points. However, this model is only applicable to the tensile curve like the one shown in Figure 8.12: “NLISO Stress-Strain Curve”. This option is suitable for large strain analyses. You can combine NLISO with Chaboche, creep, viscoplastic, and Hill anisotropy options to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. The following example illustrates a data table of temperature dependent constants at two temperature points: TB,NLISO,1 TBTEMP,100 TBDATA,1,C11,C12,C13,C14 TBTEMP,200 TBDATA,1,C21,C22,C23,C24
! ! ! ! ! ! !
Activate NLISO data table Define first temperature Values for constants C11, C12, C13, C14 at first temperature Define second temperature Values for constants C21, C22, C23, C24 at second temperature
Please see the TB, TBTEMP, and TBDATA command descriptions for more information. The Anisotropic (ANISO) option allows for different bilinear stress-strain behavior in the material x, y, and z directions as well as different behavior in tension, compression, and shear. This option is applicable to metals that have undergone some previous deformation (such as rolling). It is not recommended for cyclic or highly nonproportional load histories since work hardening is assumed. The yield stresses and slopes are not totally independent (see the ANSYS, Inc. Theory Reference for details).
8–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities To define anisotropic material plasticity, use MP commands (Main Menu> Solution> Load Step Opts> Other> Change Mat Props) to define the elastic moduli (EX, EY, EZ, NUXY, NUYZ, and NUXZ). Then, issue the TB command [TB,ANISO] followed by TBDATA commands to define the yield points and tangent moduli. (See Nonlinear StressStrain Materials in the ANSYS Elements Reference for more information.) The Hill Anisotropy (HILL) option, when combined with other material options simulates plasticity, viscoplasticity, and creep - all using the Hill potential. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. The Hill potential may only be used with the following elements: PLANE42, SOLID45, PLANE82, SOLID92, SOLID95, LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189. The Drucker-Prager (DP) option is applicable to granular (frictional) material such as soils, rock, and concrete, and uses the outer cone approximation to the Mohr-Coulomb law. MP,EX,1,5000 MP,NUXY,1,0.27 TB,DP,1 TBDATA,1,2.9,32,0
! Cohesion = 2.9 (use consistent units), ! Angle of internal friction = 32 degrees, ! Dilatancy angle = 0 degrees
See the MP, TB, and TBDATA command descriptions for more information. The Cast Iron (CAST, UNIAXIAL) option assumes a modified von Mises yield surface, which consists of the von Mises cylinder in compression and a Rankine cube in tension. It has different yield strengths, flows, and hardenings in tension and compression. Elastic behavior is isotropic, and is the same in tension and compression. The TB,CAST command is used to input the plastic Poisson's ration in tension, which can be temperature dependent. Use the TB,UNIAXIAL command to enter the yield and hardening in tension and compression. Note — Cast Iron is intended for monotonic loading only and cannot be used with any other material model. TB,CAST,1,,,ISOTROPIC TBDATA,1,0.04 TB,UNIAXIAL,1,1,5,TENSION TBTEMP,10 TBPT,,0.550E-03,0.813E+04 TBPT,,0.100E-02,0.131E+05 TBPT,,0.250E-02,0.241E+05 TBPT,,0.350E-02,0.288E+05 TBPT,,0.450E-02,0.322E+05 TB,UNIAXIAL,1,1,5,COMPRESSION TBTEMP,10 TBPT,,0.203E-02,0.300E+05 TBPT,,0.500E-02,0.500E+05 TBPT,,0.800E-02,0.581E+05 TBPT,,0.110E-01,0.656E+05 TBPT,,0.140E-01,0.700E+05
Figure 8.13: “Cast Iron Plasticity” illustrates the idealized response of gray cast iron in tension and compression.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–15
Chapter 8: Nonlinear Structural Analysis
Figure 8.13 Cast Iron Plasticity Compression
σc
σt
Tension ε
See the TB and TBPT command descriptions for more information.
8.3.1.2. Multilinear Elasticity The Multilinear Elastic (MELAS) material behavior option describes a conservative (path-independent) response in which unloading follows the same stress-strain path as loading. Thus, relatively large load steps might be appropriate for models that incorporate this type of material nonlinearity. Input format is similar to that required for the multilinear isotropic hardening option, except that the TB command now uses the label MELAS.
8.3.1.3. User Defined Material The User Defined (USER) material option describes input parameters for defining a material model based on either of two subroutines, which are ANSYS user-programmable features (see the Guide to ANSYS User Programmable Features). The choice of which subroutine to use is based on which element you are using. The USER option works with the USERMAT subroutine in defining any material model (except incompressible materials), when you use any of the following elements: LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189. The USER option works with the USERPL subroutine in defining plasticity or viscoplasticity material models, when you use any of the following elements: LINK1, PLANE2, LINK8, PIPE20, BEAM23, BEAM24, PLANE42, SHELL43, SOLID45, SHELL51, PIPE60, SOLID62, SOLID65, PLANE82, SHELL91, SOLID92, SHELL93, SOLID95. To access the user material option, issue the TB,USER command to define the material number, the number of temperatures, and the number of data points. Then define the temperatures and material constants using the TBTEMP and TBDATA commands. The following example illustrates defining a material with two temperatures and four data points: TB,USER,1,2,4
TBTEMP,1.0 TBDATA,1,19e5,0.3,1e3,100, TBTEMP,2.0
8–16
! ! ! ! ! ! ! ! !
Define material 1 as user material with 2 temperatures and 4 data points at each temperature point. First temperature. 4 material constants for first temperature. Second temperature.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities TBDATA,1,21e5,0.3,2e3,100,
! 4 material constants for ! second temperature.
If you use state variables in the USERMAT subroutine, you must first define the number of state variables using the TB,STATE command. You then use the TBDATA command to initialize the value of the state variables, as shown in the following example: TB,STATE,1,,4, TBDATA,1,C1,C2,C3,C4,
! Define material 1, which ! has 4 state variables. ! Initialize the 4 state variables.
You cannot use TB,STATE in the USERPL subroutine. See the TB, and TBDATA command descriptions for more information.
8.3.1.4. Hyperelasticity A material is said to be hyperelastic if there exists an elastic potential function (or strain energy density function), which is a scalar function of one of the strain or deformation tensors, whose derivative with respect to a strain component determines the corresponding stress component. Hyperelasticity can be used to analyze rubber-like materials (elastomers) that undergo large strains and displacements with small volume changes (nearly incompressible materials). Large strain theory is required [NLGEOM,ON]. A representative hyperelastic structure (a balloon seal) is shown in Figure 8.14: “Hyperelastic Structure”.
Figure 8.14 Hyperelastic Structure
There are two types of elements suitable for simulating hyperelastic materials: the hyperelastic elements (HYPER56, HYPER58, HYPER74, HYPER158), and all of the 18x family of elements except the link and beam elements (SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, and SOLID187). For further details on the use of hyperelastic elements, and on mixed formulation of the 18x solid elements, see Mixed u-P Formulation Elements in the ANSYS Elements Reference. The material response in ANSYS hyperelastic models is always assumed to be isotropic and isothermal. Because of this assumption, the strain energy potentials are expressed in terms of strain invariants. Unless indicated otherwise, the hyperelastic materials are also assumed to be nearly or purely incompressible. Material thermal expansion is also assumed to be isotropic.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–17
Chapter 8: Nonlinear Structural Analysis ANSYS supports several options of strain energy potentials for the simulation of incompressible or nearly incompressible hyperelastic materials. All options are applicable to elements SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, and SOLID187. Access these options through the TBOPT argument of TB,HYPER. One of the options, the Mooney-Rivlin option, is also applicable to elements HYPER56, HYPER58, HYPER74, HYPER158, and explicit dynamics elements PLANE162, SHELL163, SOLID164, and SOLID168. To access the MooneyRivlin option for these elements, use TB,MOONEY. ANSYS provides tools to help you determine the coefficients for all of the hyperelastic options defined by TB,HYPER. The TBFT command allows you to compare your experimental data with existing material data curves and visually “fit” your curve for use in the TB command. All of the TBFT command capability is available via either batch or interactive (GUI) mode. See Material Curve Fitting (also in this manual) for more information. Each of the hyperelastic options is presented in the following sections.
8.3.1.4.1. Mooney-Rivlin Hyperelastic Option (TB,HYPER) Note that this section applies to using the Mooney-Rivlin option with elements SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, and SOLID187. If you want to use the Mooney-Rivlin option with elements HYPER56, HYPER58, HYPER74, HYPER158, PLANE162, SHELL163, SOLID164, or SOLID168, see Section 8.3.1.4.11: Mooney-Rivlin Hyperelastic Option (TB,MOONEY). The Mooney-Rivlin option (TB,HYPER,,,,MOONEY), which is the default, allows you to define 2, 3, 5, or 9 parameters through the NPTS argument of the TB command. For example, to define a 5 parameter model you would issue TB,HYPER,1,,5,MOONEY. The 2 parameter Mooney-Rivlin option has an applicable strain of about 100% in tension and 30% in compression. Compared to the other options, higher orders of the Mooney-Rivlin option may provide better approximation to a solution at higher strain. The following example input listing shows a typical use of the Mooney-Rivlin option with 3 parameters: TB,HYPER,1,,3,MOONEY TBDATA,1,0.163498 TBDATA,2,0.125076 TBDATA,3,0.014719 TBDATA,4,6.93063E-5
!Activate 3 parameter Mooney-Rivlin data table !Define c10 !Define c01 !Define c11 !Define incompressibility parameter !(as 2/K, K is the bulk modulus)
Refer to Mooney-Rivlin Hyperelastic Material (TB,HYPER) in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.2. Ogden Hyperelastic Option The Ogden option (TB,HYPER,,,,OGDEN) allows you to define an unlimited number of parameters through the NPTS argument of the TB command. For example, to define a 3 parameter model, use TB,HYPER,1,,3,OGDEN. Compared to the other options, the Ogden option usually provides the best approximation to a solution at larger strain levels. The applicable strain level can be up to 700%. A higher parameter value can provide a better fit to the exact solution. It may however cause numerical difficulties in fitting the material constants, and it requires enough data to cover the whole range of deformation for which you may be interested. For these reasons, a high parameter value is not recommended. The following example input listing shows a typical use of the Ogden option with 2 parameters:
8–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities TB,HYPER,1,,2,OGDEN TBDATA,1,0.326996 TBDATA,2,2 TBDATA,3,-0.250152 TBDATA,4,-2 TBDATA,5,6.93063E-5
!Activate 2 parameter Ogden data table !Define µ1 !Define 1 !Define µ2 !Define 2 !Define incompressibility parameter !(as 2/K, K is the bulk modulus) !(Second incompressibility parameter d2 is zero)
Refer to Ogden Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.3. Neo-Hookean Hyperelastic Option The Neo-Hookean option (TB,HYPER,,,,NEO) represents the simplest form of strain energy potential, and has an applicable strain range of 20-30%. An example input listing showing a typical use of the Neo-Hookean option is presented below. TB,HYPER,1,,,NEO TBDATA,1,0.577148 TBDATA,2,7.0e-5
!Activate Neo-Hookean data table !Define mu shear modulus !Define incompressibility parameter !(as 2/K, K is the bulk modulus)
Refer to Neo-Hookean Hyperelastic Material in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.4. Polynomial Form Hyperelastic Option The polynomial form option (TB,HYPER,,,,POLY) allows you to define an unlimited number of parameters through the NPTS argument of the TB command. For example, to define a 3 parameter model you would issue TB,HYPER,1,,3,POLY. Similar to the higher order Mooney-Rivlin options, the polynomial form option may provide a better approximation to a solution at higher strain. For NPTS = 1 and constant c01 = 0, the polynomial form option is equivalent to the Neo-Hookean option (see Section 8.3.1.4.3: Neo-Hookean Hyperelastic Option for a sample input listing). Also, for NPTS = 1, it is equivalent to the 2 parameter Mooney-Rivlin option. For NPTS = 2, it is equivalent to the 5 parameter Mooney-Rivlin option, and for NPTS = 3, it is equivalent to the 9 parameter Mooney-Rivlin option (see Section 8.3.1.4.1: Mooney-Rivlin Hyperelastic Option (TB,HYPER) for a sample input listing). Refer to Polynomial Form Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.5. Arruda-Boyce Hyperelastic Option The Arruda-Boyce option (TB,HYPER,,,,BOYCE) has an applicable strain level of up to 300%. An example input listing showing a typical use of the Arruda-Boyce option is presented below. TB,HYPER,1,,,BOYCE TBDATA,1,200.0 TBDATA,2,5.0 TBDATA,3,0.001
!Activate Arruda-Boyce data table !Define initial shear modulus !Define limiting network stretch !Define incompressibility parameter !(as 2/K, K is the bulk modulus)
Refer to Arruda-Boyce Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–19
Chapter 8: Nonlinear Structural Analysis
8.3.1.4.6. Gent Hyperelastic Option The Gent option (TB,HYPER,,,,GENT) has an applicable strain level of up to 300%. An example input listing showing a typical use of the Gent option is presented below. TB,HYPER,1,,,GENT TBDATA,1,3.0 TBDATA,2,42.0 TBDATA,3,0.001
!Activate Gent data table !Define initial shear modulus !Define limiting I1 - 3 !Define incompressibility parameter !(as 2/K, K is the bulk modulus)
Refer to Gent Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.7. Yeoh Hyperelastic Option The Yeoh option (TB,HYPER,,,,YEOH) is a reduced polynomial form of the hyperelasticity option TB,HYPER,,,,POLY. An example of a 2 term Yeoh model is TB,HYPER,1,,2,YEOH. Similar to the polynomial form option, the higher order terms may provide a better approximation to a solution at higher strain. For NPTS = 1, the Yeoh form option is equivalent to the Neo-Hookean option (see Section 8.3.1.4.3: Neo-Hookean Hyperelastic Option for a sample input listing). The following example input listing shows a typical use of the Yeoh option with 2 terms and 1 incompressibility term: TB,HYPER,1,,2,YEOH TBDATA,1,0.163498 TBDATA,2,0.125076 TBDATA,3,6.93063E-5
!Activate 2 term Yeoh data table !Define C1 !Define C2 !Define first incompressibility parameter
Refer to Yeoh Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.8. Blatz-Ko Foam Hyperelastic Option The Blatz-Ko option (TB,HYPER,,,,BLATZ) is the simplest option for simulating the compressible foam type of elastomer. This option is analogous to the Neo-Hookean option of incompressible hyperelastic materials. An example input listing showing a typical use of the Blatz-Ko option is presented below. TB,HYPER,1,,,BLATZ TBDATA,1,5.0
!Activate Blatz-Ko data table !Define initial shear modulus
Refer to Blatz-Ko Foam Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.9. Ogden Compressible Foam Hyperelastic Option The Ogden compressible foam option (TB,HYPER,,,,FOAM) simulates highly compressible foam material. An example of a 3 parameter model is TB,HYPER,1,,3,FOAM. Compared to the Blatz-Ko option, the Ogden foam option usually provides the best approximation to a solution at larger strain levels. The higher the number of parameters, the better the fit to the experimental data. It may however cause numerical difficulties in fitting the material constants, and it requires sufficient data to cover the whole range of deformation for which you may be interested. For these reasons, a high parameter value is not recommended. 8–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities The following example input listing shows a typical use of the Ogden foam option with 2 parameters: TB,HYPER,1,,2,FOAM TBDATA,1,1.85 TBDATA,2,4.5 TBDATA,3,-9.20 TBDATA,4,-4.5 TBDATA,5,0.92 TBDATA,6,0.92
!Activate 2 parameter Ogden foam data table !Define µ1 !Define 1 !Define µ2 !Define 2 !Define first compressibility parameter !Define second compressibility parameter
Refer to Ogden Compressible Foam Hyperelastic Material Constants in the ANSYS Elements Reference for a description of the material constants required for this option.
8.3.1.4.10. User-Defined Hyperelastic Option The User option (TB,HYPER,,,,USER) allows you to use the subroutine USERHYPER to define the derivatives of the strain energy potential with respect to the strain invariants. Refer to the Guide to ANSYS User Programmable Features for a detailed description on writing a user hyperelasticity subroutine.
8.3.1.4.11. Mooney-Rivlin Hyperelastic Option (TB,MOONEY) Note that this section applies to using the Mooney-Rivlin option with elements HYPER56, HYPER58, HYPER74, HYPER158, PLANE162, SHELL163, SOLID164, or SOLID168. If you want to use the Mooney-Rivlin option with elements SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, and SOLID187, see Section 8.3.1.4.1: Mooney-Rivlin Hyperelastic Option (TB,HYPER). ANSYS element types HYPER56, HYPER58, HYPER74, and HYPER158 use up to a nine-term Mooney-Rivlin elastic potential function. If you already know the values for two-term, three-term, five-term, or nine-term MooneyRivlin constants, you can enter them directly with the TB family of commands. (See the ANSYS, Inc. Theory Reference for information on the Mooney-Rivlin function.) For these element types, you can also specify the material function as a User Programmable Feature (see the Guide to ANSYS User Programmable Features). An example input listing showing a typical use of the Mooney-Rivlin for these elements is presented below : MP,NUXY,1,0.49999 ! NUXY should be almost equal to, but less than 0.5 TB,MOONEY,1,1 TBDATA,1,0.163498 TBDATA,2,0.125076 TBDATA,3,-0.0047583 TBDATA,4,0.014719 TBDATA,6,0.0003882 ! (Constants 5, 7, 8, and 9 default to 0.0 in this example)
Refer to Mooney-Rivlin Hyperelastic Material Constants (TB,MOONEY) in the ANSYS Elements Reference for a description of the constants required as input for this option. The Mooney-Rivlin constants for any given hyperelastic material are not generally available in the open literature. Consequently, you can use the *MOONEY command to automatically determine a set of Mooney-Rivlin constants from a set of known experimental test data. Sometimes the manufacturer of the material will be able to supply some or all of the needed test data, but you might find that you need to obtain more data from a testing laboratory. Hyperelastic material behavior is much more complicated than typical metallic material behavior. Hyperelastic stress-strain relationships usually differ significantly for tension, compression, and shear modes of deformation. Therefore, using *MOONEY to generate a generally applicable hyperelastic material model will require test data that encompasses all possible modes of deformation: tension, compression, and shear. See the ANSYS, Inc. Theory Reference for a discussion of hyperelastic test methods and equivalent deformation modes. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–21
Chapter 8: Nonlinear Structural Analysis If an incomplete set of data is provided (for instance, if only uniaxial tension data are available), the program can still determine usable hyperelastic material properties. However, in such cases the deformations experienced in the model should be limited to be of the same nature as those experienced in the tests. In other words, the test data should represent all modes of deformation and ranges of response (strain) that will be experienced in the model. This advice is simply common sense - if you do not know how the material behaves in a certain mode of deformation or range of strain, you cannot accurately predict the behavior of a part that experiences such deformations or strains. For example, if all you have is uniaxial tension data, do not model a part that experiences significant shear deformations. If your test data extend only from 0% to 100% strain, do not model a part that experiences 150% strain. If, after reviewing your analysis, you discover that the available test data do not adequately characterize the model's response, get more test data! You can use the *MOONEY command to automatically determine a set of Mooney-Rivlin constants from experimental test data. ANSYS determines the constants and stores them in the database, and in an array parameter. Additionally, it writes an ASCII file (Jobname.TB) that records the Mooney-Rivlin constants in the form of a series of TB and TBDATA commands. Once such a file exists, you can use it in future analyses to define that same material's Mooney-Rivlin constants - you do not need to use the *MOONEY command every time to regenerate these constants. Determining and Applying Mooney-Rivlin Constants The procedure for determining and applying Mooney-Rivlin constants consists of five main steps: 1.
Dimension all arrays that will be used for data input, Mooney-Rivlin constant storage, and calculated stress-strain evaluation.
2.
Fill the input-data arrays with engineering stress and strain test data.
3.
Determine the Mooney-Rivlin constants automatically.
4.
Evaluate the quality of the automatically determined Mooney-Rivlin constants.
5.
Apply the Mooney-Rivlin constants in your analysis.
Step 1: Dimension the Arrays Command(s): *DIM GUI: Utility Menu> Parameters> Array Parameters> Define/Edit You must dimension arrays before using the *MOONEY command. In most cases, you will need to dimension at least six different arrays. (You can give these arrays any valid parameter names, but for convenience, we will use specific array names, such as STRAIN, STRESS, and so on, in our discussion. You can substitute any other valid parameter names that you like.) The arrays are STRAIN, STRESS, CONST, CALC, SORTSN, and SORTSS. STRAIN Array: An array of engineering strain data from mechanical material tests, arranged in three columns: •
Column 1: uniaxial tension and/or compression data
•
Column 2: equibiaxial tension and/or compression data
•
Column 3: shear data (planar tension and/or compression)
This array has the dimensions N x 3, where N equals the maximum number of data points in any one of the three columns. For example, if you have 20 data points from uniaxial tension/compression tests and 10 data points from shear tests, N = 20. This array must always be N x 3, even if fewer than three types of test data are available. Although it might be preferable to input the data points in order of ascending strain values, it is not necessary to do so.
8–22
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities STRESS Array: An array of engineering stress data from mechanical material tests input stress-data array, also of dimension N x 3. You must input stress data points in the same order as the corresponding strain-data input. CONST Array: A Mooney-Rivlin constant array of dimension M x 1, where M equals the desired number of Mooney-Rivlin constants. (M must be either 2, 5, or 9; any other value will produce an error message when *MOONEY is invoked.) You actually tell the program in this dimensioning operation how many Mooney-Rivlin constants you want. The *MOONEY command later reads the dimensions of this array to determine how many Mooney-Rivlin constants to generate, and then writes the values of those constants to this array. How many Mooney-Rivlin constants should you use? As a rule of thumb, you should have at least twice as many data points (N, as defined above) as the desired number of Mooney-Rivlin constants. Using more terms will usually improve the statistical quality of your curve fit (that is, it will probably be more tightly fitted through the data points), but the overall shape of the curve might be worse than that obtained with fewer terms. As a practical matter, you should probably try two-term, five-term, and nine-term functions in sequence, and examine the resulting stress-strain curves to decide which function gives you the best combination of tight fit and satisfactory curve shape.
Table 8.1 Suggested Mooney-Rivlin Constants Number of Points in the Stress-strain Curve
Suggested Mooney-Rivlin Function
No inflection points (that is, single curvature)
Two-term
One inflection point (that is, double curvature)
Five-term
Two inflection points
Nine-term
Figure 8.15 Typical Hyperelastic Stress-Strain Curves
CALC Array: An output stress-data array of dimension N x 3 (where N is as described above), in which sorted calculated stress values are stored. These stress values will be sorted into the same order as their corresponding sorted strain values (which will be sorted into ascending order). SORTSN Array: An array of dimension N x 3 in which sorted input strain data are stored. SORTSS Array: An array of dimension N x 3 in which sorted input stress data are stored. For example, if your test data contained up to 20 data points for any one test type, and if you wanted to generate a five-term set of Mooney-Rivlin constants, you might issue the following commands to dimension the necessary arrays (remember that you can substitute any valid parameter names for the ones shown here): *DIM,STRAIN,,20,3 *DIM,STRESS,,20,3 *DIM,CONST,,5,1 *DIM,CALC,,20,3 *DIM,SORTSN,,20,3 *DIM,SORTSS,,20,3
! ! ! ! ! !
Dim. Dim. Dim. Dim. Dim. Dim.
array array array array array array
(STRAIN) for 20 input strain-data points (STRESS) for input stress data (20 pts.) (CONST) for 5-term M-R constants (CALC) for sorted calculated stresses (SORTSN) for sorted input strain data (SORTSS) for sorted input stress data
See the *DIM command description for more information.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–23
Chapter 8: Nonlinear Structural Analysis Step 2: Fill the Input-Data Arrays Once you have dimensioned your arrays, you can then fill the STRAIN and STRESS arrays with test data using the *SET command (GUI path Utility Menu> Parameters> Scalar Parameters). (Again, remember that you can give these arrays any valid parameter names; particular array names are used here only for the convenience of this discussion.) Note — The *MOONEY command interprets all input stress and strain data as engineering stress and engineering strain. These arrays are of dimension N x 3, with each column of the arrays containing data from one type of test, in this order: •
First column: Uniaxial tension and/or uniaxial compression
•
Second column: Equibiaxial tension and/or equibiaxial compression
•
Third column: Shear (planar tension or compression)
Note that these do not have a 1:1 relationship with the modes of deformation and their equivalencies. The first mode of deformation, uniaxial tension, has equibiaxial compression as its equivalency, but the first column of the array contains data from uniaxial tension and/or uniaxial compression. Likewise, the second mode of deformation, equibiaxial tension, has uniaxial compression as its equivalency, but the second column of the array contains data from equibiaxial tension and/or equibiaxial compression.
Table 8.2 Data Locations in Stress and Strain Input Arrays Mode of Deformation
Equivalent Test Types
Array Location for Test Data
Uniaxial tension
Uniaxial tension Equibiaxial compression
Column one Column two
Equibiaxial tension
Equibiaxial tension Uniaxial compression
Column two Column one
Shear
Planar tension Planar compression
Column three Column three
If fewer than three types of tests are used, you must leave the missing columns blank. Schematically, data input might be represented as shown in Figure 8.16: “Data Locations in Stress and Strain Input Arrays”.
8–24
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
Figure 8.16 Data Locations in Stress and Strain Input Arrays
Consider a case in which data from uniaxial tension and shear tests are available. The commands to store the strain and stress data in the input-data arrays could look something like this (of course, the arrays can have any valid array names, and the number of data points represented by N1 and N2 in this example can be any integral numbers): ! Uniaxial Tension Data *SET,STRAIN(1,1), ... ! *SET,STRAIN(11,1),... ! *SET,STRESS(1,1), ... ! *SET,STRESS(11,1),... ! ! Shear Data *SET,STRAIN(1,3), ... ! *SET,STRESS(1,3), ... !
First 10 strain data points Strain data points 11 through N1 (if N1<21) First 10 stress data points Stress data points 11 through N1 Strain data points 1 through N2 (if N2<11) Stress data points 1 through N2
See the *SET command description for more information. Step 3: Determine the Mooney-Rivlin Constants To generate Mooney-Rivlin constants automatically, first use the TB command, with Lab = MOONEY and TBOPT = 1. Next, issue the *MOONEY command, inserting the appropriate names of arrays that you have already dimensioned (particular names have been used in this example for convenience of discussion only; you can use any valid parameter names): TB,MOONEY,MAT,NTEMP,,1 *MOONEY,STRAIN(1,1),STRESS(1,1),,CONST(1),CALC(1),SORTSN(1), SORTSS(1),Fname,Ext
The program automatically determines the Mooney-Rivlin constants, stores them in the database and in the CONST array (which can have any valid parameter name), and writes a series of TB and TBDATA commands in the ASCII file Fname.Ext (default file name = Jobname.TB). Uniaxial equations will be used for the data in column 1, equibiaxial equations for the data in column 2, and planar (pure shear) equations for the data in column 3. Note — All the laboratory test data entered in the STRAIN and STRESS arrays will be used to determine the Mooney-Rivlin hyperelastic material constants. Step 4: Evaluate the Quality of the Mooney-Rivlin Constants Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–25
Chapter 8: Nonlinear Structural Analysis In your printout (file Jobname.OUT), examine the "ROOT-MEAN-SQUARE ERROR (PERCENTAGE)" and the "COEFFICIENT OF DETERMINATION." These two values give you a statistical measure of how well your calculated stress-strain curve fits the experimental data points. The root-mean-square error, which is expressed as a percentage (that is, a value of 2.5 means 2.5 %), should be "close" to zero. The coefficient of determination will be less than 1.0, but should be "close" to 1.0 (that is, typically 0.99 or better). In addition, you should use the *EVAL and *VPLOT commands (GUI paths Main Menu> Preprocessor> Material Props> Mooney-Rivlin> Evaluate Const and Utility Menu> Plot> Array Parameters) to graph the input and calculated stress-strain curves, in order to obtain a visual check on how well the calculated curve matches the experimental data. In comparing these curves, you should compare calculated values against test data that represent the same mode of deformation. That is, you should compare the shape of the calculated uniaxial tension curve (EVPARM = 1 in the *EVAL command) against uniaxial tension data only (column 1 of the sorted STRAIN and STRESS arrays). Similarly, you should compare the calculated uniaxial compression curve against the uniaxial compression data only, and the calculated shear curve against the shear data only. When you graph your calculated stress-strain curves, you can extend the displayed curve into regions that were not defined by the experimental data. Graphing your curves over such an extended range can help you qualitatively understand your model's behavior if its response ever happens to exceed the range of experimental strain. However, realize that if you extend a displayed curve into a region that represents a different mode of deformation, then that portion of the display will be meaningless. For instance, you should graph a uniaxial tension curve only in regions of positive strain, and a uniaxial compression curve only in regions of compressive strain. Remember that good practice usually requires that the test data should represent all modes of deformation and ranges of response (strain) experienced by your model. The *MOONEY command automatically writes the Mooney-Rivlin constants to the CONST array. Because *EVAL reads these same constants from this CONST array, you can readily do a *EVAL following a *MOONEY operation in the same ANSYS session. If you already have the Mooney-Rivlin constants (and thus will not be doing a *MOONEY calculation), you must first dimension [*DIM]and fill the CONST array with the Mooney-Rivlin constants before you can evaluate the curves [*EVAL]. You can fill this array fairly easily, given that the CONST array is either 1 x 2, 1 x 5, or 1 x 9 at most. You could also add the *DIM and array-filling commands to your archived Jobname.TB file to make this operation more convenient. To check your curve's shape, you must dimension [*DIM] two more table array vectors (identified as XVAL and ECALC in the *EVAL command description; any valid parameter names may be used). Each of these table array vectors should have dimension P, where P is the number of points you want to use to plot your curve. (Typically, you will want to make P fairly large in order to generate a very smooth curve.) Next, specify the mode of deformation, define an extended range of strain, and fill the arrays with engineering strain and calculated engineering stress data, using the *EVAL command. Finally, graph [*VPLOT] the calculated stress-strain curve. The following example demonstrates how to graph a calculated curve for the uniaxial compression deformation mode: ! Dimension strain and stress arrays for the calculated curve: ! (Any valid parameter names can be used) *DIM,XVAL,TABLE,1000 *DIM,ECALC,TABLE,1000 ! Specify the mode of deformation (EVPARM), define the strain range ! (XMIN,XMAX), and use the M-R constants (CONST) to fill the strain (XVAL) ! and stress (ECALC) arrays with calculated data: *EVAL,1,2,CONST(1),XMIN,XMAX,XVAL(1),ECALC(1) ! Label the graph axes: /AXLAB,X,Engineering Strain /AXLAB,Y,Engineering Stress ! Plot the calculated uniaxial compression curve: *VPLOT,XVAL(1),ECALC(1)
See the *DIM, *EVAL, /AXLAB, and *VPLOT command descriptions for more information.
8–26
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
Figure 8.17 Typical Evaluated Hyperelastic Stress-Strain Curve
Step 5: Using the Mooney-Rivlin Constants If the curve-fit statistics and the overall curve shape are satisfactory, then you can proceed to use the generated Mooney-Rivlin material properties in your analysis. (The *MOONEY command will have stored these constants in the database.) In future analyses using the same material model, you can simply read in [/INPUT] the file Jobname.TB to load the constants into your new database. However, do not forget to define a value for Poisson's ratio [MP,NUXY,...]. Always remember to examine your analysis results carefully to determine whether or not your model's modes of deformation and values of maximum strain were properly represented by the original test data. Analyses involving hyperelastic elements are sometimes very sensitive to material property specification and load application. Some values of Mooney-Rivlin constants result in very stable stiffness matrices whereas others do not. Therefore, choose constants with caution and experiment with slightly different values. ANSYS provides internal stability checks for hyperelastic materials based on the Mooney-Rivlin constants that you enter. These checks occur at two levels: •
The first stability check occurs before the analysis. The check is for six typical stress paths (uniaxial tension and compression, equibiaxial tension and compression, and planar tension and compression), and covers a stretch ratio ranging from 0.1 to 10. If the material is not stable over the range, a message appears that states the critical values of the nominal strains where the material first becomes unstable, and lists the Mooney-Rivlin constants that you entered. If the material is stable over the range, you will not see any message or indication. The sample warning message below lists the nominal strains where Material 1 loses stability, then lists the constants that were entered for this example:
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–27
Chapter 8: Nonlinear Structural Analysis *** WARNING *** CP= 1.110 TIME= 16:59:52 Material 1 can become unstable under certain loading. The strain (nominal) limits where the material becomes unstable are: UNIAXIAL TENSION UNIAXIAL COMPRESSION EQUIBIAXIAL TENSION EQUIBIAXIAL COMPRESSION PLANAR TENSION PLANAR COMPRESSION
0.645E+00 -0.565E+00 0.516E+00 -0.220E+00 0.585E+00 -0.369E+00
Mooney-Rivlin constants of the hyperelastic material are: 0.170E+02, 0.000E+00, 0.000E+00,
•
0.000E+00, 0.000E+00, 0.000E+00,
0.150E+03 0.000E+00 0.000E+00
For the hyperelastic elements with mixed u-P formulation (HYPER56, HYPER58, HYPER74, and HYPER158), you can also have ANSYS perform a stability check during an analysis by setting KEYOPT(8) = 1. For each equilibrium iteration, the program checks every Gauss point in the problem for stability violations. If the problem fails the stability check, you will see a message in the solution history section of the ANSYS Output window reporting the total number of Gauss points that were unstable for that iteration. You will not see any messages if the problem passes the check. The sample message below shows that, during an analysis, ANSYS detected 3 Gauss points that exceeded the material stability limit: DISP CONVERGENCE VALUE = 22.81 CRITERION= 0.5000 EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 10.00 FORCE CONVERGENCE VALUE = 0.5018E+07 CRITERION= 0.1917E+05 >>> 3 Gauss points have exceeded the material stability limit
For elements that contain at least one unstable Gauss point, the instability indicator is set to 1 and stored in the result file as an item in the SMISC record. You can plot the region of instability in POST1 by plotting this SMISC record identified as STFLAG for the element. The SMISC number for STFLAG differs for some of the elements. See the appropriate table for the SMISC item that corresponds to instability indicator STFLAG, for the particular element of interest: HYPER56 Item and Sequence Numbers for ETABLE and ESOL Commands, HYPER58 Item and Sequence Numbers for ETABLE and ESOL Commands, HYPER74 Item and Sequence Numbers for ETABLE and ESOL Commands, HYPER158 Item and Sequence Numbers for ETABLE and ESOL Commands. You should be aware that even though a material failing a stability check is often an indication of convergence difficulty, it does not necessarily mean that your solution is invalid once the material enters the unstable region. The material stability check is simply a tool to help you diagnose the problem when the solution fails to converge. For nearly incompressible materials with Poisson's ratio greater than 0.49, we recommend that you use the hyperelastic elements with mixed u-P formulation (HYPER56, HYPER58, HYPER74, and HYPER158). Note — The element types HYPER84 and HYPER86 are intended primarily for modeling compressible, foam-like elastomers, using a Blatz-Ko function to describe the material properties. Select the Blatz-Ko option by setting KEYOPT(2) = 1 for these elements, then use MP commands to enter appropriate values for EX and NUXY to define the initial material shear modulus. An incompressible hyperelastic material option is also available for HYPER84 and HYPER86, but it is limited to two-term Mooney-Rivlin only. In general, it is recommended that you use HYPER56, HYPER58, HYPER74, or HYPER158 (not HYPER84 or HYPER86) for all incompressible hyperelastic materials. Problems using hyperelastic elements can be sensitive to the rate of load application. In most instances, load application should be slow so as not to over-distort elements in the converging sequence. Each problem may be unique and require special consideration. Bifurcation of the solution, indicating that two or more different geometric configurations have the same minimum potential energy, may occur at various times during the
8–28
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities loading history. Automatic time stepping with bisection [AUTOTS,ON] is often effective in overcoming these difficulties.
8.3.1.5. Creep Creep is a rate dependent material nonlinearity in which the material continues to deform under a constant load. Conversely, if a displacement is imposed, the reaction force (and stresses) will diminish over time (stress relaxation; see Figure 8.18: “Stress Relaxation and Creep”(a)). The three stages of creep are shown in Figure 8.18: “Stress Relaxation and Creep”(b). The ANSYS program has the capability of modeling the first two stages (primary and secondary). The tertiary stage is usually not analyzed since it implies impending failure.
Figure 8.18 Stress Relaxation and Creep
Creep is important in high temperature stress analyses, such as for nuclear reactors. For example, suppose you apply a preload to some part in a nuclear reactor to keep adjacent parts from moving. Over a period of time at high temperature, the preload would decrease (stress relaxation) and potentially let the adjacent parts move. Creep can also be significant for some materials such as prestressed concrete. Typically, the creep deformation is permanent. ANSYS analyzes creep using two time integration methods. Both are applicable to static or transient analyses.The implicit creep method is robust, fast, accurate, and recommended for general use. It can handle temperature dependent creep constants, as well as simultaneous coupling with isotropic hardening plasticity models. The explicit creep method is useful for cases where very small time steps are required. Creep constants cannot be dependent on temperature. Coupling with other plastic models is available by superposition only. Note — The terms “implicit” and “explicit” as applied to creep, have no relationship to “explicit dynamics,” or any elements referred to as “explicit elements.” The implicit creep method supports the following elements: PLANE42, SOLID45, PLANE82, SOLID92, SOLID95, LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189. The explicit creep method supports the following elements: LINK1, PLANE2, LINK8, PIPE20, BEAM23, BEAM24, PLANE42, SHELL43, SOLID45, SHELL51, PIPE60, SOLID62, SOLID65, PLANE82, SOLID92, and SOLID95. The creep strain rate may be a function of stress, strain, temperature, and neutron flux level. Libraries of creep strain rate equations are built into the ANSYS program for primary, secondary, and irradiation induced creep. (See Creep Equations in the ANSYS Elements Reference for discussions of, and input procedures for, these various creep equations.) Some equations require specific units. In particular, for the explicit creep option, temperatures used in the creep equations should be based on an absolute scale.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–29
Chapter 8: Nonlinear Structural Analysis
8.3.1.5.1. Implicit Creep Procedure The basic procedure for using the implicit creep method involves issuing the TB command with Lab = CREEP, and choosing a creep equation by specifying a value for TBOPT. The following example input shows the use of the implicit creep method. TBOPT = 2 specifies that the primary creep equation for model 2 will be used. Temperature dependency is specified using the TBTEMP command, and the four constants associated with this equation are specified as arguments with the TBDATA command. TB,CREEP,1,1,4,2 TBTEMP,100 TBDATA,1,C1,C2,C3,C4
You can input other creep expressions using the user programmable feature and setting TBOPT = 100. You can define the number of state variables using the TB command with Lab = STATE. The following example shows how five state variables are defined. TB,STATE,1,,5
You can simultaneously model creep [TB,CREEP] and isotropic, bilinear kinematic, and Hill anisotropy options to simulate more complex material behaviors. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. To perform an implicit creep analysis, you must also issue the solution RATE command, with Option = ON (or 1). The following example shows a procedure for a time hardening creep analysis (See Figure 8.19: “Time Hardening Creep Analysis”).
Figure 8.19 Time Hardening Creep Analysis
The user applied mechanical loading in the first load step, and turned the RATE command OFF to bypass the creep strain effect. Since the time period in this load step will affect the total time thereafter, the time period for this load step should be small. For this example, the user specified a value of 1.0E-8 seconds. The second load step is a creep analysis. The RATE command must be turned ON. Here the mechanical loading was kept constant, and the material creeps as time increases. /SOLU RATE,OFF TIME,1.0E-8
8–30
!First load step, apply mechanical loading !Creep analysis turned off !Time period set to a very small value
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities ... SOLV RATE,ON TIME,100 ... SOLV
!Solve this load step !Second load step, no further mechanical load !Creep analysis turned on !Time period set to desired value !Solve this load step
The RATE command works only when modeling implicit creep with either von Mises or Hill potentials. When modeling implicit creep with von Mises potential, you can use the RATE command with the following elements: LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189. When modeling anisotropic creep (TB,CREEP with TB,HILL), you can use the RATE command with the following elements: PLANE42, SOLID45, PLANE82, SOLID92, SOLID95, LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189. For most materials, the creep strain rate changes significantly at an early stage. Because of this, a general recommendation is to use a small initial incremental time step, then specify a large maximum incremental time step by using solution command DELTIM or NSUBST. For implicit creep, you may need to examine the effect of the time increment on the results carefully because ANSYS does not enforce any creep ratio control by default. You can always enforce a creep limit ratio using the creep ratio control option in commands CRPLIM or CUTCONTROL,CRPLIMIT. A recommended value for a creep limit ratio ranges from 1 to 10. The ratio may vary with materials so your decision on the best value to use should be based on your own experimentation to gain the required performance and accuracy. For larger analyses, a suggestion is to first perform a time increment convergence analysis on a simple small size test. ANSYS provides tools to help you determine the coefficients for all of the implicit creep options defined in TB,CREEP. The TBFT command allows you to compare your experimental data with existing material data curves and visually “fit” your curve for use in the TB command. All of the TBFT command capability is available via either batch or interactive (GUI) mode. See Material Curve Fitting (also in this manual) for more information.
8.3.1.5.2. Explicit Creep Procedure The basic procedure for using the explicit creep method involves issuing the TB command with Lab = CREEP and choosing a creep equation by adding the appropriate constant as an argument with the TBDATA command. TBOPT is either left blank or = 0. The following example input uses the explicit creep method. Note that all constants are included as arguments with the TBDATA command, and that there is no temperature dependency. TB,CREEP,1 TBDATA,1,C1,C2,C3,C4, ,C6
For the explicit creep method, you can incorporate other creep expressions into the program by using User Programmable Features (see the Guide to ANSYS User Programmable Features). For highly nonlinear creep strain vs. time curves, a small time step must be used with the explicit creep method. Creep strains are not computed if the time step is less than 1.0e-6. A creep time step optimization procedure is available [AUTOTS and CRPLIM] for automatically adjusting the time step as appropriate.
8.3.1.6. Shape Memory Alloy The Shape Memory Alloy (SMA) material behavior option describes the super-elastic behavior of nitinol alloy. Nitinol is a flexible metal alloy that can undergo very large deformations in loading-unloading cycles without permanent deformation. As illustrated in Figure 8.20: “Shape Memory Alloy Phases”, the material behavior has three distinct phases: an austenite phase (linear elastic), a martensite phase (also linear elastic), and the transition phase between these two.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–31
Chapter 8: Nonlinear Structural Analysis
Figure 8.20 Shape Memory Alloy Phases σ
σ
ε
∫
σ
σ σ
∫
ε
Use the MP command to input the linear elastic behavior of the austenite phase, and the TB,SMA command to input the behavior of the transition and martensite phases. Use the TBDATA command to enter the specifics (data sets) of the alloy material. You can enter up to six sets of data. SMAs can be specified for the following elements: PLANE182, PLANE183, SOLID185, SOLID186, SOLID187. A typical ANSYS input listing (fragment) will look similar to this: MP,EX,1,60.0E3 MP,NUXY,1.0.3
! Define austenite elastic properties !
TB,SMA,1,2 TBTEMP,10 TBDATA,1,520.0,600.0,300.0,200.0,0.07,0.12 TBDATA,7,5.0E4 TBTEMP,20 TBDATA,1,420.0,540.0,300.0,200.0,0.10,0.15 TBDATA,7,4.0E3
! ! ! ! ! ! ! ! !
Define material 1 as SMA, with two temperatures Define first starting temp Define SMA parameters
Define second starting temp Define SMA parameters
See TB, and TBDATA for more information.
8.3.1.7. Viscoplasticity Viscoplasticity is a time-dependent plasticity phenomenon, where the development of the plastic strains are dependent on the rate of loading. The primary applications are high-temperature metal forming processes such as rolling and deep drawing, which involve large plastic strains and displacements with small elastic strains (see Figure 8.21: “Viscoplastic Behavior in a Rolling Operation”). The plastic strains are typically very large (for example, 50% or greater), requiring large strain theory [NLGEOM,ON]. 8–32
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities Viscoplasticity is modeled with element types VISCO106, VISCO107, and VISCO108, using Anand's model for material properties as described in Nonlinear Stress-Strain Materials in the ANSYS Elements Reference.
Figure 8.21 Viscoplastic Behavior in a Rolling Operation
Viscoplasticity is defined by unifying plasticity and creep via a set of flow and evolutionary equations. A constraint equation is used to preserve volume in the plastic region. The Rate-Dependent Plasticity (Viscoplasticity) or TB,RATE option allows you to introduce the strain rate effect in material models to simulate the time-dependent response of materials. Two material options are available, the Perzyna model and the Peirce model (see the ANSYS, Inc. Theory Reference for details). In contrast to other rate-dependent material options in ANSYS such as Creep or Anand's model, the Perzyna and Peirce models also include a yield surface. The plasticity and thus the strain rate hardening effect are active only after plastic yielding. You must use the models in combination with the BISO, MISO, or NLISO material options to simulate viscoplasticity. Further, you can simulate anisotropic viscoplasticity by also combining the HILL option. See Material Model Combinations in the ANSYS Elements Reference for the combination possibilities. Also, see Section 8.3.2: Material Model Combinations in this chapter for sample input listings of material combinations. For isotropic hardening, the intent is for simulating the strain rate hardening of materials rather than softening. This option is also suitable for large strain analysis, and is applicable to the following elements: PLANE42, SOLID45, PLANE82, SOLID92, SOLID95, LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189. Some typical applications of these material options are metal forming and micro-electromechanical systems (MEMS).
8.3.1.8. Viscoelasticity Viscoelasticity is similar to creep, but part of the deformation is removed when the loading is taken off. A common viscoelastic material is glass. Some plastics are also considered to be viscoelastic. One type of viscoelastic response is illustrated in Figure 8.22: “Viscoelastic Behavior (Maxwell Model)”.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–33
Chapter 8: Nonlinear Structural Analysis
Figure 8.22 Viscoelastic Behavior (Maxwell Model)
Viscoelasticity is modeled with element types VISCO88 and VISCO89 for small deformation viscoelasticity and LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189 for small and large deformation viscoelasticity. You must input material properties using the TB family of commands. For SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, and SOLID187 the underlying elasticity is specified by either the MP command (hypoelasticity) or by the TB,HYPER command (hyperelasticity). For LINK180, BEAM188, and BEAM189, the underlying elasticity is specified using the MP command (hypoelasticity) only. The elasticity constants correspond to those of the fast load limit. Use the TB,PRONY and TB,SHIFT commands to input the relaxation property (see the TB command description for more information). !Small Strain Viscoelasticity mp,ex,1,20.0E5 !elastic properties mp,nuxy,1,0.3 tb,prony,1,,2,shear !define viscosity parameters (shear) tbdata,1,0.5,2.0,0.25,4.0 tb,prony,1,,2,bulk !define viscosity parameters (bulk) tbdata,1,0.5,2.0,0.25,4.0 !Large Strain Viscoelasticity tb,hyper,1,,,moon !elastic properties tbdata,1,38.462E4,,1.2E-6 tb,prony,1,,1,shear !define viscosity parameters tbdata,1,0.5,2.0 tb,prony,1,,1,bulk !define viscosity parameters tbdata,1,0.5,2.0
See Viscoelastic Material Constants in the ANSYS Elements Reference and the ANSYS, Inc. Theory Reference for details about how to input viscoelastic material properties using the TB family of commands. ANSYS provides tools to help you determine the coefficients for all of the viscoelastic options defined by TB,PRONY. The TBFT command allows you to compare your experimental data with existing material data curves and visually “fit” your curve for use in the TB command. All of the TBFT command capability is available via either batch or interactive (GUI) mode. See Material Curve Fitting (also in this manual) for more information.
8.3.1.9. Swelling Certain materials respond to neutron flux by enlarging volumetrically, or swelling. In order to include swelling effects, you must write your own swelling subroutine, USERSW. (See the Guide to ANSYS User Programmable Features for a discussion of User-Programmable Features.) Swelling Equations in the ANSYS Elements Reference discusses how to use the TB family of commands to input constants for the swelling equations. Swelling can also be related to other phenomena, such as moisture content. The ANSYS commands for nuclear swelling can be used analogously to define swelling due to other causes.
8–34
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
8.3.2. Material Model Combinations You can combine several material model options discussed in this chapter to simulate complex material behaviors. Material Model Combinations in the ANSYS Elements Reference presents the model options you can combine along with the associated TB command labels and links to sample input listings. These sample input listings are presented below in sections identified by the TB command labels.
8.3.2.1. BISO and CHAB Example This input listing illustrates an example of combining bilinear isotropic hardening plasticity with Chaboche nonlinear kinematic hardening plasticity. MP,EX,1,185.0E3 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,CHAB,1 TBDATA,1,180,100,3
! CHABOCHE TABLE
TB,BISO,1 TBDATA,1,180,200
! BISO TABLE
For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.2. MISO and CHAB Example This input listing illustrates an example of combining multilinear isotropic hardening plasticity with Chaboche nonlinear kinematic hardening plasticity. MP,EX,1,185E3 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,CHAB,1 TBDATA,1,180,100,3
! CHABOCHE TABLE ! THIS EXAMPLE ISOTHERMAL
TB,MISO,1 TBPT,,9.7E-4,180 TBPT,,1.0,380
! MISO TABLE
For information on the MISO option, see Multilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.3. NLISO and CHAB Example This input listing illustrates an example of combining nonlinear isotropic hardening plasticity with Chaboche nonlinear kinematic hardening plasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,CHAB,1,3,5 ! CHABOCHE TABLE TBTEMP,20,1 ! THIS EXAMPLE TEMPERATURE DEPENDENT TBDATA,1,500,20000,100,40000,200,10000 TBDATA,7,1000,200,100,100,0 TBTEMP,40,2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–35
Chapter 8: Nonlinear Structural Analysis TBDATA,1,880,204000,200,43800,500,10200 TBDATA,7,1000,2600,2000,500,0 TBTEMP,60,3 TBDATA,1,1080,244000,400,45800,700,12200 TBDATA,7,1400,3000,2800,900,0 TB,NLISO,1,2 TBTEMP,40,1 TBDATA,1,880,0.0,80.0,3 TBTEMP,60,2 TBDATA,1,1080,0.0,120.0,7
! NLISO TABLE
For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.4. BISO and RATE Example This input listing illustrates an example of combining bilinear isotropic hardening plasticity with the TB,RATE command to model viscoplasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,BISO,1 TBDATA,1,9000,10000
! BISO TABLE
TB,RATE,1,,,PERZYNA TBDATA,1,0.5,1
! RATE TABLE
For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the RATE option, see Rate-Dependent Viscoplastic Materials in the ANSYS Elements Reference, and Section 8.3.1.7: Viscoplasticity in this chapter.
8.3.2.5. MISO and RATE Example This input listing illustrates an example of combining multilinear isotropic hardening plasticity with the TB,RATE command to model viscoplasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,MISO,1 TBPT,,0.015,30000 TBPT,,0.020,32000 TBPT,,0.025,33800 TBPT,,0.030,35000 TBPT,,0.040,36500 TBPT,,0.050,38000 TBPT,,0.060,39000
! MISO TABLE
TB,RATE,1,,,PERZYNA TBDATA,1,0.5,1
! RATE TABLE
For information on the MISO option, see Multilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the RATE option, see Rate-Dependent Viscoplastic Materials in the ANSYS Elements Reference, and Section 8.3.1.7: Viscoplasticity in this chapter. 8–36
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
8.3.2.6. NLISO and RATE Example This input listing illustrates an example of combining nonlinear isotropic hardening plasticity with the TB,RATE command to model viscoplasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,NLISO,1 TBDATA,1,30000,100000,5200,172
! NLISO TABLE
TB,RATE,1,,,PERZYNA TBDATA,1,0.5,1
! RATE TABLE
For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the RATE option, see Rate-Dependent Viscoplastic Materials in the ANSYS Elements Reference, and Section 8.3.1.7: Viscoplasticity in this chapter.
8.3.2.7. BISO and CREEP Example This input listing illustrates an example of combining bilinear isotropic hardening plasticity with implicit creep. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,BISO,1 TBDATA,1,9000,10000
! BISO TABLE
TB,CREEP,1,,,2 ! CREEP TABLE TBDATA,1,1.5625E-14,5.0,-0.5,0.0
For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter.
8.3.2.8. MISO and CREEP Example This input listing illustrates an example of combining multilinear isotropic hardening plasticity with implicit creep. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,MISO,1 TBPT,,0.015,30000 TBPT,,0.020,32000 TBPT,,0.025,33800 TBPT,,0.030,35000 TBPT,,0.040,36500 TBPT,,0.050,38000 TBPT,,0.060,39000
! MISO TABLE
TB,CREEP,1,,,2 ! CREEP TABLE TBDATA,1,1.5625E-14,5.0,-0.5,0.0
For information on the MISO option, see Multilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–37
Chapter 8: Nonlinear Structural Analysis For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter.
8.3.2.9. NLISO and CREEP Example This input listing illustrates an example of combining nonlinear isotropic hardening plasticity with implicit creep. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,NLISO,1 TBDATA,1,30000,100000,5200,172
! NLISO TABLE
TB,CREEP,1,,,2 ! CREEP TABLE TBDATA,1,1.5625E-14,5.0,-0.5,0.0
For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter.
8.3.2.10. BKIN and CREEP Example This input listing illustrates an example of combining bilinear kinematic hardening plasticity with implicit creep. MP,EX,1,1e7 MP,NUXY,1,0.32
! ELASTIC CONSTANTS
TB,BKIN,1, TBDATA,1,42000,1000
! BKIN TABLE
TB,CREEP,1,,,6 TBDATA,1,7.4e-21,3.5,0,0,0,0
! CREEP TABLE
For information on the BKIN option, see Bilinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter.
8.3.2.11. HILL and BISO Example This input listing illustrates an example of modeling anisotropic plasticity with bilinear isotropic hardening. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,HILL,1,2 ! HILL TABLE TBTEMP,100 TBDATA,1,1,1.0402,1.24897,1.07895,1,1 TBTEMP,200 TBDATA,1,0.9,0.94,1.124,0.97,0.9,0.9 TB,BISO,1,2 TBTEMP,100 TBDATA,1,461.0,374.586 TBTEMP,200 TBDATA,1,400.0,325.0
! BISO TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8–38
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.12. HILL and MISO Example This input listing illustrates an example of modeling anisotropic plasticity with multilinear isotropic hardening. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,MISO,1 TBPT,,0.015,30000 TBPT,,0.020,32000 TBPT,,0.025,33800 TBPT,,0.030,35000 TBPT,,0.040,36500 TBPT,,0.050,38000 TBPT,,0.060,39000
! MISO TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the MISO option, see Multilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.13. HILL and NLISO Example This input listing illustrates an example of modeling anisotropic plasticity with nonlinear isotropic hardening. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,NLISO,1 TBDATA,1,30000,100000,5200,172
! NLISO TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.14. HILL and BKIN Example This input listing illustrates an example of modeling anisotropic plasticity with bilinear kinematic hardening. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,BKIN,1 TBDATA,1,9000,10000
! BKIN TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–39
Chapter 8: Nonlinear Structural Analysis For information on the BKIN option, see Bilinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.15. HILL and MKIN Example This input listing illustrates an example of modeling anisotropic plasticity with multilinear kinematic hardening. MPTEMP,1,20,400,650,800,950
! ELASTIC CONSTANTS
MPDATA,EX,1,1,30.00E6,27.36E6,25.20E6,23.11E6,20.76E6 MPDATA,EY,1,1,30.00E6,27.36E6,25.20E6,23.11E6,20.76E6 MPDATA,EZ,1,1,30.00E6,27.36E6,25.20E6,23.11E6,20.76E6 MPDATA,PRXY,1,1,0.351,0.359,0.368,0.375,0.377 MPDATA,PRYZ,1,1,0.351,0.359,0.368,0.375,0.377 MPDATA,PRXZ,1,1,0.351,0.359,0.368,0.375,0.377 MPDATA,GXY,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4 MPDATA,GYZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4 MPDATA,GXZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4
TB,MKIN,1,5,5 ! MKIN TABLE TBTEMP,,strain TBDATA,1,0.0015,0.006,0.04,0.08,0.1 TBTEMP,20 TBDATA,1,45000,60000,90000,115000,120000 TBTEMP,400 TBDATA,1,41040,54720,82080,104880,109440 TBTEMP,650 TBDATA,1,37800,50400,75600,96600,100800 TBTEMP,800 TBDATA,1,34665,46220,69330,88588,92440 TBTEMP,950 TBDATA,1,31140,41520,62280,79580,83040
TB,HILL,1,5 ! HILL TABLE TBTEMP,20.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,400.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,650.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,800.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00 TBTEMP,950.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the MKIN option, see Multilinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.16. HILL and KINH Example This input listing illustrates an example of modeling anisotropic plasticity with multilinear kinematic hardening. MP,EX,1,20E6 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,KINH,1,,3 TBPT,,5E-5,1E3 TBPT,,0.01,2E3 TBPT,,0.60,6E4
! KINH TABLE
8–40
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities TB,HILL,1 TBDATA,1,1.0,1.1,0.9,0.85,0.90,0.95
! HILL TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the KINH option, see Multilinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.17. HILL and CHAB Example This input listing illustrates an example of modeling anisotropic plasticity with Chaboche nonlinear kinematic hardening. MP,EX,1,185E3 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,CHAB,1 TBDATA,1,180,400,3,0
! CHABOCHE TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.18. HILL and BISO and CHAB Example This input listing illustrates an example of modeling anisotropic plasticity with bilinear isotropic hardening and Chaboche nonlinear kinematic hardening. MP,EX,1,185E3 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,CHAB,1 TBDATA,1,180,100,3
! CHABOCHE TABLE
TB,BISO,1 TBDATA,1,180,200
! BISO TABLE
TB,HILL,1 TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80
! HILL TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.19. HILL and MISO and CHAB Example This input listing illustrates an example of modeling anisotropic plasticity with multilinear isotropic hardening and Chaboche nonlinear kinematic hardening.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–41
Chapter 8: Nonlinear Structural Analysis MP,EX,1,185E3 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,CHAB,1 TBDATA,1,185,100,3
! CHABOCHE TABLE
TB,MISO,1 TBPT,,0.001,185 TBPT,,1.0,380
! MISO TABLE
TB,HILL,1 TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80
! HILL TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the MISO option, see Multilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.20. HILL and NLISO and CHAB Example This input listing illustrates an example of combining anisotropic plasticity with nonlinear isotropic hardening and Chaboche nonlinear kinematic hardening. MPTEMP,1,20,200,400,550,600,650 ! ELASTIC CONSTANTS MPTEMP,,700,750,800,850,900,950 ! MPDATA,EX,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EX,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,EY,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EY,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,EZ,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EZ,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,PRXY,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRXY,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,PRYZ,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRYZ,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,PRXZ,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRXZ,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,GXY,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GXY,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4 ! MPDATA,GYZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GYZ,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4 ! MPDATA,GXZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GXZ,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4
TB,NLISO,1 TBDATA,1,180,0.0,100.0,5
! NLISO TABLE
! TB,CHAB,1 TBDATA,1,180,100,3
8–42
! CHABOCHE TABLE
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
TB,HILL,1,5 TBTEMP,750.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,800.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,850.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,900.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00 TBTEMP,950.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00
! HILL TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CHAB option, see Nonlinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.21. HILL and RATE and BISO Example This input listing illustrates an example of modeling anisotropic viscoplasticity with bilinear isotropic hardening plasticity. MPTEMP,1,20,400,650,800,950 ! ELASTIC CONSTANTS ! MPDATA,EX,1,1,30.00E6,27.36E6,25.20E6,23.11E6,20.76E6 ! MPDATA,EY,1,1,30.00E6,27.36E6,25.20E6,23.11E6,20.76E6 ! MPDATA,EZ,1,1,30.00E6,27.36E6,25.20E6,23.11E6,20.76E6 ! MPDATA,PRXY,1,1,0.351,0.359,0.368,0.375,0.377 ! MPDATA,PRYZ,1,1,0.351,0.359,0.368,0.375,0.377 ! MPDATA,PRXZ,1,1,0.351,0.359,0.368,0.375,0.377 ! MPDATA,GXY,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4 ! MPDATA,GYZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4 ! MPDATA,GXZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4
TB,BISO,1, TBDATA,1,45000,760000
! BISO TABLE
TB,RATE,1,2,,PERZYNA TBTEMP,20 TBDATA,1,0.1,0.3 TBTEMP,950 TBDATA,1,0.3,0.5
! RATE TABLE
TB,HILL,1,5 ! HILL TABLE TBTEMP,750.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,800.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,850.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,900.0
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–43
Chapter 8: Nonlinear Structural Analysis TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00 TBTEMP,950.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the RATE option, see Rate-Dependent Viscoplastic Materials in the ANSYS Elements Reference, and Section 8.3.1.7: Viscoplasticity in this chapter. For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.22. HILL and RATE and MISO Example This input listing illustrates an example of modeling anisotropic viscoplasticity with multilinear isotropic hardening plasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,MISO,1 TBPT,,0.015,30000 TBPT,,0.020,32000 TBPT,,0.025,33800 TBPT,,0.030,35000 TBPT,,0.040,36500 TBPT,,0.050,38000 TBPT,,0.060,39000
! MISO TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80 TB,RATE,1,,,PERZYNA TBDATA,1,0.5,1
! RATE TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the RATE option, see Rate-Dependent Viscoplastic Materials in the ANSYS Elements Reference, and Section 8.3.1.7: Viscoplasticity in this chapter. For information on the MISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.23. HILL and RATE and NLISO Example This input listing illustrates an example of modeling anisotropic viscoplasticity with nonlinear isotropic hardening plasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,NLISO,1 TBDATA,1,30000,100000,5200,172
! NLISO TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80 TB,RATE,1,,,PERZYNA TBDATA,1,0.5,1
8–44
! RATE TABLE
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the RATE option, see Rate-Dependent Viscoplastic Materials in the ANSYS Elements Reference, and Section 8.3.1.7: Viscoplasticity in this chapter. For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.24. HILL and CREEP Example This input listing illustrates an example of modeling anisotropic implicit creep. MPTEMP,1,20,200,400,550,600,650 ! ELASTIC CONSTANTS MPTEMP,,700,750,800,850,900,950 ! MPDATA,EX,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EX,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,EY,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EY,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,EZ,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EZ,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,PRXY,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRXY,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,PRYZ,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRYZ,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,PRXZ,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRXZ,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,GXY,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GXY,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4 ! MPDATA,GYZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GYZ,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4 ! MPDATA,GXZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GXZ,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4
TB,CREEP,1,,,2 TBDATA,1,5.911E-34,6.25,-0.25
! CREEP TABLE
TB,HILL,1,5 TBTEMP,750.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,800.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,850.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,900.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00 TBTEMP,950.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00
! HILL TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–45
Chapter 8: Nonlinear Structural Analysis
8.3.2.25. HILL and CREEP and BISO Example This input listing illustrates an example of modeling anisotropic implicit creep with bilinear isotropic hardening plasticity. MPTEMP,1,20,200,400,550,600,650 ! ELASTIC CONSTANTS MPTEMP,,700,750,800,850,900,950 ! MPDATA,EX,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EX,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,EY,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EY,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,EZ,1,1,1.250E4,1.210E4,1.140E4,1.090E4,1.070E4,1.050E4 MPDATA,EZ,1,,1.020E4,0.995E4,0.963E4,0.932E4,0.890E4,0.865E4 ! MPDATA,PRXY,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRXY,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,PRYZ,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRYZ,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,PRXZ,1,1,0.351,0.359,0.368,0.375,0.377,0.380 MPDATA,PRXZ,1,,0.382,0.384,0.386,0.389,0.391,0.393 ! MPDATA,GXY,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GXY,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4 ! MPDATA,GYZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GYZ,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4 ! MPDATA,GXZ,1,1,1.190E4,1.160E4,1.110E4,1.080E4,1.060E4,1.040E4 MPDATA,GXZ,1,,1.020E4,1.000E4,0.973E4,0.946E4,0.908E4,0.887E4
TB,BISO,1 TBDATA,1,180,200
! BISO TABLE
TB,CREEP,1,,,2 TBDATA,1,5.911E-34,6.25,-0.25
! CREEP TABLE
TB,HILL,1,5 TBTEMP,750.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,800.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,850.0 TBDATA,1,1.0,1.0,1.0,0.93,0.93,0.93 TBTEMP,900.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00 TBTEMP,950.0 TBDATA,1,1.0,1.0,1.0,1.00,1.00,1.00
! HILL TABLE
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter. For information on the BISO option, see Bilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8–46
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.3: Modeling Material Nonlinearities
8.3.2.26. HILL and CREEP and MISO Example This input listing illustrates an example of modeling anisotropic implicit creep with multilinear isotropic hardening plasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,MISO,1 TBPT,,0.015,30000 TBPT,,0.020,32000 TBPT,,0.025,33800 TBPT,,0.030,35000 TBPT,,0.040,36500 TBPT,,0.050,38000 TBPT,,0.060,39000
! MISO TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80 TB,CREEP,1,,,2 ! CREEP TABLE TBDATA,1,1.5625E-14,5.0,-0.5,0.0
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter. For information on the MISO option, see Multilinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.27. HILL and CREEP and NLISO Example This input listing illustrates an example of modeling anisotropic implicit creep with nonlinear isotropic hardening plasticity. MP,EX,1,20.0E5 MP,NUXY,1,0.3
! ELASTIC CONSTANTS
TB,NLISO,1 TBDATA,1,30000,100000,5200,172
! NLISO TABLE
TB,HILL,1 ! HILL TABLE TBDATA,1,1.0,1.1,0.9,0.85,0.9,0.80 TB,CREEP,1,,,2 ! CREEP TABLE TBDATA,1,1.5625E-14,5.0,-0.5,0.0
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter. For information on the NLISO option, see Nonlinear Isotropic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.3.2.28. HILL and CREEP and BKIN Example This input listing illustrates an example of modeling anisotropic implicit creep with bilinear kinematic hardening plasticity. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–47
Chapter 8: Nonlinear Structural Analysis MP,EX,1,1e7 MP,NUXY,1,0.32
! ELASTIC CONSTANTS
TB,BKIN,1 TBDATA,1,42000,1000
! BKIN TABLE
TB,CREEP,1,,,6 TBDATA,1,7.4e-21,3.5,0,0,0,0
! CREEP TABLES
TB,HILL,1 ! HILL TABLE TBDATA,1,1.15,1.05,1.0,1.0,1.0,1.0
For information on the HILL option, see Hill's Anisotropy in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter. For information on the CREEP option, see Implicit Creep Equations in the ANSYS Elements Reference, and Section 8.3.1.5.1: Implicit Creep Procedure in this chapter. For information on the BKIN option, see Bilinear Kinematic Hardening in the ANSYS Elements Reference, and Section 8.3.1.1.1: Plastic Material Options in this chapter.
8.4. Running a Nonlinear Analysis in ANSYS ANSYS employs an automatic solution control method that, based on the physics of your problem, sets various nonlinear analysis controls to the appropriate values. If you are not satisfied with the results obtained with these values, you can manually override the settings. The following commands are set to optimal defaults: AUTOTS
PRED
MONITOR
DELTIM
NROPT
NEQIT
NSUBST
TINTP
SSTIF
CNVTOL
CUTCONTROL
KBC
LNSRCH
OPNCONTROL
EQSLV
ARCLEN
CDWRITE
LSWRITE
These commands and the settings they control are discussed in later sections. You can also refer to the individual command descriptions in the ANSYS Commands Reference. If you do choose to override the ANSYS-specified settings, or if you wish to use an input list from a previous release of ANSYS, issue SOLCONTROL,OFF in the /SOLU phase. See the SOLCONTROL command description for more details. ANSYS' automatic solution control is active for the following analyses: •
Single-field nonlinear or transient structural and solid mechanics analysis where the solution DOFs are combinations of UX, UY, UZ, ROTX, ROTY, and ROTZ.
•
Single-field nonlinear or transient thermal analysis where the solution DOF is TEMP. Note — The Solution Controls dialog box, which is described later in this chapter, cannot be used to set solution controls for a thermal analysis. Instead, you must use the standard set of ANSYS solution commands and the standard corresponding menu paths.
8.5. Performing a Nonlinear Static Analysis The procedure for performing a nonlinear static analysis consists of these tasks:
8–48
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.5: Performing a Nonlinear Static Analysis •
Section 8.5.1: Build the Model
•
Section 8.5.2: Set Solution Controls
•
Section 8.5.3: Set Additional Solution Options
•
Section 8.5.4: Apply the Loads
•
Section 8.5.5: Solve the Analysis
•
Section 8.5.6: Review the Results
8.5.1. Build the Model This step is essentially the same for both linear and nonlinear analyses, although a nonlinear analysis might include special elements or nonlinear material properties. See Section 8.9: Using Nonlinear (Changing-Status) Elements, and Section 8.3: Modeling Material Nonlinearities, for more details. If your analysis includes large-strain effects, your stress-strain data must be expressed in terms of true stress and true (or logarithmic) strain. For more information on building models in ANSYS, see the ANSYS Modeling and Meshing Guide. After you have created a model in ANSYS, you set solution controls (analysis type, analysis options, load step options, and so on), apply loads, and solve. A nonlinear solution will differ from a linear solution in that it often requires multiple load increments, and always requires equilibrium iterations. The general procedure for performing these tasks follows. See Section 8.11: Sample Nonlinear Analysis (GUI Method) for a sample problem that walks you through a specific nonlinear analysis.
8.5.2. Set Solution Controls Setting solution controls for a nonlinear analysis involves the same options and method of access (the Solution Controls dialog box) as those used for a linear structural static analysis. For a nonlinear analysis, the default settings in the Solution Controls dialog box are essentially the same settings employed by the automatic solution control method described in Section 8.4: Running a Nonlinear Analysis in ANSYS. See the following sections in Chapter 2, “Structural Static Analysis”, with exceptions noted: •
Section 2.3.2: Set Solution Controls
•
Section 2.3.2.1: Access the Solution Controls Dialog Box
•
Section 2.3.2.2: Using the Basic Tab
•
Section 2.3.2.3: The Transient Tab
•
Section 2.3.2.4: Using the Sol'n Options Tab
•
Section 2.3.2.5: Using the Nonlinear Tab
•
Section 2.3.2.6: Using the Advanced NL Tab
8.5.2.1. Using the Basic Tab: Special Considerations Special considerations for setting these options in a nonlinear structural static analysis include: •
When setting ANTYPE and NLGEOM, choose Large Displacement Static if you are performing a new analysis. (But, keep in mind that not all nonlinear analyses will produce large deformations. See Section 8.2: Using Geometric Nonlinearities for further discussion of large deformations.) Choose Restart Current Analysis if you want to restart a failed nonlinear analysis. You cannot change this setting after the first load step (that is, after you issue your first SOLVE command). You will usually choose to do a new analysis, rather than a restart. Restarts are discussed in the ANSYS Basic Analysis Guide.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–49
Chapter 8: Nonlinear Structural Analysis •
When working with time settings, remember that these options can be changed at any load step. See Chapter 2, “Loading” in the ANSYS Basic Analysis Guide for more information on these options. Advanced time/frequency options, in addition to those available on the Solution Controls dialog box, are discussed in Section 8.5.2.3: Advanced Load Step Options You Can Set on the Solution Controls Dialog Box. A nonlinear analysis requires multiple substeps (or time steps; the two terms are equivalent) within each load step so that ANSYS can apply the specified loads gradually and obtain an accurate solution. The NSUBST and DELTIM commands both achieve the same effect (establishing a load step's starting, minimum, and maximum step size), but by reciprocal means. NSUBST defines the number of substeps to be taken within a load step, whereas DELTIM defines the time step size explicitly. If automatic time stepping is off [AUTOTS], then the starting substep size is used throughout the load step.
•
OUTRES controls the data on the results file (Jobname.RST). By default, only the last substep is written to the results file in a nonlinear analysis. Only 1000 results sets (substeps) can be written to the results file, but you can use the command /CONFIG,NRES to increase the limit (see the ANSYS Basic Analysis Guide).
8.5.2.2. Advanced Analysis Options You Can Set on the Solution Controls Dialog Box The following sections provide more detail about some of the advanced analysis options that you can set on the Solution Controls dialog box.
8.5.2.2.1. Equation Solver ANSYS' automatic solution control activates the sparse direct solver (EQSLV,SPARSE) for most cases. The sparse direct solver is the default, except for the generation pass of a substructure analysis (which uses the frontal direct solver). Other choices include the frontal direct and PCG solvers. For applications using solid elements (for example, SOLID92 or SOLID45), the PCG solver may be faster, especially when doing 3-D modeling. If you are using the PCG solver, you may be able to considerably reduce your memory usage with the MSAVE command. The MSAVE command triggers an element-by-element approach for the parts of the model that use SOLID92, SOLID95, SOLID186, and/or SOLID187 elements with linear material properties. To use this command, you must be doing a static analysis or a modal analysis with the PowerDynamics method. If using SOLID186 and/or SOLID187 elements, it must be a small strain (NLGEOM,OFF) analysis. Other parts of the model that do not meet the above criteria will be solved using global assembly for the stiffness matrix. MSAVE,ON can result in a memory savings of up to 70% for the part of the model that meets the criteria, although the solution time may increase depending on the manufacturer of your computer and the speed of your processor, as well as the chosen element options (for example, 2 x 2 x 2 integration for SOLID95). The sparse direct solver, in sharp contrast to the iterative solvers included in ANSYS, is a robust solver. Although the PCG solver can solve indefinite matrix equations, when the PCG solver encounters an ill-conditioned matrix, the solver will iterate to the specified number of iterations and stop if it fails to converge. When this happens, it triggers bisection. After completing the bisection, the solver continues the solution if the resulting matrix is wellconditioned. Eventually, the entire nonlinear load step can be solved. Use the following guidelines for selecting either the sparse or the PCG solver for nonlinear structural analysis: •
If it is a beam/shell or beam/shell and solid structure, choose the sparse direct solver.
•
If it is a 3-D solid structure and the number of DOF is relatively large (that is, 200,000 or more DOF), choose the PCG solver.
8–50
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.5: Performing a Nonlinear Static Analysis •
If the problem is ill-conditioned (triggered by poor element shapes), or has a big difference in material properties in different regions of the model, or has insufficient displacement boundary constraints, choose the sparse direct solver.
8.5.2.3. Advanced Load Step Options You Can Set on the Solution Controls Dialog Box The following sections provide more detail about some of the advanced load step options that you can set on the Solution Controls dialog box.
8.5.2.3.1. Automatic Time Stepping ANSYS' automatic solution control turns automatic time stepping on [AUTOTS,ON]. An internal auto-time step scheme ensures that the time step variation is neither too aggressive (resulting in many bisection/cutbacks) nor too conservative (time step size is too small). At the end of a time step, the size of the next time step is predicted based on four factors: •
Number of equilibrium iterations used in the last time step (more iterations cause the time step size to be reduced)
•
Predictions for nonlinear element status change (time step sizes are decreased when a status change is imminent)
•
Size of the plastic strain increment
•
Size of the creep strain increment
8.5.2.3.2. Convergence Criteria The program will continue to do equilibrium iterations until the convergence criteria [CNVTOL] are satisfied (or until the maximum number of equilibrium equations is reached [NEQIT]). You can define custom criteria if the default settings are not suitable. ANSYS' automatic solution control uses L2-norm of force (and moment) tolerance (TOLER) equal to 0.5%, a setting that is appropriate for most cases. In most cases, an L2-norm check on displacement with TOLER equal to 5% is also used in addition to the force norm check. The check that the displacements are loosely set serves as a doublecheck on convergence. By default, the program will check for force (and, when rotational degrees of freedom are active, moment) convergence by comparing the square root sum of the squares (SRSS) of the force imbalances against the product of VALUE*TOLER. The default value of VALUE is the SRSS of the applied loads (or, for applied displacements, of the Newton-Raphson restoring forces), or MINREF (which defaults to 0.01), whichever is greater. The default value of TOLER is 0.005. If SOLCONTROL,OFF, TOLER defaults to 0.001 and MINREF defaults to 1.0 for force convergence. You should almost always use force convergence checking. You can also add displacement (and, when applicable, rotation) convergence checking. For displacements, the program bases convergence checking on the change in deflections (∆u) between the current (i) and the previous (i-1) iterations: ∆u=ui-ui-1. Note — If you explicitly define any custom convergence criteria [CNVTOL], the entire default criteria will be overwritten. Thus, if you define displacement convergence checking, you will have to redefine force convergence checking. (Use multiple CNVTOL commands to define multiple convergence criteria.) Using tighter convergence criteria will improve the accuracy of your results, but at the cost of more equilibrium iterations. If you want to tighten (or loosen, which is not recommended) your criteria, you should change TOLER Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–51
Chapter 8: Nonlinear Structural Analysis by one or two orders of magnitude. In general, you should continue to use the default value of VALUE; that is, change the convergence criteria by adjusting TOLER, not VALUE. You should make certain that the default value of MINREF = 0.001 makes sense in the context of your analysis. If your analysis uses certain sets of units or has very low load levels, you might want to specify a smaller value for MINREF. Also, we do not recommend putting two or more disjointed structures into one model for a nonlinear analysis because the convergence check tries to relate these disjointed structures, often producing some unwanted residual force. Checking Convergence in a Single and Multi-DOF System To check convergence in a single degree of freedom (DOF) system, you compute the force (and moment) imbalance for the one DOF, and compare this value against the established convergence criteria (VALUE*TOLER). (You can also perform a similar check for displacement (and rotation) convergence for your single DOF.) However, in a multi-DOF system, you might want to use a different method of comparison. The ANSYS program provides three different vector norms to use for convergence checking: •
The infinite norm repeats the single-DOF check at each DOF in your model.
•
The L1 norm compares the convergence criterion against the sum of the absolute values of force (and moment) imbalance for all DOFs.
•
The L2 norm performs the convergence check using the square root sum of the squares of the force (and moment) imbalances for all DOFs. (Of course, additional L1 or L2 checking can be performed for a displacement convergence check.)
Example For the following example, the substep will be considered to be converged if the out-of-balance force (checked at each DOF separately) is less than or equal to 5000*0.0005 (that is, 2.5), and if the change in displacements (checked as the square root sum of the squares) is less than or equal to 10*0.001 (that is, 0.01). CNVTOL,F,5000,0.0005,0 CNVTOL,U,10,0.001,2
8.5.2.3.3. Maximum Number of Equilibrium Iterations ANSYS' automatic solution control sets the value of NEQIT to between 15 and 26 iterations, depending upon the physics of the problem. The idea is to employ a small time step with fewer quadratically converging iterations. This option limits the maximum number of equilibrium iterations to be performed at each substep (default = 25 if solution control is off). If the convergence criteria have not been satisfied within this number of equilibrium iterations, and if auto time stepping is on [AUTOTS], the analysis will attempt to bisect. If bisection is not possible, then the analysis will either terminate or move on to the next load step, according to the instructions you issue in the NCNV command.
8.5.2.3.4. Predictor-Corrector Option ANSYS' automatic solution control will set PRED,ON if there are no beam or shell elements present. If the time step size is reduced greatly in the current substep, PRED is turned off. For transient analysis, the predictor is also turned off. You can activate a predictor on the DOF solution for the first equilibrium iteration of each substep. This feature accelerates convergence and is particularly useful if nonlinear response is relatively smooth. It is not so helpful
8–52
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.5: Performing a Nonlinear Static Analysis in analyses that incorporate large rotations or viscoelasticity. Using the predictor for large rotations can cause divergence and thus is not recommended for problems with large rotations.
8.5.2.3.5. Line Search Option ANSYS' automatic solution control will toggle line search on and off as needed. For most contact problems, LNSRCH is toggled on. For most non-contact problems, LNSRCH is toggled off. This convergence-enhancement tool multiplies the calculated displacement increment by a program-calculated scale factor (having a value between 0 and 1), whenever a stiffening response is detected. Because the line search algorithm is intended to be an alternative to the adaptive descent option [NROPT], adaptive descent is not automatically activated if the line search option is on. We do not recommend activating both line search and adaptive descent simultaneously. When an imposed displacement exists, a run cannot converge until at least one of the iterations has a line search value of 1. ANSYS scales the entire ∆U vector, including the imposed displacement value; otherwise, a "small" displacement would occur everywhere except at the imposed DOF. Until one of the iterations has a line search value of 1, ANSYS does not impose the full value of the displacement.
8.5.2.3.6. Cutback Criteria For finer control over bisections and cutback in time step size, use [CUTCONTROL, Lab, VALUE, Option]. By default, for Lab = PLSLIMIT (maximum plastic strain increment limit), VALUE is set to 15%. This field is set to such a large value for avoiding unnecessary bisections caused by high plastic strain due to a local singularity which is not normally of interest to the user. For explicit creep (Option = 0), Lab = CRPLIM (creep increment limit) and VALUE is set to 10%. This is a reasonable limit for creep analysis. For implicit creep (Option = 1), there is no maximum creep criteria by default. You can however, specify any creep ratio control. The number of points per cycle for second order dynamic equations (Lab = NPOINT) is set to VALUE = 13 by default to gain efficiency at little cost to accuracy.
8.5.3. Set Additional Solution Options This section discusses additional options that you can set for the solution. These options do not appear on the Solution Controls dialog box because they are used infrequently, and their default settings rarely need to be changed. ANSYS menu paths are provided in this section to help you access these options for those cases in which you choose to override the ANSYS-assigned defaults.
8.5.3.1. Advanced Analysis Options You Cannot Set on the Solution Controls Dialog Box The following sections describe some advanced analysis options that you can set for your analysis. As noted above in Section 8.5.3: Set Additional Solution Options, you cannot use the Solution Controls dialog box to set the options described below. Instead, you must set them using the standard set of ANSYS solution commands and the standard corresponding menu paths.
8.5.3.1.1. Stress Stiffness To account for buckling, bifurcation behavior, ANSYS includes stress stiffness in all geometrically nonlinear analyses. If you are confident of ignoring such effects, you can turn stress stiffening off (SSTIF,OFF). This command has no effect when used with several ANSYS elements; see the ANSYS Elements Reference for the description of the specific elements you are using. Command(s): SSTIF GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–53
Chapter 8: Nonlinear Structural Analysis
8.5.3.1.2. Newton-Raphson Option ANSYS' automatic solution control will use the FULL Newton-Raphson option with adaptive descent off if there is a nonlinearity present. However, when node-to-node, node-to-surface contact elements are used for contact analysis with friction, then adaptive descent is automatically turned on (for example, PIPE20, BEAM23, BEAM24, and PIPE60). The underlying contact elements require adaptive descent for convergence. Command(s): NROPT GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options Use this option only in a nonlinear analysis. This option specifies how often the tangent matrix is updated during solution. If you choose to override the default, you can specify one of these values: •
Program-chosen (NROPT,AUTO): The program chooses which of the options to use, based on the kinds of nonlinearities present in your model. Adaptive descent will be automatically activated, when appropriate.
•
Full (NROPT,FULL): The program uses the full Newton-Raphson procedure, in which the stiffness matrix is updated at every equilibrium iteration. If adaptive descent is on (optional), the program will use the tangent stiffness matrix only as long as the iterations remain stable (that is, as long as the residual decreases, and no negative main diagonal pivot occurs). If divergent trends are detected on an iteration, the program discards the divergent iteration and restarts the solution, using a weighted combination of the secant and tangent stiffness matrices. When the iterations return to a convergent pattern, the program will resume using the tangent stiffness matrix. Activating adaptive descent will usually enhance the program's ability to obtain converged solutions for complicated nonlinear problems but is supported only for elements indicated under "Special Features" in the Input Summary table (Table 4.n.1 for an element, where n is the element number) in the ANSYS Elements Reference.
•
Modified (NROPT,MODI): The program uses the modified Newton-Raphson technique, in which the tangent stiffness matrix is updated at each substep. The matrix is not changed during equilibrium iterations at a substep. This option is not applicable to large deformation analyses. Adaptive descent is not available.
•
Initial Stiffness (NROPT,INIT): The program uses the initial stiffness matrix in every equilibrium iteration. This option can be less likely to diverge than the full option, but it often requires more iterations to achieve convergence. It is not applicable to large deformation analyses. Adaptive descent is not available.
•
Full with unsymmetric matrix (NROPT,UNSYM): The program uses the full Newton-Raphson procedure, in which the stiffness matrix is updated at every equilibrium iteration. In addition, it generates and uses unsymmetric matrices that you can use for any of the following: –
If you are running a pressure-driven collapse analysis, an unsymmetric pressure load stiffness might be helpful in obtaining convergence. You can include pressure load stiffness using SOLCONTROL,INCP.
–
If you are defining an unsymmetric material model using TB,USER, you would need NROPT,UNSYM to fully use the property you defined.
–
If you are running a contact analysis, an unsymmetric contact stiffness matrix would fully couple the sliding and the normal stiffnesses. See Section 11.4.8.4: Determining Contact Stiffness and Allowable Penetration in this manual for details.
You should first try NROPT,FULL; then try NROPT,UNSYM if you experience convergence difficulties. Note that using an unsymmetric solver requires more computer time to obtain a solution, than if you use a symmetric solver. •
8–54
If a multistatus element is in the model, however, it would be updated at the iteration in which it changes status, irrespective of the Newton-Raphson option.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.5: Performing a Nonlinear Static Analysis
8.5.3.2. Advanced Load Step Options You Cannot Set on the Solution Controls Dialog Box The following sections describe some advanced load step options that you can set for your analysis. As noted above in Section 8.5.3: Set Additional Solution Options, you cannot use the Solution Controls dialog box to set the options described below. Instead, you must set them using the standard set of ANSYS solution commands and the standard corresponding menu paths.
8.5.3.2.1. Creep Criteria If your structure exhibits creep behavior, you can specify a creep criterion for automatic time step adjustment [CRPLIM,CRCR, Option]. (If automatic time stepping [AUTOTS] is off, this creep criterion will have no effect.) The program will compute the ratio of creep strain increment (∆εcr, the change in creep strain in the last time step) to the elastic strain (εel), for all elements. If the maximum ratio is greater than the criterion CRCR, the program will then decrease the next time step size; if it is less, the program might increase the next time step size. (The program will also base automatic time stepping on the number of equilibrium iterations, impending element status change, and plastic strain increment. The time step size will be adjusted to the minimum size calculated for any of these items.) For explicit creep (Option = 0), if the ratio ∆εcr / εel is above the stability limit of 0.25, and if the time increment cannot be decreased, a divergent solution is possible and the analysis will be terminated with an error message. This problem can be avoided by making the minimum time step size sufficiently small [DELTIM and NSUBST]. For implicit creep (Option = 1), there is no maximum creep limit by default. You can however, specify any creep ratio control. Command(s): CRPLIM GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Creep Criterion Note — If you do not want to include the effects of creep in your analysis, use the RATE command with Option = OFF, or set the time steps to be longer than the previous time step, but not more than 1.0e-6 longer.
8.5.3.2.2. Time Step Open Control This option is available for thermal analysis. (Remember that you cannot perform a thermal analysis using the Solution Controls dialog box; you must use the standard set of ANSYS solution commands or the standard corresponding menu paths instead.) This option's primary use is in unsteady state thermal analysis where the final temperature stage reaches a steady state. In such cases, the time step can be opened quickly. The default is that if the TEMP increment is smaller than 0.1 in three (NUMSTEP = 3) contiguous substeps, the time step size can be "opened-up" (value = 0.1 by default). The time step size can then be opened continuously for greater solution efficiency. Command(s): OPNCONTROL GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Open Control
8.5.3.2.3. Solution Monitoring This option provides a facility to monitor a solution value at a specified node in a specified DOF. The command also provides the user with a means to quickly review the solution convergence efficiency, rather than attempting to gather this information from a lengthy output file. For instance, if an excessive number of attempts were made for a substep, the information contained in the file provides hints to either reduce the initial time step size or increase the minimum number of substeps allowed through the NSUBST command to avoid an excessive number of bisections. Command(s): MONITOR GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Monitor
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–55
Chapter 8: Nonlinear Structural Analysis
8.5.3.2.4. Birth and Death Specify birth and death options as necessary. You can deactivate [EKILL] and reactivate [EALIVE] selected elements to model the removal or addition of material in your structure. As an alternative to the standard birth and death method, you can change the material properties for selected elements [MPCHG] between load steps. Command(s): EKILL, EALIVE GUI: Main Menu> Solution> Load Step Opts> Other> Birth & Death> Kill Elements Main Menu> Solution> Load Step Opts> Other> Birth & Death> Activate Elem The program “deactivates” an element by multiplying its stiffness by a very small number (which is set by the ESTIF command), and by removing its mass from the overall mass matrix. Element loads (pressure, heat flux, thermal strains, and so on) for inactive elements are also set to zero. You need to define all possible elements during preprocessing; you cannot create new elements in SOLUTION. Those elements to be “born” in later stages of your analysis should be deactivated before the first load step, and then reactivated at the beginning of the appropriate load step. When elements are reactivated, they have a zero strain state, and (if NLGEOM,ON) their geometric configuration (length, area, and so on) is updated to match the current displaced positions of their nodes. See the ANSYS Advanced Analysis Techniques Guide for more information on birth and death. Another way to affect element behavior during solution is to change the material property reference number for selected elements: Command(s): MPCHG GUI: Main Menu> Solution> Load Step Opts> Other> Change Mat Props> Change Mat Num Note — Use MPCHG with caution. Changing material properties in a nonlinear analysis may produce unintended results, particularly if you change nonlinear [TB] material properties.
8.5.3.2.5. Output Control In addition to OUTRES, which you can set on the Solution Controls dialog box, there are several other output control options that you can set for an analysis: Command(s): OUTPR, ERESX GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Output Ctrls> Solu Printout Main Menu> Solution> Unabridged Menu> Load Step Opts> Output Ctrls> Integration Pt Printed output [OUTPR] includes any results data on the output file (Jobname.OUT). Extrapolation of results [ERESX] copies an element's integration point stress and elastic strain results to the nodes instead of extrapolating them, if nonlinear strains (plasticity, creep, swelling) are present in the element. The integration point nonlinear strains are always copied to the nodes. See Chapter 2, “Loading” in the ANSYS Basic Analysis Guide for more information on these options.
8.5.4. Apply the Loads Apply loads on the model. See Chapter 2, “Structural Static Analysis” in this guide and Chapter 2, “Loading” in the ANSYS Basic Analysis Guide for load information. Remember that inertia and point loads will maintain constant direction, but surface loads will "follow" the structure in a large-deformation analysis. You can apply complex boundary conditions by defining a one-dimensional table (TABLE type array parameter). See Section 2.3.4.2.1: Applying Loads Using TABLE Type Array Parameters in this guide for more information.
8–56
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.5: Performing a Nonlinear Static Analysis
8.5.5. Solve the Analysis You solve a nonlinear analysis using the same commands and procedure as you do in solving a linear static analysis. See Section 2.3.5: Solve the Analysis in Chapter 2, “Structural Static Analysis”. If you need to define multiple load steps, you must respecify time settings, load step options, and so on, and then save and solve for each of the additional load steps. Other methods for multiple load steps - the load step file method and the array parameter method - are described in the ANSYS Basic Analysis Guide.
8.5.6. Review the Results Results from a nonlinear static analysis consist mainly of displacements, stresses, strains, and reaction forces. You can review these results in POST1, the general postprocessor, or in POST26, the time-history postprocessor. Remember that in POST1, only one substep can be read in at a time, and that the results from that substep should have been written to Jobname.RST. (The load step option command OUTRES controls which substep results are stored on Jobname.RST.) A typical POST1 postprocessing sequence is described below.
8.5.6.1. Points to Remember •
To review results in POST1, the database must contain the same model for which the solution was calculated.
•
The results file (Jobname.RST) must be available.
8.5.6.2. Reviewing Results in POST1 1.
Verify from your output file (Jobname.OUT) whether or not the analysis converged at all load steps. •
If not, you probably will not want to postprocess the results, other than to determine why convergence failed.
•
If your solution converged, then continue postprocessing.
2.
Enter POST1. If your model is not currently in the database, issue RESUME. Command(s): /POST1 GUI: Main Menu> General Postproc
3.
Read in results for the desired load step and substep, which can be identified by load step and substep numbers or by time. (Note, however, that arc-length results should not be identified by time.) Command(s): SET GUI: Main Menu> General Postproc> Read Results> load step You can also use the SUBSET or APPEND commands to read in or merge results data for selected portions of the model only. The LIST argument on any of these commands lists the available solutions on the results file. You can also limit the amount of data written from the results file to the database through the INRES command. Additionally, you can use the ETABLE command to store result items for selected elements. See the individual command descriptions in the ANSYS Commands Reference for more information. Caution: If you specify a TIME value for which no results are available, the ANSYS program will perform a linear interpolation to calculate the results at that value of TIME. Realize that this interpolation will usually cause some loss of accuracy in a nonlinear analysis (see Figure 8.23: “Linear Interpolation of Nonlinear Results Can Introduce Some Error”). Thus, for a nonlinear analysis, you should usually postprocess at a TIME that corresponds exactly to the desired substep. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–57
Chapter 8: Nonlinear Structural Analysis
Figure 8.23 Linear Interpolation of Nonlinear Results Can Introduce Some Error
4.
Display the results using any of the following options: Option: Display Deformed Shape Command(s): PLDISP GUI: Main Menu> General Postproc> Plot Results> Deformed Shape In a large deformation analysis, you might prefer to use a true scale display [/DSCALE,,1]. Option: Contour Displays Command(s): PLNSOL or PLESOL GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu Use these options to display contours of stresses, strains, or any other applicable item. If you have adjacent elements with different material behavior (such as can occur with plastic or multilinear elastic material properties, with different material types, or with adjacent deactivated and activated elements), you should take care to avoid nodal stress averaging errors in your results. Selecting logic (described in the ANSYS Basic Analysis Guide) provides a means of avoiding such errors. The KUND field on PLNSOL and PLESOL gives you the option of overlaying the undeformed shape on the display. You can also contour element table data and line element data: Command(s): PLETAB, PLLS GUI: Main Menu> General Postproc> Element Table> Plot Element Table Main Menu> General Postproc> Plot Results> Contour Plot> Line Elem Res Use PLETAB to contour element table data and PLLS to contour line element data. Option: Tabular Listings Command(s): PRNSOL (nodal results) PRESOL (element-by-element results) PRRSOL (reaction data) PRETAB PRITER (substep summary data), and so on. NSORT ESORT GUI: Main Menu> General Postproc> List Results> Nodal Solution Main Menu> General Postproc> List Results> Element Solution Main Menu> General Postproc> List Results> Reaction Solution Use the NSORT and ESORT commands to sort the data before listing them.
8–58
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.6: Performing a Nonlinear Transient Analysis Other Capabilities Many other postprocessing functions - mapping results onto a path, report quality listings, and so on are available in POST1. See The General Postprocessor (POST1) in the ANSYS Basic Analysis Guide for details. Load case combinations usually are not valid for nonlinear analyses.
8.5.6.3. Reviewing Results in POST26 You can also review the load-history response of a nonlinear structure using POST26, the time-history postprocessor. Use POST26 to compare one ANSYS variable against another. For instance, you might graph the displacement at a node versus the corresponding level of applied load, or you might list the plastic strain at a node and the corresponding TIME value. A typical POST26 postprocessing sequence might follow these steps: 1.
Verify from your output file (Jobname.OUT) whether or not the analysis converged at all desired load steps. You should not base design decisions on unconverged results.
2.
If your solution converged, enter POST26. If your model is not currently in the database, issue RESUME. Command(s): /POST26 GUI: Main Menu> TimeHist Postpro
3.
Define the variables to be used in your postprocessing session. The SOLU command will cause various iteration and convergence parameters to be read into the database, where you can incorporate them into your postprocessing. Command(s): NSOL, ESOL, RFORCE GUI: Main Menu> TimeHist Postpro> Define Variables
4.
Graph or list the variables. Command(s): PLVAR (graph variables) PRVAR EXTREM (list variables) GUI: Main Menu> TimeHist Postpro> Graph Variables Main Menu> TimeHist Postpro> List Variables Main Menu> TimeHist Postpro> List Extremes
Other Capabilities Many other postprocessing functions are available in POST26. See Chapter 6, “The Time-History Postprocessor (POST26)” in the ANSYS Basic Analysis Guide for details. See the NLGEOM, SSTIF, NROPT, TIME, NSUBST, AUTOTS, KBC, CNVTOL, NEQIT, NCNV, PRED, OUTRES, and SOLU command descriptions for more information.
8.5.7. Terminating a Running Job; Restarting You can stop a nonlinear analysis by creating an "abort" file (Jobname.ABT). See Chapter 3, “Solution” in the ANSYS Basic Analysis Guide for details. The program will also stop upon successful completion of the solution, or if a convergence failure occurs. You can often restart an analysis if it successfully completed one or more iterations before it terminated. Restart procedures are covered in Section 3.16: Restarting an Analysis in the ANSYS Basic Analysis Guide.
8.6. Performing a Nonlinear Transient Analysis Many of the tasks that you need to perform in a nonlinear transient analysis are the same as (or similar to) those that you perform in nonlinear static analyses (described in Section 8.5: Performing a Nonlinear Static Analysis) and linear full transient dynamic analyses (described in Chapter 2, “Structural Static Analysis”). However, this section describes some additional considerations for performing a nonlinear transient analysis. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–59
Chapter 8: Nonlinear Structural Analysis Remember that the Solution Controls dialog box, which is the method described in Section 8.5: Performing a Nonlinear Static Analysis, cannot be used to set solution controls for a thermal analysis. Instead, you must use the standard set of ANSYS solution commands and the standard corresponding menu paths.
8.6.1. Build the Model This step is the same as for a nonlinear static analysis. However, if your analysis includes time-integration effects, be sure to include a value for mass density [MP,DENS]. If you want to, you can also define material-dependent structural damping [MP,DAMP].
8.6.2. Apply Loads and Obtain the Solution 1.
2.
Specify transient analysis type and define analysis options as you would for a nonlinear static analysis: •
New Analysis or Restart [ANTYPE]
•
Analysis Type: Transient [ANTYPE]
•
Large Deformation Effects [NLGEOM]
•
Large Displacement Transient (if using the Solution Controls dialog box to set analysis type)
Apply loads and specify load step options in the same manner as you would for a linear full transient dynamic analysis. A transient load history usually requires multiple load steps, with the first load step typically used to establish initial conditions (see the ANSYS Basic Analysis Guide). The general, nonlinear, birth and death, and output control options available for a nonlinear static analysis are also available for a nonlinear transient analysis. In a nonlinear transient analysis, time must be greater than zero. See Chapter 5, “Transient Dynamic Analysis” for procedures for defining nonzero initial conditions. For a nonlinear transient analysis, you must specify whether you want stepped or ramped loads [KBC]. See the ANSYS Basic Analysis Guide for further discussion about ramped vs. stepped loads. You can also specify dynamics options: alpha and beta damping, time integration effects, and transient integration parameters. Command(s): ALPHAD, BETAD, TIMINT, TINTP GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Transient Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Damping Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Time Integration An explanation of the dynamics options follows. •
Damping Rayleigh damping constants are defined using the constant mass [ALPHAD] and stiffness [BETAD] matrix multipliers. In a nonlinear analysis the stiffness may change drastically - do not use BETAD, except with care. See Section 5.10.3: Damping for details about damping.
•
Time Integration Effects [TIMINT] Time integration effects are ON by default in a transient analysis. For creep, viscoelasticity, viscoplasticity, or swelling, you should turn the time integration effects off (that is, use a static analysis). These
8–60
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.7: Sample Input for a Nonlinear Transient Analysis time-dependent effects are usually not included in dynamic analyses because the transient dynamic time step sizes are often too short for any significant amount of long-term deformation to occur. Except in kinematic (rigid-body motion) analyses, you will rarely need to adjust the transient integration parameters [TINTP], which provide numerical damping to the Newmark and HHT methods. (See your ANSYS, Inc. Theory Reference for more information about these parameters.) ANSYS' automatic solution control sets the defaults to a new time integration scheme for use by first order transient equations. This is typically used for unsteady state thermal problems where θ = 1.0 (set by SOLCONTROL, ON); this is the backward Euler scheme. It is unconditionally stable and more robust for highly nonlinear thermal problems such as phase changes. The oscillation limit tolerance defaults to 0.0, so that the response first order eigenvalues can be used to more precisely determine a new time step value. Note — If you are using the Solution Controls dialog box to set solution controls, you can access all of these options [ALPHAD, BETAD, KBC, TIMINT, TINTP, TRNOPT] on the Transient tab. 3.
Write load data for each load step to a load step file. Command(s): LSWRITE GUI: Main Menu> Solution> Load Step Opts> Write LS File
4.
Save a backup copy of the database to a named file. Command(s): SAVE GUI: Utility Menu> File> Save As
5.
Start solution calculations. Other methods for multiple load steps are described in Chapter 1, “Getting Started with ANSYS” in the ANSYS Basic Analysis Guide. Command(s): LSSOLVE GUI: Main Menu> Solution> Solve> From LS Files
6.
After you have solved all load steps, leave SOLUTION. Command(s): FINISH GUI: Close the Solution menu.
8.6.3. Review the Results As in a nonlinear static analysis, you can use POST1 to postprocess results at a specific moment in time. Procedures are much the same as described previously for nonlinear static analyses. Again, you should verify that your solution has converged before you attempt to postprocess the results. Time-history postprocessing using POST26 is essentially the same for nonlinear as for linear transient analyses. See the postprocessing procedures outlined in Chapter 5, “Transient Dynamic Analysis”. More details of postprocessing procedures can be found in the ANSYS Basic Analysis Guide.
8.7. Sample Input for a Nonlinear Transient Analysis A sample input listing for a nonlinear transient analysis is shown below: ! Build the Model: /PREP7 --------FINISH !
! Similar to a linear full transient model, with ! these possible additions: nonlinear material ! properties, nonlinear elements
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–61
Chapter 8: Nonlinear Structural Analysis ! Apply Loads and Obtain the Solution: /SOLU ANTYPE,TRANS ! TRNOPT,FULL by default --! Establish initial conditions as in linear full --! transient analysis LSWRITE ! Initial-condition load step NLGEOM,ON ! Nonlinear geometric effects (large deformations) SSTIF,ON ! Stress stiffening effects ! NROPT=AUTO by default: Program will choose appropriate Newton-Raphson and ! Adaptive Descent options, depending on ! nonlinearities encountered ! Loads: F,... D,... ! Load Step Options: TIME,... ! TIME at end of load step DELTIM,... ! Time step controls (starting, min, max) AUTOTS,ON ! Automatic time stepping, including bisection ! KBC=0 by default (ramped loading) ! Dynamic Options: ALPHAD,... ! Mass damping TIMINT,ON ! TIMINT,ON by default, unless you turned it OFF for ! initial-condition load step ! Nonlinear Options: CNVTOL,... ! Convergence criteria ! NEQIT=25 by default NCNV,,,... ! Nonconvergence termination controls PRED,ON ! Predictor ON OUTRES,ALL,ALL ! Results for every substep written to database LSWRITE ! First "real" transient load step --! Additional load steps, as needed --LSSOLVE,1,3 ! Initiate multiple l.s. solution SAVE FINISH ! ! Review the Results: /POST26 ! Time-History Postprocessor SOLU,2,CNVG ! Check convergence SOLU,3,FOCV PRVAR,2,3 NSOL,... ! Store results (displacements, stresses, etc.) as ! variables PLVAR,... ! Graph results vs. TIME to evaluate general quality ! of analysis, determine critical time step, etc. FINISH ! /POST1 ! General Postprocessor SET,... ! Read results from desired time step PLDISP,... ! Postprocess as desired PLNSOL,... NSORT,... PRNSOL,... FINISH
See the ANTYPE, TRNOPT, LSWRITE, NLGEOM, SSTIF, NROPT, TIME, DELTIM, AUTOTS, KBC, ALPHAD, TIMINT, CNVTOL, NEQIT, NCNV, PRED, OUTRES, LSSOLVE, and SOLU command descriptions for more information.
8.8. Restarts Restart procedures for a transient analysis are essentially the same as for a static analysis; see Section 3.16: Restarting an Analysis in the ANSYS Basic Analysis Guide.
8–62
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.10: Tips and Guidelines for Nonlinear Analysis
8.9. Using Nonlinear (Changing-Status) Elements Nonlinear elements display an abrupt change in stiffness when they experience a change in status. For example, when a cable goes slack, its stiffness suddenly drops to zero. When two separate bodies come into contact, their overall stiffness changes drastically. These and other status-dependent stiffness changes can be modeled by using nonlinear elements (described below), by applying birth and death options to applicable elements (see the ANSYS Advanced Analysis Techniques Guide), or by changing material properties [MPCHG]. Some of the nonlinear element features described below are available only in the ANSYS Multiphysics, ANSYS Mechanical, and ANSYS Structural products only. See the ANSYS Elements Reference for details. •
COMBIN7
•
COMBIN14
•
COMBIN37
•
COMBIN39
•
COMBIN40
•
CONTAC12 and CONTAC52
•
TARGE169, TARGE170, CONTA171, CONTA172, CONTA173, CONTA174, and CONTA175
•
LINK10
•
SHELL41
•
SOLID65
8.9.1. Element Birth and Death Sometimes, an element's status changes between "existent" and "nonexistent." The birth and death options [EKILL, EALIVE, ESTIF] (Main Menu> Solution> Load Step Opts> Other) can be used to deactivate or reactivate selected elements in such cases. The birth and death feature is discussed in detail in Chapter 11, “Element Birth and Death” in the ANSYS Advanced Analysis Techniques Guide.
8.10. Tips and Guidelines for Nonlinear Analysis This section describes tips and guidelines that can help you to perform a nonlinear analysis.
8.10.1. Starting Out with Nonlinear Analysis By taking your time and proceeding with reasonable caution, you can avoid many difficulties commonly associated with nonlinear analyses. The following suggestions should be useful.
8.10.1.1. Be Aware of How the Program and Your Structure Behave If you have not used a particular nonlinear feature before, construct a very simple model (that is, containing only a few elements), and make sure you understand how to handle this feature before you use it in a large, complicated model. •
Gain preliminary insight into your structure's behavior by analyzing a preliminary simplified model first. For nonlinear static models, a preliminary linear static analysis can reveal which regions of your model will first experience nonlinear response, and at what load levels these nonlinearities will come into play. For nonlinear transient dynamic analyses, a preliminary model of beams, masses, and springs can provide insight into the structure's dynamics at minimal cost. Preliminary nonlinear static, linear transient dynamic,
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–63
Chapter 8: Nonlinear Structural Analysis and/or modal analyses can also help you to understand various aspects of your structure's nonlinear dynamic response before you undertake the final nonlinear transient dynamic analysis. •
Read and understand the program's output messages and warnings. At a minimum, before you try to postprocess your results, make sure your problem converged. For path-dependent problems, the printout's equilibrium iteration record can be especially important in helping you to determine if your results are valid or not.
8.10.1.2. Keep It Simple •
Keep your final model as simple as possible. If you can represent your 3-D structure as a 2-D plane stress, plane strain, or axisymmetric model, do so. If you can reduce your model size through the use of symmetry or antisymmetry surfaces, do so. (However, if your model is loaded antisymmetrically, you can generally not take advantage of antisymmetry to reduce a nonlinear model's size. Antisymmetry can also be rendered inapplicable by large deflections.) If you can omit a nonlinear detail without affecting results in critical regions of your model, do so.
•
Model transient dynamic loading in terms of static-equivalent loads whenever possible.
•
Consider substructuring the linear portions of your model to reduce the computational effort required for intermediate load or time increments and equilibrium iterations.
8.10.1.3. Use an Adequate Mesh Density •
Recognize that regions undergoing plastic deformation require a reasonable integration point density (mesh density is particularly important in plastic-hinge regions). Higher-order elements use only the corner integration points for nonlinear analyses, thus lower-order elements provide the same accuracy as higherorder elements. However, the 18x elements are recommended for nonlinear analyses.
•
Provide an adequate mesh density on contact surfaces to allow contact stresses to be distributed in a smooth fashion.
•
Provide a mesh density adequate for resolving stresses. Areas where stresses or strains are of interest require a relatively fine mesh compared to that needed for displacement or nonlinearity resolution.
•
Use a mesh density adequate to characterize the highest mode shape of interest. The number of elements needed depends on the elements' assumed displacement shape functions, as well as on the mode shape itself.
•
Use a mesh density adequate to resolve any transient dynamic wave propagation through your structure. If wave propagation is important, then provide at least 20 elements to resolve one wavelength.
8.10.1.4. Apply the Load Gradually •
For nonconservative, path-dependent systems, you need to apply the load in small enough increments to ensure that your analysis will closely follow the structure's load-response curve.
•
You can sometimes improve the convergence behavior of conservative systems by applying the load gradually, so as to minimize the number of Newton-Raphson equilibrium iterations required.
8.10.2. Overcoming Convergence Problems When performing a nonlinear analysis you may encounter convergence difficulties due to a number of reasons. Some examples may be initially open contact surfaces causing rigid body motion, large load increments causing nonconvergence, material instabilities, or large deformations causing mesh distortion that result in element shape errors. Solution control (SOLCONTROL) automatically adjusts solution parameters and attempts to obtain
8–64
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.10: Tips and Guidelines for Nonlinear Analysis a robust, accurate solution. In addition, several tools are available in ANSYS that can help you identify potential problems before, during, and after a solution. CHECK, MCHECK, and CNCHECK commands help you verify if there are any obvious problems with the model before you start the solution. The CHECK command does an overall verification of the model, including missing elastic properties, unconstrained model, and element shape checks. The MCHECK command can help you identify defects in the mesh such as holes or cracks, especially when the mesh is imported from a third party software. The CNCHECK command provides the initial contact status of contact pairs, identifying whether the contacts are initially open or closed. If, for example, a part in your model is constrained only through contact with other parts and if the contact surfaces are open, the CNCHECK command can help you identify this potential error condition. When you analyze models with large deformations, some portions of the initial mesh can become highly distorted. Highly distorted elements can take on unacceptable shapes, providing inaccurate results. This can cause your nonlinear solution to stop. When this happens, use the ESCHECK command to perform shape checking of deformed elements in the postprocessor (based on the current set of results in database). This deformed-shape checker will help you to identify the portions of your model that require different meshing, thereby allowing them to retain acceptable shapes. Using ESCHECK at different time points will help you to identify the load conditions that cause mesh deterioration. A convergence failure can also indicate a physical instability in the structure, or it can merely be the result of some numerical problem in the finite element model. The following sections detail some of the techniques that you can use to attempt to improve the convergence performance of your analysis.
8.10.2.1. Performing Nonlinear Diagnostics The nonlinear diagnostics tool NLDIAG can help you find problems in your model when an analysis will not converge. Identify Regions of High Residual Forces Issue the NLDIAG,NRRE command to write the Newton-Raphson residuals from equilibrium iterations to a file. You can then contour plot the residual forces via the PLNSOL,NRRE command, which will help to identify regions of high residual forces. Such a capability can be useful when you experience convergence difficulties in the middle of a load step, where the model has a large number of contact surfaces and other nonlinearities. You can restart the analysis and issue an NLDIAG,NRRE command to write out the residuals. By tracking the way the residuals change over several equilibrium iterations you can identify a portion of your model where large residuals persist. You can then focus on the nonlinearities in that area (for example, a contact pair's properties) instead of having to deal with the entire model. Identify Problem Elements
Typically, nonlinear analyses fail to converge for the following reasons:
•
Too large a distortion
•
Elements contain nodes that have near zero pivots (nonlinear analyses)
•
Too large a plastic or creep strain increment
•
Elements where mixed u-P constraints are not satisfied (mixed U-P option of 18x solid elements only)
ANSYS has default limits which, when exceeded, determine when convergence criteria have been violated. Some limits are user-controlled; for example, the CUTCONTROL command sets the maximum plastic/creep strain increments allowed in an iteration. Other limits are fixed.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–65
Chapter 8: Nonlinear Structural Analysis The NLDIAG,EFLG command identifies elements that violate the above criteria and records them in a file (Jobname.ndxxx). Process the Tracked Results Issue the NLDPOST command to process the .ndxxx nonlinear diagnostics files. The command creates components of elements that violate a certain criterion for a particular equilibrium iteration (or iterations). Monitor the Diagnostics Results in Real Time The NLHIST command allows you to monitor results of interest in real time during solution. Before starting the solution, you can request nodal data such as displacements or reaction forces at specific nodes. You can also request element nodal data such as stresses and strains at specific elements to be graphed. Pair-based contact data are also available. The result data are written to a file named Jobname.nlh. For example, a reaction force-deflection curve could indicate when possible buckling behavior occurs. Nodal results and contact results are monitored at every converged substep while element nodal data are written as specified via the OUTRES setting. You can also track results during batch runs. Either access the ANSYS Launcher and select File Tracking from the Tools menu, or type nlhist81 at the command line. Use the supplied file browser to navigate to your Jobname.nlh file, and click on it to invoke the tracking utilty. You can use this utilty to read the file at any time, even after the solution is complete (the data in the file must be formatted correctly).
8.10.2.2. Tracking Convergence Graphically As a nonlinear structural analysis proceeds, ANSYS computes convergence norms with corresponding convergence criteria each equilibrium iteration. Available in both batch and interactive sessions, the Graphical Solution Tracking (GST) feature displays the computed convergence norms and criteria while the solution is in process. By default, GST is ON for interactive sessions and OFF for batch runs. To turn GST on or off, use either of the following: Command(s): /GST GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> Grph Solu Track Figure 8.24: “Convergence Norms Displayed By the Graphical Solution Tracking (GST) Feature” shows a typical GST display:
8–66
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.10: Tips and Guidelines for Nonlinear Analysis
Figure 8.24 Convergence Norms Displayed By the Graphical Solution Tracking (GST) Feature
8.10.2.3. Using Automatic Time Stepping •
•
Be sure to place an upper limit on the time step size using DELTIM or NSUBST, especially for complicated models. This ensures that all of the modes and behaviors of interest will be accurately included. This can be important in the following situations: –
Problems that have only localized dynamic behavior (for example, turbine blade and hub assemblies) in which the low-frequency energy content of the system could dominate the high-frequency areas.
–
Problems with short ramp times on some of their loads. If the time step size is allowed to become too large, ramped portions of the load history may be inaccurately characterized.
–
Problems that include structures that are continuously excited over a range of frequencies (for example, seismic problems).
Take care when modeling kinematic structures (systems with rigid-body motions). These guidelines can usually help you obtain a good solution: –
Incorporate significant numerical damping (0.05 < γ < 0.1 on the TINTP command) into the solution to filter out the high frequency noise, especially if a coarse time step is used. Do not use α-damping (mass matrix multiplier, ALPHAD command) in a dynamic kinematic analysis, as it will dampen the rigid body motion (zero frequency mode) of the system.
– Avoid imposed displacement history specifications, because imposed displacement input has (theoretically) infinite jumps in acceleration, which causes stability problems for the Newmark time-integration algorithm. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–67
Chapter 8: Nonlinear Structural Analysis
8.10.2.4. Using Line Search Line search [LNSRCH] can be useful for enhancing convergence, but it can be expensive (especially with plasticity). You might consider setting line search on in the following cases: •
When your structure is force-loaded (as opposed to displacement-controlled).
•
If you are analyzing a "flimsy" structure which exhibits increasing stiffness (such as a fishing pole).
•
If you notice (from the program output messages) oscillatory convergence patterns.
8.10.2.5. Using the Arc-Length Method You can use the arc-length method [ARCLEN and ARCTRM] to obtain numerically stable solutions for many physically unstable structures. When using the arc-length method, please keep in mind the following considerations: •
The arc-length method is restricted to static analyses with proportional (ramped) loads only.
•
The program calculates the reference arc-length radius from the load (or displacement) increment of the first iteration of the first substep, using the following formula:
Reference Arc -Length Radius =
(Total Load or Displacement) NSB BSTP
where NSBSTP is the number of substeps specified in the NSUBST command. When choosing the number of substeps, consider that more substeps will result in a longer solution time. Ideally, you want to choose the minimum number of substeps required to produce an optimally efficient solution. You might have to take an "educated guess" of the desired number of substeps, and adjust and re-analyze as needed. •
Do not use line search [LNSRCH], the predictor [PRED], adaptive descent [NROPT,,,ON], automatic time stepping [AUTOTS, TIME, DELTIM], or time-integration effects [TIMINT] when the arc-length method is active.
•
Do not attempt to base convergence on displacement [CNVTOL,U]. Use the force criteria [CNVTOL,F] instead.
•
To help minimize solution time with the arc-length method, the maximum number of equilibrium iterations in a single substep [NEQIT] should be less than or equal to 15.
•
If an arc-length solution fails to converge within the prescribed maximum number of iterations [NEQIT], the program will automatically bisect and continue the analysis. Bisection will continue either until a converged solution is obtained, or until the minimum arc-length radius is used (the minimum radius is defined by NSBSTP [NSUBST] and MINARC [ARCLEN]).
•
In general, you cannot use this method to obtain a solution at a specified load or displacement value because the value changes (along the spherical arc) as equilibrium is achieved. Note in Figure 8.4: “Traditional Newton-Raphson Method vs. Arc-Length Method” how the specified load point. The actual load at convergence is somewhat less.
•
8–68
F1a
is only used as a starting
Similarly, it can be difficult to determine a value of limiting load or deflection within some known tolerance when using the arc-length method in a nonlinear buckling analysis. You generally have to adjust the reference arc-length radius (using NSUBST) by trial-and-error to obtain a solution at the limit point. It might
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.10: Tips and Guidelines for Nonlinear Analysis be more convenient to use standard Newton-Raphson iterations with bisection [AUTOTS] to determine values of nonlinear buckling loads. •
You should usually avoid using the JCG solver [EQSLV] in conjunction with the arc-length method, because the arc-length procedure might result in a negative definite stiffness matrix (negative pivot), which can cause a solution failure with this solver.
•
You can freely switch from the Newton-Raphson iteration method to the arc-length method at the start of any load step. However, to switch from arc-length to Newton-Raphson iterations, you must terminate the analysis and restart, deactivating the arc-length method in the first load step of the restart [ARCLEN,OFF]. An arc-length solution terminates under these conditions: – When limits defined by the ARCTRM or NCNV commands are reached – When the solution converges at the applied load – When you use an abort file (Jobname.ABT) See the ANSYS Basic Analysis Guide for a discussion of termination and restart procedures.
•
Use the load-deflection curve as a guide for evaluating and adjusting your analysis to help you achieve the desired results. It is usually good practice to graph your load-deflection curve (using POST26 commands) with every analysis.
•
Often, an unsuccessful arc-length analysis can be traced to an arc-length radius that is either too large or too small. "Drifting back," in which the analysis retraces its steps back along the load-deflection curve, is one typical difficulty that is caused by using too large or too small an arc-length radius. Study the loaddeflection curve to understand this problem. You can then use the NSUBST and ARCLEN commands to adjust the arc-length radius size and range, as appropriate.
•
The total arc-length load factor (item ALLF on the SOLU command) can be either positive or negative. Similarly, TIME, which in an arc-length analysis is related to the total arc-length load factor, can also be either positive or negative. Negative values of ALLF or TIME indicate that the arc-length feature is applying load in the reverse direction, in order to maintain stability in the structure. Negative ALLF or TIME values can be commonly encountered in various snap-through analyses.
•
When reading arc-length results into the database for POST1 postprocessing [SET], you should always reference the desired results data set by its load step and substep number (LSTEP and SBSTEP) or by its data set number (NSET). Do not reference results by a TIME value, because TIME in an arc-length analysis is not always monotonically increasing. (A single value of TIME might reference more than one solution.) Additionally, the program cannot correctly interpret negative TIME values (which might be encountered in a snap-through analysis).
•
If TIME becomes negative, remember to define an appropriate variable range [/XRANGE or /YRANGE] before creating any POST26 graphs.
8.10.2.6. Artificially Inhibit Divergence in Your Model's Response If you do not want to use the arc-length method to analyze a force-loaded structure that starts at, or passes through, a singular (zero stiffness) configuration, you can sometimes use other techniques to artificially inhibit divergence in your model's response: •
In some cases, you can use imposed displacements instead of applied forces. This approach can be used to start a static analysis closer to the equilibrium position, or to control displacements through periods of unstable response (for example, snap-through or postbuckling).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–69
Chapter 8: Nonlinear Structural Analysis •
Another technique that can be effective in circumventing problems due to initial instability is running a static problem as a "slow dynamic" analysis (that is, using time-integration effects in an attempt to prevent the solution from diverging in any one load step).
•
You can also apply temporary artificial stiffness to unstable DOFs, using control elements (such as COMBIN37), or using the birth and death option on other elements. The idea here is to artificially restrain the system during intermediate load steps in order to prevent unrealistically large displacements from being calculated. As the system displaces into a stable configuration, the artificial stiffness is removed.
8.10.2.7. Turn Off Extra Element Shapes ANSYS provides "incompatible" modes" formulation (also referred to as "extra shapes") for modeling bending applications. If your problem is predominantly bulk deformation, then you may choose to turn extra shapes off to reduce CPU/storage requirements and enhance convergence. However, doing so precludes the ability to model any bending.
8.10.2.8. Using Birth and Death Wisely Realize that any sudden change in your structure's stiffness matrix is likely to cause convergence problems. When activating or deactivating elements, try to spread the changes out over a number of substeps. (Use a small time step size if necessary to accomplish this.) Also be aware of possible singularities (such as sharp reentrant corners) that might be created as you activate or deactivate elements. Such singularities can cause convergence problems.
8.10.2.9. Read Your Output Remember that the ANSYS program performs a nonlinear analysis as a series of linear approximations with corrections. The program printout gives you continuous feedback on the progress of these approximations and corrections. (Printout either appears directly on your screen, is captured on Jobname.OUT, or is written to some other file [/OUTPUT].) You can examine some of this same information in POST1, using the PRITER command, or in POST26, using the SOLU and PRVAR commands. You should make sure that you understand the iteration history of your analysis before you accept the results. In particular, do not dismiss any program error or warning statements without fully understanding their meaning. A typical nonlinear output listing is shown in Figure 8.25: “Typical Nonlinear Output Listing”.
Figure 8.25 Typical Nonlinear Output Listing SOLVE command echo
*****
Checking Logic
*** NOTE *** CP= 13.891 TIME= 11:09:22 Nonlinear analysis, NROPT set to 1 (full Newton-Raphson solution procedure) for all DOFs.
Load step summary table
8–70
ANSYS SOLVE
COMMAND
L O A D
*****
S T E P
O P T I O N S
LOAD STEP NUMBER. . . . . . . . . . . . . TIME AT END OF THE LOAD STEP. . . . . . . AUTOMATIC TIME STEPPING . . . . . . . . . INITIAL NUMBER OF SUBSTEPS . . . . . . MAXIMUM NUMBER OF SUBSTEPS . . . . . . MINIMUM NUMBER OF SUBSTEPS . . . . . . MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS. STEP CHANGE BOUNDARY CONDITIONS . . . . . TERMINATE ANALYSIS IF NOT CONVERGED . . . CONVERGENCE CONTROLS. . . . . . . . . . . PRINT OUTPUT CONTROLS . . . . . . . . . . DATABASE OUTPUT CONTROLS ITEM FREQUENCY COMPONENT BASI -10
. . . . . . . . . . .
. . . . . . . . . . .
. 2 . 200.00 . ON . 100 . 10000 . 10 . 15 . NO .YES (EXIT) .USE DEFAULTS .NO PRINTOUT
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.11: Sample Nonlinear Analysis (GUI Method) Load step 2 substep 1
FORCE CONVERGENCE VALUE = 0.2006E+06 CRITERION= 1125. EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1272E-01 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.1272E-01 FORCE CONVERGENCE VALUE = 4267. CRITERION= 480.2 EQUIL ITER 2 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.9019E-03 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = -0.9019E-03 FORCE CONVERGENCE VALUE = 1751. CRITERION= 488.2 EQUIL ITER 3 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1746E-03 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.1746E-03 FORCE CONVERGENCE VALUE = 778.5 CRITERION= 497.7 EQUIL ITER 4 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.6943E-04 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.6943E-04 FORCE CONVERGENCE VALUE = 347.4 CRITERION= 507.7 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 4 *** LOAD STEP 2 SUBSTEP 1 COMPLETED. CUM ITER = 7 *** TIME = 101.000 TIME INC = 1.00000
Load step 2 substep 2
FORCE CONVERGENCE VALUE = 0.6674E+05 CRITERION= 594.3 EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.4318E-02 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.4318E-02 FORCE CONVERGENCE VALUE = 626.2 CRITERION= 502.9 EQUIL ITER 2 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.8570E-04 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.8570E-04 FORCE CONVERGENCE VALUE = 77.87 CRITERION= 512.9 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 2 *** LOAD STEP 2 SUBSTEP 2 COMPLETED. CUM ITER = 9 *** TIME = 102.000 TIME INC = 1.00000
Load step 2 substep 3 Equilbrium iteration summaries
FORCE CONVERGENCE VALUE = 0.1333E+05 CRITERION= 575.4 EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.5329E-02 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = -0.5329E-02 FORCE CONVERGENCE VALUE = 8237. CRITERION= 534.2 EQUIL ITER 2 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.3628E-02 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.3628E-02 FORCE CONVERGENCE VALUE = 3905. CRITERION= 532.9 EQUIL ITER 3 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1451E-02 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.1451E-02 FORCE CONVERGENCE VALUE = 1135. CRITERION= 540.3 EQUIL ITER 4 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1034E-03 LINE SEARCH PARAMETER = 0.9578 SCALED MAX DOF INC = 0.9905E-04 FORCE CONVERGENCE VALUE = 41.95 CRITERION= 551.4 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 4
Substep summary
*** LOAD STEP 2 *** TIME = 103.500
SUBSTEP
3 COMPLETED. TIME INC = 1.50000
CUM ITER =
13
8.10.2.10. Graph the Load and Response History This verification technique may be considered to be a graphical combination of two other techniques: checking for reasonableness, and reviewing the iteration history. POST26 graphs of load and response histories should agree with your informed expectations about your structure's behavior. The results of interest (displacements, reaction forces, stresses, and so on) should show relatively smooth response histories. Any non-smoothness may indicate that too coarse of a time step was used.
8.11. Sample Nonlinear Analysis (GUI Method) In this sample analysis, you will run a nonlinear analysis of an elastic-plastic circular plate under the action of a dead load and a cyclic point load. You will define a kinematic hardening plasticity curve, as well as load step options, the maximum and minimum number of substeps for a load step, and the various load steps that describe externally applied loads. You will also learn how to interpret the monitor file that ANSYS writes for a nonlinear analysis.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–71
Chapter 8: Nonlinear Structural Analysis ANSYS uses an incremental solution procedure to obtain a solution to a nonlinear analysis. In this example, the total external load within a load step is applied in increments over a certain number of substeps. As described earlier in this chapter, ANSYS uses a Newton-Raphson iterative procedure to solve each substep. You must specify the number of substeps for each load step, since this number controls the size of the initial load increment applied in the first substep of the each load step. ANSYS automatically determines the size of the load increment for each subsequent substep in a load step. You can control the size of the load increment for these subsequent substeps by specifying the maximum and minimum number of substeps. If you define the number of substeps, the maximum and minimum number of substeps all to be the same, then ANSYS uses a constant load increment for all substeps within the load step.
8.11.1. Problem Description In this example, you will use an axisymmetric model for the plate, using four-node PLANE42 elements with the axisymmetric option to mesh the model. You will perform a geometrically nonlinear analysis. Specify the kinematic constraints as follows: The nodes located at the center of the plate are constrained to have zero radial displacement. The nodes located at the outer edge are constrained to have zero radial and axial displacement. You will apply the dead load in load step 1 and the cyclic point load in six subsequent load steps. See Section 8.11.3: Problem Sketch. You will specify 10 substeps for the first load to ensure that the increment of the dead load applied over the first substep is 1/10 of the total load of 0.125 N/m2. You will also specify a maximum of 50 and a minimum of 5 substeps to ensure that if the plate exhibits a severe nonlinear behavior during the solution, then the load increment can be cut back to 1/50 the total load. If the plate exhibits mild nonlinear behavior, then the load increment can be increased up to 1/5 the size of the total load. For the subsequent six load steps that apply the cyclic point load, you will specify 4 substeps, with a maximum of 25 and a minimum of 2 substeps. For this example, you will monitor the history over the entire solution of the vertical displacement of the node at the location where the point cyclic load is applied and the reaction force at the node located at the bottom of the clamped edge.
8.11.2. Problem Specifications The circular plate has a radius of 1.0 m and a thickness of 0.1 m. The following material properties are used for this problem: EX = 16911.23 Pa PRXY = 0.3 The kinematic hardening plasticity curve for the material is: Log Strain
True Stress (Pa)
0.001123514
19.00
0.001865643
22.80
0.002562402
25.08
0.004471788
29.07
0.006422389
31.73
The plate has a dead load acting as a uniform pressure of 0.125N/m2. The history of the cyclic point load is shown here: 8–72
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.11: Sample Nonlinear Analysis (GUI Method)
Figure 8.26 Cyclic Point Load History
8.11.3. Problem Sketch 23 45563 4 ,7./ 098:1; <%=
!" # !%$&'# ()" &*+-,-.'/ .0..'1
" *><$ 4 +
8.11.3.1. Set the Analysis Title and Jobname 1.
Choose menu path Utility Menu> File> Change Title.
2.
Type the text "Cyclic loading of a fixed circular plate."
3.
Click on OK.
4.
Choose menu path Utility Menu> File> Change Jobname. The Change Jobname dialog box appears.
5.
Type the text “axplate” in the entry box and click OK.
8.11.3.2. Define the Element Types 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
In the list on the left, click once on "Structural Solid."
4.
In the list on the right, click once on "Quad 4node 42."
5.
Click on OK. The Library of Element Types dialog box closes.
6.
Click on Options. The PLANE42 element type options dialog box appears.
7.
In the scroll box for element behavior, scroll to "Axisymmetric" and select it.
8.
Click on OK.
9.
Click on Close in the Element Types dialog box.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–73
Chapter 8: Nonlinear Structural Analysis
8.11.3.3. Define Material Properties 1.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
2.
In the Material Models Available window, double-click on the icons next to the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
3.
Enter 16911.23 for EX (Young's modulus).
4.
Enter .3 for PRXY (Poisson's ratio).
5.
Click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
8.11.3.4. Specify the Kinematic Hardening material model (KINH) 1.
In the Material Models Available window, double-click on the following options: Nonlinear, Inelastic, Rate Independent, Kinematic Hardening Plasticity, von Mises Plasticity, Multilinear (General). A dialog box appears.
2.
Enter the following Strain/Stress value pair in the table: 0.00112, 19.0.
3.
Click on the Add Point button, and enter the next Strain/Stress value pair: 0.00187, 22.8.
4.
Repeat the previous step to enter the following Strain/Stress value pairs: 0.00256, 25.1; 0.00447, 29.1; 0.00642, 31.7.
5.
Click on OK.
6.
Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
8.11.3.5. Label Graph Axes and Plot Data Tables 1.
Choose menu path Utility Menu> PlotCtrls> Style> Graphs> Modify Axes. The Axes Modifications for Graph Plots dialog box appears.
2.
Enter Total Strain for the X-axis label.
3.
Enter True Stress for the Y-axis label and click OK.
4.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
5.
In the Material Models Defined window, double-click in Material Model Number 1, and Multilinear Kinematic (General). The dialog box appears that includes the Strain/Stress data pairs that you entered.
6.
Click on the Graph button. A graph of the data table values appears in the Graphics window. If necessary, revise the stress/strain values and click on the Graph button again. Repeat revisions and graphing as needed until you are satisfied with the graphed results. Click on OK.
7.
Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
8.
Click on SAVE_DB on the ANSYS Toolbar.
8.11.3.6. Create Rectangle 1.
Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.
2.
Type "radius=1.0" in the Selection field and click Accept. This value is the radius of the plate.
3.
Type "thick=0.1" in the Selection field and click Accept. This value is the thickness of the plate. Click Close.
8–74
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.11: Sample Nonlinear Analysis (GUI Method) 4.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Areas> Rectangle> By Dimensions. The Create Rectangle by Dimensions dialog box appears.
5.
Enter "0, radius" for X-coordinates.
6.
Enter "0, thick" for Y-coordinates and click on OK. A rectangle appears in the ANSYS Graphics window.
7.
Choose menu path Utility Menu> Plot> Lines.
8.11.3.7. Set Element Size 1.
Choose menu path Main Menu> Preprocessor> Meshing> MeshTool. The MeshTool dialog box appears.
2.
Click Size Controls> Lines> Set. The Element Size on Picked Lines picking menu appears. Click on the two vertical lines (2 and 4). Click OK on the picking menu. The Element Sizes on Picked Lines dialog box appears.
3.
Enter 8 for number of element divisions and click on OK.
4.
Repeat these steps (1-3), but choose horizontal lines 1 and 3, and specify 40 element divisions.
8.11.3.8. Mesh the Rectangle 1.
On the MeshTool, pick Quad and Map, then click MESH. The Mesh Areas picking menu appears.
2.
Click on Pick All.
3.
Click on SAVE_DB on the ANSYS Toolbar.
4.
Click on Close on the MeshTool.
8.11.3.9. Assign Analysis and Load Step Options 1.
Choose menu path Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options. The Static or Steady-State Analysis dialog box appears.
2.
Turn large deformation effects ON and click OK.
3.
Choose menu path Main Menu> Solution> Load Step Opts> Output Ctrls> DB/Results File. The Controls for Database and Results File Writing dialog box appears.
4.
Verify that All items are selected, and choose Every substep for the File write frequency. Click OK.
8.11.3.10. Monitor the Displacement In this step, you monitor the displacement of the node located at the axes of symmetry, as well as the reaction force at the fixed end of the plate. 1.
Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.
2.
Type "ntop = node(0,thick,0.0)" in the Selection field and click Accept.
3.
Type "nright = node(radius,0.0,0.0)" in the Selection field and click Accept, then Close.
4.
Choose menu path Main Menu> Solution> Load Step Opts> Nonlinear> Monitor. The Monitor picking menu appears.
5.
Type "ntop" in the picker and press RETURN. Click OK in the picking menu. The Monitor dialog box appears.
6.
In the scroll box for Quantity to be monitored, scroll to "UY" and select it. Click OK.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–75
Chapter 8: Nonlinear Structural Analysis 7.
Choose menu path Main Menu> Solution> Load Step Opts> Nonlinear> Monitor. The Monitor picking menu appears.
8.
Type "nright" in the picker and press RETURN. Click OK in the picking menu. The Monitor dialog box appears.
9.
In the scroll box for Variable to redefine, scroll to "Variable 2" and select it. In the scroll box for Quantity to be monitored, scroll to "FY" and select it. Click OK.
8.11.3.11. Apply Constraints 1.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears.
2.
Select Nodes and By Location in the first two selection boxes. Verify that X coordinates are selected, and enter "radius" in the Min, Max field. Click OK.
3.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears.
4.
Click Pick All. The Apply U,ROT on Nodes dialog box appears.
5.
Click on "All DOF" for DOFs to be constrained. Click OK.
6.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears. Verify that Nodes, By Location, and X coordinates are selected. Enter "0" in the Min, Max field and click OK. This will select the nodes at the X=0 position.
7.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears.
8.
Click Pick All. The Apply U,ROT on Nodes dialog box appears.
9.
Click on "UX" for DOFs to be constrained. Click on All DOF to deselect it.
10. Enter "0.0" as the Displacement value. Click OK. 11. Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears. Verify that Nodes and By Location are selected. 12. Click on Y coordinates and enter "thick" in the Min, Max field. Click OK. 13. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Pressure> On Nodes. The Apply PRES on Nodes picking menu appears. 14. Click on Pick All. The Apply PRES on nodes dialog box appears. 15. Enter "0.125" in the Load PRES value field and click OK. 16. Choose menu path Utility Menu> Select> Everything. 17. Click on SAVE_DB on the ANSYS Toolbar.
8.11.3.12. Solve the First Load Step 1.
Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Time and Substps. The Time and Substep Options dialog appears.
2.
Enter 10 as the number of substeps, enter 50 as the maximum number of substeps, and enter 5 as the minimum number of substeps. Click OK.
3.
Choose menu path Main Menu> Solution> Solve> Current LS. Review the information in the /STAT window, and click on Close.
4.
Click on OK on the Solve Current Load Step dialog box.
8–76
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.11: Sample Nonlinear Analysis (GUI Method) 5.
Click on Close on the Information dialog box when the solution is done.
6.
Choose Utility Menu> Plot> Elements.
8.11.3.13. Solve the Next Six Load Steps 1.
Choose Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.
2.
Enter "f = 0.010" in the Selection field and click on Accept. Click on Close.
3.
Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Time and Substps. The Time and Substep Options dialog appears.
4.
Enter "4" for the number of substeps, "25" for the maximum number of substeps, and "2" for the minimum number of substeps. Click OK.
5.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment> On Nodes. The Apply F/M on Nodes picking menu appears.
6.
Enter "ntop" in the picker and press RETURN. Click OK in the Apply F/M on Nodes picking menu. The Apply F/M on Nodes dialog box appears.
7.
Select "FY" in the Direction of force/mom selection box. Enter "-f" in the Force/moment value field. Click OK.
8.
Choose menu path Main Menu> Solution> Solve> Current LS. Review the information in the /STAT window, and click on Close.
9.
Click on OK on the Solve Current Load Step dialog box.
10. Click on Close on the Information dialog box when the solution is done. 11. Repeat Steps 5-10, entering "f" in the Force/moment value field at Step 7. 12. Repeat Steps 5-11 two more times, for a total of three cycles (six substeps). 13. Click on SAVE_DB on the ANSYS Toolbar.
8.11.3.14. Review the Monitor File 1.
Choose menu path Utility Menu> List> Files> Other. The List File dialog box appears. Select the axplate.mntr file and click on OK.
2.
Review the time step size, vertical displacement, and reaction force evolution over the entire solution.
3.
Click Close.
8.11.3.15. Use the General Postprocessor to Plot Results. 1.
Choose menu path Main Menu> General Postproc> Read Results> Last Set.
2.
Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears.
3.
Click on Def + undef edge for items to be plotted. Click OK. The deformed mesh appears in the ANSYS Graphics window.
4.
Choose menu path Main Menu> General Postproc> Plot Results> Contour Plot> Element Solu. The Contour Element Solution Data dialog box appears.
5.
In the selection box on the left, choose Strain-plastic. In the selection box on the right, choose Eqv plastic EPEQ. Click OK. The contour plot appears in the Graphics window.
6.
Choose Utility Menu> Plot> Elements. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–77
Chapter 8: Nonlinear Structural Analysis
8.11.3.16. Define Variables for Time-History Postprocessing 1.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears.
2.
Verify that Nodes and By Num/Pick are selected in the first two boxes. Click OK. The Select nodes picking menu appears.
3.
Type "ntop" in the picker and press RETURN. Click OK.
4.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears. Choose Elements in the first drop-down selection box. Choose Attached to in the second drop-down selection box. Verify that Nodes is selected. Click OK.
5.
Choose Utility Menu> Select> Everything.
6.
Choose Main Menu> TimeHist Postpro> Define Variables. The Defined Time-History Variables dialog box appears. Click on Add. The Add Time-History Variable dialog box appears.
7.
Click on Element results. Click OK. The Define Elemental Data picking menu appears.
8.
Click on the top left element in the ANSYS Graphics window. Click OK on the picking menu. The Define Nodal Data picking menu appears.
9.
Click on the top left node of the top left element. Click OK on the picking menu. The Define Element Results Variable dialog box appears.
10. Verify that the reference number of the variable is 2. 11. Choose Stress in the selection list on the left. Choose Y-direction SY in the selection list on the right. Click OK. The Defined Time-History Variables dialog box reappears, with a second variable listed (ESOL). The dialog box should show element number 281, node number 50, item S, component Y, and name SY. 12. Click on Add. Repeat steps 7-10, with variable reference number 3. 13. In the Define Element Results Variable dialog box, choose Strain-elastic in the selection list on the left. Choose Y-dir'n EPEL Y in the selection list on the right. Click OK. 14. Click on Add. Repeat steps 7-10, with variable reference number 4. 15. In the Define Element Results Variable dialog box, choose Strain-plastic in the selection list on the left. Choose Y-dir'n EPPL Y in the selection list on the right. Click OK. 16. Click on Close on the Defined Time-History Variables dialog box. 17. Choose menu path Main Menu> TimeHist Postpro> Math Operations> Add. The Add Time-History Variables dialog box appears. 18. Enter 5 for the reference number for result, enter 3 as the 1st variable, and enter 4 as the 2nd variable. Click OK. This adds the elastic and plastic strains that you stored as variables 3 and 4. Their sum is the total strain, and it is stored as variable 5.
8.11.3.17. Plot Time-History Results 1.
Choose menu path Main Menu> TimeHist Postpro> Settings> Graph. The Graph Settings dialog box appears.
2.
Click on Single variable for the X-axis variable and enter 5 as the single variable number. Click OK.
3.
Choose menu path Utility Menu> PlotCtrls> Style> Graphs> Modify Axes. The Axes Modifications for Graph Plots dialog box appears.
4.
Enter Total Y-Strain as the X-axis label.
5.
Enter Y-Stress as the Y-axis label. Click OK.
8–78
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.12: Sample Nonlinear Analysis (Command or Batch Method) 6.
Choose menu path Main Menu> TimeHist Postpro> Graph Variables. The Graph Time-History Variables dialog box appears.
7.
Enter 2 as the first variable to graph. Click OK.
8.11.3.18. Exit ANSYS 1.
Choose QUIT from the ANSYS Toolbar.
2.
Click on the save option you want, and click on OK.
8.12. Sample Nonlinear Analysis (Command or Batch Method) You can perform the example nonlinear static analysis of a copper cylinder impacting a rigid wall using the ANSYS commands shown below instead of GUI choices. Items prefaced by an exclamation point (!) are comments. /BATCH,LIST /title, Cyclic loading of a fixed circular plate /filnam,axplate /prep7 radius=1.0 ! Radius of the plate (m) thick=0.1 ! Thickness of plate (m) YM=16911.23 et,1,PLANE42,,,1 ! PLANE42 axisymmetric element mp,ex,1,YM mp,nuxy,1,0.3 ! Define a Kinematic Hardening Plasticity curve using the KINH material model tb,KINH,1,1,5 ! Define the true stress vs. total log strain curve for this material model ! using 5 points. First point defines the elastic limit tbpt,,0.001123514,19.00 tbpt,,0.001865643,22.80 tbpt,,0.002562402,25.08 tbpt,,0.004471788,29.07 tbpt,,0.006422389,31.73 ! Set the axles labels for the stress-strain curve plot /axlab,X,Log Strain (N/m^2) /axlab,Y,True Stress (N/m^2) tbpl,KINH,1
! Plot and verify the material stress-strain curve
! Define a rectangle which is the axisymmetric cross section of the plate. ! The rectangle has a length equal to the radius of the plate and a height equal ! to the thickness of the plate rect,,radius,,thick ! Select the left and right bounding lines of the created rectangle and set ! the line division to 8 (8 elements through the thickness of the plate) FLST,5,2,4,ORDE,2 FITEM,5,2 FITEM,5,4 CM,_Y,LINE LSEL, , , ,P51X !* CM,_Y1,LINE CMSEL,,_Y LESIZE,_Y1, , ,8,1, CMDEL,_Y CMDEL,_Y1 !*
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–79
Chapter 8: Nonlinear Structural Analysis
! Select the top and bottom bounding lines of the created rectangle and set ! the line division to 40 (40 elements through the radius of the plate) FLST,5,2,4,ORDE,2 FITEM,5,1 FITEM,5,3 CM,_Y,LINE LSEL, , , ,P51X !* CM,_Y1,LINE CMSEL,,_Y LESIZE,_Y1, , ,40,1, CMDEL,_Y CMDEL,_Y1 !* CM,_Y,AREA ASEL, , , , 1 CM,_Y1,AREA CHKMSH,'AREA' CMSEL,S,_Y amesh,all CMDEL,_Y CMDEL,_Y1 CMDEL,_Y2 fini /solve nlgeom,on! Turn on geometric nonlinearity ! Get the node numbers for the nodes located at the top ! of the axis of symmetry and at bottom right of the model ntop = node(0,thick,0) nright = node(radius,0,0) ! Activate the monitoring of the displacement and reaction force histories ! during the analysis. This will be written out to the monitor file ratch.mntr monitor,1,ntop,uy monitor,2,nright,fy outres,all,all
! Output all the results for all substeps to the ! results file for later postprocessing
! Select the nodes located at right end and constrain their radial (x) and ! axial (y) direction displacement to be zero. nsel,s,loc,x,radius d,all,all ! Select the nodes located at left end and constrain their radial (x) direction ! displacement to be zero. nsel,s,loc,x,0.0 d,all,ux,0.0 ! Define the load for Load Step 1. ! Select the nodes located at top surface of plate and apply a uniform pressure ! of 0.125 N/m^2 as dead load on the plate. nsel,s,loc,y,thick sf,all,pres,0.125 alls! Select all nodes ! Define the number of substeps (10). Also define maximum number of ! substeps (50), and the minimum number of substeps (5) for the automatic ! time stepping algorithm. nsub,10,50,5
8–80
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.12: Sample Nonlinear Analysis (Command or Batch Method) solve f = 0.01
! Solve load step 1 ! Define the parameter, f, used to apply ! the cyclic point load.
! Over six load steps apply a cyclic point load of magnitude f = 0.01 units ! applied at the center of the plate over three cycles ! Start Cycle 1 ! ---------------nsel,s,node,,ntop f,all,fy,-f nsel,all nsubst,4,25,2 solve nsel,s,node,,ntop f,all,fy,f nsel,all nsubst,4,25,2 solve
! Define load for load step 2 ! Set the number of substeps, max and min number ! of substeps ! Solve load step 2
! Define load for load step 3 ! Set the number of substeps, max and min number ! of substeps ! Solve load step 3
! Start Cycle 2 ! ---------------nsel,s,node,,ntop f,all,fy,-f nsel,all nsubst,4,25,2 solve nsel,s,node,,ntop f,all,fy,f nsel,all nsubst,4,25,2 solve
! Define load for load step 4 ! Set the number of substeps, max and min number ! of substeps ! Solve load step 4
! Define load for load step 5 ! Set the number of substeps, max and min number ! of substeps ! Solve load step 5
! Start Cycle 3 ! ---------------nsel,s,node,,ntop f,all,fy,-f nsel,all nsubst,4,25,2 solve nsel,s,node,,ntop f,all,fy,f nsel,all nsubst,4,25,2 solve save fini /post1 set,last ! (final state) pldi,2 ples,nl,epeq
! Define load for load step 6 ! Set the number of substeps, max and min number ! of substeps ! Solve load step 6 ! Define load for load step 7 ! Set the number of substeps, max and min number ! of substeps. ! Solve load step 7
! Read in the results from the last substep of ! the last step. ! ! ! !
Plot the deformed mesh with the undeformed edge only Plot the total accumulated equivalent plastic strains
fini /post26 eplo nsel,s,node,,ntop
! Plot the mesh ! Select the node where the point load is attached
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–81
Chapter 8: Nonlinear Structural Analysis esln elem=elnext(0) alls
! Select the element attached to this node ! Get the number of this element ! Select back everything in the model
! Define variable 2 to be Y component of stress at the node where the point ! load is applied ESOL,2,elem,ntop,S,Y,
! Define variable 3 to be Y component of elastic strain at the node where the ! point load is applied ESOL,3,elem,ntop,EPEL,Y, ! Define variable 4 to be Y component of plastic strain at the node where the ! point load is applied ESOL,4,elem,ntop,EPPL,Y, ! Add the elastic and plastic strains in variables 3 and 4 and store the total ! strain in variable 5. ADD,5,3,4, , , , ,1,1,0, xvar,5
! Set the axes for subsequent x-y plot to be variable 5
! Define the x and y axes labels for subsequent x-y plot /axlab,x,Total Y-Strain /axlab,y,Y-Stress plvar,2 fini /eof /exit,nosav
! Plot the Y-stress stored in variable 2
8.13. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional nonlinear analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS program. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual includes a variety of nonlinear analysis test cases: VM7 - Plastic Compression of a Pipe Assembly VM11 - Residual Stress Problem VM24 - Plastic Hinge in a Rectangular Beam VM38 - Plastic Loading of a Thick-Walled Cylinder Under Pressure VM56 - Hyperelastic Thick Cylinder Under Internal Pressure VM78 - Transverse Shear Stresses in a Cantilever Beam VM80 - Plastic Response to a Suddenly Applied Constant Force VM104 - Liquid-Solid Phase Change VM124 - Discharge of Water from a Reservoir VM126 - Heat Transferred to a Flowing Fluid VM132 - Stress Relaxation of a Bolt Due to Creep VM133 - Motion of a Rod Due to Irradiation Induced Creep VM134 - Plastic Bending of a Clamped I-Beam VM146 - Bending of a Reinforced Concrete Beam
8–82
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 8.13: Where to Find Other Examples VM185 - Current Carrying Ferromagnetic Conductor VM198 - Large Strain In-Plane Torsion Test VM199 - Viscoplastic Analysis of a Body Undergoing Shear Deformation VM200 - Viscoelastic Sandwich Seal Analysis VM218 - Hyperelastic Circular Plate VM220 - Eddy Current Loss in Thick Steel Plate
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
8–83
8–84
Chapter 9: Material Curve Fitting Use the ANSYS material curve fitting feature to evaluate experimental data for use as coefficients for certain nonlinear material models built into ANSYS. With this feature, you compare experimental stress data versus ANSYS-calculated stress data for different nonlinear models. Based on these comparisons, you decide which material model to use during solution. Curve fitting is based on the data table configurations outlined in the TB command. The data manipulations and constructions are performed by the TBFT command.
9.1. Applicable Material Behavior Types ANSYS supports Hyperelastic, Creep and Viscoelastic material behavior for Curve Fitting •
Section 9.2: Hyperelastic Material Curve Fitting For Hyperelastic material models, your stress-strain curves can be converted to any of the available ANSYSsupported hyperelastic models, including Mooney-Rivlin, Ogden, Neo-Hookean, Polynomial, Arruda-Boyce, Gent, and Yeoh. Compressible hyperelastic models Ogden hyper-foam and Blatz-Ko are also supported.
•
Section 9.3: Creep Material Curve Fitting For creep material models, your creep strain rate or creep strain as a function of time, stress or temperature can be converted to any of the thirteen ANSYS supported implicit creep models.
•
Section 9.4: Viscoelastic Material Curve Fitting For viscoelastic material models, your shear modulus vs time and/or bulk modulus vs. time data is converted to ANSYS supported Prony series format. Curve fitting for temperature dependency is supported using the SHIFT option.
9.2. Hyperelastic Material Curve Fitting Hyperelastic curve fitting is a tool for estimating the material constants for your material by inputting your experimental data and comparing it to the ANSYS supported hyperelastic material models. You perform curve fitting either through an interactive user interface or via batch commands. You input your experimental data, choose a model from one of nine hyperelastic models supplied, perform a regression analysis, graphically view the curve fitting results, compare the fits to the experimental data, and write the fitted coefficients as ANSYS nonlinear data table commands to the database for the subsequent finite elements analyses. ANSYS hyperelastic models can define three types of behavior: Purely Incompressible, Nearly Incompressible and Compressible. Curve fitting helps you estimate coefficients for these situations. Hyperelastic curve fitting is based on the HYPER option of the TB command.
9.2.1. Using Curve Fitting to Determine Your Hyperelastic Material Behavior The steps for Hyperelastic Curve Fitting are defined as follows: 1
Section 9.2.1.1: Prepare Experimental Data
The experimental data must be a plain text file delimited by a space or a comma.
2
Section 9.2.1.2: Input the Data into The experimental data can be read into ANSYS by browsing ANSYS to the file location in the GUI or by specifying the filename and path (batch) on the command line. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 9: Material Curve Fitting 3
Section 9.2.1.3: Select a Material Model Option
The material options for the applicable curve fitting regimen are defined in the TB command. Nine hyperelastic models are supported. Once you pick a model, you can still change to another model if an ideal fit is not realized.
4
Section 9.2.1.4: Initialize the Coeffi- Hyperelastic curve fitting can be a linear regression or a cients nonlinear regression process, depending on the model. The hyperelastic material models, and the associated process for each are listed in Table 9.3: “Hyperelastic Curve Fitting Model Types”.
5
Section 9.2.1.5: Specify Control Parameters and Solve
You will specify the type of error norm to be used to generate the curve fit.
6
Section 9.2.1.6: Plot Your Experimental Data and Analyze
You review and verify the results by comparing the experimental data and the regression errors. If the results you obtain are not acceptable repeat steps 3 to 5 to perform a new curve fitting solution.
7
Section 9.2.1.7: Write Data to TB Command
Write curve fitting results as the TB command to ANSYS database.
9.2.1.1. Prepare Experimental Data Curve fitting requires experimental test data. Your hyperelastic curve fitting data needs to be a comma or space delimited file, referencing your stress vs. strain values. Hyperelastic curve fitting does not support temperature dependent data. Hyperelastic curve-fitting supports three main behaviors: •
Case 1 - Totally Incompressible Models (see Table 9.1: “Experimental Details for Case 1 and 2 Models and Blatz-Ko”)
•
Case 2 - Nearly Incompressible Models (see Table 9.1: “Experimental Details for Case 1 and 2 Models and Blatz-Ko”)
•
Case 3 - Compressible Models (see Table 9.2: “Experimental Details for Case 3 Models”)
The types of data required for each of these cases is defined in the tables below.
Table 9.1 Experimental Details for Case 1 and 2 Models and Blatz-Ko Experimental Type
Column 1
Column 2
Uniaxial Test
Engineering Strain
Engineering Stress
Biaxial Test
Engineering Strain
Engineering Stress
Shear Test
Engineering Strain
Engineering Stress
Volumetric Test
Volumetric Strain(J)
True Stress
Table 9.2 Experimental Details for Case 3 Models Experimental Type
Column 1
Uniaxial Test
Longitudinal Engineering Lateral Direction Engineer- Engineering Stress Strain ing Strain
Biaxial Test
Biaxial Engineering Strain Thickness Direction Engin- Engineering Stress eering Strain
9–2
Column 2
Column 3
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.2: Hyperelastic Material Curve Fitting Experimental Type
Column 1
Column 2
Column 3
Shear Test
Shear Engineering Strain Thickness Direction Engin- Engineering Stress eering Strain
Volumetric Test
Volumetric Strain(J)
True Stress
Note — J is the ratio of current volume to the original volume. All stresses that ANSYS outputs in POST1/POST26 are true stresses and logarithmic strains.
9.2.1.2. Input the Data into ANSYS The EADD argument for the TBFT command determines how you input your data files. First you designate whether they are uniaxial, biaxial, shear or volumetric, and then you designate the location in the Option2, Option3, Option4 fields. All of the stress values will be engineering stress, except for the volumetric option (true stress). The file should be a simple, delimited set of stress and strain values similar to the following: 0.9703 0.9412 0.9127 0.8847
60.00 118.2 175.2 231.1
9.2.1.2.1. Batch TBFT,EADD,ID,Option1,Option2,Option3,Option4
Option1 = UNIA, BIAX, SHEA, or VOLU Option2 = name of file containing experimental data Option3 = file name extension Option4 = file directory
9.2.1.2.2. GUI The Material Properties GUI provides an input field where you can type the filename of your data file, and also include the appropriate path. You can also “Browse” to a file in a specified location. Separate input is performed for each Option1 value (UNIA, BIAX, SHEA, etc.).
9.2.1.3. Select a Material Model Option Table 9.3: “Hyperelastic Curve Fitting Model Types”, below lists the models that are available for hyperelastic curve fitting. When volumetric data is supplied, a compressible, or nearly incompressible model is implied, and only the available options will be available. When no volumetric data is supplied, the model is understood to be incompressible, and those model options will be available. Supplying zero coefficients for the volumetric data field will also denote an incompressible model.
Table 9.3 Hyperelastic Curve Fitting Model Types Model Name
Abbreviation
Order/Options
No. of Coefficients Linear/Nonlinear [1] Fitting
Mooney-Rivlin
moon
2, 3, 5, 9
2/3/5/9+1
Linear
Polynomial
poly
1 to N
see below [2]
Linear
Yeoh
yeoh
1 to N
N+N
Linear
Neo-Hookean
neoh
-
1+1
Linear
Ogden
ogde
1 to N
2*N+N
Nonlinear
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–3
Chapter 9: Material Curve Fitting Model Name
Abbreviation
Order/Options
No. of Coefficients Linear/Nonlinear [1] Fitting
Arruda-Boyce
boyc
-
2+1
Nonlinear
Gent
gent
-
2+1
Nonlinear
Blatz-Ko
blat
-
1
Nonlinear
1 to N
2*N+N
Nonlinear
Ogden Hyper-foam foam
1.
The number of coefficients is usually the sum of the number of deviatoric coefficients and the number of volumetric coefficients.
2.
The number of coefficients for a polynomial will be dependent on the polynomial order N. N
Number of Coefficients = ∑ (1 + i) + N i =1
Blatz-Ko and Ogden hyper-foam are compressible models. For Ogden hyper-foam, the experimental data you supply will require additional fields. More information on the hyperelastic models ANSYS supplies for curve fitting can be found in Section 2.5.2: Hyperelastic Material Constants.
9.2.1.3.1. Batch TBFT,FADD,ID,HYPER,Option2,Option3
Option2 = Model name, as specified in Table 9.3: “Hyperelastic Curve Fitting Model Types” (above). Option3 = Order or number of coefficients, where applicable. Table 9.3: “Hyperelastic Curve Fitting Model Types”
(above) specifies the number and type of coefficient(s) necessary for each hyperelastic model type.
9.2.1.3.2. GUI You can navigate to a pull-down selection menu in the material GUI to pick the applicable material model option. The options displayed will be dependent on the format of your experimental data file.
9.2.1.4. Initialize the Coefficients Depending on the model you choose, hyperelastic curve fitting can be a linear or a nonlinear regression process; the initial coefficients you supply will determine how accurate and efficient your curve fit will be. The initial values of the coefficients generally come from experience, and also from studying the function that defines the model you are attempting to compare/fit your data to. For most hyperelastic models, 1 or -1 is a good starting point. However, coefficient values can vary greatly depending on the model chosen. The Gent model, for instance, provides good fit with initial coefficient values as high as 1000. You can also fix (hold constant) your coefficients. You specify a value for a coefficient and keep it unchanged, while allowing the other coefficients to be operated on. You can then release the fixed coefficient later if desired. By default, all of the coefficients are free to vary.
9.2.1.4.1. Batch TBFT,SET,ID,HYPER,Option2,Option3,Option4,Option5
Option2 = Model name. See Table 9.3: “Hyperelastic Curve Fitting Model Types” (above) for the models available. Option3 = not applicable
9–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.2: Hyperelastic Material Curve Fitting Option4 = index of coefficient Option5 = entr “0” for variable, 1 for fixed.
9.2.1.4.2. GUI The GUI automatically updates your coefficient tables depending on the model you pick. You can modify these values to initialize them at values you believe more appropriate.
9.2.1.5. Specify Control Parameters and Solve Depending on the model, your hyperelastic curve fitting will be either a linear or nonlinear regression process (see Table 9.3: “Hyperelastic Curve Fitting Model Types” (above) for details). Your error norms can be either normalized and unnormalized. The normalized error norm is the default regression option. Normalized error norms generally give better results than the unnormalized error norms, since normalized error gives equal weight to all of your data points. The solution control parameters of a nonlinear regression include: 1.
number of iterations
2.
residual tolerance
3.
coefficient change tolerance
The solution stops when both residual tolerance of error norm and coefficient change tolerance is met or if the number of iterations criteria is met. Wherever nonlinear regression is used, you need to initialize your coefficients.
9.2.1.5.1. Batch TBFT,SOLVE,ID,HYPER,Option2,Option3,Option4, ..., Option7
Option2 = Model name. See Table 9.3: “Hyperelastic Curve Fitting Model Types” (above) for the models available. Option3 = The order or number of your coefficients. See Table 9.3: “Hyperelastic Curve Fitting Model Types”
(above) for possible values. Option4 = curve fitting procedure: 0 = unnormalized least squares, 1 = normalized least squares Option5 = maximum number of iterations Option6 = tolerance of residual changes Option7 = tolerance of coefficient changes
Other solution parameters are available. See the TBFT command for details.
9.2.1.5.2. GUI The GUI lets you specify all of your control parameters (error norm, solution control parameters, and the solver options) interactively. Select the options and Solve to generate the coefficients. Change the parameters and repeat the solution as necessary to ensure the accuracy of the results. The unused options are disabled whenever necessary.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–5
Chapter 9: Material Curve Fitting
9.2.1.6. Plot Your Experimental Data and Analyze After you initiate Solve, the coefficient tables will contain the fitted coefficients and also the residual errors. You can then plot your data and visually interpret the results. Column one is always your X- axis, with each additional column plotted separately as a function of column one.
9.2.1.6.1. Batch TBFT,PLOT,ID,Option1,HYPER,Option3,Option4
Option1 = UNIA, BIAX, SHEA, or VOLU Option3 = Model name. See Table 9.3: “Hyperelastic Curve Fitting Model Types” (above) for the models available. Option4 = The order or number of your coefficients. See Table 9.3: “Hyperelastic Curve Fitting Model Types”
(above) for possible values. You use the /WINDOW command to configure the graphs for each of the resultant curves for the individual stress types.
9.2.1.6.2. GUI Use the GRAPH button to plot the data. Your plots will show Columns 2 and above as separate curves, plotted as a function of column 1. The data in column 1 is always the X-axis. By default all the experiments are plotted in separated graphs in the GUI window. To view a specific data and its corresponding fitting result, you can use the right click of mouse button on the specific dataset, and pick a desired option to view the results. Other plotting utilities can be found by using the right click of mouse button on the listed data in the curve fitting GUI window. You can also turn the legend and/or axis displays on and off, and switch the scales between log scale and regular scale. You can use the middle-mouse button to eliminate a specific curve and clarify or refine the remaining curve.
9.2.1.6.3. Review/Verify After plotting the curve fitting results, you can then review them and also verify the error norm/residual values that are printed in the curve fitting GUI window. These values help you determine the quality of curve fitting and whether to accept the results. Error norm values are not always the best indicator of a valid curve fit. Plotting the curves and visually assessing the result is often the best indication. If the results are unacceptable, you may want to go back to step 3 and solve again, either by picking a different model, increasing the order, or redefining your initial values of the coefficients or other control parameters. Repeat steps 3-7 until you get an acceptable solution.
9.2.1.7. Write Data to TB Command After you are satisfied with your curve fitting results, you can write the curve fitting data to the ANSYS database using TBFT, FSET. The GUI or the command line converts the coefficients to the appropriate form before writing to ANSYS TB tables. ANSYS stores the data as part of the material property set for use in subsequent analyses.
9.2.1.7.1. Batch TBFT,FSET,ID,HYPER,Option2,Option3
Option2 = Model name. See Table 9.3: “Hyperelastic Curve Fitting Model Types” (above) for the models available.
9–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.3: Creep Material Curve Fitting Option3 = The order or number of your coefficients. See Table 9.3: “Hyperelastic Curve Fitting Model Types”
(above) for possible values.
9.2.1.7.2. GUI Once you complete the process and update your material data properties with the representative curve data, you are returned to the material properties dialog. The curve data can now be accessed for the full range of material behavior.
9.3. Creep Material Curve Fitting ANSYS provides a number of creep models, along with the tools to fit derived coefficients to your experimental data. You can use either the interactive user interface (GUI) or batch commands. You input your experimental data, choose a model from one of the supplied creep models, and then perform a regression analysis. You then graphically view the curve fitting result, and compare it for fit with your experimental data. If the curve is acceptable, you write the fitted coefficients as ANSYS nonlinear data table commands (ANSYS TB command format) to the database for the subsequent finite element analyses. All thirteen implicit creep models are supported.
9.3.1. Using Curve Fitting to Determine Your Creep Material Behavior The steps for creep curve fitting are defined as follows: 1
Section 9.3.1.1: Prepare Experimental Data
The experimental data must be a plain text file with headers to describe the data types and attributes. The test data must be delimited by a space or a comma.
2
Section 9.3.1.2: Input the Data into The experimental data can be read into ANSYS by browsing ANSYS to the file location in the GUI or by specifying the path (batch) on the command line.
3
Section 9.3.1.3: Select a Material Model Option
4
Section 9.3.1.4: Initialize the Coeffi- Creep curve fitting is a nonlinear regression; the initial values cients of the coefficients to be determined can be very important for a successful solution.
5
Section 9.3.1.5: Specify Control Parameters and Solve
You choose the error norm to be used for an acceptable curve fit.
6
Section 9.3.1.6: Plot the Experimental Data and Analyze
You review and verify the results by comparing them with the experimental data and the regression errors. If they are not acceptable, repeat steps 3 to 5 to obtain a new curve fitting solution.
7
Section 9.3.1.7: Write Data to TB Command
Write curve fitting results in the TB command format to the ANSYS database.
The material options for the applicable curve fitting regimen are defined in the TB command. Thirteen implicit creep models are supported. Once you pick a model, you can still switch to another model if an ideal fit is not realized.
9.3.1.1. Prepare Experimental Data You need to provide accurate experimental test data in order to achieve valid curve fitting results. For the creep analysis, you will use either the creep strain value or creep strain rate, derived as a function of time, temperature, stress and/or creep strain. The type of data you need to provide will depend on the creep model chosen. The experimental data is named “creep” to distinguish it from other types of data such as uniaxial, tension, biaxial, etc. The creep data must be a plain text file, which contains the headers and the test data as a table, delimited by a space or a comma. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–7
Chapter 9: Material Curve Fitting The header can be used to describe the data types that characterize the test data columns or attributes of the data. There are a total of five different creep data types, see Table 9.4: “Creep Data Types and Abbreviations”.
Table 9.4 Creep Data Types and Abbreviations Time
time
Equivalent Creep Strain
creq
Equivalent Creep Strain Rate
dcreq
Equivalent Stress
seqv
Temperature
temp
The header format that defines the type of data column is /n, abbr, where n is the index of the data column in the file, and abbr is the abbreviation for the type of data in the column, as described in Table 9.4: “Creep Data Types and Abbreviations”. An example of a typical data input is shown here: /1,seqv ! indicates first column is stress /2,creq ! indicates second column is creep strain /3,temp ! indicates third column is temperature /4,dcreq ! indicates fourth column is creep strain rate 4000 0.00215869 100 0.000203055 4000 0.00406109 100 0.000181314 4000 0.00664691 100 0.000165303 4000 0.0102068 100 0.000152217 4000 0.0151416 100 0.000140946
When a particular column is unchanged over the loading history, you can define it as an attribute. For instance, in the above example, the stress and temperature are constant throughout the range. You define a data attribute in the header as follows: The header format to define a data attribute is /attr, value, where attr is the abbreviation of data type, and value is the value of the attribute. An example of a typical input data using attributes is shown here: /seqv,4000 ! indicate this creep has a constant stress of 4000 /temp,100 ! indicate this creep data is at a constant temperature of 100 /1,creq ! indicate first column is creep strain /2,dcreq ! indicate second column is creep strain rate 0.00215869 0.000203055 0.00406109 0.000181314 0.00664691 0.000165303 0.0102068 0.000152217 0.0151416 0.000140946 0.0220102 0.000130945
There are thirteen model types available from ANSYS for creep curve fitting. The model you choose will determine the experimental data required for the curve fitting process. The following tables describe the creep data required to perform curve fitting for each model type. Please note that for strain hardening and modified strain hardening, you need to input both creep strain and creep strain rate in the experimental data.
Table 9.5 Creep Model and Data/Type Attribute Creep Model
creq
dcreq
Strain Hardening
x
x
time
seqv
temp
x
x
Time Hardening
x
x
x
x
Generalized Exponential
x
x
x
x
Generalized Graham
x
x
x
x
9–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.3: Creep Material Curve Fitting Creep Model
creq
Generalized Blackburn Modified Time Hardening
x
Modified Strain Hardening
x
dcreq
time
seqv
x
x
x
x
x
temp x
x
x
Generalized Garofalo
x
x
x
Exponential Form
x
x
x
Norton
x
x
x
x
x
x
Prim+Sec Time Hardening
x
Prim+Sec Rational Polynomial
x
x
x
Generalized Time Hardening
x
x
x
x
9.3.1.2. Input the Data into ANSYS The experimental data must be read into ANSYS from a plain text file. You prepare this file according to the previous section, including both header information and formatted test data. The header portion is absolutely required for creep analyses. Each file is viewed as a data set in ANSYS, and can be a complete set of experimental test data or a part of a series of files of experimental test data. You can include several data sets, such as tests performed at different stress levels and/or temperatures, to perform a creep curve fitting. There are two ways to input the experimental data.
9.3.1.2.1. Batch The EADD argument of the TBFT command is used to identify and specify the location of your data files. The command syntax is: TBFT,EADD,ID,Option1,Option2,Option3,Option4
Option1 = creep Option2 = name of file containing experimental data Option3 = file name extension Option4 = file directory
9.3.1.2.2. GUI In interactive mode you can input experimental data by typing the filename (with the appropriate path if the file is not in the default directory) into the appropriate area. You can also “Browse” to a file in a particular location. Use the Add Data Set button to add additional data sets for creep curve fitting. There is no restriction on the number of data sets you can add.
9.3.1.3. Select a Material Model Option There are thirteen models available for curve fitting. You pick the one that best satisfies your requirements. You will use the creep model abbreviation in subsequent equations to identify the creep model (see Table 9.6: “Creep Models and Abbreviations”). Use the creep models table (below) to view the formulae of the creep models and to determine the number of coefficients. You'll find it helpful to view the formula before you proceed to solve. It will tell you what initial coefficients you might use and also lets you determine the format of your experimental data. Also see Table 9.6: “Creep Models and Abbreviations” to determine a starting point for the initial creep model coefficients.
9.3.1.3.1. Batch TBFT,FADD,ID,CREEP,Option2,Option3 Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–9
Chapter 9: Material Curve Fitting Option2 = Creep model abbreviation, see Table 9.6: “Creep Models and Abbreviations”. Option3 = not used for creep curve fitting.
The following table describes the creep models available and their abbreviated names for Option2 (above).
Table 9.6 Creep Models and Abbreviations Model Number
Name
Fitting Name/Option2
1
Strain Hardening
shar
2
Time Hardening
thar
3
Generalized Exponential
gexp
4
Generalized Graham
ggra
5
Generalized Blackburn
gbla
6
Modified Time Hardening
mtha
7
Modified Strain Hardening
msha
8
Generalized Garofalo
ggar
9
Exponential Form
expo
10
Norton
nort
11
Prim+Sec Time Hardening
psth
12
Prim+Sec Rational Polynomial
psrp
13
Generalized Time Hardening
gtha
Note — It is very important for the experimental data to be consistent with the creep model you choose. See Table 9.5: “Creep Model and Data/Type Attribute” for the data types required for each creep model.
9.3.1.3.2. GUI You can pick the appropriate model option from a menu in the data entry area. All of the options and constraints listed for batch input apply.
9.3.1.4. Initialize the Coefficients Creep curve fitting is a nonlinear regression process. A successful curve fit depends greatly on the initial coefficient values. For some creep models the initial value of certain coefficients is critical to achieving a successful fit. This suggests that certain variances may cause your curve fit to fail to converge. When this happens you can adjust the initial value of specific coefficients and rerun the problem again. In general the more parameters a model has, the more difficult it is to get the solution to converge. You can also fix (hold constant) your coefficients. You specify a value for a coefficient and keep it unchanged, while allowing the other coefficients to be operated on. You can then release the fixed coefficients to obtain a solution. By default, all of the coefficients are free to vary.
9.3.1.4.1. Batch You define your coefficient values using the SET option of the TBFT command, as follows: TBFT,SET,ID,CREEP,Option2,Option3,Option4,Option5
Option2 = Creep model name Option3 = not applicable Option4 = index of coefficient
9–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.3: Creep Material Curve Fitting Option5 = value of coefficient
Then you can modify the coefficients with the FIX option of the TBFT command. TBFT,FIX,ID,CREEP,Option2,Option3,Option4,Option5
Option2 = Creep model name Option3 = not applicable Option4 = index of coefficient Option5 = 0 variable, 1 fixed
9.3.1.4.2. GUI You pick your creep model from the choices on the creep model tree. ANSYS automatically configures the coefficients for the model. You can then make modifications, including initializing and/or fixing certain coefficients.
9.3.1.5. Specify Control Parameters and Solve Error norm, maximum number of the allowed iterations and the error tolerance will affect the accuracy of your results. There are two available error norms available for the regression. Normalized curve fitting is the default option used to calculate error norms. It generally gives better results than unnormalized curve fitting since normalized fitting gives equal weight to all data points when minimizing the errors norms. Other available solve criteria are number of iterations, residual tolerance and coefficient change tolerance. The solution stops when both residual tolerance and coefficient change tolerance is met or if the number of iterations criteria is met. The coefficients are updated after every iteration during the solve process.
9.3.1.5.1. Batch The batch command is TBFT,SOLVE,ID,CREEP,Option2,Option3,Option4, ..., Option7
Option2 = Creep function name (See Table 9.6: “Creep Models and Abbreviations”) Option3 = not applicable for Creep models Option4 = error norm: 0 = unnormalized, 1 = normalized (default) Option5 = maximum number of iterations Option6 = tolerance of residual changes Option7 = tolerance of coefficient changes
Other solving parameters are available. See the TBFT command for details.
9.3.1.5.2. GUI The solution phase is entered automatically after you fill in the last set of coefficient values. Each of the options specified in the command line description is presented as a pull down menu or fill in box, and each option must be specified before Solve will begin. The coefficients are updated in the GUI after the solution is complete.
9.3.1.6. Plot the Experimental Data and Analyze After you initiate Solve, the coefficient tables will contain the fitted coefficients and also the residual errors. You can then plot your data and visually interpret the results. Column one is generally your X- axis, with each additional column plotted separately as a function of column one. The plot utility also incorporates many “right mouse click” context sensitive functions that will help you to configure and optimize your plot(s).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–11
Chapter 9: Material Curve Fitting Clicking in various areas of the display window brings up context sensitive functions that are particular to that area. (e.g., clicking on the legend area brings up controls to define and configure your graph legend). These functions change according to the type of graph you are creating and to the entity you click on in the graph. You can also use a middle mouse click to hide a particular curve within a graph.
9.3.1.6.1. Batch TBFT,PLOT,ID,Option1,Option2,Option3,Option4
Option1 = CREEP Option3 = Creep model name Option4 = Not Used
9.3.1.6.2. GUI You can simultaneously display many data sets for each function plotted. Each window of your display can be used to display each one of the data sets you are plotting against column one.
9.3.1.6.3. Analyze Your Curves for Proper Fit You use the GUI to graphically review the curve fitting result. In this way you can ensure a good fit throughout the range of data. Use the plotted curve fitting results both to determine the degree of fit at various locations, and also to verify the error norm/residual value. You can then determine the quality of a curve fitting and decide whether to accept the results. If the results are unacceptable, you may want to go back to step 3, and then solve again with a new model, redefining certain initial values of the coefficients, and also modifying some of the other control parameters. Repeat steps 3-6 until you obtain a satisfactory solution.
9.3.1.7. Write Data to TB Command After you are satisfied with your curve fitting results, you can write the curve fitting data to the ANSYS database using TBFT, FSET. The GUI or the command line converts the coefficients to the appropriate form before writing to ANSYS TB tables. ANSYS stores the data as part of the material property set for use in subsequent analyses.
9.3.1.7.1. Batch TBFT,FSET,ID,CREEP,Option2,Option3
Option2 = Creep Model Abbreviation Option3 = Not applicable
9.3.1.7.2. GUI When you complete the process, click the Write to Database button to write the fitted coefficients of your creep model as a creep data table in ANSYS material database. You are then returned to the material properties dialog. The curve data can now be accessed for the full range of material behavior.
9.3.2. Tips For Curve Fitting Creep Models The following are some useful tips that will ensure successful curve fitting. These tips are not hard and fast specifications, only suggestions. Also, following them does not guarantee a solution. Refer to Section 2.5.11: Creep Equations for additional details on each implicit creep model . Name
9–12
Notes
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.3: Creep Material Curve Fitting 1
Strain Hardening
Strain hardening has 4 coefficients. C4 is for temperature dependency. If you do not have temperature dependent data, set C4 to zero. If you have difficulty solving temperature dependent data. Use experimental data for only one temperature and fix C4 to zero. Then solve. Then add data for other temperature, release C4 and solve for all coefficients or just C4 by fixing the C1, C2 and C3.
2
Time Hardening
Time hardening has 4 coefficients. C4 is for temperature dependency. If you do not have temperature dependent data, set C4 to zero. If you have difficulty solving temperature dependent data. Use experimental data for only one temperature, fix C4 to zero. Then solve. Then add data for other temperature, release C4 and solve for all coefficients or just C4 by fixing the C1, C2 and C3.
3
Generalized Exponential
Generalized Exponential has 5 coefficients. C4 is for temperature dependency. If you do not have temperature dependent data, set C4 to zero. Use a low value of C5 (e.g., 1e-3) to avoid floating-point overflows in the exponential term of this model. If you have difficulty solving temperature dependent data. Use experimental data for only one temperature, fix C4 to zero. Then solve. Then add data for other temperature, release C4 and solve for all coefficients or just C4 by fixing the C1, C2 and C3.
4
Generalized Graham
Generalized Graham has 8 coefficients. You use C8 for temperature dependency. If you do not have temperature dependent data, set C8 to zero. If you have difficulty solving temperature dependent data, use experimental data for only one temperature, fix C8 to zero, and solve. Then add data for other temperatures, release C8 and solve for the remaining coefficients individually.
5
Generalized Blackburn
Generalized Blackburn has 7 coefficients. It is advisable to look at exponential term and try to keep them from floatingpoint overflows. To keep eC2σ within floating-point range, make sure the initial value of C2 is such that C2σ is close to 1. Similarly try to keep σ/C4 and C7σ close to 1.
6
Modified Time Hardening
Modified Time Hardening has 4 coefficients. C4 is for temperature dependency. If you do not have temperature dependent data, fix C4 to zero.
7
Modified Strain Hardening
Modified Strain Hardening has 3 coefficients. This model is complex as far as curve fitting is concerned. To keep the
C1σC2 [(C3 + 1)ε]C3 term from going negative, C1 was replaced with C12 but converted to the right form before it was written to ANSYS database. 8
Generalized Garofalo
Generalized Garofalo has 4 coefficients. C4 is for temperature dependency. If you do not have temperature dependent data, set C4 to zero. To keep the Sinh term within floating-point range, keep c2σ close to one when you initialize the coefficients.
9
Exponential Form
Exponential Term has 3 coefficients. C3 is for temperature dependency. If you do not have temperature dependent data, set C3 to zero. To keep eσC2 within floating-point range, keep σ/C2 close to one.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–13
Chapter 9: Material Curve Fitting 10
Norton
Norton model has 3 coefficients. C3 is for temperature dependency. If you do not have temperature dependent data, set C3 to zero.
11
Prim+Sec Time Hardening
Time Hardening has 7 coefficients. This is a complex model. Here it is advisable to solve for temperature independent data first and then introduce temperature related data.
12
Prim+Sec Rational Polynomial
Rational Polynomial is a very complex model for curve fitting with 10 coefficients. If you find it hard to fit this data, it is advisable for you to split experimental data into primary creep data and secondary creep data. Primary creep data is the initial part of the curve that covers the nonlinearity in the strain rate. Fit only the secondary data by fixing C1 to 1 and then set all other coefficients except C2, C3 and C4 to zero. Use a low value of C3 to keep 10C3σ within floating-point range. Coefficients C5 to C10 in curve fitting refers to coefficients C7 to C12 in the implicit creep equation. Then add the primary creep data, release all coefficients, and solve.
13
Generalized Time Hardening
Generalized Time Hardening has 6 coefficients. Set C6 to zero if you have temperature independent data. When initializing coefficients set C5σ close to 1 to avoid floating-point overflows.
9.4. Viscoelastic Material Curve Fitting Viscoelastic material curve fitting is a tool to determine the material constants of the Prony series expansion for both shear and bulk modulus of the ANSYS hypoviscoelastic material option from experimental data. Either through an interactive user interface or the batch commands, users can input the experimental data, define the order of Prony series expansion, perform nonlinear regression, view the curve fitting results graphically, compare to the experimental data, and write the fitted coefficients as ANSYS nonlinear data table commands to the database for the subsequent finite elements analyses. Currently the tools allow you to fit shear modulus and/or bulk modulus and/or shift functions.
9.4.1. Using Curve Fitting to Determine the Coefficients of Viscoelastic Material Model The steps for Viscoelastic Curve Fitting are defined as follows: 1
Section 9.4.1.1: Prepare Experimental Data
2
Section 9.4.1.2: Input the Data into The experimental data can be read into ANSYS from GUI or ANSYS batch command line as a plain text file.
3
Section 9.4.1.3: Select a Material Model Option
4
Section 9.4.1.4: Initialize the Coeffi- Viscoelastic curve fitting is a nonlinear regression, the initial cients values of the coefficients to be determined can be very important for a successful solution.
5
Section 9.4.1.5: Specify Control Parameters and Solve
9–14
The experimental data must be a plain text file delimited by a space or a comma.
This includes Prony series expansion of shear and/or bulk moduli as well as shift function. The supported shift functions include WLF and TN.
Specify the error norm to be used, the solution control parameters, and perform the nonlinear regression.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.4: Viscoelastic Material Curve Fitting 6
Section 9.4.1.6: Plot the Experimental Data and Analyze
View graphically the curve fitting results. Review and verify the results by comparing with the experimental data and the regression errors, if not acceptable, repeat steps 3 to 7 to perform a new curve fitting solution.
7
Section 9.4.1.7: Write Data to TB Command
Write curve fitting results as the TB command to ANSYS database.
9.4.1.1. Prepare Experimental Data Curve fitting requires experimental test data. For curve fitting viscoelastic materials, the experimental data must be shear modulus and/or bulk modulus as a function of time and temperature. The experimental data is named “viscoelastic” to distinguish it from other data types, such as hyperelasticity or creep. This also makes documenting your analyses more convenient. The viscoelastic test data must be a plain text file containing the headers, along with the test data as a table of data delimited by a space or a comma. The header is used to define the test data type and the temperature for your test data. For viscoelastic curve fitting with multiple temperatures, you don't calculate each temperature point and write it as a temperature-dependent Prony data table. Instead, when multiple temperatures are present, either WLF or TN shift functions are used to account for the temperature dependency. Each file must contain only one temperature, and the temperatures of each of the files can be the same or different. The viscoelastic test data have 4 data types, seeTable 9.7: “Viscoelastic Data Types and Abbreviations”.
Table 9.7 Viscoelastic Data Types and Abbreviations Time
time
Shear modulus
smod
Bulk modulus
bmod
Temperature
temp
The headers are used to describe the data types that characterize the test data columns or attributes of the data. The following listing contains the appropriate headers, followed by the delimited data: /temp,100 ! define temperature attribute 0.01 2992.53 1 2978.514207 2 2965.45541 4 2942.293214 6 2922.530649 8 2905.612202 10 2891.073456 20 2842.506984 40 2798.142793 60 2772.383729 80 2750.631843 100 2730.398114 200 2643.125432 400 2517.475394 600 2431.262053 800 2366.580897 1000 2313.955396 2000 2117.922594 4000 1833.734397 6000 1627.199197 8000 1470.6806 10000 1347.264527 20000 964.0141125 40000 586.1405449 60000 392.186777 80000 277.2706253 Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–15
Chapter 9: Material Curve Fitting 100000 202.0025278 200000 46.87056342 400000 2.669209118 600000 0.156653269 800000 0.0137224 1000000 0.005591539
9.4.1.2. Input the Data into ANSYS You use the EADD argument of the TBFT command to input your data files. The experimental data must be read into ANSYS from a plain text file. The experimental data must be prepared as discussed in the previous section, and include both the header information and the formatted test data. Each file is viewed as a dataset in ANSYS, and can be the complete set of experimental test data or a part of an experimental test data. You can include several datasets, including tests performed at different temperatures. Although different datasets can have the same/or different temperature, each file can have only one temperature. Multiple temperature datasets must be input with multiple files. Two types of data may be required for viscoelastic curve fitting, either shear modulus vs time and/or bulk modulus vs. time. The data can also be a function of temperature, which can then be accounted for by either WLF or TN shift function. You can use the GUI window or batch command to input your experimental data.
9.4.1.2.1. Batch TBFT,EADD,ID,Option1,Option2,Option3,Option4
ID = Index corresponding to the ANSYS material number. Option1 = Experimental Date Type, either shear or bulk Option2 = name of file containing experimental data Option3 = file name extension Option4 = file directory
Note — “sdec” refers to the shear modulus as a function of time and “bdec” refers to the bulk modulus as a function of time.
9.4.1.2.2. GUI Click on the Add Dataset button and type the filename into the area provided. You can also “Browse” to a file in a specified location. Separate input is performed for each data type (Option1 = sdec, or bdec)
9.4.1.3. Select a Material Model Option The TBFT command provides the curve fitting tools for viscoelastic material modeling. You represent your viscoelastic material behavior by a set of Prony series expansions of shear and/or bulk moduli to characterize the shear and the bulk deformation of the material. You can also use the shift functions to characterize the material's temperature dependency. First you define a case “casename” to associate the set of coefficients for the Prony expansions with the shift functions that characterize the material behavior. You can use the “casename” to define several different options that characterize the same test data, and then to compare the curve fitting results. To define the material model, you must first define a “casename”, and then specify the order of shear and bulk moduli and the type of the shift function(s), if required. You need to create an additional case to define different shear order, bulk order or shift options. Once you create a case, the number of shear terms, bulk terms, or shift options cannot be changed.
9–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.4: Viscoelastic Material Curve Fitting
9.4.1.3.1. Batch You define a viscoelastic material with the Prony series expansion by creating a case and setting the order of shear modulus, bulk modulus and shift options. You create the case with the TBFT, FCASE command. The first line will include FCASE, ID, NEW. Then you specify the number of shear terms, bulk terms, and the shift function. The case is actually created only after the option is issued. The follow syntax examples and argument descriptions illustrate the relationship of these activities. TBFT,FCASE,ID,NEW,Option2,Option3
Option2 = PVHE (Refers to Prony Viscohypoelastic) Option3 = User Specified casename TBFT,FADD,ID,CATEGORY,Option2,Option3
CATEGORY = VISCO Option2 = pshear or pbulk or shift Option3 = Dependent on Option2 as follows:
•
Option2 = pshear or bulk, Option3 = NONE, or 1 to N
•
Option2 = shift, Option3 = NONE or TN or WLF TBFT,FCASE,ID,FINI
9.4.1.3.2. GUI You can use the GUI to interactively navigate the tree structure of the curve fitting window. Each of the shear, bulk and shift options can be selected, and you can fill in the appropriate “casename” in a text box field. As you choose the options, the coefficient table is automatically created.
9.4.1.4. Initialize the Coefficients The initial values you choose for your coefficients will determine the success of your viscoelastic curve fitting operations. A complete model has (2*NG+1)+(2* Nk +1)+ NS number of the coefficients. NG is the order of the Prony series expansion of the Shear modulus. Nk is the order of the Prony series expansion of the bulk modulus. NS is the number of coefficients of the shift function (NS = 2 for the TN option and NS =3 for the WLF option). The coefficients are ordered as shear terms first, then the bulk terms, and then the shift function. The coefficients are ordered as α0G, α1G, τ1G, α2G, τ2G, … αnG, and τnG for shear modulus, and α0K, α1K, τ1K, α2K, τ2K, … αnK, and τnK for bulk modulus. A shift function must be used together with your shear and/or bulk modulus for temperature dependent experimental data. The default coefficient is set to “one,” but you should redefine the initial values before solving. While initializing the coefficients, you should set αnKs to 1 and τnKs to time values that are equally distributed in the log scale, spanning the data range from minimum to maximum time. For example, in the shear decay versus time data file, if the time values vary from 1 to 10000, and if you use 3rd order Prony, logical guesses for τ1G , τ2G and τ3G that span this range could be τ1G = 1, τ2G = 100, and τ3G = 10,000 (also (1), (10) and (10,000) or (1), (1,000) and (10,000), respectively). You should also note that αnG used in curve fitting is the square root of the αnG used in ANSYS TB tables. This was done to keep all αnG used in the TB tables positive. A good guess for the WLF or TN parameter is the reference temperature you used during your partial solve for shear and bulk. The index of the reference/base temperatures is the sum of NumShear + NumBulk + 1. You can also fix (hold constant) your coefficients. You specify a value for a coefficient and keep it unchanged, while allowing the other coefficients to be operated on. You can then release the fixed coefficient later if desired. By default, all of the coefficients are free to vary. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–17
Chapter 9: Material Curve Fitting
9.4.1.4.1. Batch TBFT,SET,ID,CASE,Option2,Option3,Option4,Option5
Option2 = casename Option3 = Not Applicable Option4 = index of coefficient Option5 = value of coefficient
For example: TBFT,SET,1, myvisco1,,1,1.2 TBFT,SET,1, myvisco1,,2,1.5
! Initialize the first coefficient to 1.2 ! Initialize the second coefficient to 1.5
Use the TBFT,FIX command to fix a coefficient to a value set by the TBFT, SET command or to release a previously fixed coefficient. By default, coefficients are not fixed. TBFT,FIX,ID,CASE,Option2,Option3,Option4,Option5
Option2 = casename Option3 = Not Applicable Option4 = Index of coefficient Option5 = 1 to fix, 0 to vary
For example: TBFT,FIX,1, myvisco1,,1,1. TBFT,FIX,1, myvisco1,,2,1
! Fix the first coefficient to a value set via TBFT,SET ! Fix the second coefficient to a value set via TBFT,SET
9.4.1.4.2. GUI The coefficients table is automatically updated in the viscoelastic curve fitting GUI window when the order of shear modulus and/or bulk modulus and/or shift function are defined. Specify values for your coefficients in the coefficients table in the curve fitting GUI window, and check the appropriate boxes to fix them or allow them to vary.
9.4.1.5. Specify Control Parameters and Solve Viscoelastic curve fitting is a nonlinear regression process. You can use either normalized or unnormalized error norm for the regression. The normalized error norm is the default regression option for calculation of the error. This error norm generally gives better results than the unnormalized error norm option, since the normalized error gives equal weight to all data points. The solution control parameter of a nonlinear regression includes number of iterations, residual tolerance and coefficient change tolerance. The solution stops when both residual tolerance of error norm and coefficient change tolerance is met or if the number of iterations criteria is met. The coefficients are updated when the solution is completed. In general it is very difficult to directly solve a complete case including coefficients of the shear modulus, the bulk modulus and the shift function. Three solver options including shear modulus only, bulk modulus, and shift function (or all) are provided to allow user to solve only Prony coefficients of the shear modulus, Prony coefficients of the bulk modulus and coefficients of the shift function. However the coefficients of shift function can't be solved before the shear or bulk modulus are solved. It is normal for a solution to not converge at first, but to stop as the maximum iterations criteria is reached. You can then examine the curve fitting results and the solution history before proceeding any further. You can then adjust parameters and resolve the problem whenever it is necessary. For viscoelastic curve fitting, you should follow these three steps to perform the regression:
9–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.4: Viscoelastic Material Curve Fitting 1.
Solve the shear coefficients (if there are any). Set the partial solve option using TBFT, SET,,,,,COMP, PSHEAR. Set the reference temperature at which your partial solution will be performed using TBFT, SET,,,,,TREF, TX. Only data at temperature TX will be used to estimate shear coefficients Solve
2.
Solve the bulk coefficients (if there are any). Set the partial solve option using TBFT, SET,,,,,COMP, PBULK. Set the reference temperature at which your partial solution will be performed using TBFT, SET,,,,,TREF, TX. The reference temperature should be the same for both shear and bulk. Only data at temperature TX will be used to estimate shear coefficients Solve
3.
Solve the shift function (or all) coefficients. Set the partial solve option using TBFT, SET,,,,,COMP, PVHE. TREF is not used when you solve for all parameters. All temperature data is used to estimate the coefficients. Solve
Note — When only the shear and bulk buttons are checked, only your shear coefficients are solved. To solve for both shear and bulk, you must check all three buttons.
9.4.1.5.1. Batch Solution option command is: TBFT,SET,ID,CASE,Option2,Option3,Option4,Option5
Option2 = casename Option3 = Not Applicable Option4 = comp Option5 = pshea (for Shear only) or pbulk (for bulk only).
The SOLVE command allows you to specify procedure types, tolerances and number of iterations. TBFT,SOLVE,ID,CASE,Option2,Option3,Option4, ..., Option7
Option2 = Creep Function Name (See Table 9.6: “Creep Models and Abbreviations”) Option3 = Not Applicable Option4 = Curve Fitting Procedure: 0 = unnormalized least squares, 1 = normalized least squares (default) Option5 = maximum number of iterations Option6 = tolerance of residual changes Option7 = tolerance of coefficient changes
Other solving parameters are available. See the TBFT command for details.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–19
Chapter 9: Material Curve Fitting
9.4.1.5.2. GUI The GUI provides access for you to choose your error norm, solution control parameters, and solver options. Once you complete these specifications and solve, you can go back and modify your parameters as necessary to obtain a good curve fit.
9.4.1.6. Plot the Experimental Data and Analyze The best way to verify a good fit between your experimental data and the provided curves is to plot your curves and visually inspect them.
9.4.1.6.1. Batch You enter the plotting parameters from the command line as follows: TBFT,PLOT,ID,ExpIndex,CASE,Option3
Option3 = casename
9.4.1.6.2. GUI Graph button provides direct means to plot the data.
9.4.1.6.3. Analyze Your Curves for Proper Fit All of your data is plotted as a function of column 1 for the X-axis. Columns 2 and above are each plotted in a separate graph, in a separate window, with the corresponding fitted data as a function of column 1. By default all the shear datasets and/or the bulk datasets as well as the corresponding fitting results are plotted in two separated graphs in a GUI window. To view a specific data and its corresponding fitting result, you click the right mouse button on the specific dataset, and pick a desired option. You can also use the right mouse button to turn the legend and/or axis on and off. The scales can be also switched between log scale and regular scale. With the middle button you can eliminate certain curves from each window's display in order to see the remaining data more clearly. Reviewing your curve fitting result graphically is the only way to ensure a good fit. After plotting the curve fitting results, you can then review it and also verify the error norm/residual value that is printed in the curve fitting GUI window. This information helps you determine the quality of a curve fitting and decide whether to accept the results. If not, you may want to go back to step 3, solve again by changing the order of the Prony series, redefining certain initial values of the coefficients, and possibly other control parameters. Repeat steps 3-7 until you are satisfied with the solution.
9.4.1.7. Write Data to TB Command After a successful curve fitting, the last step is to write the curve fitting data as ANSYS Prony data table (the TB,Prony command) to ANSYS database. The GUI or the command line converts the coefficients to the appropriate form before writing TB commands.
9.4.1.7.1. Batch TBFT,FSET,ID,Option2,Option3
Option2 = CASE Option3 = casename
9–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 9.4: Viscoelastic Material Curve Fitting
9.4.1.7.2. GUI Click the “Write to Database” button and the fitted coefficients are automatically written to the ANSYS material database according Prony data table. Please note that the coefficients you see in the curve fitting module are different from those in the TB tables. The τ values remain the same, but the α values are different. The α values shown in ANSYS are the square of the α values derived during curve fitting. They are also normalized to make α at time 0 = 1.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
9–21
9–22
Chapter 10: Gasket Joints Simulation 10.1. Overview of Gasket Joints Gasket joints are essential components in most structural assemblies. Gaskets as sealing components between structural components are usually very thin and made of many materials, such as steel, rubber and composites. From a mechanics point of view, gaskets act to transfer force between components. The primary deformation of a gasket is usually confined to one direction, namely, through thickness. The stiffness contributions from membrane (in plane) and transverse shear are much smaller in general compared to the through thickness. The stiffness contribution therefore is assumed to be negligible, although the TB command provides options to account for transverse shear. A typical example of a gasket joint is in engine assemblies. A thorough understanding of the gasket joint is critical in engine design and operation. This includes an understanding of the behavior of gasket joint components themselves in an engine operation, and the interaction of the gasket joint with other components. Elements within the ANSYS family of interface element are used to model gaskets. By default, these elements are designed to account for gasket through-thickness behavior. However, you can account for transverse shear behavior by using an element Keyopt setting and transverse shear option of the gasket material data table. See the TB command documentation and the specific element documentation for more information.
10.2. Performing a Gasket Joint Analysis A gasket joint analysis involves the same overall steps that are involved in any ANSYS nonlinear analysis procedure. Most of these steps however warrant special considerations for a gasket joint analysis. Presented below are the overall steps with the special considerations noted, along with links to applicable sections where more detailed information is included on that topic. 1.
Build or import the model. There are no special considerations for building or importing the model for a gasket joint analysis. You perform this step as you would in any typical ANSYS analysis. See Section 1.2: Building a Model in the ANSYS Basic Analysis Guide. For further details on building the model, see the ANSYS Modeling and Meshing Guide.
2.
Define element type. To properly simulate gasket joints, you must define structural element types and corresponding interface element types. See Section 10.4: ANSYS Family of Interface Elements in this chapter for more details on this topic, and in particular, see Section 10.4.1: Element Selection for a table of corresponding structural and interface elements.
3.
Define material. Use TB,GASKET to define the gasket joint material. You can use TB,GASKET to define four types of data input: general parameters, transverse shear stiffness, compression (loading), and tension (unloading). You specify the type using TBOPT. You then input the sets of data using the TBDATA and TBPT commands, as applicable. You can also plot most of the gasket data types using the TBPLOT command. See Section 10.5: Material Definition in this chapter for more details on this topic.
4.
Mesh the model. Use the AMESH or VMESH commands to mesh the structural element types, and use the IMESH command to mesh the gasket layer. Special restrictions apply to the IMESH command in terms of matching the source and target. Also, the order in which you execute these commands is critical. You can also mesh interface layers using the VDRAG command, and can generate interface elements directly using the EGEN command. Each of these commands involve special considerations for interface elements. See Section 10.6: Meshing Interface Elements in this chapter for more details on this topic.
5.
Solve. There are special solving considerations when you perform a gasket joint analysis. These are primarily concerned with the gasket element stiffness loss, and the gasket element's use with contact
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 10: Gasket Joints Simulation elements. See Section 10.7: Solution Procedure and Result Output in this chapter for more details on this topic. 6.
Review Results. You can print or plot any of four gasket output items: stresses (also pressure), total closure, total inelastic closure, and thermal closure, using the PRESOL, PRNSOL, PLESOL, PLNSOL, or ESOL commands. You can also use these items with the *GET command in POST1. See Section 10.8: Reviewing the Results in this chapter for more details on this topic.
10.3. Finite Element Formulation The primary deformation behavior of gasket joints is through-thickness deformation. It is therefore difficult to use solid continuum elements to effectively model gasket joints. The interface elements, which are based on the relative deformation of the top and bottom surfaces, offer a direct means to quantify through-thickness deformation of the gasket joints. Thus the pressure versus closure behavior can be directly applied to characterize the gasket material. The element formulation is based on a corotational procedure. Refer to Gasket Material in the ANSYS, Inc. Theory Reference for further details.
10.3.1. Element Topologies An interface element is composed of bottom and top surfaces. ANSYS provides several types of interface elements for the analysis of the gasket joints. Figure 10.1: “Element Topology of a 3-D 8-Node Interface Element” shows the geometry of a 3-D 8-node interface element available in ANSYS. An element midplane is created by averaging the coordinates of node pairs from the bottom and top surfaces of the elements. The numerical integration of interface elements is performed in the element midplane. The Gauss integration scheme is used for the numerical integration.
Figure 10.1 Element Topology of a 3-D 8-Node Interface Element
10.3.2. Thickness Direction The thickness direction is defined as the normal direction of the mid plane of the element at the integration point, and computed inside of ANSYS. The positive direction is defined by the right-hand rule going around the nodes in the midplane. The through thickness deformation is quantified by the relative deformation of bottom and top surfaces along the thickness direction. The thickness direction is then noted as the X-direction according to the ANSYS notation convention. No ESYS coordinate system is allowed for the elements.
10–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.4: ANSYS Family of Interface Elements
10.4. ANSYS Family of Interface Elements ANSYS offers 4 types of elements to simulate gaskets. They are referred to as interface elements and are summarized as follows: •
INTER192 - 2-D, 4-node, linear element.
•
INTER193 - 2-D, 6-node, quadratic element.
•
INTER194 - 3-D, 16-node, quadratic element.
•
INTER195 - 3-D, 8-node, linear element
The 2-D elements, INTER192 and INTER193, use a KEYOPT to define various stress state options.
10.4.1. Element Selection The simulation of an entire gasket joint assembly, consisting of the gasket and the structural elements on either side of the gasket, involves choosing interface elements and structural elements that have the same characteristics. Use the following table as a guideline for choosing interface and structural elements that have the same characteristics: For elements with these characteristics:
... use this interface element:
... with one of these structural elements:
2-D, linear
INTER192
PLANE42, HYPER56, VISCO106, PLANE182
2-D, quadratic
INTER193
PLANE2, PLANE82, HYPER84, VISCO88, PLANE183
3-D, quadratic
INTER194
VISCO89, SOLID92, SOLID95, SOLID96, SOLID186, SOLID187
3-D, linear
INTER195
SOLID45, SOLID46, HYPER58, SOLID62, SOLID64, SOLID65, HYPER86, SOLID185
Proper element type is chosen based on the stress states of interest and structural element types used. Element selection is done by the element type command, ET, for example, ET,1,195
defines element type 1 as element INTER195.
10.4.2. Applications In general, linear and quadratic elements are chosen for the following reasons: •
Fewer nodes produce a smaller model that runs faster with less computer resources.
•
Quadratic elements are necessary if stress gradients are present in surrounding bodies.
•
If elements are to follow a curved boundary closely, quadratic elements are ideal because their edges are arcs.
•
With a free mesh (tetrahedral elements) the mid-node (quadratic) is required for an accurate solution.
When a surrounding structure can be considered as a 2-D structure, for example, plane stress / strain / axisymmetric, 2-D elements are the ideal choice. A good example of the use of 2-D element INTER192 or INTER193 is the gasket between the "flanged" ends of pipe line. In this case the gasket properties do not vary significantly with geometric location.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–3
Chapter 10: Gasket Joints Simulation For a 3-D structure such as an internal combustion engine, 3-D element INTER194 or INTER195 is a good choice for simulating the gasket between the cylinder head and block. In this case there is no "nice" geometry because the gasket must fill in between two complicated surfaces, in between cylinders, and around other holes and passages. Also the gasket properties can vary in different zones. For example in a cylinder head, there is usually a much stiffer zone immediately around the cylinder to contain combustion pressure (called the "fire ring"). The remainder of the gasket is much softer.
10.5. Material Definition 10.5.1. Material Characteristics The TB command option GASKET allows gasket joints to be simulated with the ANSYS interface elements, in which there is only one element through the thickness, and the through thickness deformation is decoupled from the in plane deformation. The gasket material is usually under compression. The material under compression is highly nonlinear. The gasket material also exhibits quite complicated unloading behavior when compression is released. The GASKET option allows you to directly input data for the experimentally measured complex pressure closure curve for the material model (compression curve), and also for several unloading pressure closure curves. When no unloading curves are defined, the material behavior follows the compression curve while it is unloaded. As it is a joint component, there often exists an initial gap or void. On the other hand, from a modeling point of view, it is a lot easier to fill the spaces or volumes between the adjacent components with the interface meshes, and then set an initial gap for the gasket material to account for it. As long as the closure is less than the initial gap, no pressure is acted on the gaskets. Also, when it is under tension loading, there will be an open gap. Therefore, gasket joints generally do not have tension pressure. A stress cap is used to restrict tension pressure in the gasket joint elements. The GASKET material option must be used with interface elements INTER192, INTER193, INTER194, and INTER195. Figure 10.2: “Pressure vs. Closure Behavior of a Gasket Material” shows the experimental pressure vs. closure (relative displacement of top and bottom gasket surfaces) data for a graphite composite gasket material. The sample was unloaded and reloaded 5 times along the loading path and then unloaded at the end of the test to determine the materials unloading stiffness.
10–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.5: Material Definition
Figure 10.2 Pressure vs. Closure Behavior of a Gasket Material
10.5.2. Input Format You input gasket material data using TB,GASKET. The material data consists of 2 main parts: general parameters and pressure closure behaviors. The general parameters define initial gasket gap, stable stiffness for numerical stabilization, and stress cap for a gasket in tension. The pressure closure behavior includes gasket compression (loading) and tension data (unloading). The TB command specification for defining a gasket material is: TB,GASKET,MAT,NTEMP,NPTS,TBOPT where TBOPT = one of the following types of gasket material data: •
PARA: gasket material general parameters.
•
COMP: gasket compression data.
•
LUNL: gasket linear unloading data.
•
NUNL: gasket nonlinear unloading data.
•
TSS: gasket transverse shear stiffness data.
You input the general parameters using the TBDATA command, then input the compression and unloading data using the TBPT command. Presented in the following sections are examples of inputs for the various types of gasket data.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–5
Chapter 10: Gasket Joints Simulation
10.5.2.1. Define General Parameters (TBOPT = PARA) The gasket material general parameters include the initial gap, stable stiffness and the maximum tension stress cap. These parameters are defined as C1, C2, and C3 in the following example: TB,GASKET,MAT,NTEMP,NPTS,PARA TBDATA,1,C1,C2,C3
Refer to Gasket Materials in the ANSYS Elements Reference for further details on these parameters.
10.5.2.2. Define Compression Load Closure Curve (TBOPT = COMP) The compression pressure closure curve gasket material definition option is defined as follows: TB,GASKET,MAT,NTEMP,NPTS,COMP TBPT,,x1,y1 TBPT,,x2,y2 TBPT,,xi,yi
where: xi, yi are pairs of closure and pressure values. The following input listing is an example defining a compressive pressure vs. closure behavior of a gasket joint material with 10 data points. TB,GASKET,1, ,10,COMP TBPT,, 0.20000E-04, 0.54000E+08 TBPT,, 0.40000E-04, 0.15150E+09 TBPT,, 0.60000E-04, 0.24900E+09 TBPT,, 0.78000E-04, 0.30000E+09 TBPT,, 0.12000E-03, 0.37200E+09 TBPT,, 0.19000E-03, 0.47400E+09 TBPT,, 0.28600E-03, 0.58500E+09 TBPT,, 0.35800E-03, 0.67350E+09 TBPT,, 0.43200E-03, 0.78000E+09 TBPT,, 0.50500E-03, 0.89550E+09
! define compression data
10.5.2.3. Define Linear Unloading Data (TBOPT = LUNL) The linear unloading gasket material definition option is a simple way to define the gasket unloading behavior. Several unloading slopes can be defined to accommodate the comprehensive unloading behavior as follows: TB,GASKET,MAT,NTEMP,NPTS,LUNL TBPT,,x1,y1 TBPT,,x2,y2 TBPT,,xi,yi
where: NPTS is the number of unloading points; xi is the closure where unloading started, and yi is unloading slope. The following input listing is an example showing the linear unloading behavior of a gasket joint material with 3 unloading points TB,GASKET,1, ,3,LUNL ! define linear unloading data TBPT,, 0.78000E-04, 0.25100E+12
10–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.5: Material Definition TBPT,, 0.28600E-03, 0.25500E+12 TBPT,, 0.50500E-03, 0.10600E+13
A sample plot representing linear unloading curves is shown in Figure 10.3: “Gasket Material Input: Linear Unloading Curves”.
Figure 10.3 Gasket Material Input: Linear Unloading Curves
10.5.2.4. Define Nonlinear Unloading Data (TBOPT = NUNL) The nonlinear unloading gasket material definition option provides a more comprehensive way of defining gasket material unloading behavior. The input listing format is: TB,GASKET,MAT,NTEMP,NPTS,NUNL TBPT,,x1,y1 TBPT,,x2,y2 TBPT,,xi,yi
where: xi, yi are pairs of closure and pressure values. Several unloading curves can be defined. An example showing the nonlinear unloading behavior of a gasket joint material with 3 unloading points is as follows: TB,GASKET,1, ,5,NUNL ! define first nonlinear unloading data TBPT,, 0.78000E-04, 0.30000E+09 TBPT,, 0.66900E-04, 0.24750E+08 TBPT,, 0.63100E-04, 0.82500E+07 TBPT,, 0.54100E-04, 0.15000E+07 TBPT,, 0.00000E+00, 0.00000E+00 TB,GASKET,1, ,5,NUNL
! define second nonlinear unloading data
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–7
Chapter 10: Gasket Joints Simulation TBPT,, TBPT,, TBPT,, TBPT,, TBPT,,
0.28600E-03, 0.26400E-03, 0.26100E-03, 0.25600E-03, 0.00000E+00,
0.58500E+09 0.22350E+08 0.90000E+07 0.15000E+07 0.00000E+00
TB,GASKET,1, ,5,NUNL TBPT,, 0.50500E-03, 0.89550E+09 TBPT,, 0.47800E-03, 0.33900E+08 TBPT,, 0.47500E-03, 0.13500E+08 TBPT,, 0.46800E-03, 0.15000E+07 TBPT,, 0.00000E+00, 0.00000E+00
! define third nonlinear unloading data
A sample plot representing nonlinear unloading curves is shown in Figure 10.4: “Gasket Material Input: Nonlinear Unloading Curves”.
Figure 10.4 Gasket Material Input: Nonlinear Unloading Curves
10.5.3. Temperature Dependencies Inputting temperature dependent gasket material properties follows the standard ANSYS procedure for inputting temperature dependent data for other materials. The following format shows this procedure. TB,GASKET,MAT,NTEMP,NPTS,LUNL TBTEMP,T1 TBPT,,x1,y1 TBPT,,x2,y2 TBTEMP,T2 TBPT,,x1,y1 TBPT,,x2,y2
ANSYS will automatically interpolate the temperature data to the material points using linear interpolation. When the temperature is out of the specified range, the closest temperature point is used.
10–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.5: Material Definition The following is an example input listing defining a compressive pressure vs. closure behavior of a gasket joint material with 5 temperature points and up to 10 data points for each temperature point, and 3 nonlinear unloading curves with each curve having 5 temperatures and 5 data points. TB,GASKET,1, 5,10,COMP ! define compression data with 5 temperatures TBTEMP, 100.000 TBPT,, 0.20000E-04, 0.54000E+08 TBPT,, 0.40000E-04, 0.15150E+09 TBPT,, 0.60000E-04, 0.24900E+09 TBPT,, 0.78000E-04, 0.30000E+09 TBPT,, 0.12000E-03, 0.37200E+09 TBPT,, 0.19000E-03, 0.47400E+09 TBPT,, 0.28600E-03, 0.58500E+09 TBPT,, 0.35800E-03, 0.67350E+09 TBPT,, 0.43200E-03, 0.78000E+09 TBPT,, 0.50500E-03, 0.89550E+09 TBTEMP, 200.000 TBPT,, 0.20000E-04, TBPT,, 0.40000E-04, TBPT,, 0.60000E-04, TBPT,, 0.78000E-04, TBPT,, 0.12000E-03, TBPT,, 0.19000E-03, TBPT,, 0.28600E-03, TBPT,, 0.35800E-03, TBPT,, 0.43200E-03, TBPT,, 0.50500E-03,
0.18000E+08 0.50500E+08 0.83000E+08 0.10000E+09 0.12400E+09 0.15800E+09 0.19500E+09 0.22450E+09 0.26000E+09 0.29850E+09
TBTEMP, 300.000 TBPT,, 0.20000E-04, TBPT,, 0.40000E-04, TBPT,, 0.60000E-04, TBPT,, 0.78000E-04, TBPT,, 0.12000E-03, TBPT,, 0.19000E-03, TBPT,, 0.28600E-03, TBPT,, 0.35800E-03, TBPT,, 0.43200E-03, TBPT,, 0.50500E-03,
0.90000E+07 0.25250E+08 0.41500E+08 0.50000E+08 0.62000E+08 0.79000E+08 0.97500E+08 0.11225E+09 0.13000E+09 0.14925E+09
TBTEMP, 400.000 TBPT,, 0.20000E-04, TBPT,, 0.40000E-04, TBPT,, 0.60000E-04, TBPT,, 0.78000E-04, TBPT,, 0.12000E-03, TBPT,, 0.19000E-03, TBPT,, 0.28600E-03, TBPT,, 0.35800E-03, TBPT,, 0.43200E-03, TBPT,, 0.50500E-03,
0.36000E+07 0.10100E+08 0.16600E+08 0.20000E+08 0.24800E+08 0.31600E+08 0.39000E+08 0.44900E+08 0.52000E+08 0.59700E+08
TBTEMP, 500.000 TBPT,, 0.20000E-04, TBPT,, 0.40000E-04, TBPT,, 0.60000E-04, TBPT,, 0.78000E-04, TBPT,, 0.12000E-03, TBPT,, 0.19000E-03, TBPT,, 0.28600E-03, TBPT,, 0.35800E-03, TBPT,, 0.43200E-03, TBPT,, 0.50500E-03,
0.18000E+07 0.50500E+07 0.83000E+07 0.10000E+08 0.12400E+08 0.15800E+08 0.19500E+08 0.22450E+08 0.26000E+08 0.29850E+08
TB,GASKET,1, 5,5,NUNL ! define first nonlinear unloading data with 5 temperatures TBTEMP, 100.000 TBPT,, 0.78000E-04, 0.30000E+09 TBPT,, 0.66900E-04, 0.24750E+08 TBPT,, 0.63100E-04, 0.82500E+07 TBPT,, 0.54100E-04, 0.15000E+07
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–9
Chapter 10: Gasket Joints Simulation TBPT,, 0.00000E+00, 0.00000E+00 TBTEMP, 200.000 TBPT,, 0.78000E-04, TBPT,, 0.66900E-04, TBPT,, 0.63100E-04, TBPT,, 0.54100E-04, TBPT,, 0.00000E+00,
0.10000E+09 0.82500E+07 0.27500E+07 0.50000E+06 0.00000E+00
TBTEMP, 300.000 TBPT,, 0.78000E-04, TBPT,, 0.66900E-04, TBPT,, 0.63100E-04, TBPT,, 0.54100E-04, TBPT,, 0.00000E+00,
0.50000E+08 0.41250E+07 0.13750E+07 0.25000E+06 0.00000E+00
TBTEMP, 400.000 TBPT,, 0.78000E-04, TBPT,, 0.66900E-04, TBPT,, 0.63100E-04, TBPT,, 0.54100E-04, TBPT,, 0.00000E+00,
0.20000E+08 0.16500E+07 0.55000E+06 0.10000E+06 0.00000E+00
TBTEMP, 500.000 TBPT,, 0.78000E-04, TBPT,, 0.66900E-04, TBPT,, 0.63100E-04, TBPT,, 0.54100E-04, TBPT,, 0.00000E+00,
0.10000E+08 0.82500E+06 0.27500E+06 0.50000E+05 0.00000E+00
TB,GASKET,1, 5,5,NUNL ! define second nonlinear unloading data with 5 temperatures TBTEMP, 100.000 TBPT,, 0.28600E-03, 0.58500E+09 TBPT,, 0.26400E-03, 0.22350E+08 TBPT,, 0.26100E-03, 0.90000E+07 TBPT,, 0.25600E-03, 0.15000E+07 TBPT,, 0.00000E+00, 0.00000E+00 TBTEMP, 200.000 TBPT,, 0.28600E-03, TBPT,, 0.26400E-03, TBPT,, 0.26100E-03, TBPT,, 0.25600E-03, TBPT,, 0.00000E+00,
0.19500E+09 0.74500E+07 0.30000E+07 0.50000E+06 0.00000E+00
TBTEMP, 300.000 TBPT,, 0.28600E-03, TBPT,, 0.26400E-03, TBPT,, 0.26100E-03, TBPT,, 0.25600E-03, TBPT,, 0.00000E+00,
0.97500E+08 0.37250E+07 0.15000E+07 0.25000E+06 0.00000E+00
TBTEMP, 400.000 TBPT,, 0.28600E-03, TBPT,, 0.26400E-03, TBPT,, 0.26100E-03, TBPT,, 0.25600E-03, TBPT,, 0.00000E+00,
0.39000E+08 0.14900E+07 0.60000E+06 0.10000E+06 0.00000E+00
TBTEMP, 500.000 TBPT,, 0.28600E-03, TBPT,, 0.26400E-03, TBPT,, 0.26100E-03, TBPT,, 0.25600E-03, TBPT,, 0.00000E+00,
0.19500E+08 0.74500E+06 0.30000E+06 0.50000E+05 0.00000E+00
TB,GASKET,1, 5,5,NUNL ! define third nonlinear unloading data with 5 temperatures TBTEMP, 100.000 TBPT,, 0.50500E-03, 0.89550E+09 TBPT,, 0.47800E-03, 0.33900E+08 TBPT,, 0.47500E-03, 0.13500E+08 TBPT,, 0.46800E-03, 0.15000E+07
10–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.5: Material Definition TBPT,, 0.00000E+00, 0.00000E+00 TBTEMP, 200.000 TBPT,, 0.50500E-03, TBPT,, 0.47800E-03, TBPT,, 0.47500E-03, TBPT,, 0.46800E-03, TBPT,, 0.00000E+00,
0.29850E+09 0.11300E+08 0.45000E+07 0.50000E+06 0.00000E+00
TBTEMP, 300.000 TBPT,, 0.50500E-03, TBPT,, 0.47800E-03, TBPT,, 0.47500E-03, TBPT,, 0.46800E-03, TBPT,, 0.00000E+00,
0.14925E+09 0.56500E+07 0.22500E+07 0.25000E+06 0.00000E+00
TBTEMP, 400.000 TBPT,, 0.50500E-03, TBPT,, 0.47800E-03, TBPT,, 0.47500E-03, TBPT,, 0.46800E-03, TBPT,, 0.00000E+00,
0.59700E+08 0.22600E+07 0.90000E+06 0.10000E+06 0.00000E+00
TBTEMP, 500.000 TBPT,, 0.50500E-03, TBPT,, 0.47800E-03, TBPT,, 0.47500E-03, TBPT,, 0.46800E-03, TBPT,, 0.00000E+00,
0.29850E+08 0.11300E+07 0.45000E+06 0.50000E+05 0.00000E+00
Sample plots of compression and unloading curves for gasket data to two temperatures is shown in Figure 10.5: “Gasket Compression and Unloading Curves at Two Temperatures”.
Figure 10.5 Gasket Compression and Unloading Curves at Two Temperatures
"
#
!
!$ #
10.5.4. Plotting Gasket Data You can plot gasket compression, linear unloading and nonlinear unloading data using the TBPLOT command. The use of this command to plot gasket data is as follows: Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–11
Chapter 10: Gasket Joints Simulation TBPLOT,GASKET,MAT,TBOPT,TEMP,SEGN where TBOPT specifies the gasket material option to be plotted, TEMP specifies plotting either all of the temperature dependent data curves, or a curve at a specified temperature, and SEGN specifies whether or not to add the segment numbers to the curves.
10.6. Meshing Interface Elements Three options are available for meshing interface elements: •
For meshing gasket layers as an area or volume, use the IMESH command.
•
For meshing gasket layers by dragging an area mesh along a path, use the VDRAG command.
•
For generating interface elements directly from a pattern, use the EGEN command.
There are special requirements for meshing interface elements. See Section 7.5.6: Generating an Interface Mesh for Gasket Simulations in the ANSYS Modeling and Meshing Guide for further details on this type of meshing. The following example input listing shows the use of the IMESH command. /batch,list /title, Test to demonstrate the use of IMESH command /com, ************************************************************ /com, * * /com, * This is a simple test to demonstrate the use of IMESH * /com, * command to generate gasket elements. The model consists * /com, * of two blocks with gasket elements (INTER194) defined * /com, * between them. * /com, * * /com, ************************************************************ /prep7 !*+++++++++++++++++++++++++++++++++++++++ !* Define Element Types !*+++++++++++++++++++++++++++++++++++++++ et,1,187 ! Solid tetrahedral element et,2,194 ! Interface layer element !*+++++++++++++++++++++++++++++++++++++++ !* Define Parameters !*+++++++++++++++++++++++++++++++++++++++ EH=1.0 IH=0.1 DX=0 DY=0 DZ=IH Z1=EH Z2=Z1+IH Z3=Z2+EH !*+++++++++++++++++++++++++++++++++++++++ !* Generate Keypoints !*+++++++++++++++++++++++++++++++++++++++ k,1,0,0 k,2,1,0 k,3,1,1 k,4,0,1 k,5,0,0,z1 k,6,1,0,z1 k,7,1,1,z1 k,8,0,1,z1 k,9,0,0,z2 k,10,1,0,z2 k,11,1,1,z2 k,12,0,1,z2
10–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.6: Meshing Interface Elements k,13,0,0,z3 k,14,1,0,z3 k,15,1,1,z3 k,16,0,1,z3 !*+++++++++++++++++++++++++++++++++++++++ !* Generate First Volume !*+++++++++++++++++++++++++++++++++++++++ v,1,2,3,4,5,6,7,8 !*+++++++++++++++++++++++++++++++++++++++ !* Generate Second Volume !*+++++++++++++++++++++++++++++++++++++++ v,9,10,11,12,13,14,15,16 !*+++++++++++++++++++++++++++++++++++++++ !* Generate Middle Volume !*+++++++++++++++++++++++++++++++++++++++ v,5,6,7,8,9,10,11,12 !*+++++++++++++++++++++++++++++++++++++++ !* Define Element Size !*+++++++++++++++++++++++++++++++++++++++ esize,,4 ! !*+++++++++++++++++++++++++++++++++++++++ !* Mesh First Volume with Element Type 1 !*+++++++++++++++++++++++++++++++++++++++ type,1 mat,1 vmesh,1 !*++++++++++++++++++++++++++++++++++++++++++++ !* Generate Interface Layer with IMESH command !* using Element Type 2 (INTER194) !*++++++++++++++++++++++++++++++++++++++++++++ type,2 mat,2 imesh,area,6,7,0,DX,DY,DZ,TOL !*+++++++++++++++++++++++++++++++++++++++ !* Mesh Second Volume with Element Type 1 !*+++++++++++++++++++++++++++++++++++++++ type,1 mat,1 vmesh,2 !*+++++++++++++++++++++++++++++++++++++++ !* Plot Elements !*+++++++++++++++++++++++++++++++++++++++ /view,1 ,1,1,1 eplot finish
Figure 10.6: “Gasket Finite Element Model Geometry” shows the geometry of the finite element model, a thin interface layer between two block volumes. Figure 10.7: “Whole Model Mesh with Brick Element” shows the mesh with solid brick element, SOLID185, in top and bottom of block volumes, and Figure 10.8: “Interface Layer Mesh” shows the mesh of interface element, INTER195, in the interface layer between the two blocks. Figure 10.9: “Whole Model Tetrahedral Mesh” shows the mesh with solid tetrahedral element, SOLID187, in top and bottom of block volumes, and Figure 10.10: “Interface Layer Mesh with Degenerated Wedge Elements” shows the mesh of interface element (degenerated wedge), INTER194, in the interface layer between the two blocks.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–13
Chapter 10: Gasket Joints Simulation
Figure 10.6 Gasket Finite Element Model Geometry
Figure 10.7 Whole Model Mesh with Brick Element
10–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.6: Meshing Interface Elements
Figure 10.8 Interface Layer Mesh
Figure 10.9 Whole Model Tetrahedral Mesh
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–15
Chapter 10: Gasket Joints Simulation
Figure 10.10 Interface Layer Mesh with Degenerated Wedge Elements
10.7. Solution Procedure and Result Output Gasket material behavior is highly nonlinear. The full Newton-Raphson solution procedure (the standard ANSYS nonlinear method), is the default method for performing this type of analysis. Other solution procedures for gasket solutions are not recommended. Like most nonlinear problems, convergence behavior of a gasket joint analysis depends strongly on the particular problem to be solved. ANSYS has provided a comprehensive solution hierarchy, therefore it is always recommended that you use the ANSYS default solution options, unless you are sure about the benefits of the changes. Some special considerations for solving a gasket problem are as follows: •
By default a zero stress cap has been enforced on the gasket. When the element goes into tension, it will lose its stiffness and may cause numerical instability.
•
It is always a good practice to place the lower and upper limit on the time step size using the DELTIM or NSUBST commands, and to start with a small time step, then subsequently ramp it up . This ensures that all of the modes and behaviors of interest will be accurately included and that the problem is solved effectively.
•
Gasket elements must be configured to support transverse shear. Even if you do so, errors can result, especially for contact and other nonlinear applications. You should not use gasket elements with contact elements unless you configure the elements accordingly, and ascertain the mesh compatibility of the gasket layer and its mating components.
Like any other type of nonlinear analysis, the ANSYS program performs a series of linear approximations with corrections. A convergence failure can indicate a physical instability in the structure, or it can merely be the result of some numerical problem in the finite element model. The program printout gives you continuous feedback on the progress of these approximations and corrections. (The printout either appears directly on your screen, is captured on Jobname.OUT, or is written to some other file [/OUTPUT].) You can examine some of this same information in POST1, using the PRITER command, or in POST26, using the SOLU and PRVAR commands. You should make sure that you understand the iteration history of your analysis before you accept the results. In 10–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.7: Solution Procedure and Result Output particular, do not dismiss any program error or warning statements without fully understanding their meaning. A typical output listing with gasket nonlinearity only is shown in Section 10.7.1: Typical Gasket Solution Output Listing. When other types of nonlinearity such as contact or materials are included, additional information will be printed out.
10.7.1. Typical Gasket Solution Output Listing S O L U T I O N PROBLEM DIMENSIONALITY. . . DEGREES OF FREEDOM. . . . . ANALYSIS TYPE . . . . . . . PLASTIC MATERIAL PROPERTIES NEWTON-RAPHSON OPTION . . .
. . . . . . UX UY . . . . . INCLUDED. . . . . .
O P T I O N S . . . UZ . . . . . . . . .
. .3-D . .STATIC (STEADY-STATE) . .YES . .PROGRAM CHOSEN
*** NOTE *** CP= 0.000 TIME= 00:00:00 Present time 0 is less than or equal to the previous time. Time will default to 1. *** NOTE ***
CP=
0.000
TIME= 00:00:00
Nonlinear analysis, NROPT set to the FULL Newton-Raphson solution procedure for ALL DOFs. *** NOTE ***
CP=
0.000
The conditions for direct assembly have been met. files will be produced. L O A D
S T E P
TIME= 00:00:00
No .emat or .erot
O P T I O N S
LOAD STEP NUMBER. . . . . . . . . . . . . TIME AT END OF THE LOAD STEP. . . . . . . AUTOMATIC TIME STEPPING . . . . . . . . . INITIAL NUMBER OF SUBSTEPS . . . . . . MAXIMUM NUMBER OF SUBSTEPS . . . . . . MINIMUM NUMBER OF SUBSTEPS . . . . . . MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS. STEP CHANGE BOUNDARY CONDITIONS . . . . . TERMINATE ANALYSIS IF NOT CONVERGED . . . CONVERGENCE CONTROLS. . . . . . . . . . . COPY INTEGRATION POINT VALUES TO NODE . .
. . . . . . . . . . .
. . . . . . . . . . .
. 1 . 1.0000 . ON . 200 . 20000 . 20 . 15 . NO .YES (EXIT) .USE DEFAULTS .YES, FOR ELEMENTS WITH ACTIVE MAT. NONLINEARITIES PRINT OUTPUT CONTROLS . . . . . . . . . . . . .NO PRINTOUT DATABASE OUTPUT CONTROLS ITEM FREQUENCY COMPONENT ALL ALL SVAR ALL
Range of element maximum matrix coefficients in global coordinates Maximum= 4.326388889E+11 at element 0. Minimum= 388758681 at element 0. *** ELEMENT MATRIX FORMULATION TIMES TYPE NUMBER ENAME TOTAL CP AVE CP 1 2 SOLID185 0.000 0.000000 2 1 INTER195 0.000 0.000000 Time at end of element matrix formulation CP= 0. ALL CURRENT ANSYS DATA WRITTEN TO FILE NAME= FOR POSSIBLE RESUME FROM THIS POINT FORCE CONVERGENCE VALUE = 0.4200E+07 CRITERION= 0.2143E+05 SPARSE MATRIX DIRECT SOLVER. Number of equations = 24, Memory available (MB) = 0.0 DISP CONVERGENCE VALUE EQUIL ITER 1 COMPLETED.
Maximum wavefront = , Memory required (MB)
0 =
0.0
= 0.1130E-04 CRITERION= 0.2000E-06 NEW TRIANG MATRIX. MAX DOF INC= -0.4000E-05
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–17
Chapter 10: Gasket Joints Simulation
FORCE CONVERGENCE VALUE = 0.1367E-08 CRITERION= 51.35 <<< CONVERGED DISP CONVERGENCE VALUE = 0.3257E-20 CRITERION= 0.2000E-06 <<< CONVERGED EQUIL ITER 2 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC = -0.2234E-20 >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 2 *** ELEMENT RESULT CALCULATION TIMES TYPE
NUMBER 1 2
ENAME 2 1
SOLID185 INTER195
TOTAL CP 0.000 0.000
*** NODAL LOAD CALCULATION TIMES TYPE NUMBER ENAME TOTAL CP 1 2
2 1
SOLID185 INTER195
0.000 0.000
AVE CP 0.000000 0.000000
AVE CP 0.000000 0.000000
*** LOAD STEP 1 SUBSTEP 1 COMPLETED. CUM ITER = *** TIME = 0.500000E-02 TIME INC = 0.500000E-02 *** AUTO STEP TIME: NEXT TIME INC = 0.50000E-02 UNCHANGED
2
FORCE CONVERGENCE VALUE = 0.7716E-09 CRITERION= 100.6 DISP CONVERGENCE VALUE = 0.1951E-20 CRITERION= 0.2000E-06 <<< CONVERGED EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1642E-20 FORCE CONVERGENCE VALUE = 0.4624E-09 CRITERION= 102.7 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 1 *** LOAD STEP 1 SUBSTEP 2 COMPLETED. CUM ITER = 3 *** TIME = 0.100000E-01 TIME INC = 0.500000E-02 *** AUTO TIME STEP: NEXT TIME INC = 0.75000E-02 INCREASED (FACTOR = 1.5000) FORCE CONVERGENCE VALUE = 0.1964E-08 CRITERION= 176.1 DISP CONVERGENCE VALUE = 0.3748E-20 CRITERION= 0.3000E-06 <<< CONVERGED EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.2744E-20 FORCE CONVERGENCE VALUE = 0.8307E-09 CRITERION= 179.7 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 1 *** LOAD STEP 1 SUBSTEP 3 COMPLETED. CUM ITER = 4 *** TIME = 0.175000E-01 TIME INC = 0.750000E-02 *** AUTO TIME STEP: NEXT TIME INC = 0.11250E-01 INCREASED (FACTOR = 1.5000) FORCE CONVERGENCE VALUE = 0.3713E-08 CRITERION= 289.4 DISP CONVERGENCE VALUE = 0.7198E-20 CRITERION= 0.4500E-06 <<< CONVERGED EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.4503E-20 FORCE CONVERGENCE VALUE = 0.1468E-08 CRITERION= 295.3 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 1 *** LOAD STEP 1 SUBSTEP 4 COMPLETED. CUM ITER = 5 *** TIME = 0.287500E-01 TIME INC = 0.112500E-01 *** AUTO TIME STEP: NEXT TIME INC = 0.16875E-01 INCREASED (FACTOR = 1.5000) FORCE CONVERGENCE VALUE = 0.1833E-07 CRITERION= 459.2 DISP CONVERGENCE VALUE = 0.3753E-19 CRITERION= 0.6750E-06 <<< CONVERGED EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1800E-19 FORCE CONVERGENCE VALUE = 0.3550E-08 CRITERION= 468.6 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 1 *** LOAD STEP 1 SUBSTEP 5 COMPLETED. CUM ITER = 6 *** TIME = 0.456250E-01 TIME INC = 0.168750E-01 *** AUTO TIME STEP: NEXT TIME INC = 0.25313E-01 INCREASED (FACTOR = 1.5000) FORCE CONVERGENCE VALUE = 0.2322E-07 CRITERION= 714.0 DISP CONVERGENCE VALUE = 0.4656E-19 CRITERION= 0.1013E-05 <<< CONVERGED EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.2664E-19 FORCE CONVERGENCE VALUE = 0.6406E-08 CRITERION= 728.5 <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 1 *** LOAD STEP 1 SUBSTEP 6 COMPLETED. CUM ITER = 7 *** TIME = 0.709375E-01 TIME INC = 0.253125E-01 *** AUTO TIME STEP: NEXT TIME INC = 0.37969E-01 INCREASED (FACTOR = 1.5000)
10–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.8: Reviewing the Results
10.8. Reviewing the Results Results from a gasket joint analysis consist mainly of displacements, stresses, strains and reaction forces of the structural components and the gasket joint layer information (gasket pressure, closure, etc.). You can review these results in POST1, the general postprocessor, or in POST26, the time-history postprocessor. See the Output Data sections of the element descriptions for any of the interface elements (for example INTER192) for a description of the available output components. Note that in POST1, only one substep can be read in at a time, and that the results from that substep should have been written to Jobname.RST. (The load step option command OUTRES controls which substep results are stored on Jobname.RST.) A typical POST1 postprocessing sequence is described below.
10.8.1. Points to Remember •
To review results in POST1, the database must contain the same model for which the solution was calculated.
•
The results file (Jobname.RST) must be available.
10.8.2. Reviewing Results in POST1 1.
Verify from your output file (Jobname.OUT) whether or not the analysis converged at all load steps. •
If not, you probably won't want to postprocess the results, other than to determine why convergence failed.
•
If your solution converged, then continue postprocessing.
2.
Enter POST1. If your model is not currently in the database, issue RESUME. Command(s): /POST1 GUI: Main Menu> General Postproc
3.
Read in results for the desired load step and substep, which can be identified by load step and substep numbers or by time. Command(s): SET GUI: Main Menu> General Postproc> Read Results> load step
4.
Display the results using any of the following options. Note that gasket results, such as pressure and closure, are always displayed and listed in the local coordinate system. Option: Display Deformed Shape Command(s): PLDISP GUI: Main Menu> General Postproc> Plot Results> Deformed Shape Option: Contour Displays Command(s): PLNSOL or PLESOL GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu Use these options to display contours of stresses, strains, or any other applicable item. When displaying the gasket pressure distribution, if other structural mating components are not included, ANSYS will plot the geometry of those components in gray. To have a better visualization of a gasket pressure plot, it is better for you to select gasket elements only.
Option: Tabular Listings Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–19
Chapter 10: Gasket Joints Simulation Command(s): PRNSOL (nodal results) PRESOL (element-by-element results) PRRSOL (reaction data) PRITER (substep summary data), etc. GUI: Main Menu> General Postproc> List Results> Nodal Solution Main Menu> General Postproc> List Results> Element Solution Main Menu> General Postproc> List Results> Reaction Solution Option: Animation You can also animate gasket results over time: Command(s): ANTIME GUI: Utility Menu> PlotCtrls> Animate> Over Time Other Capabilities Many other postprocessing functions are available in POST1. See The General Postprocessor (POST1) in the ANSYS Basic Analysis Guide for details. Load case combinations usually are not valid for nonlinear analyses.
10.8.3. Reviewing Results in POST26 You can also review the load-history response of a nonlinear structure using POST26, the time-history postprocessor. Use POST26 to compare one ANSYS variable against another. For instance, you might graph the gasket closure vs. gasket pressure, which should correspond to the material behavior defined by TB,GASKET. You might also graph the displacement at a node versus the corresponding level of applied load, or you might list the gasket pressure at a node and the corresponding TIME value. A typical POST26 postprocessing sequence for a gasket analysis is the same as the sequence for a typical nonlinear analysis. See steps 1 through 4 in Section 8.5.6.3: Reviewing Results in POST26 included in Chapter 8, “Nonlinear Structural Analysis”.
10.9. Sample Gasket Element Verification Analysis (Command or Batch Method) This is a simple finite element model created to demonstrate the gasket material simulation. Two block elements with element type SOLID185 were generated as supporters and a gasket element INTER195 was created. The whole system is fixed along one side of each axes to prevent rigid body motion. A prescribed displacement is placed on top of the supporter element. The gasket material is assumed to have a nonlinear compression behavior with 5 different linear unloading slopes. A pressure stress cap of 1.0e-5 is imposed so that no tension stress is generated. Two load steps were used. The ANSYS commands are shown below. /batch,list /title, Test to Verify Gasket Material and Element /com, ************************************************************** /com, * * /com, * This is a simple test case to verify gasket material and * /com, * element. * /com, * * /com, * The test case is set up with two solid SOLID185 elements * /com, * with gasket element (INTER195) defined between them. * /com, * Displacement is applied to one SOLID185 element while the * /com, * other SOLID185 element is fixed. * /com, * The problem is solved in two load steps. In the first * /com, * load step negative z-displacement is applied to one * /com, * SOLID195 element causing compression of gasket elements. * /com, * Then, in the second load step, a reverse displacement is * /com, * applied causing the unloading (tension) of gasket element. * /com, * A Stress Cap of 1.0E-05 is enforced so that there is no * /com, * tension pressure in gasket material. * /com, * *
10–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.9: Sample Gasket Element Verification Analysis (Command or Batch Method) /com, ************************************************************** /prep7 !*+++++++++++++++++++++ !* Define Element Types !*+++++++++++++++++++++ et,1,185 et,2,195 !*++++++++++++++++++++++++++++++++++++++ !* Define Linear Elastic Material Type 1 !*++++++++++++++++++++++++++++++++++++++ mp,ex,1,2.1E12 mp,nuxy,1,0.0 !*+++++++++++++++++++++++++++++++++++++++++++++++++ !* Define Initial Gap, Stable Stiffness, Stress Cap !*+++++++++++++++++++++++++++++++++++++++++++++++++ delta0 = 0.00e-3 stiff0 = 0.0e7 scap = 1.0e-5 tb,gasket,2,,,para tbdata, 1,delta0,stiff0,scap !*++++++++++++++++++++++++++++++++ !* Define Gasket Compression Curve !*++++++++++++++++++++++++++++++++ tb,gask,2,1,13,comp tbpt,,0.460800E-03, 0.161226E+07 tbpt,,0.511600E-03, 0.520884E+07 tbpt,,0.562400E-03, 0.113134E+08 tbpt,,0.613200E-03, 0.200499E+08 tbpt,,0.664000E-03, 0.259960E+08 tbpt,,0.714800E-03, 0.290345E+08 tbpt,,0.765600E-03, 0.357453E+08 tbpt,,0.816400E-03, 0.440064E+08 tbpt,,0.867200E-03, 0.563189E+08 tbpt,,0.918000E-03, 0.748254E+08 tbpt,,0.968800E-03, 0.967287E+08 tbpt,,0.101960E-02, 0.129001E+09 tbpt,,0.109326E-02, 0.157147E+09 !*+++++++++++++++++++++++++++++++++++++ !* Define Gasket Linear Unloading Curve !*+++++++++++++++++++++++++++++++++++++ tb,gask,2,1,5,lunl tbpt,,0.460800E-03, 2.430000E+11 tbpt,,0.714800E-03, 3.565000E+11 tbpt,,0.816400E-03, 5.92300E+11 tbpt,,0.968800E-03, 1.088000e+12 tbpt,,0.109326E-02, 1.490000E+12 !*+++++++++++++++++++++++++++ !* List Gasket Material Model !*+++++++++++++++++++++++++++ tblist,gask,all !*++++++++++++++++++ !* Define Parameters !*++++++++++++++++++ n1 = 20 n2 = n1*100 n3 = n1 dis1 = -0.0008 dis2 = -0.000001 pres = 1.0e7 pres2 = 10 pres3 = 1.4E8 dp = -2.0e7 elb = 1.0 elg = 0.1
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–21
Chapter 10: Gasket Joints Simulation !*+++++++++++++++ !* Generate Nodes !*+++++++++++++++ n,1, n,2,1.0 n,3,1.0,1.0 n,4,0.0,1.0 ngen,2,4,1,4,,0.0,0.0,elb ngen,2,8,1,4,,0.0,0.0,elb+elg ngen,2,12,1,4,,0.0,0.0,2*elb+elg !*+++++++++++++++++++++++++++++++++++++++++ !* Generate Front and Back SOLID185 Element !*+++++++++++++++++++++++++++++++++++++++++ et,1,185,,1 mat,1 e,1,2,3,4,5,6,7,8 e,9,10,11,12,13,14,15,16 !*+++++++++++++++++++++++++++++++++ !* Generate Middle INTER195 Element !*+++++++++++++++++++++++++++++++++ et,2,195,, type,2 mat,2 e,5,6,7,8,9,10,11,12 !*++++++++++++++++++++++++++ !* Define Boundary Condition !*++++++++++++++++++++++++++ nsel,s,loc,z d,all,uz nsel,all nsel,s,loc,x d,all,ux nsel,all nsel,s,loc,y d,all,uy nsel,all finish /solu !*+++++++++++++++++++ !* Apply Displacement !*+++++++++++++++++++ nsel,s,loc,z,elb*2+elg d,all,uz,dis1 nsel,all !*+++++++++++++++++++++++++++++++++++++++++++++ !* Solve First Load Step, Compress the Elements !*+++++++++++++++++++++++++++++++++++++++++++++ nsubst,n1,n2,n3 outres,all,all outres,svar,all solve !*++++++++++++++++++++++++++++++++++++++++++ !* Solve Second Load Step, Open the Elements !*++++++++++++++++++++++++++++++++++++++++++ nsubst,n1,n2,n3 outres,all,all outres,svar,all nsel,s,loc,z,elb*2+elg d,all,uz,dis2 nall solve finish !*++++++++++++++++++++++++ !* Postprocess the Results !*++++++++++++++++++++++++
10–22
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 10.9: Sample Gasket Element Verification Analysis (Command or Batch Method) /post1 set,last pres,s pres,epto pres,epel prns,epel finish !*++++++++++++++++++++++++++++++++++++++++++++++ !* Post26, Print and Plot Gasket Element Results !*++++++++++++++++++++++++++++++++++++++++++++++ /post26 esol,2,3, ,s,x,press esol,3,3, ,epel,x,delta add,4,2, , ,press,,,-1, ! change sign for plotting add,5,3,,,delta,,,-1, ! change sign for plotting prvar,2,3,4,5 xvar,5 plvar,4 finish /exit,nosave
Presented below is the POST26 output resulting from this analysis. -----------------------------------------------------------------------***** ANSYS POST26 VARIABLE LISTING ***** TIME 0.50000E-01 0.10000 0.15000 0.20000 0.25000 0.30000 0.35000 0.40000 0.45000 0.50000 0.55000 0.60000 0.65000 0.70000 0.75000 0.80000 0.85000 0.90000 0.95000 1.0000 1.0500 1.1000 1.1500 1.2000 1.2500 1.3000 1.3500 1.4000 1.4500 1.5000 1.5500 1.6000 1.6500 1.7000 1.7500 1.8000 1.8500 1.9000 1.9500 2.0000
3 S X press -139488. -278977. -418465. -557953. -697442. -836930. -976418. -0.111591E+07 -0.125539E+07 -0.139488E+07 -0.153437E+07 -0.278389E+07 -0.557968E+07 -0.989280E+07 -0.152775E+08 -0.208613E+08 -0.250737E+08 -0.277640E+08 -0.310936E+08 -0.357955E+08 -0.227277E+08 -0.965988E+07 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04 -0.100000E-04
3 EPELX delta -0.398672E-04 -0.797343E-04 -0.119601E-03 -0.159469E-03 -0.199336E-03 -0.239203E-03 -0.279070E-03 -0.318937E-03 -0.358804E-03 -0.398672E-03 -0.438539E-03 -0.477349E-03 -0.514686E-03 -0.550578E-03 -0.585450E-03 -0.620132E-03 -0.656120E-03 -0.693558E-03 -0.730387E-03 -0.765909E-03 -0.738405E-03 -0.710900E-03 -0.680150E-03 -0.640200E-03 -0.600250E-03 -0.560300E-03 -0.520350E-03 -0.480400E-03 -0.440450E-03 -0.400500E-03 -0.360550E-03 -0.320600E-03 -0.280650E-03 -0.240700E-03 -0.200750E-03 -0.160800E-03 -0.120850E-03 -0.809000E-04 -0.409500E-04 -0.100000E-05
4 ADD press 139488. 278977. 418465. 557953. 697442. 836930. 976418. 0.111591E+07 0.125539E+07 0.139488E+07 0.153437E+07 0.278389E+07 0.557968E+07 0.989280E+07 0.152775E+08 0.208613E+08 0.250737E+08 0.277640E+08 0.310936E+08 0.357955E+08 0.227277E+08 0.965988E+07 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04 0.100000E-04
5 ADD delta 0.398672E-04 0.797343E-04 0.119601E-03 0.159469E-03 0.199336E-03 0.239203E-03 0.279070E-03 0.318937E-03 0.358804E-03 0.398672E-03 0.438539E-03 0.477349E-03 0.514686E-03 0.550578E-03 0.585450E-03 0.620132E-03 0.656120E-03 0.693558E-03 0.730387E-03 0.765909E-03 0.738405E-03 0.710900E-03 0.680150E-03 0.640200E-03 0.600250E-03 0.560300E-03 0.520350E-03 0.480400E-03 0.440450E-03 0.400500E-03 0.360550E-03 0.320600E-03 0.280650E-03 0.240700E-03 0.200750E-03 0.160800E-03 0.120850E-03 0.809000E-04 0.409500E-04 0.100000E-05
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
10–23
10–24
Chapter 11: Contact This chapter covers the following topics: 11.1. Contact Overview 11.2. General Contact Classification 11.3. ANSYS Contact Capabilities 11.4. Performing a Surface-to-Surface Contact Analysis 11.5. GUI Aids for Contact Analyses 11.6. Performing a Node-to-Surface Contact Analysis 11.7. Using the Internal MPC Approach for Assemblies and Kinematic Constraints 11.8. Performing a Node-to-Node Contact Analysis
11.1. Contact Overview Contact problems are highly nonlinear and require significant computer resources to solve. It is important that you understand the physics of the problem and take the time to set up your model to run as efficiently as possible. Contact problems present two significant difficulties. First, you generally do not know the regions of contact until you've run the problem. Depending on the loads, material, boundary conditions, and other factors, surfaces can come into and go out of contact with each other in a largely unpredictable and abrupt manner. Second, most contact problems need to account for friction. There are several friction laws and models to choose from, and all are nonlinear. Frictional response can be chaotic, making solution convergence difficult. In addition to these two difficulties, many contact problems must also address multi-field effects, such as the conductance of heat, electrical currents, and magnetic flux in the areas of contact. If you do not need to account for friction in your model, and the interaction between the bodies is always bonded, you may be able to use the internal multipoint constraint (MPC) feature (available for certain contact elements) to model various types of contact assemblies and surface-based constraints (see Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints for more information). Another alternative is to use constraint equations or coupled degrees of freedom instead of contact to model these situations (see Chapter 12, “Coupling and Constraint Equations” in the ANSYS Modeling and Meshing Guide for more information). Constraint equations are only available for small strain applications (NLGEOM,off).
11.1.1. Explicit Dynamics Contact Capabilities In addition to the implicit contact capabilities discussed in this chapter, ANSYS also offers explicit contact capabilities with the ANSYS LS-DYNA explicit dynamics product. Explicit capabilities are ideally suited for short-duration contact-impact problems. For more information on the ANSYS LS-DYNA product and its contact capabilities, see the ANSYS LS-DYNA User's Guide.
11.2. General Contact Classification Contact problems fall into two general classes: rigid-to-flexible and flexible-to-flexible. In rigid-to-flexible contact problems, one or more of the contacting surfaces are treated as rigid (i.e., it has a much higher stiffness relative to the deformable body it contacts). In general, any time a soft material comes in contact with a hard material, the problem may be assumed to be rigid-to-flexible. Many metal forming problems fall into this category. The other class, flexible-to-flexible, is the more common type. In this case, both (or all) contacting bodies are deformable (i.e., have similar stiffnesses). An example of a flexible-to-flexible contact is bolted flanges.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 11: Contact
11.3. ANSYS Contact Capabilities ANSYS supports three contact models: node-to-node, node-to-surface, and surface-to-surface. Each type of model uses a different set of ANSYS contact elements and is appropriate for specific types of problems as shown in Table 11.1: “ANSYS Contact Capabilities”.
Table 11.1 ANSYS Contact Capabilities
Point-to-Point
Node-to-Node
Node-to- Surface-to-Surface Surface
CONTAC CONTAC CONTA 12 52 178
CONTA CONTA CONTA 175, 171,172 173,174 TARGET TARGET TARGET 169, 170 169 170
Y
Y
Y
Point-to-Surface
Y
Surface-to-Surface
Y
Y
Y
Y
Y
Y
Y
Y
small
small
large
large
large
2-D
Y
3-D Sliding Cylindrical Gap
small Y
Y Y
Y
Pure Lagrange Multiplier
Y
Y
Y
Y
Augmented Lagrange Multiplier
Y
Y
Y
Y
Lagrange Multiplier on Normal and Penalty on Tangent
Y
Y
Y
Y
Y
Y
Y
Internal Multipoint Constraint (MPC) Contact Stiffness
Auto-meshing Tools Lower-Order
userdefined
usersemisemisemisemidefined automat- automat- automat- automatic ic ic ic
EINTF
EINTF
EINTF
ESURF
ESURF
ESURF
Y
Y
Y
Y
Y
Y
Y (2-D only)
Y
Y
Higher- Order Rigid-Flexible
Y
Y
Y
Y
Y
Y
Flexible- Flexible
Y
Y
Y
Y
Y
Y
Thermal Contact
Y
Y
Y
Electric Contact
Y
Y
Y
Magnetic Contact
Y
Y
Y
To model a contact problem, you first must identify the parts to be analyzed for their possible interaction. If one of the interactions is at a point, the corresponding component of your model is a node. If one of the interactions is at a surface, the corresponding component of your model is an element: either a beam, shell, or solid element. 11–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.3: ANSYS Contact Capabilities The finite element model recognizes possible contact pairs by the presence of specific contact elements. These contact elements are overlaid on the parts of the model that are being analyzed for interaction. The different contact elements that ANSYS uses, and procedures for using them, are described in the remainder of this chapter. An overview of the ANSYS contact elements and their capabilities follows. For detailed information on any of these elements, refer to the ANSYS Elements Reference and the ANSYS, Inc. Theory Reference.
11.3.1. Surface-to-Surface Contact Elements ANSYS supports both rigid-to-flexible and flexible-to-flexible surface-to-surface contact elements. These contact elements use a "target surface" and a "contact surface" to form a contact pair. •
The target surface is modeled with either TARGE169 or TARGE170 (for 2-D and 3-D, respectively).
•
The contact surface is modeled with elements CONTA171, CONTA172, CONTA173, and CONTA174.
To create a contact pair, assign the same real constant number to both the target and contact elements. You can find more details on defining these elements and their shared real constant sets in Section 11.4: Performing a Surface-to-Surface Contact Analysis. These surface-to-surface elements are well-suited for applications such as interference fit assembly contact or entry contact, forging, and deep-drawing problems. The surface-to-surface contact elements have several advantages over the node-to-node element CONTA175. These elements: •
Support lower and higher order elements on the contact and target surfaces (in other words, cornernoded or midside-noded elements).
•
Provide better contact results needed for typical engineering purposes, such as normal pressure and friction stress contour plots.
•
Have no restrictions on the shape of the target surface. Surface discontinuities can be physical or due to mesh discretization.
Using these elements for a rigid target surface, you can model straight and curved surfaces in 2-D and 3-D, often using simple geometric shapes such as circles, parabolas, spheres, cones, and cylinders. More complex rigid forms or general deformable forms can be modeled using special preprocessing techniques (see Step 3 of Section 11.4: Performing a Surface-to-Surface Contact Analysis for more information). Surface-to-surface contact elements are not well-suited for point-to-point, point-to-surface, or edge-to-surface contact applications, such as pipe whip or snap-fit assemblies. You should use the node-to-surface or node-tonode elements in these cases. You also can use surface-to-surface contact elements for most contact regions and use a few node-to-surface contact elements near contact corners. The surface-to-surface contact elements only support general static and transient analyses, buckling, harmonic, modal or spectrum analyses, or substructure analyses.
11.3.2. Node-to-Surface Contact Elements CONTA175 is a node-to-surface contact element. It supports large sliding, large deformation, and different meshes between the contacting components. CONTA175 is typically used to model point-to-surface contact applications, such as two beams contacting each other (at a beam tip or sharp corner node), and the corners of snap-fit parts.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–3
Chapter 11: Contact You can also use CONTA175 to model surface-to-surface contact, if the contacting surface is defined by a group of nodes and multiple elements are generated. The surfaces can be either rigid or deformable. An example of this type of contact problem is a wire inserted into a slot. Unlike the node-to-node contact elements, you do not need to know the exact location of the contacting area beforehand, nor do the contacting components need to have a compatible mesh. Large deformation and large relative sliding are allowed, although this capability can also model small sliding. CONTA175 does not support 3-D higher-order elements on the contact surface side. The element can fail if the target surface is severely discontinous. No contour plots are available for contact results.
11.3.3. Node-to-Node Contact Elements Node-to-node contact elements are typically used to model point-to-point contact applications. To use nodeto-node contact elements, you need to know the location of contact beforehand. These types of contact problems usually involve small relative sliding between contacting surfaces (even in the case of geometric nonlinearities). An example of a node-to-node contact application is the traditional pipe whip model, where the contact point is always located between the pipe tip and the restraint. Node-to-node contact elements can also be used to solve a surface-to-surface problem if the nodes of the two surfaces line up, the relative sliding deformation is negligible, and deflections (rotations) of the two surfaces remain small. These are typically problems with faceted and simple geometry. An interference fit problem is an example of a surface-to-surface problem where the use of node-to-node contact may be sufficient. Another use of node-to-node contact elements is in extremely precise analysis of surface stresses, such as in turbine blade analysis. ANSYS element CONTA178 is the best choice for most node-to-node problems. It offers a wider range of options and solver types than the other elements. CONTAC12 and CONTAC52 are available largely for reasons of backward compatibility with existing models.
11.4. Performing a Surface-to-Surface Contact Analysis You can use the surface-to-surface contact elements to model either rigid-flexible or flexible-flexible contact between surfaces. The Contact Manager provides an easy-to-use interface to help you construct and manage contact definitions. You can access the manager via the Contact Manager icon in the ANSYS Standard Toolbar, or via the menu path Main Menu> Preprocessor> Modeling> Create> Contact Pair. See Section 11.5: GUI Aids for Contact Analyses for more information on using the Contact Manager. The following sections explain how to set up a contact analysis using the both command and GUI approaches. Note — The following sections also apply to node-to-surface contact analyses using CONTA175, unless otherwise noted.
11.4.1. Using Surface-to-Surface Contact Elements In problems involving contact between two boundaries, one of the boundaries is conventionally established as the "target" surface, and the other as the "contact" surface. For rigid-flexible contact, the target surface is always the rigid surface, and the contact surface is the deformable surface. For flexible-to-flexible contact, both contact and target surfaces are associated with the deformable bodies. These two surfaces together comprise the "contact pair." Use TARGE169 with CONTA171, CONTA172, or CONTA175 to define a 2-D contact pair. For 3-D contact
11–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis pairs, use TARGE170 with CONTA173, CONTA174, or CONTA175. Each contact pair is identified via the same real constant number. Note — If you prefer a graphical approach to setting up your contact analysis, you can use the Contact Toolbar, as discussed in Section 11.5.1: The Contact Manager.
11.4.2. Steps in a Contact Analysis The basic steps for performing a typical surface-to-surface contact analysis are listed below. Each step is then explained in detail in the following pages. 1.
Create the model geometry and mesh
2.
Identify the contact pairs
3.
Designate contact and target surfaces
4.
Define the target surface
5.
Define the contact surface
6.
Set the element KEYOPTS and real constants
7.
Define/control the motion of the target surface (rigid-to-flexible only)
8.
Apply necessary boundary conditions
9.
Define solution options and load steps
10. Solve the contact problem 11. Review the results Each contact-specific step also has a corresponding GUI approach where you use functions and features on the Contact Toolbar.
11.4.3. Creating the Model Geometry and Mesh First, create solid model entities that represent the geometry of the contacting bodies. Set element types, real constants, and material properties as you would for any ANSYS analysis. Mesh the contacting bodies by meshing the areas or volumes with the element type that you have chosen. For more information, see the ANSYS Modeling and Meshing Guide. Command(s): AMESH, VMESH GUI: Main Menu> Preprocessor> Meshing> Mesh Note — You should avoid midside-noded elemets for 3-D contact surfaces when using node-to-surface element CONTA175.
11.4.4. Identifying Contact Pairs You must identify where contact might occur during the deformation of your model. Once you've identified potential contact surfaces, you define them via target and contact elements, which will then track the kinematics of the deformation process. Target and contact elements that make up a contact pair are associated with each other via a shared real constant set. The contact zone can be arbitrary; however, for the most efficient solution (primarily in CPU time), you may want to define smaller, localized contacting zones, but be sure your zones are adequate to capture all necessary contact. Different contact pairs must be defined by a different real constant set, even if the element real constant values do not change. There is no limit on the number of surfaces allowed. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–5
Chapter 11: Contact
Figure 11.1 Localized Contact Zones
Depending on the geometry of the model (and the potential deformation), multiple target surfaces could interact with the same zone of the contact surface. In such cases, you must define multiple contact pairs (using multiple overlapping contact elements), each with its own real constant number. See Figure 11.1: “Localized Contact Zones”.
11.4.5. Designating Contact and Target Surfaces Contact elements are constrained against penetrating the target surface. However, target elements can penetrate through the contact surface. For rigid-to-flexible contact, the designation is obvious: the target surface is always the rigid surface and the contact surface is always the deformable surface. For flexible-to-flexible contact, the choice of which surface is designated contact or target can cause a different amount of penetration and thus affect the solution accuracy. Consider the following guidelines when designating the surfaces: •
If a convex surface is expected to come into contact with a flat or concave surface, the flat/concave surface should be the target surface.
•
If one surface has a fine surface mesh and, in comparison, the other has a coarse mesh, the fine mesh should be the contact surface and the coarse mesh should be the target surface.
•
If one surface is stiffer then the other, the softer surface should be the contact surface and the stiffer surface should be the target surface.
11–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis •
If higher-order elements underly one of the external surfaces and lower-order elements underly the other surface, the surface with the underlying higher-order elements should be the contact surface and the other surface should be the target. However, for 3-D node-to-surface contact, the lower-order elements should be the contact surface. The higher-order elements should be the target surface.
•
If one surface is markedly larger than the other surface, such as in the instance where one surface surrounds the other surface, the larger surface should be the target surface.
These guidelines are true for asymmetric contact; however, asymmetric contact may not perform satisfactorily for your model. The following section details the difference between asymmetric and symmetric contact and outlines some of the situations that require symmetric contact.
11.4.5.1. Asymmetric Contact vs. Symmetric Contact 11.4.5.1.1. Background Asymmetric contact is defined as having all contact elements on one surface and all target elements on the other surface. This is sometimes called "one-pass contact." This is usually the most efficient way to model surfaceto-surface contact. However, under some circumstances asymmetric contact does not perform satisfactorily. In such cases, you can designate each surface to be both a target and a contact surface. You can then generate two sets of contact pairs between the contacting surfaces (or just one contact pair; for example, a self-contact case). This is known as symmetric contact (or "two-pass contact"). Obviously, symmetric contact is less efficient than asymmetric contact. However, many analyses will require its use (typically to reduce penetration). Specific situations that require symmetric contact include models where •
The distinction between the contact and target surfaces is not clear.
•
Both surfaces have very coarse meshes. The symmetric contact algorithm enforces the contact constraint conditions at more surface locations than the asymmetric contact algorithm.
If the meshes on both surfaces are identical and sufficiently refined, the symmetric contact algorithm may not significantly improve performance and may, in fact, be more "expensive" in CPU time. In such circumstances, pick one surface to be the target and the other the contact surface. For a symmetric contact definition, ANSYS may find one side of a contact surface as closed and the other side of the surface as closed. In this case, it can be difficult to interpret the results. The total contact pressure acting on both sides is the average of the contact pressures on each side of the surface.
11.4.5.1.2. Using KEYOPT(8) When there are several contact pairs involved in the model, and the graphical picking of contact and target surfaces is difficult, you can just define the symmetric contact pairs and, by setting KEYOPT(8) = 2, ANSYS will internally select which asymmetric pair is to be used at the solution stage based on the guidelines mentioned above in Designating Contact and Target Surfaces. Note — In any contact model, you can mix different types of contact pairs: rigid-to-flexible or flexible-toflexible contact; symmetric contact or asymmetric contact. However, only one type can exist with a contact pair.
11.4.6. Defining the Target Surface The target surface can be 2-D or 3-D and either rigid or deformable. For deformable target surfaces, you will normally use the ESURF command to generate the target elements along the boundaries of an existing mesh. You can follow the same method to generate the deformable contact surface (see Section 11.4.7: Defining the
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–7
Chapter 11: Contact Deformable Contact Surface for details). You should not use the following rigid target segments for a deformable target surface: ARC, CARC, CIRC, CYL1, CONE, SPHE, or PILO. For rigid target surfaces, the following provides general guidelines. In 2-D cases, the shape of the target surface is described by a sequence of straight lines, circular arcs, and parabolas, all of which can be represented with the target segment element TARGE169. You can use any combination to define the complex target surface geometry. In 3-D cases, the shape of the target surfaces is described by a sequence of triangles, quadrilaterals, cylinders, cones, and spheres, which can be represented with TARGE170. You can use any combination of low/high-order triangles and quadrilaterals to model a target surface with a complex, arbitrary geometry.
11.4.6.1. Pilot Nodes The rigid target surface can also be associated with a "pilot node," which is really an element with one node, whose motion governs the motion of the entire target surface. You can think of a pilot node as a handle for the rigid target surface. Forces/moments or rotations/displacements for the entire target surface can be prescribed on just the pilot node. The pilot node can be one of the nodes on the target element or a node at any arbitrary location. The location of the pilot node is important only when rotation or moment loading is required. If you define a pilot node, ANSYS checks for boundary conditions only on the pilot node and ignores any constraints on other nodes.
11.4.6.2. Primitives You can use circle, cylinder, cone, and sphere primitives to model the target (which require real constants to define the radius). You can combine primitive segments with general segments (such as lines, parabolas, triangles, and quadrilaterals) to define a target surface. Primitives cannot be defined directly in the Contact Wizard.
11.4.6.3. Element Types and Real Constants Before generating the target element, first define the element type (TARGE169 for 2-D or TARGE170 for 3-D): Command(s): ET GUI: Main Menu> Preprocessor> Element Type> Add/Edit/Delete
11.4.6.3.1. Defining Target Element Geometry You define characteristics of the target element geometry through real constants R1 and R2 as follows: •
•
For CONTA171 and CONTA172: –
R1 is the radius if the target shape (TARGE169) is a circle.
–
R2 is the element thickness if the underlying element is a superelement set as plane stress with thickness (KEYOPT(3) = 3). The default value is 1.
For CONTA173 and CONTA174 (also applies to node-to-surface element CONTA175): –
R1 is the radius if the target shape (TARGE170) is a cylinder, cone, or sphere.
–
R2 is the radius of a cone at the second node.
To set the real constant number for the target elements: Command(s): REAL GUI: Main Menu> Preprocessor> Real Constants
11–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis For TARGE169 and TARGE170, you need only set real constants R1 and R2 (if required). For a complete description of the target elements, element shapes, and real constants, see the description of TARGE169 and TARGE170 in the ANSYS Elements Reference. Note — Specifying real constants (R1, R2) manually is necessary only if you use direct generation to create your target elements. You can also use the ANSYS meshing tools to create the elements, or use the Contact Toolbar.
11.4.6.4. Using Direct Generation to Create Rigid Target Elements To generate target elements directly, use the following command or GUI path: Command(s): TSHAP GUI: Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes You then specify the element shape. Possible shapes are: •
Straight line (2-D)
•
Parabola (2-D)
•
Clockwise arc (2-D)
•
Counterclockwise arc (2-D)
•
Circle (2-D)
•
Three-node triangle (3-D)
•
Six-node triangle (3-D)
•
Four-node quadrilateral (3-D)
•
Eight-node quadrilateral (3-D)
•
Cylinder (3-D)
•
Cone (3-D)
•
Sphere (3-D)
•
Pilot node (both 2-D and 3-D)
Once you specify a target element shape, all subsequent elements will have that shape until you specify another shape. Note — You cannot mix 2-D and 3-D target elements on the same target surface. You cannot mix rigid target elements with deformable target elements on the same target surface. During solution, ANSYS assigns a deformable status to target elements with underlying elements and assigns a rigid status to target elements without underlying elements. If a portion of the underlying elements of a deformable surface are deleted, an error will occur in solution. You can generate the nodes and elements using standard ANSYS direct generation techniques. For more information on direct generation modeling techniques, see Chapter 9, “Direct Generation” in the ANSYS Modeling and Meshing Guide. Command(s): N, E GUI: Main Menu> Preprocessor> Modeling> Create> Nodes Main Menu> Preprocessor> Modeling> Create> Elements You can then verify your element shapes by listing the elements. Command(s): ELIST Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–9
Chapter 11: Contact GUI: Utility Menu> List> Elements> Nodes + Attributes
11.4.6.5. Using ANSYS Meshing Tools to Create Rigid Target Elements You can also let ANSYS generate the elements automatically using the standard ANSYS meshing capabilities. ANSYS will recognize the proper target element shape based on the solid model and will ignore the TSHAP setting. To generate a pilot node, use the following command or GUI path: Command(s): KMESH GUI: Main Menu> Preprocessor> Meshing> Mesh> Keypoints Note — KMESH always creates pilot nodes. To generate 2-D rigid target elements, use the following command or GUI path. ANSYS creates a single line over each line, parabolic segments over B-splines, and arc segments over each arc and line fillet (see Figure 11.2: “ANSYS Geometric Entities and Their Corresponding Rigid Target Elements”). If all the arcs form a closed circle, ANSYS creates a single circular segment (see Figure 11.3: “A Single Circular Target Segment Created From Arc Line Segments”). However, if the arcs that form a closed circle are created from imported or archived geometry (such as IGES), ANSYS might not create a single circular segment. Command(s): LMESH GUI: Main Menu> Preprocessor> Meshing> Mesh> Lines
Figure 11.2 ANSYS Geometric Entities and Their Corresponding Rigid Target Elements
11–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
Figure 11.3 A Single Circular Target Segment Created From Arc Line Segments
To generate 3-D rigid target elements, use the following command or GUI path. Command(s): AMESH GUI: Main Menu> Preprocessor> Meshing> Mesh> Areas If the surface segments on the solid model form a complete sphere, cylinder, or cone, then ANSYS automatically generates a single primitive 3-D target element through the AMESH command. By creating fewer elements, the analysis becomes more computationally efficient. For arbitrary surfaces, you should use AMESH to generate target elements. In these cases, the quality of the meshed target shape is not important. It is more important that the target elements represent the rigid surface geometry well. We recommend using mapped meshing on all possible areas. If there is no curvature on the edges of the surface, assign one division on that edge. TARGE169 with a rigid specification will always mesh with one element division, per line, ignoring any LESIZE setting. The default target element shape is quadrilateral. If you want a triangular target element shape, use MSHAPE,1. Figure 11.4: “Meshing Patterns for Arbitrary Target Surfaces” shows the meshing patterns for arbitrary target surfaces. The following command or GUI path will generate a mapped mesh wherever possible (otherwise, if not possible, it will generate a free mesh). Command(s): MSHKEY,2 GUI: Main Menu> Preprocessor> Meshing> Mesh> Areas> Target Surf If the target surface is flat (or nearly flat), you may select low-order target elements (3-node triangular or 4-node quadrilateral elements). If the target surface is curved you should select high-order target elements (6-node triangular or 8-node quadrilateral). By doing so, set KEYOPT(1) = 1 in the target element definition. Note — Low-order target elements result in "cheaper" CPU usage in getting penetration and gap; however, the meshed surface may not be smooth. Higher-order target elements are more "expensive" to use in getting the penetration and gap, but they need many fewer elements to discretize the whole curved target surface. Note — If target elements are created via program meshing (through the KMESH, LMESH, or ESURF commands) the TSHAP command is ignored and ANSYS chooses the correct shape codes automatically.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–11
Chapter 11: Contact
Figure 11.4 Meshing Patterns for Arbitrary Target Surfaces
11.4.6.5.1. Some Modeling and Meshing Tips A target surface can be made up of two or more disconnected regions. Where possible, you should localize the contact zone by defining multiple target surfaces (each with a different real constant number). There are no restrictions on the shape of the rigid surfaces. Smoothing is not required. However, you must ensure that the mesh discretization of the curved surfaces on the rigid target surface is adequate. Excessively coarse discretization can cause numerical convergence problems. It can be difficult to obtain a converged solution in a large sliding simulation if the target surface has sharp convex corners. To avoid such modeling problems, use line or area fillet functions on the solid model to smooth out the sharp corner, use a more refined mesh, or use high-order element in the region of abrupt curvature changes (see Figure 11.5: “Smoothing Convex Corner”).
11–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
Figure 11.5 Smoothing Convex Corner
11.4.6.5.2. Verifying Nodal Number Ordering (Contact Direction) of Target Surface The node order of the target surface elements is critical because it defines contact direction. For 2-D contact, the associated (deformable) contact elements must lie to the right of the target surface when moving from the first node to the second node along the target surface line (see Figure 11.6: “Correct Node Ordering”).
Figure 11.6 Correct Node Ordering
For 3-D contact, the target triangular element numbering should be such that the rigid surface's outward normal points toward the contact surface. The outward normal is determined by the right-hand rule. To check the direction of the normals, turn on the element coordinate systems. Command(s): /PSYMB,ESYS,1 Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–13
Chapter 11: Contact GUI: Utility Menu> PlotCtrls> Symbols If the element normals do not point toward the contact surface, select this element and reverse the direction of the surface normals. Command(s): ESURF,,REVE GUI: Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surf to Surf or, reorient the element normals: Command(s): ENORM GUI: Main Menu> Preprocessor> Modeling> Move/Modify> Elements> Shell Normals Note — Contact on target primitives (such as a complete circle, cylinder, cone, or sphere), can occur only on the outside surfaces of such target bodies.
11.4.7. Defining the Deformable Contact Surface To create the deformable contact surface, you must define that surface using contact elements CONTA171 or CONTA172 (for 2-D), or CONTA173 or CONTA174 (for 3-D), or CONTA175 for (2- or 3-D). The contact surface is defined by the set of contact elements that comprise the surface of the deformable body. These contact elements have the same geometric characteristics as the underlying elements of the deformable body. The contact surface elements are of the same order as the underlying elements (lower- or higher-order), with compatible nodes along the edges. The higher-order contact elements can match lower-order underlying elements by dropping the midside nodes. The underlying elements can be solid, shell, or 2-D beam elements. The contact surface can be on either side of the shell or beam elements. The underlying elements may also be a superelement. However, axisymmetric harmonic elements may not be used as underlying elements. As with the target surface elements, you must define the contact surface element type, then select the correct real constant number (the real constant number must be the same as the one used for the target surface for each contact pair), and finally generate the elements.
11.4.7.1. Element Type The four contact element types are listed below, along with a brief description. For complete information on these element types, see the ANSYS Elements Reference.
11–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
Figure 11.7 Contact Element Types
•
CONTA171: This element is a 2-D, 2-node, lower-order line element that can be located on the surfaces of 2-D solid, shell, or beam elements (such as BEAM3, PLANE42, or SHELL51).
•
CONTA172: This element is a 2-D, 3-node, higher-order parabolic element that can be located on the surfaces of 2-D solid or beam elements with midside nodes (such as PLANE82 or VISCO88).
•
CONTA173: This element is a 3-D, 4-node, lower-order quadrilateral element that can be located on the surfaces of 3-D solid or shell elements (such as SOLID45 or SHELL181). It can be degenerated to a 3-node triangular element.
•
CONTA174: This element is a 3-D, 8-node, higher-order quadrilateral element that can be located on the surfaces of 3-D solid or shell elements with midside nodes (such as SOLID92, SOLID95, or SHELL93). It can be degenerated to 3 - 7 node quadrilateral/triangular shapes.
•
CONTA175: This element is a 2- or 3-D 1-node element that can be located on the surface of 2-D low order and higher order solid or beam elements or 3-D low order solid or shell elements. Command(s): ET GUI: Main Menu> Preprocessor> Element Type> Add/Edit/Delete Note — Use CONTA175 for node-to-surface contact.
11.4.7.2. Real Constants and Material Properties After defining the element type, you need to select the correct real constant set. The real constant set for each contact surface must be the same one used for the corresponding target surface for each contact pair. Each contact pair must reference its own real constant number. ANSYS uses the material properties of the underlying elements to calculate an appropriate contact (or penalty) stiffness. In cases where the underlying element has TB plasticity material properties defined (whether active or not), the contact normal stiffness will be reduced by a factor of 100. ANSYS automatically defines a default value for tangent (sliding) contact stiffness that is proportional to MU and the normal stiffness. If the underlying element is a superelement, the material property set for the contact elements must be the same as that of the original structural elements used during the formation of the superelement. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–15
Chapter 11: Contact
11.4.7.3. Generating Contact Elements You can generate contact elements either through direct generation or by generating the surface automatically from the exterior faces of the underlying elements. We recommend that you use automatic generation; this approach is simpler and more reliable. To automatically generate contact elements, follow these steps: 1.
Select the nodes on the meshed deformable body. For each surface, view the node list. If you are certain that particular nodes will never come into contact, you can omit those nodes and reduce CPU time. However, you should always include more nodes than you think you'll need so that you don't miss unexpected areas of contact. Command(s): NSEL GUI: Utility Menu> Select> Entities
2.
Generate the contact elements. Command(s): ESURF GUI: Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surf to Surf If the contact surface is attached to areas or volumes that are meshed with solid elements, ANSYS automatically determines the outward normal needed for contact calculations. If the underlying elements are beam or shell elements, you must indicate which surface (top or bottom) is the target surface. Command(s): ESURF,,TOP or BOTTOM GUI: Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surf to Surf Use the TOP setting (default) to generate contact elements with their outward normals the same as the beam or shell elements' normals. Use the BOTTOM setting to generate contact elements with their outward normals opposite the beam or shell elements' normals. You must make sure that all elements in the beam or shell element selection have their normals consistently oriented. If the underlying elements are solid elements, then the TOP or BOTTOM setting has no effect.
3.
11–16
Check the direction of the outward normals for the contact elements. The direction of the contact surface's outward normal is critical for proper contact detection. For 3-D elements, the node numbering follows the right hand rule to define its outward normal. The contact surface's outward normal should point toward the target surface. Otherwise, ANSYS may detect over-penetration of the surfaces at the beginning of the analysis and have difficulty finding an initial solution. In most of these cases, the analysis will fail immediately. Figure 11.8: “Specification of the Contact Surface's Outward Normal” illustrates both proper and improper specification of the contact surface's outward normal. Command(s): /PSYMB,ESYS GUI: Utility Menu> PlotCtrls> Symbols
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
Figure 11.8 Specification of the Contact Surface's Outward Normal
If the surface normals are specified incorrectly, you must either change them by reversing the node number order of the selected elements. Command(s): ESURF,,REVE GUI: Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surf to Surf or, reorient the element normals. Command(s): ENORM GUI: Main Menu> Preprocessor> Modeling> Move/Modify> Elements> Shell Normals Note — ESURF,,TOP or BOTTOM and checking the direction of outward normals will not apply to nodeto-surface contact (CONTA175) because it is a single-node element with no surface normal associated with it.
11.4.8. Set the Real Constants and Element KEYOPTS ANSYS uses several real constants and KEYOPTs to control contact behavior using these surface-to-surface contact elements. For more information in addition to what is presented here, refer to the individual contact element descriptions in the ANSYS Elements Reference.
11.4.8.1. Real Constants Two real constants, R1 and R2, are used to define the geometry of the target surface elements. The remaining are used by the contact surface elements. •
R1 and R2 define the target element geometry.
•
FKN defines a normal contact stiffness factor.
•
FTOLN is a factor based on the thickness of the element which is used to calculate allowable penetration.
•
ICONT defines an initial closure factor (or adjustment band).
•
PINB defines a "pinball" region.
•
PMIN and PMAX define an allowable penetration range for initial penetration.
•
TAUMAX specifies the maximum contact friction.
•
CNOF specifies the positive or negative offset value applied to the contact surface.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–17
Chapter 11: Contact •
FKOP specifies the stiffness factor applied when contact opens.
•
FKT specifies the tangent contact stiffness.
•
COHE specifies the cohesion sliding resistance.
•
TCC specifies the thermal contact conductance coefficient.
•
FHTG specifies the fraction of frictional dissipated energy converted into heat.
•
SBCT specifies the Stefan-Boltzmann constant.
•
RDVF specifies the radiation view factor.
•
FWGT specifies the weight factor for the distribution of heat between the contact and target surfaces for thermal contact or for electric contact.
•
ECC specifies the electric contact conductance or capacitance per unit area.
•
FHEG specifies the fraction of electric dissipated energy converted into heat.
•
FACT specifies the ratio of static to dynamic coefficients of friction.
•
DC specifies the decay coefficient for static/dynamic friction.
•
SLTO controls maximum sliding distance when MU is nonzero and the tangent contact stiffness (FKT) is updated at each iteration (KEYOPT(10) = 2).
•
TNOP specifies the maximum allowable tensile contact pressure.
•
TOLS adds a small tolerance that extends the edge of the target surface.
•
MCC specifies the magnetic contact permeance (3-D only).
Real constant defaults can vary depending on the environment you are working in. The following table compares the default values between ANSYS and the ANSYS Workbench. See your ANSYS sales representative for more information about ANSYS Workbench.
Table 11.2 Summary of Real Constant Defaults in Different Environments Real Constants
Description
ANSYS Default ANSYS Workbench Default
No.
Name
1
R1
Target circle radius
0
n/a
2
R2
Superelement thickness
1
n/a
3
FKN
Normal penalty stiffness factor
1
[1]
4
FTOLN
Penetration tolerance factor
0.1
0.1
5
ICONT
Initial contact closure
0
0
6
PINB
Pinball region
[2]
[2]
7
PMAX
Upper limit of initial penetration
0
0
8
PMIN
Lower limit of initial penetration
0
0
9
TAUMAX
Maximum friction stress
1.00E+20
1.00E+20
10
CNOF
Contact surface offset
0
0
11
FKOP
Contact opening stiffness
1
1
12
FKT
Tangent penalty stiffness
1
1
13
COHE
Contact cohesion
0
0
14
TCC
Thermal contact conductance
0
[3]
11–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis Real Constants
Description
ANSYS Default ANSYS Workbench Default
No.
Name
15
FHTG
Frictional heating factor
1
1
16
SBCT
Stefan-Boltzmann constant
0
n/a
17
RDVF
Radiation view factor
1
n/a
18
FWGT
Heat distribution weighing factor
0.5
0.5
19
ECC
Electric contact conductance
0
n/a
20
FHEG
Joule dissipation weighting factor
1
n/a
21
FACT
Static/dynamic ratio
1
1
22
DC
Exponential decay coefficient
0
0
23
SLTO
Allowable elastic slip
1%
1%
24
(blank)
25
TOLS
Target edge extension factor
[4]
[4]
26
MCC
Magnetic contact permeance
0
n/a
1.
FKN = 10 for bonded. For all other, FKN = 1.0, but if bonded and other contact behavior exists, FKN = 1 for all.
2.
Depends on contact behavior (rigid vs. flex target), NLGEOM,ON or OFF, KEYOPT(9) setting, KEYOPT(12) setting, and the value of CNOF (see Section 11.4.8.9.2: Using PINB).
3.
Calculated as a function of highest conductivity and overall model size.
4.
10% of target length for NLGEOM,OFF. 2% of target length for NLGEOM,ON. Command(s): R GUI: Main Menu> Preprocessor> Real Constants
11.4.8.1.1. Positive and Negative Real Constant Values For the real constants FKN, FTOLN, ICONT, PINB, PMAX, PMIN, FKOP, FKT, SLTO, and TNOP, you can specify either a positive or negative value. ANSYS interprets a positive value as a scaling factor and interprets a negative value as the absolute value. ANSYS uses the depth of the underlying element as the reference value to be used for ICONT, FTOLN, PINB, PMAX, and PMIN. For example, a positive value of 0.1 for ICONT indicates an initial closure factor of 0.1 x depth of the underlying element. However, a negative value of 0.1 indicates an actual adjustment band of 0.1 units. When KEYOPT(10) = 0, 1, or 2, all the contact related settings (ICONT, FTOLN, PINB, PMAX, PMIN, FKN, FKT, SLTO) are averaged across all contact elements in a contact pair. However, when KEYOPT(10) = 3, 4, or 5, the settings are based on each individual contact element (geometry and material behaviors). Figure 11.9: “Depth of the Underlying Element” shows the depth of the underlying element for a solid element. If the underlying elements are shell or beam elements, the depth will usually be 4 times the element thickness.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–19
Chapter 11: Contact
Figure 11.9 Depth of the Underlying Element
When KEYOPT(10) = 0, 1, or 2, each contact pair has a pair-based depth which is obtained by averaging the depth of each contact element across all the contact elements in a contact pair. This can avoid the problem of very different element-based depths when there are meshes with large variations in element sizes. Note — When the contact pair depth is too small (for example, 10-5), the machine precision may not guarantee the accuracy of penetration to be calculated. You should scale the length unit in the model.
11.4.8.2. Element KEYOPTS Each contact element includes several KEYOPTS. We recommend using the default settings, which are suitable for most contact problems. For some specific applications, you can override the defaults. The element KEYOPTS allow you to control several aspects of contact behavior. •
Degrees of freedom (KEYOPT(1))
•
Contact algorithm (defaults to augmented Lagrangian) (KEYOPT(2))
•
Stress state when superelements are present (KEYOPT(3)) for 2-D surface-to-surface contact. Contact model for node-to-surface contact.
•
Location of contact detection point (KEYOPT(4))
•
CNOF Automated adjustment (KEYOPT(5))
•
Time step control (KEYOPT(7))
•
Asymmetric contact selection (KEYOPT(8))
•
Effect of initial penetration or gap (KEYOPT(9))
•
Contact stiffness update (KEYOPT(10))
•
Shell thickness effect (KEYOPT(11))
•
Behavior of contact surface (rough, bonded, etc.) (KEYOPT(12))
11–20
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis KEYOPT defaults can vary depending on the environment you are working in. The following table compares the default values between ANSYS, the ANSYS Contact Wizard, and the ANSYS Workbench. See your ANSYS sales representative for more information about ANSYS Workbench.
Table 11.3 Summary of KEYOPT Defaults in Different Environments KEYOPT Description
ANSYS
ANSYS Contact Wizard
ANSYS Workbench Default Linear (bonded, no sep)
ANSYS Workbench, Default Nonlinear (standard, rough)
1
Selects DOF*
Manual
Auto
Auto
Auto
2
Contact Algorithm
Aug. Lagr. Aug. Lagr. Pure Penalty
3
Stress state when superelement no super is present elem
no super elem
n/a
n/a
4
Location of contact detection point
gauss
gauss
gauss
gauss
5
CNOF/ICONT adjustment
No adjust
No adjust
No adjust
No adjust
6
(blank)
7
Element level time increment control
No control No control No control
No control
8
Asymmetric contact selection
No action
No action
9
Effect of initial penetration or gap
Include all Include all Exclude all
Include all/ramped
10
Contact stiffness update
Between Between load steps substeps
Between load steps
Between load steps
11
Beam/shell thickness effect
Exclude
Exclude
Exclude
Exclude
12
Behavior of contact surface
Standard
Standard
Bonded
n/a
No action
No action
Pure Penalty
*Manual: Requires user to define. Auto: Selection is based on DOF of underlying element. Command(s): KEYOPT, ET GUI: Main Menu> Preprocessor> Element Type> Add/Edit/Delete
11.4.8.3. Selecting a Contact Algorithm (KEYOPT(2)) 11.4.8.3.1. Background For surface-to-surface contact elements, ANSYS offers several different contact algorithms: •
Penalty method (KEYOPT(2) = 1)
•
Augmented Lagrangian (default) (KEYOPT(2) = 0)
•
Lagrange multiplier on contact normal and penalty on tangent (KEYOPT(2) = 3)
•
Pure Lagrange multiplier on contact normal and tangent (KEYOPT(2) = 4)
•
Internal multipoint constraint (MPC) (KEYOPT(2) = 2)
The penalty method uses a contact “spring” to establish a relationship between the two contact surfaces. The spring stiffness is called the contact stiffness. This method uses the following real constants: FKN and FKS for all values of KEYOPT(10), plus FTOLN and SLTO if KEYOPT(10) = 1 or 2. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–21
Chapter 11: Contact The augmented Lagrangian method (which is the default) is an iterative series of penalty methods. The contact tractions (pressure and frictional stresses) are augmented during equilibrium iterations so that the final penetration is smaller than the allowable tolerance (FTOLN). Compared to the penalty method, the augmented Lagrangian method usually leads to better conditioning and is less sensitive to the magnitude of the contact stiffness. However, in some analyses, the augmented Lagrangian method may require additional iterations, especially if the deformed mesh becomes too distorted. The pure Lagrange multiplier method enforces zero penetration when contact is closed and “zero slip” when sticking contact occurs. The pure Lagrange multiplier method does not require contact stiffness, FKN and FKS. Instead it requires chattering control parameters, FTOLN and TNOP. This method adds contact traction to the model as additional degrees of freedom and requires additional iterations to stabilize contact conditions. It often increases the computational cost compared to the augmented Lagrangian method. An alternative algorithm is the Lagrange multiplier method applied on the contact normal and the penalty method (tangential contact stiffness) on the frictional plane. This methods enforces zero penetration and allows a small amount of slip for the sticking contact condition. It requires chattering control parameters, FTOLN and TNOP, as well as the maximum allowable elastic slip parameter SLTO. Another method, the internal multipoint constraint (MPC) algorithm, is used in conjunction with bonded contact (KEYOPT(2) = 5 or 6) to model several types of contact assemblies and kinematic constraints. See Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints for more information on how to use this feature. Note — The Lagrange multiplier methods (KEYOPT(2) = 3, 4) and MPC approach (KEYOPT(2) = 2) do not support the Gauss point detection option (KEYOPT(4) = 0) for surface-to-surface contact. They support the nodal detection options for surface-to-surface contact and node-to-surface contact. When using these options, be careful not to overconstrain the model. The model is overconstrained when a contact node has prescribed boundary conditions, CE and CP equations. ANSYS usually detects and eliminates the overconstraints. However, there is no guarantee that the program will eliminate all the cases of overconstraint. You should always verify your model carefully to address this issue. The Lagrange multiplier also introduces more degrees of freedom which may result in spurious modes for modal and linear eigenvalue buckling analyses. The augmented Lagrangian method would be a better choice for these analysis types. Note — The Lagrange multiplier methods (KEYOPT(2) = 3, 4) introduce zero diagonal terms in the stiffness matrix. Any iterative solver (PCG or AMG) will encounter a preconditioning matrix singularity with these methods. Therefore, you should switch to sparse solver.
11.4.8.4. Determining Contact Stiffness and Allowable Penetration 11.4.8.4.1. Background For the augmented Lagrangian method and penalty method, normal and tangential contact stiffnesses are required. The amount of penetration between contact and target surfaces depends on the normal stiffness. The amount of slip in sticking contact depends on the tangential stiffness. Higher stiffness values decrease the amount of penetration/slip, but can lead to ill-conditioning of the global stiffness matrix and to convergence difficulties. Lower stiffness values can lead to a certain amount of penetration/slip and produce an inaccurate solution. Ideally, you want a high enough stiffness that the penetration/slip is acceptably small, but a low enough stiffness that the problem will be well-behaved in terms of convergence. ANSYS provides default values for contact stiffnesses (FKN, FKT), allowable penetration (FTOLN), and allowable slip (SLTO). In most cases, you do not need to define the contact stiffness. In addition, we recommend that you use KEYOPT(10) = 1 to allow the program to update the contact stiffness automatically. 11–22
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
11.4.8.4.2. Using FKN and FTOLN For certain contact problems, you may choose to use the real constant FKN to define a normal contact stiffness factor. The usual factor range is from 0.01-1.0, with a default of 1.0. The default value is appropriate for bulk deformation. If bending deformation dominates, we recommend using a smaller value (0.1). In cases where the underlying element has a TB plasticity material defined (whether plasticity is active or not), the contact normal stiffness will be reduced by a factor of 100. Use real constant FTOLN in conjunction with the augmented Lagrangian method. FTOLN is a tolerance factor to be applied in the direction of the surface normal. The range for this factor is less than 1.0 (usually less than 0.2), with a default of 0.1, and is based on the depth of the underlying solid, shell, or beam element (see Figure 11.9: “Depth of the Underlying Element”). This factor is used to determine if penetration compatibility is satisfied. Contact compatibility is satisfied if penetration is within an allowable tolerance (FTOLN times the depth of underlying elements). The depth is defined by the average depth of each individual contact element in the pair. If ANSYS detects any penetration larger than this tolerance, the global solution is still considered unconverged, even though the residual forces and displacement increments have met convergence criteria. You can also define an absolute allowable penetration by specifying a negative value for FTOLN. Note — When the contact stiffness is too large (for example, 1016), the machine precision may not guarantee good conditioning of the global stiffness matrix. In this case, you should scale the force unit in the model if possible. Note — FTOLN is also used in the Lagrange multiplier methods (KEYOPT(2) = 3, 4) as a chattering control parameter.
11.4.8.4.3. Using FKT and SLTO ANSYS automatically defines a default tangential contact stiffness that is proportional to MU and the normal stiffness FKN. The default tangential stiffness corresponds to a default value of FKT = 1.0. A positive value for FKT is a factor; a negative value indicates an absolute value of tangential stiffness. For KEYOPT(10) = 1 or 2, or when the Lagrange multiplier on normal and penalty on tangent option is used (KEYOPT(2) = 3), ANSYS updates tangential contact stiffness based on current contact normal pressure, PRES, and maximum allowable elastic slip, SLTO (FKT = MU* PRES/SLTO). The real constant SLTO is used to control maximum sliding distance when FKT is updated at each iteration. ANSYS provides default tolerance values which work well in most cases. You can override the default values for SLTO (1% of average contact length in pair) by defining a scaling factor (positive value when using command input) or an absolute value (negative value when using command input). A larger value will enhance convergence but compromise accuracy. Based on the tolerance, current normal pressure, and friction coefficient, the tangential contact stiffness FKT can be obtained automatically. In certain cases users can override FKT by defining a scaling factor (positive input value) or absolute value (negative input value) (see Positive and Negative Real Constants for more information).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–23
Chapter 11: Contact Note — FKN, FTOLN, FKT, and SLTO can be modified from one load step to another. They can also be adjusted in a restart run. Determining a good stiffness value may require some experimentation on your part. To arrive at a good stiffness value, you can try the following procedure as a “trial run”: 1.
Use a low value for the contact stiffness to start. In general, it is better to underestimate this value rather than overestimate it. Penetration problems resulting from a low stiffness are easier to fix than convergence difficulties that arise from a high stiffness.
2.
Run the analysis up to a fraction of the final load (just enough to get the contact fully established).
3.
Check the penetration and the number of equilibrium iterations used in each substep. If the global convergence difficulty is caused by too much penetration (rather than by residual forces and displacement increments), FKN may be underestimated or FTOLN may be too small. If the global convergence requires many equilibrium iterations for achieving convergence tolerances of residual forces and displacements rather than the resulting penetration, FKN or FKT may be overestimated.
4.
Adjust FKN, FKT, FTOLN, or SLTO as necessary and run the full analysis. If the penetration control becomes dominant in the global equilibrium iterations (that is, if more iterations were used to converge the problem to within the penetration tolerance than to converge the residual forces), you may increase FTOLN to permit more allowable penetration or increase FKN.
Note — Generally, the contact stiffness FKN, FKT has units FORCE/LENGTH3. However, for contact forcebased models (KEYOPT(3) = 0) in CONTA175, the contact stiffness has units FORCE/LENGTH.
11.4.8.4.4. Using KEYOPT(10) The normal and tangential contact stiffness can be updated during the course of an analysis, either automatically (due to large strain effects that change the underlying element's stiffness) or explicitly (by user-specified FKN or FKT values). KEYOPT(10) governs how the normal and tangential contact stiffness is updated when the augmented Lagrangian or penalty method is used. In most cases we recommend that you use KEYOPT(10) = 1 to allow the program to update contact stiffnesses automatically. The possible settings for KEYOPT(10) are outlined below. •
KEYOPT(10) = 0, the contact stiffness will be updated at each load step if FKN or FKT is redefined by the user. Stiffness and other settings (ICONT, FTOLN, SLTO, PINB, PMAX, and PMIN) are averaged across contact elements in a contact pair. The default contact stiffness is determined by underlying element depth and material properties.
•
KEYOPT(10) = 1 (covers KEYOPT(10) = 0), the normal contact stiffness will be updated at every substep based on the mean stress of the underlying elements from the previous substep and the allowable penetration, FTOLN, except in the first substep of the first load step. The default normal contact stiffness for the first substep of the first load step is the same as described for KEYOPT(10) = 0. If bisections occur in the beginning of the analysis, the normal contact stiffness will be reduced by a factor of 0.2 for each bisection. The tangential contact stiffness will be updated at each iteration based on the current contact pressure, MU, and allowable slip (SLTO).
•
KEYOPT(10) = 2 (covers KEYOPT(10) = 1), the normal contact stiffness will be updated at each iteration based on the current mean stress of the underlying elements and the allowable penetration, FTOLN, except in the very first iteration. The default normal contact stiffness for the first iteration is the same as described for KEYOPT(10) = 0. If bisections occur in the beginning of the analysis, the normal contact stiffness will be reduced by a factor of 0.2 for each bisection. The tangential contact stiffness will be updated at each iteration based on the current contact pressure, MU, and allowable slip (SLTO).
•
KEYOPT(10) = 3, same as KEYOPT(10) = 0, except stiffness and settings are not averaged across the contact elements in a contact pair. If bisections occur in the beginning of the analysis, the normal contact stiffness will be reduced by a factor of 0.2 for each bisection.
11–24
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis •
KEYOPT(10) = 4, same as KEYOPT(10) = 1, except stiffness and settings are not averaged across the contact elements in a contact pair.
•
KEYOPT(10) = 5, same as KEYOPT(10) = 2, except stiffness and settings are not averaged across the contact elements in a contact pair. Note — When a Lagrange multiplier method (KEYOPT(2) = 3, 4) or MPC algorithm (KEYOPT(2) = 2) is used, KEYOPT(10) is ignored.
11.4.8.4.5. Chattering Control Parameters The Lagrange multiplier methods (KEYOPT(2) = 3, 4) do not require contact stiffness, FKN and FKT. Instead they require chattering control parameters, FTOLN and TNOP, by which ANSYS assumes that the contact status remains unchanged. FTOLN is the maximum allowable penetration and TNOP is the maximum allowable tensile contact pressure. Note — A negative contact pressure occurs when the contact status is closed. A tensile contact pressure (positive) refers to a separation between the contact surfaces, but not necessarily an open contact status. The behavior can be described as follows: •
If the contact status from the previous iteration is open and the current calculated penetration is smaller than FTOLN, then contact remains open. Otherwise the contact status switches to closed and another iteration is processed.
•
If the contact status from the previous iteration is closed and the current calculated contact pressure is positive but smaller than TNOP, then contact remains closed. If the tensile contact pressure is larger than TNOP, then the contact status changes from closed to open and ANSYS continues to the next iteration.
ANSYS will provide reasonable defaults for FTOLN and TNOP. FTOLN defaults to the displacement convergence tolerance. TNOP defaults to the force convergence tolerance divided by contact area at contact nodes. Keep in mind the following when providing values for FTOLN and TNOP: •
A positive value is a scaling factor applied to the default values.
•
A negative value is used as an absolute value (which overrides the default).
The objective of FTOLN and TNOP is to provide stability to models which exhibit contact chattering due to changing contact status. If the values you use for these tolerances are too small, the solution will require more iterations. However, if the values are too large, the accuracy of the solution will be affected since a certain amount of penetration or tensile contact force is allowed.
11.4.8.5. Choosing a Friction Model 11.4.8.5.1. Background In the basic Coulomb friction model, two contacting surfaces can carry shear stresses up to a certain magnitude across their interface before they start sliding relative to each other. This state is known as sticking. The Coulomb friction model defines an equivalent shear stress τ, at which sliding on the surface begins as a fraction of the contact pressure p (τ = µp + COHE, where µ is the friction coefficient and COHE specifies the cohesion sliding resistance). Once the shear stress is exceeded, the two surfaces will slide relative to each other. This state is known as sliding. The sticking/sliding calculations determine when a point transitions from sticking to sliding or vice versa.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–25
Chapter 11: Contact For frictionless, rough, and bonded contact, the contact element stiffness matrices are symmetric. Contact problems involving friction produce unsymmetric stiffnesses. Using an unsymmetric solver is more computationally expensive than a symmetric solver for each iteration. For this reason, ANSYS uses a symmetrization algorithm by which most frictional contact problems can be solved using solvers for symmetric systems. If frictional stresses have a substantial influence on the overall displacement field and the magnitude of the frictional stresses is highly solution dependent, the symmetric approximation to the stiffness matrix may provide a low rate of convergence. In such cases, choose the unsymmetric solution option (NROPT,UNSYM) to improve convergence.
11.4.8.5.2. Using TAUMAX, FACT, DC, and COHE One of the material properties used for contact elements is input via the interface coefficient of friction, MU, for the Coulomb friction model. Use MU = 0 for frictionless contact. For rough or bonded contact (KEYOPT(12) = 1, 3, 5, or 6, see Selecting Surface Interaction Models), ANSYS assumes infinite frictional resistance regardless of specified value of µ. MU can be specified as a function of temperature. If the underlying element is a superelement (MATRIX50), the material property set must be the same as the one used for the original elements that were assembled into the superelement. ANSYS provides one extension of classical Coulomb friction: TAUMAX is maximum contact friction with units of stress. This maximum contact friction stress can be introduced so that, regardless of the magnitude of normal contact pressure, sliding will occur if the friction stress reaches this value. You typically use TAUMAX when the contact pressure becomes very large (such as in bulk metal forming processes). TAUMAX defaults to 1.0e20. σy Empirical data is often the best source for TAUMAX. Its value may be close to the material being deformed.
3
, where σy is the yield stress of
Another real constant used for the friction law is the cohesion, COHE (default COHE = 0), which has units of stress. It provides sliding resistance, even with zero normal pressure (see Figure 11.10: “Sliding Contact Resistance”).
Figure 11.10 Sliding Contact Resistance
Two other real constants, FACT and DC are involved in specifying static and dynamic friction coefficients, as described in the next section.
11.4.8.5.3. Static and Dynamic Friction Coefficients The coefficient of friction can depend on the relative velocity of the surfaces in contact. Typically, the static coefficient of friction is higher than the dynamic coefficient of friction. ANSYS provides the following exponential decay friction model:
µ = MU × (1 + (FACT − 1)exp( − DC × Vrel )) where: 11–26
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis µ = coefficient of friction. MU = dynamic coefficient of friction input using the MP command. FACT = ratio of static to dynamic coefficients of friction. It defaults to the minimum value of 1.0 DC = decay coefficient. It defaults to 0.0 and it has units of time/length. Therefore, time has some meaning in a static analysis. Vrel = slip rate calculated by ANSYS. Figure 11.11: “Friction Decay” shows the exponential decay curve where the static coefficient of friction is given by:
µs
= FACT × MU
Figure 11.11 Friction Decay
You can determine the decay coefficient if you know the static and dynamic coefficients of friction and at least one data point (µ1 ; Vrel1). The equation for friction decay can be rearranged to give:
DC = −
µ1 − MU × ln Vrel1 (FACT − 1) × MU 1
If you do not specify a decay coefficient and FACT is greater than 1.0, the coefficient of friction will change suddenly from the static to the dynamic value as soon as contact reaches the sliding state. This behavior is not recommended because the discontinuity may lead to convergence difficulties.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–27
Chapter 11: Contact
11.4.8.6. Selecting Location of Contact Detection 11.4.8.6.1. Background Contact detection points are located at the integration points of the contact elements which are interior to the element surface. The contact element is constrained against penetration into the target surface at its integration points. However, the target surface can, in principle, penetrate through into the contact surface, see Figure 11.12: “Contact Detection Located at Gauss Point”.
Figure 11.12 Contact Detection Located at Gauss Point
ANSYS surface-to-surface contact elements use Gauss integration points as a default, which generally provide more accurate results than the nodal detection scheme, which uses the nodes themselves as the integration points. The node-to-surface contact element CONTA175 always uses the nodal detection scheme.
11.4.8.6.2. Using KEYOPT(4) and TOLS The nodal detection algorithms require the smoothing of the contact surface (KEYOPT(4) = 1) or the smoothing of the target surface (KEYOPT(4) = 2), which is quite time consuming. You should use this option only to deal with corner, point-surface, or edge-surface contact (see Figure 11.13: “Contact Detection Point Location at Nodal Point”). KEYOPT(4) = 1 specifies that the contact normal be perpendicular to the contact surface. KEYOPT(4) = 2 specifies that the contact normal be perpendicular to the target surface. Use this option (KEYOPT(4) = 2) when the target surface is smoother than the contact surface.
11–28
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
Figure 11.13 Contact Detection Point Location at Nodal Point
Be aware, however, that using nodes as the contact detection points can lead to other convergence difficulties, such as "node slippage," where the node slips off the edge of the target surface, see Figure 11.14: “Node Slippage Using Nodal Integration KEYOPT(4) = 1 or 2”. In order to prevent node slippage, you can use real constant TOLS to extend the target surface when the default setting still cannot avoid the problem. For most point-to-surface contact problems, we recommend using CONTA175; see Section 11.6: Performing a Node-to-Surface Contact Analysis later in this chapter.
Figure 11.14 Node Slippage Using Nodal Integration KEYOPT(4) = 1 or 2
Smoothing is required for nodal detection algroithms, and it is performed by averaging surface normals connected to the node. As a result, the variation of the surface normal is continuous over the surface, which leads to a better calculation of friction behavior and a better convergence.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–29
Chapter 11: Contact Real constant TOLS is used to add a small tolerance that will internally extend the edge of the target surface when you define the contact detection at the nodal point (KEYOPT(4) = 1 or 2). TOLS is useful for problems where contact nodes are likely to lie on the edge of targets (as at symmetry planes or for models generated in a nodeto-node contact pattern). In these situations, the contact node may repeatedly "slip" off the target surface and go completely out of contact, resulting in convergence difficulties from oscillations. Units for TOLS are percent (1.0 implies a 1.0% increase in the target edge length). A small value of TOLS will usually prevent this situation from occurring. The default value is 10 for small deflection and 2 for large deflection (NLGEOM, ON). Note — The definition of KEYOPT(4) in node-to-surface contact element CONTA175 is different. KEYOPT(4) = 1 for surface-to-surface contact is equivalent to KEYOPT(4) = 1 for node-to-surface contact. However, KEYOPT(4) = 2 for surface-to-surface contact is equivalent to KEYOPT(4) = 0 for node-to surface contact. See Section 11.6.1.1.2: KEYOPT(4).
11.4.8.7. Adjusting Initial Contact Conditions 11.4.8.7.1. Background Rigid body motion is usually not a problem in dynamic analyses. However, in static analyses, rigid body motion occurs when a body is not sufficiently restrained. "Zero or negative pivot" warning messages and impractical, excessively large displacements indicate unconstrained motion in a static analysis. In simulations where rigid body motions are constrained only by the presence of contact, you must ensure that the contact pairs are in contact in the initial geometry. In other words, you want to build your model so that the contact pairs are "just touching." However, you can encounter various problems in doing so: •
Rigid body profiles are often complicated, making it difficult to determine where the first point of contact might occur.
•
Small gaps between element meshes on both sides of the element pair can be introduced by numerical round-off, even if the solid model is built in an initially-contacting state.
•
Small gaps can exist between the integration points of the contact elements and target surface elements.
For the same reasons, too much initial penetration between target and contact surfaces can occur. In such cases, the contact elements may overestimate the contact forces, resulting in nonconvergence or in breaking-away of the components in contact. The definition of initial contact is perhaps the most important aspect of building a contact analysis model. Therefore, you should always issue the CNCHECK command before starting the solution to verify the initial contact status. You may find that you need to adjust the initial contact conditions. ANSYS offers several ways to adjust the initial contact conditions of a contact pair.
11.4.8.7.2. Using PMIN, PMAX, CNOF, ICONT, KEYOPT(5), and KEYOPT(9) The following techniques can be performed independently or in combinations of one or more at the beginning of the analysis. They are intended to eliminate small gaps or penetrations caused by numerical round-off due to mesh generation. They are not intended to correct gross errors in either the mesh or in the geometric data. 1.
Use real constant CNOF to specify a contact surface offset. Specify a positive value to offset the entire contact surface towards the target surface. Use a negative value to offset the contact surface away from the target surface.
11–30
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis Note — If user-defined values are input for both CNOF and PINB, you must ensure that PINB is greater than CNOF. Otherwise, CNOF will be ignored. However, if a user-defined CNOF is input and the PINB value is left at its default value, the PINB value will be adjusted so that it is larger than the CNOF value, as described in Using PINB. ANSYS can automatically provide the CNOF value to either just close the gap or reduce initial penetration. Set KEYOPT(5) as follows: 1: Closes the gap 2: Reduces initial penetration 3: Either closes the gap or reduces initial penetration 2.
Use the real constant ICONT to specify a small initial contact closure. This is the depth of an "adjustment band" around the target surface. A positive value for ICONT indicates a scaling factor relative to the depth of the underlying elements. A negative value indicates an absolute contact closure value. The value of ICONT defaults to zero if KEYOPT(5) = 0, 1, 2, or 3. (The ICONT default is different when KEYOPT(12) = 6 for bonded-initial contact; see Section 11.4.8.11: Selecting Surface Interaction Models for more information). If KEYOPT(5) = 4, ANSYS provides a small (but meaningful) value for ICONT according to the geometric dimensions, and prints a warning message stating what value was assigned. Any contact detection points that fall within this adjustment band are internally shifted to be on the target surface (see Figure 11.15: “Contact Surface Adjustment With ICONT”(a)). Only a very small correction is suggested; otherwise, severe discontinuity may occur (see Figure (b)). The difference between CNOF and ICONT is that the former shifts the entire contact surface with the distance value CNOF, the latter moves all initially open contact points which are inside of adjustment band ICONT onto the target surface.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–31
Chapter 11: Contact
Figure 11.15 Contact Surface Adjustment With ICONT
!" # $%& '# A B& + $%& '#
0 1324%5
13678 9: 8 ;=<&>'? 9:@
!" ( #
* + , -
$%& ) #
, (# , &, /. A /B& + $=& '#
3.
Use real constants PMIN and PMAX to specify an initial allowable penetration range. When either PMAX or PMIN is specified, ANSYS brings the target surface into a state of initial contact at the beginning of the analysis (see Figure 11.16: “Contact Surface Adjustment (PMIN, PMAX)”). If the initial penetration is larger than PMAX, ANSYS adjusts the target surface to reduce penetration. If the initial penetration is smaller than PMIN (and within the pinball region), ANSYS adjusts the target surface to ensure initial contact. Initial adjustment for contact status is performed only in translational modes. Such adjustment of initial contact status will be performed for a rigid target surface that has either prescribed loads or displacements. Similarly, a target surface that has no boundary conditions specified may also be adjusted for initial contact. When all the target surface nodes have a prescribed value of zero, the initial adjustment using PMAX and PMIN will not be performed. Note that ANSYS treats applicable degrees of freedom for target surface nodes independently. For example, if you specify the UX degree of freedom to be "zero," then no initial adjustment is possible along the X direction. However, the PMAX and PMIN options will still be activated in the Y and Z directions.
11–32
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis The initial status adjustment is an iterative process. ANSYS uses a maximum of 20 iterations. If the target surface cannot be brought into an acceptable penetration range (i.e., in the range of PMIN to PMAX), the analysis proceeds with the original geometry. ANSYS issues a warning message in such circumstances, and you may need to manually adjust your initial geometry. Figure 11.17: “A Scenario in Which Initial Adjustment Will Fail” illustrates a problem in which initial contact adjustment iteration will fail. The UY degree of freedom for the target has been restrained. Therefore, the only possible adjustment for initial contact is in the X direction. However, in this problem, any movement of the rigid target surface in the X direction will not establish initial contact. For flexible-to-flexible contact, this technique not only moves the entire target surface but also moves the whole deformable body which attaches to the target surface. Make sure there is no other contact surface or target surface connecting with the deformable body.
Figure 11.16 Contact Surface Adjustment (PMIN, PMAX)
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–33
Chapter 11: Contact
Figure 11.17 A Scenario in Which Initial Adjustment Will Fail
4.
Set KEYOPT(9) to adjust initial penetration or gap; see Figure 11.18: “Ignoring Initial Penetration, KEYOPT(9) = 1”. True initial penetration includes two parts: •
Penetration or gap due to geometry
•
Penetration or gap due to user-defined contact surface offset (CNOF).
See Figure 11.19: “Components of True Penetration”. KEYOPT(9) provides the following capabilities: •
To include initial penetration from both geometry and contact surface offset, set KEYOPT(9) = 0. This is the default.
•
To ignore initial penetration from both effects, set KEYOPT(9) = 1. When KEYOPT(12) = 4 or 5, this setting for KEYOPT(9) will also ignore the initial force in open-gap springs, thus creating an initially "perfect" contacting surface having no initial forces acting across the contact interface.
•
To include the defined contact surface offset (CNOF) but ignore the initial penetration due to geometry, set KEYOPT(9) = 3. When KEYOPT(12) = 4 or 5, this setting for KEYOPT(9) will also ignore the initial force in open-gap springs, thus creating an initially "perfect" contacting surface having no initial forces acting across the contact interface.
For problems such as an interference fit, over-penetration is expected. These problems often have convergence difficulties if the initial penetration is step-applied in the first load step. You may overcome convergence difficulties by ramping the initial penetration over the first load step, see Figure 11.20: “Ramping Initial Interference”. The following KEYOPT(9) settings provide ramped capabilities:
11–34
•
To ramp the total initial penetration (CNOF + the offset due to geometry), set KEYOPT(9) = 2.
•
To ramp the defined contact surface penetration, but ignore the penetration due to geometry, set KEYOPT(9) = 4.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis For both of the above KEYOPT(9) settings, you should also set KBC,0 and not specify any external loads in the first load step. Also, be sure that the pinball region is big enough to capture the initial interference. You can use the above techniques in conjunction with each other. For example, you may wish to set a very precise initial penetration or gap but the initial coordinates of the finite element nodes may not be able to provide sufficient precision. To accomplish this, you could: 1.
Use ICONT to move the initial open contact points just onto the target surface.
2.
Use CNOF to specify a penetration (positive value) or gap (negative value).
3.
Use KEYOPT(9) = 3 to resolve the initial penetration in the first substep (or KEYOPT(9) = 4 to gradually resolve the initial penetration).
Figure 11.18 Ignoring Initial Penetration, KEYOPT(9) = 1
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–35
Chapter 11: Contact
Figure 11.19 Components of True Penetration
11–36
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
Figure 11.20 Ramping Initial Interference
ANSYS provides a printout (in the output window or file or via the CNCHECK) of the model's initial contact state for each target surface at the beginning of the analysis. This information is helpful for determining the maximum penetration or minimum gap for each target surface. If no contact is detected for a specific target surface, ANSYS issues a warning. This occurs when the target surface is far from contact (i.e., outside of the pinball region), or when the contact/target elements have been killed. See Positive and Negative Real Constants for more information on these real constants.
11.4.8.8. Physically Moving Contact Nodes Towards the Target Surface The initial contact status can be adjusted to close the gap by defining real constant ICONT or by ignoring the penetration (setting KEYOPT(9) = 1). However the initial contact adjustment is kept during the entire analysis as a rigid zone. The initial contact adjustment can cause a certain amount of residual force if a large rotation appears at the contact surface. This problem can be alleviated by issuing the CNCHECK,ADJUST command, which physically moves contact nodes towards the target surface under the following circumstances:
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–37
Chapter 11: Contact •
Only when using the nodal detection option (KEYOPT(4) = 1 or 2), or when using CONTA175.
•
Initially open contact nodes inside the ICONT zone.
•
Initially penetrated nodes with KEYOPT(9) = 1.
After issuing the CNCHECK,ADJUST command, the coordinates of the nodes that have been moved are modified as shown in Figure 11.21: “Effect of Moving Contact Nodes”. You can change other contact related settings in PREP7 (for example, set KEYOPT(4) = 0 to use the Gauss detection option) and save the db file. Issuing the SAVE command before issuing the CNCHECK,ADJUST command is recommended in order to resume the .DB file with the original contact configuration. For those contact pairs whose contact nodes you do not wish to physically move towards target surface, do not define KEYOPT(4) = 1 or 2.
Figure 11.21 Effect of Moving Contact Nodes
11.4.8.9. Determining Contact Status and the Pinball Region 11.4.8.9.1. Background The position and motion of a contact element relative to its associated target surface determines the contact element status. ANSYS monitors each contact element and assigns a status: •
STAT = 0 Open far-field contact
•
STAT = 1 Open near-field contact
•
STAT = 2 Sliding contact
•
STAT = 3 Sticking contact
A contact element is considered to be in near-field contact when its integration points (Gauss points or nodal points) are within a code-calculated (or user-defined) distance to the corresponding target surface. This distance 11–38
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis is referred to as the pinball region. The pinball region is a circle (in 2-D) or a sphere (in 3-D) centered about the Gauss point.
11.4.8.9.2. Using PINB Use real constant PINB to specify a scaling factor (positive value for PINB when using command input) or absolute value (negative value for PINB when using command input) for the pinball region. You can specify PINB to have any value. By default, and assuming that large deflection effects apply (NLGEOM,ON), ANSYS defines the pinball region as a circle for 2-D or a sphere for 3-D of radius 4*depth (if rigid-to-flexible contact) or 2*depth (if flexibleto-flexible contact) of the underlying element. (See the discussion of element depth in Section 11.4.8.1.1: Positive and Negative Real Constant Values.) If you include no large-deflection effects (NLGEOM,OFF), the default pinball region is half that of the large-deflection case. (For the no-separation (KEYOPT(12) = 4) and bonded-always (KEYOPT(12) = 5 options, the PINB default is different than described here. See Section 11.4.8.11: Selecting Surface Interaction Models for more information.) Note — If you input a value for real constant CNOF (contact surface offset) and the default PINB value (as described above) is less than the absolute value of CNOF, the default for PINB will be set to the absolute value of (1.1*CNOF). The computational cost of searching for contact depends on the size of the pinball region. Far-field contact element calculations are simple and add little computational demands. The near-field calculations (for contact elements that are nearly or actually in contact) are slower and more complex. The most complex calculations occur once the elements are in actual contact. Setting a proper pinball region is useful to overcome spurious contact definitions if the target surface has several convex regions. However, the default setting should be appropriate for most contact problems. See Positive and Negative Real Constants for more information on this real constant.
11.4.8.10. Avoiding Spurious Contact in Self Contact Problems In some cases of self contact, ANSYS may erroneously assume contact between a contact and target surface that are in very close geometrical position as shown below.
Figure 11.22 Auto Spurious Prevention
! ! " # $% &' !
( #*)+ '
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–39
Chapter 11: Contact ANSYS will alert you when it first detects spurious contact in each load step. If ANSYS encounters such contact on the first load step, you'll see the following error message: Contact element x has too much penetration related to target element y. We assume it (may be more elements) is spurious contact.
If ANSYS encounters an abrupt change in contact that it classifies as spurious contact, you'll see the following message: Contact element x status changed abruptly with target element y. We assume it (may be more elements) is spurious contact.
ANSYS issues such messages only once per load step. It does not notify you of additional cases of spurious contact that were ignored during the load step.
11.4.8.11. Selecting Surface Interaction Models 11.4.8.11.1. Background The surface-to-surface contact elements support normal unilateral contact models as well as other mechanical surface interaction models.
11.4.8.11.2. Using KEYOPT(12) and FKOP Use KEYOPT(12) to model different contact surface behaviors. •
KEYOPT(12) = 0 models standard unilateral contact; that is, normal pressure equals zero if separation occurs.
•
KEYOPT(12) = 1 models perfectly rough frictional contact where there is no sliding. This case corresponds to an infinite friction coefficient and ignores the material property MU.
•
KEYOPT(12) = 2 models no separation contact, in which the target and contact surfaces are tied (although sliding is permitted) for the remainder of the analysis once contact is established.
•
KEYOPT(12) = 3 models "bonded" contact, in which the target and contact surfaces are bonded in all directions (once contact is established) for the remainder of the analysis.
•
KEYOPT(12) = 4 models no separation contact, in which contact detection points that are either initially inside the pinball region or that once involve contact always attach to the target surface along the normal direction to the contact surface (sliding is permitted).
•
KEYOPT(12) = 5 models bonded contact, in which contact detection points that are either initially inside the pinball region or that once involve contact always attach to the target surface along the normal and tangent directions to the contact surface (fully bonded).
•
KEYOPT(12) = 6 models bonded contact, in which the contact detection points that are initially in a closed state will remain attached to the target surface and the contact detection points that are initially in an open state will remain open throughout the analysis.
For modeling either no-separation or bonded contact, you may need to set a value for the FKOP real constant. This provides a stiffness factor applied when contact opens. If FKOP is a scaling factor (positive value for command input), the true contact opening stiffness equals FKOP times the contact stiffness applied when contact closes. If FKOP is an absolute value (negative value for command input), the value is applied as an absolute contact opening stiffness. The default FKOP value is 1. No separation and bonded contact generate a "pull-back" force when contact opening occurs, and that force may not completely prevent separation. To reduce separation, define a larger value for FKOP. Also, in some cases separation is expected while connection between the contacting surfaces is required to prevent rigid body
11–40
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis motion. In such instances, you can specify a small value for FKOP to maintain the connection between the contact surfaces (this is a "weak spring" effect). For the no-separation option (KEYOPT(12) = 4) and the bonded-always option (KEYOPT(12) = 5), a relatively small PINB value (pinball region) may be used to prevent any false contact. For these KEYOPT(12) settings, the default for PINB is 0.25 (25% of the contact depth) for small deformation analysis (NLGEOM,OFF) and 0.5 (50% of the contact depth) for large deformation analysis (NLGEOM,ON). (The default PINB value may differ from what is described here if CNOF is input. See Section 11.4.8.9.2: Using PINB for more information.) For the bonded-initial option (KEYOPT(12) = 6), a relatively large ICONT value (initial contact closure) may be used to capture the contact. For this KEYOPT(12) setting, the default for ICONT is 0.05 (5% of the contact depth) when KEYOPT(5) = 0 or 4. See Positive and Negative Real Constants for more information on these real constants.
11.4.8.12. Modeling Contact with Superelements 11.4.8.12.1. Background The surface-to-surface contact elements can model a rigid body (or one linear elastic body) contacting another linear elastic body undergoing small motions. These elastic bodies can be modeled using superelements, which greatly reduces the number of degrees of freedom involved in the contact iteration. Remember that any contact or target nodes must be either all master nodes of the superelements or all slave nodes of the superelements. When the contact pair is built in original elements used to generate superelements, the contact status will not change from its initial status. Because the superelement consists only of a group of retained nodal degrees of freedom, it has no surface geometry on which ANSYS can define a contact and target surface. Therefore, the contact and target surface must be defined on the surface of the original elements before they are assembled into a superelement. Information taken from the superelement includes nodal connection and assembly stiffness, but no material property or stress states (whether axisymmetric, plane stress, or plane strain). One restriction is that the material property set used for the contact elements must be the same as the one used for the original elements before they were assembled into superelements.
11.4.8.12.2. Using KEYOPT(3) Use KEYOPT(3) to provide information for the 2-D analysis with superelements. In elements CONTA171 and CONTA172, the options are as follows: •
No superelement used (KEYOPT(3) = 0)
•
Axisymmetric, use with superelements only (KEYOPT(3) = 1)
•
Plane strain or plane stress with unit thickness, use with superelements only (KEYOPT(3) = 2)
•
Plane stress with thickness input use with superelements only (KEYOPT(3) = 3). Note that for this case, use real constant R2 to specify the thickness.
In 3-D contact analysis, KEYOPT(3) in elements CONTA173 and CONTA174 is ignored. ANSYS will automatically detect whether the underlying element is a superelement.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–41
Chapter 11: Contact Note — KEYOPT(3) in node-to surface contact element CONTA175 has a different meaning. In CONTA175, KEYOPT(3) = 1 defines the contact traction-based model. In this case, all of the real constant inputs and contact result quantities have the same units as the surface-to-surface contact elements. KEYOPT(3) = 0 (default) defines the contact force model. In this model, certain real constants and contact result quantities can have different units (a factor of AREA (Length2) difference). See Section 11.6.1.1.1: KEYOPT(3).
11.4.8.13. Accounting for Thickness Effect 11.4.8.13.1. Background You can account for the thickness of shells (2-D and 3-D) and beams (2-D) using KEYOPT(11). For rigid-to-flexible contact, ANSYS will automatically shift the contact surface to the bottom or top of the shell/beam surface. For flexible-to-flexible contact, ANSYS will automatically shift both the contact and target surfaces which are attached to shell/beam elements. By default, ANSYS does not account for the element thickness, and beams and shells are discretized at their mid-surface in which penetration distance is calculated from the mid-surface.
11.4.8.13.2. Using KEYOPT(11) When you set KEYOPT(11) = 1 to account for beam or shell thickness, the contact distance is calculated from either the top or the bottom surface as specified previously in Section 11.4.2: Steps in a Contact Analysis. Note — Only use KEYOPT(11) = 1 to account for thickness when you have shell or beam elements with nodes located at the middle surface (for example, KEYOPT(11) = 0 for SHELL91). When building your model geometry, if you are going to account for thickness, remember the offsets which may come from either the contact surface or target surface or from both. When you specify a contact offset (CNOF) along with setting KEYOPT(11) = 1, it is defined from the top or bottom of the shell/beam, not the mid-surface. When used with SHELL181, changes in thickness during deformation are also taken into account.
11.4.8.14. Using Time Step Control 11.4.8.14.1. Background Time step control is an automatic time stepping feature that predicts when the status of a contact element will change and cuts the current time step back.
11.4.8.14.2. Using KEYOPT(7) Use KEYOPT(7) to take one of four actions to control time stepping, where KEYOPT(7) = 0 provides no control (the default), and KEYOPT(7) = 3 provides the most control. •
KEYOPT(7) = 0: No control. The time step size is unaffected by the prediction. This setting is appropriate for most analyses when automatic time stepping is activated and a small time step size is allowed.
•
KEYOPT(7) = 1: Time step size is bisected if too much penetration occurs during an iteration, or if the contact status changes dramatically.
•
KEYOPT(7) = 2: Predict a reasonable increment for the next substep.
•
KEYOPT(7) = 3: Predict a minimal time increment for the next substep.
11.4.8.15. Using the Birth and Death Option The surface-to-surface contact and target elements allow birth and death and also follow the birth and death status of their underlying elements. The elements can be removed for part of an analysis and then reactivated 11–42
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis for a later stage. This feature is useful for modeling complex metal forming processes where multiple rigid target surfaces need to interact with the contact surface at different stages of the analysis. Springback modeling often requires removing the rigid tools at the end of the forming processes. This option cannot be used with "no separation" or bonded contact.
11.4.9. Controlling the Motion of the Rigid Target Surface (Rigid-to-Flexible Contact) Rigid target surfaces are defined in their original configuration, and the motion of the entire surface is then defined by the imposed displacements on the pilot node (or the different nodes of the target surface if no pilot node was defined). You must use a pilot node in any of the following situations to control the boundary conditions (and motion) of the entire target surface: •
The target surface is subjected to applied forces.
•
The target surface is subjected to rotations.
•
The target surface is connected to other elements (e.g., structural mass element MASS21).
•
The motion of the target surface is adjusted by the equilibrium condition.
The degrees of freedom of the pilot node represent the motion of the entire rigid surface, including two translational and one rotational degree of freedom in 2-D, and three translational and three rotational degrees of freedom in 3-D. You can apply boundary conditions (displacement, initial velocity), concentrated loads, rotations, etc. to the pilot node. To account for a rigid body's mass, define a mass element (MASS21) on the pilot node. Keep in mind the following restrictions on the target surface when using a pilot node: •
Each target surface can have only one pilot node.
•
ANSYS ignores all boundary conditions on all nodes other than the pilot node.
•
Only the pilot node can connect to other elements. If you need to attach the rigid surface to another element, you must use the pilot node to do so.
•
You cannot use constraint equations (CE) or node coupling (CP) to control the degree of freedom of the target surface when a pilot node has been defined. If you want to apply any loads or constraints on the rigid target surface, you must define a pilot node and apply the loads to that pilot node. If you do not use a pilot node, you can have rigid body motions only. Note — The pilot node can be one of the nodes on the target elements or a node at any arbitrary location. However, it should not be the node on the contact element. The location of the pilot node becomes important only when rotations or moments are to be applied. For each pilot node, ANSYS will automatically define an internal node and an internal constraint equation. The rotational DOF of the pilot node is connected to the translational DOF of the internal node by the internal constraint equation.
By default, KEYOPT(2) = 0 for the target element, ANSYS checks the boundary conditions for each target surface. If all of the following conditions are met, then ANSYS treats the target nodes along the respective degree of freedom as fixed: •
There are no explicit boundary conditions or prescribed forces for target surface nodes.
•
Target surface nodes are not connected to other elements.
•
Neither constraint equations nor node coupling have been used to constrain such nodes.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–43
Chapter 11: Contact At the end of each load step, ANSYS releases the constraint conditions that were set internally. The constraint conditions stored in the results file (Jobname.RST) and the database file (Jobname.DB) may be updated due to this change. You should carefully verify whether the current constraint conditions are expected before restarting an analysis or resolving the problem in interactive mode. If you wish, you can control the constraint conditions of target nodes by setting KEYOPT(2) = 1 in the target element definition.
11.4.10. Modeling Thermal Contact You can use surface-to-surface contact elements and the node-to-surface contact element, in combination with thermal-structural coupled field solid elements or thermal elements, to model heat transfer that occurs in the contact surface. To activate both the structural and thermal DOFs, set KEYOPT(1) = 1. To activate the thermal DOF only, set KEYOPT(1) = 2. The following thermal contact features are supported. •
Thermal contact conduction between two contacting surfaces.
•
Heat convection from a “free surface” to the environment or between two open surfaces separated by small gap (“near field” convection).
•
Heat radiation from a “free surface” to the environment or between two open surfaces separated by a small gap (“near field” radiation).
•
Heat generation due to frictional dissipation.
•
Heat flux input. Note — When KEYOPT(1) is set to 2, ANSYS ignores heat generation due to friction.
11.4.10.1. Thermal Contact Behavior vs. Contact Status Each contact pair can cover one or more thermal contact features. Which feature is active depends on the contact status: Closed Contact: Thermal contact conduction transfers heat between two contacting surfaces. Frictional Sliding: Frictional dissipated energy generates the heat to both the contact and target surfaces. Near-Field Contact: Both heat convection and radiation between the contact and target surfaces are taken into account. The external flux value contributes to the contact surface. Free-Surface Contact: Heat convection and radiation between the contact surface and the environment are taken into account. The external flux value only contributes to both contact and target surfaces.
11.4.10.2. Free Thermal Surface If you wish to model free surface convection, free surface radiation, or a surface with a supplied heat flux value, you can define a “free” thermal surface. A free thermal surface can be a contact surface with no associated target (that is, the contact pair lacks target elements). You can also set KEYOPT(3) = 1 of the target element type definition to define a free thermal surface. When this KEYOPT is set, both free surface radiation and convection are considered as long as open contact is detected. In this case, there is no convective and radiative heat transfer between the contact and target surfaces.
11–44
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
11.4.10.3. Temperature on Target Surface For interface heat conduction, near field convection, or near field radiation, a temperature for both the contact and target surfaces is required. The temperature at the intersection between the target surface and the normal from the contact detection point represents the target temperature. The temperature on the pilot node represents the entire rigid target surface temperature if the pilot node exists.
Figure 11.23 Target Temperature
!#"%$ & '
11.4.10.4. Modeling Conduction To take into account the conductive heat transfer between contact and target surfaces, you need to specify the thermal contact conductance coefficient TCC through a real constant table.
11.4.10.4.1. Using TCC The conductive heat transfer between two contacting surfaces is defined by q = TCC X (Tt -Tc) where: q: is the heat flux per area. TCC: is the thermal contact conductance coefficient, having units of HEAT/(TIME * TEMPERATURE * AREA) for force-based node-to-surface contact, or units of HEAT/(TIME * TEMPERATURE) for the traction-based model. Tt and Tc: are the temperatures of the contact points on the target and contact surfaces. The TCC value is input through a real constant, which can be made a function of temperature [(Tc + Tt)/2], pressure, time, and location by using the %TABLE% option. TCC has units of heat/(time x area x temp). If contact occurs, a small value of TCC yields a measure amount of imperfect contact and a temperature discontinuity across the interface. For large values of TCC, the resulting temperature discontinuity tends to vanish and perfect thermal contact is approached. When not in contact, however, it is assumed that no heat is transferred across the interface. To model contact conduction between two surfaces where a small gap exists, use KEYOPT(12) = 4 or 5 to define either the “bonded contact” or “no-separation contact” options (see Selecting Surface Interaction Models).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–45
Chapter 11: Contact
11.4.10.4.2. Using the Quasi Solver Option You can take advantage of the fast thermal transient solver option (THOPT,QUASI) in the contact analysis. (See Nonlinear Options in the ANSYS Thermal Analysis Guide for more information on this solver option.) To do so, you must use the following contact element key options: KEYOPT(1) = 2 - Temperature DOF only KEYOPT(12) = 5 or 6 - Bonded always or bonded initial The following solver options must also be set: ANTYPE,TRANS THOPT,QUASI EQSLV,JCG/ICCG The following two cases are supported: •
Thermal conductivity at contact. The only real constant used is TCC, which can be a function of time and temperature.
•
Perfect thermal contact which supports dissimilar meshes on both sides of the contacting interface (TCC = infinity). This case requires the internal MPC approach (KEYOPT(2) = 2) and contact nodal detections (KEYOPT(4) = 1 or 2) or CONTA175.
11.4.10.5. Modeling Convection To model convective heat transfer, you must specify the heat convection coefficient CONV using the SFE command. CONV can be a constant value (only uniform is allowed) or a function of temperature, time, and location as specified through tabular input. For free surface convection, you must specify bulk temperature through the SFE command. You can access this command through the following GUI paths: Main Menu> Preprocessor> Loads> Define Loads> Apply> Thermal> Convection> On Elements> Uniform Main Menu> Solution> Define Loads> Apply> Thermal> Convection> On Elements> Uniform
11.4.10.6. Modeling Radiation 11.4.10.6.1. Background To model radiative heat transfer, you need to specify one of the following: •
Emissivity value EMIS, specified through the material property definition.
•
Stefan-Boltzmann constant SBCT through a real constant.
•
Offset temperature TOFFST. If you define your data in terms of degrees Fahrenheit or degrees Celsius, you must specify a temperature offset using the TOFFST command. You can access this command through the following GUI paths: Main Menu> Preprocessor> Loads> Analysis Type> Analysis Options Main Menu> Preprocessor> Material Props
•
Radiation view factor RDVF, specified through a real constant.
•
Environment (ambient) temperature. It is only used for free radiation and input on the SFE command with KVAL = 2 and CONV as a table parameter (this is the same as the bulk temperature in free surface convection modeling).
11–46
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
11.4.10.6.2. Using SBCT and RDVF When contact is open, heat transfer through radiation can occur. The equation is defined by q = RDVF x EMIS x SBCT [(Te + TOFFST)4 - (Tc + TOFFST)4] Where TOFFST: The temperature offset from absolute zero to zero (defined through the TOFFST command.) EMIS: The surface emissivity (input as material property). SBCT: The Stefan-Boltzmann constant (input as a real constant). There is no default for SBCT, and if this is not defined the radiation effect is excluded. RDVF: The radiation view factor input as a real constant (defaults to 1). RDVF can be defined as a function of temperature, gap distance, time, and location by using the %TABLE% option. It is only used for near field radiation. For far field radiation, RDVF is set to 1.0 and a user-assigned value is ignored. Other freesurface conditions recognize user-specified RDVF. For “near field” radiation, when an intersection from a contact detection point to the target surface (in the direction of normal to the contact point) is detected, and the gap distance is smaller than the pinball radius, Te is the target temperature at the intersection. The radiation modeling here assumes that the radiative heat transfer occurs in the direction of the normal between two surfaces with a small gap. By defining RDVF as a function of gap, you can account for geometry effects. Use the Radiosity Solver method for more generalized radiation problems (see the ANSYS Thermal Analysis Guide for more information). For “free surface” radiation, Te becomes the “ambient” temperature defined by “bulk temperature” input from the SFE command (using KVAL = 2 and CONV as the table).
11.4.10.7. Modeling Heat Generation Due to Friction 11.4.10.7.1. Background In order to model heat generation due to frictional dissipated energy, you should perform a coupled transient thermal-structural analysis. If you wish you can turn off transient effects on structural DOFs by using TIMINT,STRUC,OFF. However, you must include transient effects on the thermal DOF. Two real constants are required: •
FHTG is the frictional dissipated energy converted into heat.
•
FWGT is the weight factor for the distribution of heat between contact and target surfaces.
11.4.10.7.2. Using FHTG and FWGT In the coupled thermal-structural contact modeling, the rate of frictional dissipation is given by q = FHTG x τ x V Where τ: The equivalent frictional stress. V: The sliding rate. FHTG: The fraction of frictional dissipated energy converted into heat. This value defaults to 1 and can be input as a real constant. For an input of true 0, you must enter a very small value (for example, 1E-8). If you enter 0, ANSYS interprets this as an input of the default value. The amount of frictional dissipation on contact and target surfaces is defined by
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–47
Chapter 11: Contact qc = FWGT x FHTG x τ x V and qT = (1 - FWGT) x FHTG x τ x V Where qc is the contact side and qT is the target side, and FWGT is the weight factor for the distribution of heat between the contact and target surfaces (input as a real constant). By default, FWGT = 0.5. For an input of true 0, you must enter a very small value (for example, 1E-8). If you enter 0, ANSYS interprets this as an input of the default value.
11.4.10.8. Modeling External Heat Flux You can apply heat flux on the contact elements through the SFE command. Only uniform flux can be applied. Heat flux cannot be applied on target elements. However, for near field contact, the external flux is applied on contact and will contribute to target elements. For a free thermal surface, if KEYOPT(3) of the target element is set to 1, the external flux is only applied on the contact side. On a given contact element either CONV or HFLUX (but not both) may be specified. However, you can define two different contact pairs: one models convection and the other models heat flux.
11.4.11. Modeling Electric Contact You can use surface-to-surface contact elements or the node-to-surface contact element, in combination with thermal-electric elements and solid coupled field elements to model electric current conduction. You can also use surface-to-surface contact elements, in combination with piezoelectric and electrostatic elements, to model electric charge across a contacting interface. KEYOPT(1) provides degree of freedom options for modeling electric contact. For combined structural/thermal/electric contact, set KEYOPT(1) = 3 to activate the structural, thermal, and electric current DOFs. For pure thermal/electric contact, set KEYOPT(1) = 4 to activate the thermal and electric current DOFs. For piezoelectric contact, set KEYOPT(1) = 5 to activate the structural and piezoelectric DOFs. For electrostatic contact, set KEYOPT(1) = 6 to activate the electrostatic DOF. The electric contact features are: •
Electric conduction between two contacting surfaces.
•
Heat generation due to electric dissipation.
•
Electric charge across the contacting interface.
11.4.11.1. Modeling Surface Interaction 11.4.11.1.1. Background To take into account the surface interaction for electric contact, you need to specify the electric contact conductance per unit area if you are using the electric current degree of freedom, or the electric contact capacitance per unit area if you are using the piezoelectric or electrostatic degrees of freedom. For either case, this parameter is ECC. You specify ECC through a real constant table. You can use a tabular input to define ECC as a function of contact pressure (pressure as a table), average temperature on contact detection point (temperature as a table), and time. If the “bonded contact” or “no-separation contact” option is set, contact interaction can occur between two surfaces separated by a narrow gap.
11–48
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
11.4.11.1.2. Using ECC The interaction between two contacting surfaces is defined by J = ECC x (Vt - Vc) where: J = current density for the electric potential (VOLT) degree of freedom (KEYOPT(1) = 3 or 4), or the electric charge density (KEYOPT(1) = 5, or 6). ECC = electric contact conductance for the electric potential (VOLT) degree of freedom (KEYOPT(1) = 3 or 4), or the electric contact capacitance per unit area for (KEYOPT(1) = 5, or 6). Vt and Vc = voltages at the contact points on the target and contact surfaces. The ECC value is input through a real constant, which can be a function of temperature [(Tt + Tc)/2], pressure, and time, by using the %TABLE% option. For the current conduction option, the electric contact conductance ECC has units of electric conductivity/length. For the piezoelectric and electrostatic options, the electric contact capacitance ECC has units of capacitance per unit area. To model surface interaction between two surfaces where a small gap exists, use KEYOPT(12) = 4 or 5 to define either the “bonded contact” or “no-separation contact” options (see Selecting Surface Interaction Models). Note — For force-based node-to-surface contact, ECC has units of (electric conductivity)(LENGTH) or the capacitance.
11.4.11.2. Modeling Heat Generation Due to Electric Current For electric current field analyses (KEYOPT(1) = 3 or 4), the heat generation due to electric current is given by q = FHEG x J x (VT - VC) Where FHEG: The fraction of electric dissipated energy converted into heat (Joule heating). This value defaults to 1 and can be input as a real constant. For an input of true 0, you must enter a very small value (for example, 1E-8). If you enter 0, ANSYS interprets this as an input of the default value. J: The current density. Vt and Vc: The voltages at the contact points on the target and contact surfaces. The amount of electric heat dissipation on contact and target surfaces is defined by qc = FWGT x q and qT = (1 - FWGT) x q Where qc is the contact side and qT is the target side, and FWGT is the weight factor for the contact heat dissipation between the contact and target surfaces (input as a real constant). FWGT is the same real constant used for frictional heat generation. By default, FWGT = 0.5. For an input of true 0, you must enter a very small value (for example, 1E-8). If you enter 0, ANSYS interprets this as an input of the default value.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–49
Chapter 11: Contact
11.4.12. Modeling Magnetic Contact You can use surface-to-surface contact elements or the node-to-surface contact element to model magnetic flux across two contacted bodies. The following situations are possible. •
Non-perfect contact to account for the effects of a small air gap between mating components. This typically occurs at the interface between adjoining bodies. In this situation, there is a gap permeance effect where an MMF drop occurs. You can model this effect by inputting the gap permeance real constant, MCC. This option works best if the magnetic flux is normal to the gap interface.
•
Perfect contact across dissimilar meshes. This is typically used to model the air gap in a machine, for example, where the rotor and stator meshes meet.
For both types of magnetic contact, you must set KEYOPT(1) = 7 to select the degree-of-freedom option. For the 2-D case, the magnetic potential degree of fredom, AZ, is active. For the 3-D case, only the scalar potential degree of freedom, MAG, is active, and scalar potential formulations (reduced (RSP), difference (DSP), or general (GSP)) are available (see MAGOPT). Note — 3-D magnetic contact is not supported for the MVP formulation (AX, AY, AZ), and the edge-based formulation (AZ). Note — Non-perfect magnetic contact is only available for the 3–D contact elements, CONTA173 and CONTA174. For more information on which element types should be used for a particular analysis, see the element discussions in the appropriate chapter of the ANSYS Low-Frequency Electromagnetic Analysis Guide. For information on the use of the AZ degree of freedom, see Section 2.3.1.3: Specifying Element Types and Options. For more information on the use of the MAG DOF, see Section 5.3.5: Building the Model. For details on how to set up a contact analysis, see Steps in a Contact Analysis. For an example input listing showing a 2-D static magnetic contact analysis, see Section 2.6: Doing an Example 2-D Static Magnetic Contact Analysis (Command Method).
11.4.12.1. Using MCC The magnetic flux across the contacting interface is defined by: MFLUX = MCC x (Mt - Mc) where: MFLUX = magnetic flux density Mt , Mc = magnetic potential at the contact points on the target and contact surfaces MCC = contact permeance coefficient (Henries/meters2 in MKS units) The MCC value is input through a real constant, which can be a function of temperature [(Tt + Tc)/2], pressure, and time, by using the %TABLE% option. MCC values can be approximated as µ/t, where µ is the gap permeability and t is the gap width. If the “no-separation contact” or “bonded contact” option is set (KEYOPT(12) = 4 or 5), contact interaction can occur between two surfaces separated by a narrow gap.
11–50
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis
11.4.12.2. Modeling Perfect Magnetic Contact Perfect magnetic contact supports dissimilar meshes on both sides of the contacting interface (MCC = infinity). You must use the internal MPC approach by setting KEYOPT(2) = 2. You must also set KEYOPT(4) = 1 or 2 for contact nodal detection, and KEYOPT(12) = 5, 6 for bonded contact.
11.4.13. Applying Necessary Boundary Conditions to the Deformable Elements You can now apply any necessary boundary conditions as you would for any ANSYS analysis. For more information on applying boundary conditions, see the appropriate analysis descriptions in earlier chapters of this guide.
11.4.14. Defining Solution and Load Step Options Convergence behavior for contact problems depends strongly on the particular problem. The options listed below are either typical or recommended for most surface-to-surface contact analyses. Please see the ANSYS Commands Reference for further details. The time step size must be small enough to capture the proper contact zone. The smooth transfer of contact forces is disrupted if the time step size is too large. The time step size is specified by a number of substeps or the time step size itself. The following commands adjust these parameters. Command(s): NSUBST GUI: Main Menu> Preprocessor> Loads> Load Step Opts> Time/Frequenc> Freq and Substps Main Menu> Preprocessor> Loads> Load Step Opts> Time/Frequenc> Time and Substps Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Freq and Substps Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Time and Substps Command(s): DELTIM GUI: Main Menu> Preprocessor> Loads> Load Step Opts> Time/Frequenc> Time-Time Step Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc>Time-Time Step Note — A reliable way to set an accurate time step size is to turn automatic time stepping on. The following options are automatically invoked, but may override them if needed. Command(s): AUTOTS,ON GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Time-Time Step or Time and Substps If the contact status changes during the iteration process, discontinuity can occur. To avoid a slow convergence rate and use an updated stiffness matrix, set the Newton-Raphson option to FULL. Command(s): NROPT,FULL,,OFF GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–51
Chapter 11: Contact Also, do not use adaptive descent. Adaptive descent usually does not provide any help for surface-to-surface contact applications, and we recommend turning it off. In cases where frictional sliding dominates, set the unsymmetric solver option (NROPT, UNSYM,,OFF) to avoid slow convergence or divergence. Set the number of equilibrium equations to a number that is appropriate for a reasonable time step size. This command defaults to between 15 and 26 iterations, depending upon the physics of the problem. Command(s): NEQIT GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Nonlinear Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Equilibrium Iter Because the iterations tend to become unstable for large increments, use the line search option to stabilize the calculations. Command(s): LNSRCH GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Nonlinear Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Line Search Turn the predictor-corrector option on, except for large rotations or dynamic analyses. Command(s): PRED GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Nonlinear Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Predictor Many convergence failures in contact analyses are the result of using too large a value for contact stiffness (real constant FKN). Be sure to follow the recommendations given earlier in this chapter for estimating contact stiffness. If such estimated values lead to a convergence failure, reduce the contact stiffness and restart. Conversely, if overpenetration occurs in your contact analysis, you probably need a larger value of FKN. In this case, gradually increase the contact stiffness value to an appropriate level by redefining it using RMODIF commands over several load steps in a restart. Note — For most small strains, small displacements, and small sliding problems, set NLGEOM, OFF. This setting will speed up the searching time; however, if the contact problem involves large sliding, set NLGEOM, ON.
11.4.15. Solving the Problem You can now solve the analysis the same as you would for any nonlinear analysis. Keep the following points in mind: •
Always check the real constant sets which are related to contact pairs and check the constraint conditions on the target surfaces. Any previous "trial runs" could have changed the settings.
•
Always check the target surface contact status in the beginning of the analysis. If you detect any unexpected gap (or no contact) or overestimated penetration, abort the analysis and then check your geometric model. You can issue the CNCHECK command to verify the initial contact status.
•
If your model is experiencing convergence difficulties due to contact, use the NLHIST command as a debugging tool to monitor contact information during the solution. Before starting the solution, issue NLHIST to specify the pair-based contact items (such as contact penetration or gap, contact normal stiffness, etc.) to be tracked. The resulting data are written to a file named Jobname.nlh.
•
Always check your results carefully using standard engineering guidelines.
See Section 2.3.5: Solve the Analysis in Chapter 2, “Structural Static Analysis”. 11–52
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.4: Performing a Surface-to-Surface Contact Analysis If you are restarting a contact analysis, follow the normal restart procedures as discussed in Section 3.16: Restarting an Analysis in the ANSYS Basic Analysis Guide. However, be aware that the constraint conditions of target surfaces may have been set internally. Verify the constraints carefully before restarting an analysis. Only the real constants FKN, FTOLN, PINB, and FKOP can be changed, and they can only be changed at the point of restart or at the beginning of a new load step.
11.4.16. Reviewing the Results Results from a contact analysis consist mainly of displacements, stresses, strains, reaction forces, and the contact information (e.g., contact pressure, sliding, etc.). You can review these results in POST1, the general postprocessor, or in POST26, the time-history postprocessor. For contact-related results, you can select CONT as a plotting or list item. While in POST1, you can also review the results from within the Contact Manager (via the Contact Manager icon in the ANSYS Standard Toolbar). See the "Output Data" section of the element descriptions (the ANSYS Elements Reference) for the available output components. Remember that in POST1, only one substep can be read in at a time, and that the results from that substep should have been written to Jobname.RST (or Jobname.RCN for the initial contact configuration calculated by CNCHECK,POST). (The load step option command OUTRES controls which substep results are stored on Jobname.RST.) A typical POST1 postprocessing sequence is described below.
11.4.16.1. Points to Remember See Section 2.3.6.2: Points to Remember in Chapter 2, “Structural Static Analysis”.
11.4.16.2. Reviewing Results in POST1 The steps for reviewing results in POST1 are the same as those for a typical nonlinear analysis (see Section 8.5.6.2: Reviewing Results in POST1 in Chapter 8, “Nonlinear Structural Analysis”) with the following exceptions: For step 4, the following shows the various CONT options for the PLNSOL and PLESOL commands. CONT
STAT
Contact status. 3-closed and sticking, 2-closed and sliding, 1-open but near contact, 0-open and not near contact.
“
PENE
Contact penetration
“
PRES
Contact pressure
“
SFRIC
Contact friction stress
“
STOT
Contact total stress (pressure plus friction)
“
SLIDE
Contact sliding distance
“
GAP
Contact gap distance
“
FLUX
Heat flux at contact surface
“
CNOS
Total number of contact status changes during substep
Note — You can set these options through the Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu menu item. Choose Contact for Item, Comp and you'll see a list of the options detailed above. For rigid-to-flexible contact or asymmetric flexible-to-flexible contact, the contact element provides the true pressure and friction stress. However, for symmetric flexible-to-flexible contact, the true pressure and friction stress is the average of the pressures and friction stresses from both sides of the contact elements.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–53
Chapter 11: Contact Note — For the contact force-based model (KEYOPT(3) = 0) in CONTA175, PRES, SFRIC, and STOT are the contact normal force, contact friction force, and total contact force, respectively. Note that the contact-specific information (CONT) plots as follows. For 2-D contact analyses, the model will plot in gray and the requested item will be contoured as an area (trapezoid) along the edge of the model where the contact elements are located. Use the FACT item to scale 2-D contour size. For 3-D contact analyses, the model will plot in gray and the requested item will be contoured as a 2-D surface where the contact elements overlay the model. For tabular listings, you may also list contact-specific information by using the CONT label and its arguments with the PRNSOL or PRESOL commands or their related menu items You can also animate contact results over time. See the ANTIME command for details. Command(s): ANTIME GUI: Utility Menu> PlotCtrls> Animate> Over Time If you used CNCHECK,POST to evaluate the initial contact state, you can view the contact results items for the initial contact configuration as you would for any other load step. To do so, you must explicitly read the results of the first load step from the results file Jobname.RCN by issuing the FILE and SET,FIRST commands before postprocessing. Otherwise, the result file may be read improperly.
11.4.16.3. Reviewing Results in POST26 The steps for reviewing results in POST26 are the same as those for a typical nonlinear analysis See Section 8.5.6.3: Reviewing Results in POST26 in Chapter 8, “Nonlinear Structural Analysis”.
11.5. GUI Aids for Contact Analyses 11.5.1. The Contact Manager in the ANSYS Standard To use the GUI method, access the Contact Manager via the Contact Manager icon Toolbar, or via the menu path Preprocessor> Modeling> Create> Contact Pair. You can access the Contact Manager at the Begin level and in the following processors: preprocessor (PREP7), solution (SOLU), and general postprocessor (POST1). The Contact Manager Toolbar provides an intuitive interface for the creation and management of contact pairs. The manager supports surface-to-surface contact analysis, node-to-surface contact analysis (using CONTA175), and the internal multipoint constraint (MPC) method of contact .
Figure 11.24 Contact Manager Toolbar
•
Contact Wizard - Accesses the Contact Wizard GUI described in Section 11.5.2: The Contact Wizard. Allows you to manually define target and contact surfaces. Supports both 2-D and 3-D geometries as well as rigidflexible (with optional pilot node) or flexible-flexible contact. (Primitives are not supported by contact wizard.) The wizard also supports surface-based constraint contact pairs.
•
Contact Properties - Allows you to specify the properties of the contact pair(s) via real constants and KEYOPTs for the contact elements used.
11–54
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.5: GUI Aids for Contact Analyses •
Delete Contact Pairs - Deletes the contact pairs selected in the contact pair list.
•
Contact Selection Options - Specifies display of contact elements, target elements, or both.
•
Plot Elements/Results - Displays the elements of selected contact pairs; or displays the contact results, if available (POST1 only), specified in the Contact Results field for selected contact pairs. Results are displayed if Model Context is specified as “Result-”; otherwise, elements are displayed. The display can be limited to contact, or target, or both as specified in the Contact Selection Options field. (Note that CONTA175 results will not display graphically, but can be listed with the List Elements/Results icon.)
•
Show Normals - Specifies whether or not to display the normals on the elements when plotting contact pairs
•
Flip Normals - Flips the element normals of the selected contact pair. This action is limited to the elements specified in the Contact Selection Options field.
•
Switch Contact and Target - Inverts the target surface and the contact surface with each other. This is applicable only to flexible-to-flexible surface-to-surface contact pairs.
•
List Elements/Results - Lists the elements of the selected contact pairs; or lists the contact results, if available (POST1 only), specified in the Contact Results field for selected contact pairs. Results are listed if Model Context is specified as “Result-”; otherwise, elements are listed. The listing is restricted to the elements specified in the Contact Selection Options field.
•
Model Context - Displays the contact pairs in the context of the entire model using a translucent plot, or shows only the contact pairs. If set to “Result-” (POST1 only), controls display/listing of contact pair results.
•
Check Contact Status - Provides contact status information for selected contact pairs. Several options are available (click and hold down the Check Contact Status button to access these options):
•
–
Display a detailed listing of status information for each contact pair.
–
Run a partial solution of the initial contact state (CNCHECK,POST command) that can be subsequently postprocessed from the contact manager. (See CNCHECK for more information.)
–
Physically move contact nodes to the target surface (CNCHECK,ADJUST command) in order to close a gap or reduce a penetration (see Section 11.4.8.8: Physically Moving Contact Nodes Towards the Target Surface.)
Contact Results - Shows the contact result items for subsequent viewing using the Plot Elements/Results and List Elements/Results icons.
The bar below the toolbar icons minimizes or maximizes the Contact Pair list box below it. The Contact Pair list box displays the defined contact pairs. You can select contact pairs from this list for displaying or editing purposes.
11.5.2. The Contact Wizard This Contact Wizard will lead you through the process of manually creating contact pairs. The wizard supports rigid-flexible (with optional pilot node) and flexible-flexible contact, and supports both surface-to-surface and node-to-surface configurations. (Note that the wizard does not support rigid target primitives.) The Contact Wizard also supports surface-based constraint contact pairs. To use the Contact Wizard, access the Contact Manager Toolbar and click on the Contact Wizard icon. The wizard steps you through setting up the contact analysis. Below is an example of the screens you will see.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–55
Chapter 11: Contact
Figure 11.25 Example of a Contact Wizard Dialog
The Contact Wizard remains unavailable (dimmed) if you haven't meshed any portion of your model. If you wish to create a rigid-flexible model, mesh only those parts of the model which will be used as flexible contact surfaces (do not mesh the rigid target surfaces) before launching the wizard. If you wish to create a flexible-flexible model, mesh all parts of the model which will be used as contact surfaces (including target surfaces) before launching the wizard. You can specify target and contact surfaces using lines, areas, volumes, selected set of nodes, or node components. Note that the wizard allows you to choose more than one area for the target and contact surfaces, thus allowing multiple areas to form a single contact surface. If you specify a rigid target surface, you will then have the option to define a pilot node for that contact pair. (The pilot node step is mandatory if you define a surface-based constraint contact pair by picking the Pilot Node Only option.) After you specify the target and contact surfaces, you can specify properties of the contact pair (real constants and KEYOPTs) before creating the contact pair. When you finish specifying all the required data, click the Create button to create the contact and target element types, a unique real constant set with the real constant values, and the elements that make up the contact and target surfaces.
11.5.3. Managing Contact Pairs As discussed in Section 11.4: Performing a Surface-to-Surface Contact Analysis it is paramount that the contact elements be oriented correctly for proper contact detection. The contact manager provides tools that help you 1.
Verify that the normals of the contact and target surfaces are in the correct direction
2.
Reverse normals of elements that are not oriented correctly
11–56
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.6: Performing a Node-to-Surface Contact Analysis You can choose to display one or more contact pairs on which to perform the above listed operations. Then you have an additional option of only displaying the contact surface or the target surface when verifying or reversing the element normals. In addition these elements can be displayed independently or in the context of your entire model. In the later case the contact elements are highlighted in a translucent plot of your model. Another important function is to edit the properties of the contact pair(s) as needed. The properties include real constant values and key option values as discussed earlier. The Contact Properties button in the contact manager provides a simple to use interface that allows the properties of the selected contact pair(s) to be reviewed and modified if needed. Note that when you have multiple contact pairs, it is possible to have conflicts in the real constant values or in the KEYOPT settings. When you have such conflicts, the properties dialog for those real constants or KEYOPT settings is left blank. Finally, you can display or list specific contact result items (contact status, penetration, pressure, etc.) for the selected contact pairs. This option is only available in POST1, and only if a result set is available. The contact results can be displayed independently or in the context of your entire model. (For CONTA175, results can be listed but not displayed graphically.) Note — Prior to displaying or listing result items associated with the initial contact configuration resulting from the CNCHECK,POST command, you need to issue the appropriate FILE and SET,FIRST commands to read the results from the proper results file (see CNCHECK for details).
11.6. Performing a Node-to-Surface Contact Analysis You can use our node-to-surface contact element CONTA175 to model flexible-flexible or rigid-flexible contact between a surface and a node. Additionally, you can use these elements to represent contact between two surfaces by specifying one surface as a group of nodes. Node-to-surface contact is a phenomenon that occurs in most engineering applications: fasteners (nuts, bolts, rivets, pins), metal forming, rolling operations, dynamic pipe whip, etc. Engineers are interested in the stresses, deflections, forces, and temperature changes that occur due to contact between structural parts.
11.6.1. Using the Node-to-Surface Contact Elements Node-to-surface contact is represented in the ANSYS program by following the positions of points on one surface (the contact surface, modeled by CONTA175) relative to lines or areas of another surface (the target surface, modeled by TARGE169 or TARGE170). CONTA175, in two or three dimensions, is depicted in Figure 11.26: “Node-to-Surface Contact Elements”.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–57
Chapter 11: Contact
Figure 11.26 Node-to-Surface Contact Elements
: 64 5-7 '8.29 @BADCBE=F<@HGIDCJKAML !" # $% &')(+*-,+. / 0
> ;<=( <
465-7 '8.29
@NAMCNEOF<@HG
>
Presented below are characteristics of CONTA175: •
Has one node and its target surface is defined by TARGE169 or TARGE170. CONTA175 uses the same real constant set as the surface-to-surface contact elements. See Real Constants for more information.
•
Supports 2-D/3-D rigid-flexible and flexible-flexible contact.
•
Does not support 3-D contact surfaces with midside nodes, but can support 2-D/3-D target surfaces with midside nodes or 2-D contact surfaces with midside nodes.
•
Generates elements using the ESURF command, as do the surface-to-surface contact elements.
•
Supports structural, thermal, electric, and magnetic analyses. Note — CONTA175 is recommended for point-to-surface or edge-to-surface problems. It can also be used to supplement a surface-to-surface pair at strategic locations where edge contact exists. For general surface-to-surface contact, CONTA171 through CONTA174 are recommended.
CONTA175 follows the contact pair concept used by surface-to-surface elements CONTA171 through CONTA174. CONTA175 is paired off with target elements TARGE169 and TARGE170. See Identifying Contact Pairs for more information. CONTA175 uses most of the same element KEYOPTS and real constants as the surface-to-surface contact elements. These are described below. You should avoid midside-noded underlying elements of the contact surface, especially in 3-D. The “effective stiffness” at the contact surface nodes is very nonuniform. For instance, for the 20-node bricks SOLID95 or HYPER86, the corner nodes have a negative stiffness associated with them. However, the node-to-surface contact algorithm assumes that the stiffness is uniformly distributed across all the surface nodes when contact is made. This condition can lead to convergence difficulties when using midside-noded elements in contact. The midside-noded elements can only be used when bonded or no-separation contact is defined. You can still use midside nodes on 2-D contact surfaces or on 2-D/3-D target surfaces. The basic steps for performing a node-to-surface contact analysis using CONTA175 are the same as those used for a typical surface-to-surface analysis using CONTA171 through CONTA174. See Steps in a Contact Analysis for details. The Contact Manager provides an easy-to-use interface to help you construct and manage contact definitions. You can access the manager via the Contact Manager icon
11–58
in the ANSYS Standard Toolbar, or via the menu
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.6: Performing a Node-to-Surface Contact Analysis path Main Menu> Preprocessor> Modeling> Create> Contact Pair. See Section 11.5: GUI Aids for Contact Analyses for more information on using the Contact Manager. As mentioned, CONTA175 uses the ESURF command to generate elements between corresponding contact pairs, similar to the surface-to-surface contact elements. The GUI path is: Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Node to Surf Since CONTA175 is a one node element, you are not able to plot the contact results. However, you can list the results using the PLESOL,CONT or PRETAB commands.
11.6.1.1. CONTA175 KEYOPTS CONTA175 uses most of the same KEYOPTS that are used by the surface-to-surface contact elements CONTA171 through CONTA174. KEYOPT(3) and KEYOPT(4) are used but have different meanings when used with CONTA175. See Section 11.4.8.2: Element KEYOPTS for a listing of the remaining KEYOPTS.
11.6.1.1.1. KEYOPT(3) KEYOPT(3) in CONTA175 allows you to choose between a contact force-based model (KEYOPT(3) = 0, default), and a contact traction-based model (KEYOPT(3) = 1). For the contact traction-based model, ANSYS can determine the area associated with the contact node. For the single point contact case, a unit area will be used which is equivalent to the contact force-based model. When the traction-based model is defined, the real constants FKN, FKT, TCC, ECC, and MCC have the same units used in surface-to-surface contact elements (CONTA171 through CONTA174), as do postprocessing items PRES, TAUR, and TAUS. When the force-based model is defined, the units of these quantities have a factor of AREA with respect to those used in the traction-based model. For instance, contact stiffness FKN has units FORCE/LENGTH for the forcebased model, but FORCE/LENGTH3 for the traction-based model. PRES is the contact normal force in the forcebased model, but contact pressure in the traction-based model.
11.6.1.1.2. KEYOPT(4) KEYOPT(4) in CONTA175 allows you to choose the contact normal direction. The contact normal can be either perpendicular to the target surface (KEYOPT(4) = 0, default or KEYOPT(4) = 3), or perpendicular to the contact surface (KEYOPT(4) = 1, 2). When contact occurs on the bottom surface of a shell or beam, and shell thickness effect is included (KEYOPT(11) = 1), or CNOF is defined, KEYOPT(4) = 2 or 3 should be used in order to capture the contact. Real constant TOLS is used to add a small tolerance that will internally extend the edge of the target surface. TOLS is useful for problems where contact nodes are likely to lie on the edge of the target (as at symmetry planes or for models generated in a node-to-node contact pattern). In these situations, the contact node may repeatedly “slip” off the target surface and so completely out of contact, resulting in convergence difficulties from oscillations. Units for TOLS are percent (1.0 implies a 1.0% increase in the target edge length). A small value of TOLS will usually prevent this situation from occurring. The default value is 10 for small deflection and 2 for large deflection (NLGEOM,ON).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–59
Chapter 11: Contact
11.6.1.2. CONTA175 Real Constants CONTA175 uses the same real constants used by the surface-to-surface contact elements CONTA171 through CONTA174), except the units of TCC, ECC, and MCC for the contact force-based model. See a listing of the real constants in Section 11.4.8.1: Real Constants.
11.6.1.3. Multiphysics Contact You can use node-to-surface contact element CONTA175 to model thermal contact, electric contact, and magnetic contact as you would use the surface-to-surface contact elements. For multiphysics contact, we recommend that you use the contact traction-based model (KEYOPT(3) = 1), which allows you to use TCC, FCC, and MCC consistently with the surface-to-surface contact elements. If you use the contact force-based model (KEYOPT(3) = 0), you should adjust the values of TCC, ECC, and MCC up or down as you make the element mesh coarser or finer.
11.7. Using the Internal MPC Approach for Assemblies and Kinematic Constraints You can use the internal multipoint constraint (MPC) approach (KEYOPT(2) = 2), in conjunction with the bonded contact definition (KEYOPT(12) = 5 or 6), to define various contact assemblies and kinematic constraints. This capability is available for contact elements CONTA171, CONTA172, CONTA173, CONTA174, and CONTA175. By this method, the program builds MPC equations internally based on the contact kinematics. You can use this method to model the following contact assemblies and surface-based constraints: •
Solid-solid assembly - both contact and target surfaces paste onto solid element faces
•
Shell-shell assembly - both contact and target surfaces paste onto shell element faces
•
Shell-solid assembly - the contact surface pastes onto shell element faces and the target surfaces paste onto solid element faces
•
Rigid constraint surface - the contact nodes are constrained to the rigid body motion defined by the pilot node (similar to the CERIG command)
•
Force-distributed surface - the forces or displacements applied to the pilot node are distributed to contact nodes, in an average sense, through shape functions (similar to the RBE3 command)
•
Beam-solid assembly - one beam end-node is the pilot node which connects to the solid or shell surface (use the rigid constraint surface or force-distributed surface type of MPC)
The internal MPC approach can overcome the drawbacks of the traditional contact algorithms and other multipoint constraint tools available in ANSYS. For example: •
Degrees of freedom of the contact surface nodes are eliminated. This reduces the wave front size of the system equation solver.
•
No contact stiffness is required as input. For a small deformation problem, this represents true linear contact behavior; no iteration is needed in solving the system of equations. For large deformation problems, the MPC equations are updated during each iteration. This overcomes the small strain restriction in conventional constraint equations.
•
Both translational and rotational degrees of freedom can be constrained.
•
The generation of internal MPC is simple because it utilizes contact pair definitions.
•
Shape functions are taken into account automatically; no weight factor is needed for a force-distributed multipoint constraint (which is similar to the RBE3 command) if high order elements or axisymmetric
11–60
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints elements are used. In addition to forces, displacements can be applied on the pilot node for this type of MPC. The following sections describe how to use the internal MPC approach to define assemblies and surface-based constraints. Before using the internal MPC feature, be sure to review Section 11.7.4: Restrictions and Recommendations for Internal MPC.
11.7.1. Modeling Solid-solid and Shell-shell Assemblies To define solid-solid or shell-shell assemblies using the internal MPC approach, you must set the following key options on the contact elements: KEYOPT(2) = 2 - MPC based approach KEYOPT(12) = 5 or 6 - Bonded always or bonded initial KEYOPT(4) = 1 or 2 - Nodal detection for CONTA171, CONTA172, CONTA173, CONTA174 KEYOPT(4) = 0 or 1 - Contact normal direction for CONTA175 The following key options are ignored: KEYOPT(8) (it is always set to 2 internally), KEYOPT(10). The following real constants are used: R1, R2, ICONT, PINB, CNOF, PMAX, PMIN, TOLS. All other real constants are ignored. This function works similarly to the CEINTF command for small deformation analysis (NLGEOM,OFF). Comparing it to the CEINTF command, the contact surface acts as “region A nodes,” and the target surface acts as “region B elements.” As usual, the contact surface must be defined on the deformable bodies, and the target surface must be defined on either deformable or rigid bodies in the contact pair. In order to prevent over-constraint, only asymmetric contact is supported. If symmetric pairs are defined, ANSYS will automatically pick one pair and ignore the other pair (acting as KEYOPT(8) = 2). The self-contact pair definition is not supported. If the temperature degree of freedom is active in the model (KEYOPT(1) = 1 or 2), ANSYS will build MPC equations not only for structural degrees of freedom, but also for the temperature DOF. In this case, the real constant TCC is ignored. If only the temperature DOF is set (KEYOPT(1) = 2) and other solution options are defined (ANTYPE,,TRANS; THOPT,QUASI; EQSLV,JCG/ICCG), the internal MPC approach can support fast thermal transient analysis (see Section 3.5.4: Nonlinear Options in the ANSYS Thermal Analysis Guide). Internal MPC equations for temperature DOF are built to support heat transfer between the two bonded surfaces. For the “bonded always” option (KEYOPT(12) = 5), any contact node that lies inside the pinball region (PINB) can be the constrained node in the MPC definition if an intersection with the target surface is detected in the contact normal direction. This holds true at the beginning of deformation, as well as during the deformation process. A relatively small PINB may be used to prevent any false contact. When the “bonded always” option is set, the default for PINB is 0.25 (25% of the contact depth) for small deformation analysis (NLGEOM,OFF), and 0.5 (50% of the contact depth) for large deformation analysis (NLGEOM,ON). (The default PINB value may differ from what is described here if CNOF is input. See Section 11.4.8.9.2: Using PINB for more information.) For the “bonded initial” option (KEYOPT(12) = 6), only those contact nodes that are initially in contact or have a very small gap but lie inside the adjustment zone (ICONT) are always constrained via internal MPC. Those contact nodes that are initially open will never be constrained, even though they may later penetrate into the target surface during the deformation process. In order to capture contact, you should specify proper ICONT or CNOF values. Use CNCHECK in conjunction with ICONT to move all the contact nodes that are inside the ICONT zone onto the target surface in the initial configuration, without causing any strain. When the “bonded initial” option is set and KEYOPT(5) = 0 or 4, ICONT defaults to 0.05. See Section 11.4.8.7: Adjusting Initial Contact Conditions for more information on using KEYOPT(5), CNOF, and ICONT. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–61
Chapter 11: Contact In most cases, ANSYS will automatically constrain the translational degrees of freedom for a solid-solid assembly and constrain both translational and rotational degrees of freedom for a shell-shell assembly. However, you can use KEYOPT(5) of the target element (TARGE170) to explicitly define the type of constraint: KEYOPT(5) = 0 - Auto constraint type detection KEYOPT(5) = 1 - Solid-solid constraint (no rotational DOFs are constrained) KEYOPT(5) = 2 - Shell-shell constraint (both translational and rotational DOFs are constrained)
11.7.2. Modeling a Shell-solid Assembly The 3-D shell-solid assembly provides a transition from a shell element region to a solid element region. This approach is useful when local modeling requires a full three-dimensional model with a relatively fine mesh, but other parts of the structure can be represented by shell elements (see Figure 11.27: “Example of Shell-solid Assembly”). No alignment is required between the solid element mesh and the shell element mesh. The contact surface or edge must be built on the shell element side. The target surface must be built on the solid elements side.
Figure 11.27 Example of Shell-solid Assembly
!
To define a shell-solid assembly using the internal MPC approach, you must set the following key options on the contact elements: KEYOPT(2) = 2 - MPC based approach. KEYOPT(12) = 5 or 6 - Bonded always or bonded initial KEYOPT(4) = 1 or 2 - Nodal detection for CONTA171, CONTA172, CONTA173, CONTA174 KEYOPT(4) = 0 or 1 - Contact normal direction for CONTA175 11–62
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints The following real constants are also used: ICONT, FTOL, PINB, CNOF, PMAX, PMIN, TOLS. The following key options are ignored: KEYOPT(8), KEYOPT(10), KEYOPT(1)>0. In most cases, ANSYS will automatically constrain both translational and rotational degrees of freedom for a shell-solid assembly (see Figure 11.28: “Shell-solid Assembly (Original Mesh)”). However, you can use KEYOPT(5) of the target element (TARGE170) to explicitly define the type of constraint: KEYOPT(5) = 0 - Auto constraint type detection KEYOPT(5) = 1 - Solid-solid constraint; no rotational DOFs are constrained (see Figure 11.29: “Shell-solid Assembly with Solid-solid Constraint Option”) KEYOPT(5) = 2 - Shell-shell constraint; both translational and rotational DOFs are constrained (see Figure 11.30: “Shell-solid Assembly with Shell-shell Constraint Option”) KEYOPT(5) = 3 - Shell-solid constraint; both translational and rotational DOFs are constrained on shell nodes, only translational DOFs are constrained on solid nodes (see Figure 11.31: “Shell-solid Assembly with Shellsolid Constraint Option”) KEYOPT(5) = 4 - Shell-solid constraint, all directions. This option acts the same as KEYOPT(5) = 3 if an intersection is found from the contact normal to the target surface. Otherwise, constraint equations are still built as long as contact nodes and target segments are inside the pinball region. The solid-solid and shell-shell constraint types (KEYOPT(5) = 1 or 2) may require additional shell elements at the interface. These shell elements can be defined by typical modeling methods, or you can use the SHSD command to generate these elements automatically. SHSD is a meshing tool used to build solid-solid and shell-shell constraint types. This command can be used only when the contact pair consists of CONTA175 and TARGE170 elements. Additional shell elements (SHELL181) and/or contact elements (CONTA175) are created through this command (see the SHSD command description for more information). For the shell-solid constraint type, no special mesh tool is required.
Figure 11.28 Shell-solid Assembly (Original Mesh)
#%$ & ' ' & ' &()&*+-, .+$ / 021* &,,3 4 !" #65 ' / 78& ' &(&*+,
9!:;< &2+ & ' &(&*+, 9=?>A@B%CDE .5*F+5G)5 H ,!5 ' / 7 4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–63
Chapter 11: Contact
Figure 11.29 Shell-solid Assembly with Solid-solid Constraint Option
!"! $#&%('')*+) 4 !<J9 6 6 A"" 7 K#KK8L 2MN" !A> / 2!6 !D / : FEG )HI ,.-0/ 1 2!3 54 6 !3 7 2!98:<;92! => 5 ? @ 32 A< CB
Figure 11.30 Shell-solid Assembly with Shell-shell Constraint Option
O P3QRS TU VWX K YZ PX X P X P!["P!\U Y b n W!\
].^0_P`VWU7S a!\ Y b U T6W!\ Y X WU7S a!\
11–64
g s0f"t O b S \ i X VP!\ n PNj!S Y UW!\ n Ph
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints
Figure 11.31 Shell-solid Assembly with Shell-solid Constraint Option
! " # $
% &('*)+ , $-. / $- 0
For the shell-solid constraint option (KEYOPT(5) = 3 on TARGE170), ANSYS automatically creates an internal set of force-distributed constraints (similar to the RBE3 command) between nodes on the shell edges and nodes on the solid surface. The program uses the pinball region (PINB), initial adjustment zone (ICONT), and influence distance (FTOLN) to determine which nodes on the shell edge will be constrained with which nodes on the solid surface. Each shell node acts as the master node, and associated solid nodes act as slave nodes. For the “bonded always” option (KEYOPT(12) = 5), any shell node that lies inside the pinball region (PINB) will be included in the constraint if an intersection with the target surface is detected in the contact normal direction. This holds true at the beginning of deformation, as well as during the deformation process. A relatively small PINB value may be used to prevent any false contact. The default for PINB is 0.25 (25% of the contact depth) for small deformation analysis (NLGEOM,OFF), and 0.5 (50% of the contact depth) for large deformation analysis (NLGEOM,ON). (The default PINB value may differ from what is described here if CNOF is input. See Section 11.4.8.9.2: Using PINB for more information.) For the “bonded initial” option (KEYOPT(12) = 6), only the shell nodes that initially lie inside the adjustment zone (ICONT) are included in the constraint sets. Shell nodes that lie outside ICONT are not constrained with the solid nodes. The default for ICONT is 0.05 (5% of the contact depth). The influence distance (FTOLN) is used for the shell-solid constraint option (KEYOPT(5) =3 on TARGE170). Each solid node is included in the constraint set if the perpendicular distance from the solid node to any shell edge is smaller than the influence distance. FTOLN defaults to half the thickness of the shell. A positive FTOLN value represents a scaling factor on the shell half-thickness, and a negative value represents an absolute distance value. A shell-solid assembly can be used in a substructure analysis. However, if a superelement is defined to represent the shell elements, shell thickness is unknown in the use pass. In this case, you must overwrite the default setting of FTOLN (originally a factor of the shell thickness) to account for the zero thickness of the superelement. Input an absolute value for FTOLN (that is, input a negative value) to capture all constrained nodes when the constraint equations are built.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–65
Chapter 11: Contact Among the four constraint types, the shell-shell constraint approach (KEYOPT(5) = 2 on TARGE170) often provides a better solution. The solid-solid constraint (KEYOPT(5) = 1) can result in higher local stresses near the interface between the virtual shell surface and solid surface. The shell-solid constraint (KEYOPT(5) = 3 or 4 ) is not always capable of transmitting all components of the moment at the shell nodes due to transverse shear locking of shell elements. A typical example is the moment component that parallels to the normal of the solid surface. The KEYOPT(5) = 4 option (shell-solid constraint , all directions) is recommended for detecting contact in bodies that do not overlap or intersect. For the solid-solid and shell-shell constraint types (KEYOPT(5) = 1 or 2 on TARGE170), any initial penetration or gap is closed if KEYOPT(9) = 0; the initial penetration or gap remains if KEYOPT(9) = 1. However, for the shellsolid constraint type (KEYOPT(5) = 3 or 4), KEYOPT(9) is ignored, and initial penetration or gap always remains constant. In order to close the initial penetration or gap, issue the command CNCHECK,ADJUST in the beginning of the analysis.
11.7.3. Surface-based Constraints A surface-based constraint can be used to couple the motion of nodes on the contact surface to a single pilot node on the target surface. The multipoint constraint (MPC) capability of the contact elements (KEYOPT(2) = 2) allows you to define two types of surface-based constraints: •
Rigid constraint surface - In this type of constraint, the contact nodes are constrained to the rigid body motion defined by the pilot node (see Figure 11.32: “Rigid Constraint Surface”). This is similar to a constraint defined by the CERIG command.
•
Force-distributed constraint surface - In this type of constraint, forces or displacements applied on the pilot node are distributed to contact nodes (in an average sense) through shape functions (see Figure 11.33: “Force-distributed Surface”). This is similar to a constraint defined by the RBE3 command.
Figure 11.32 Rigid Constraint Surface "!$# %'&
*)+ ,- )/.0 ()0 1 )2 34
+ 5 1 6 (
11–66
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints
Figure 11.33 Force-distributed Surface !#"%$ &('
*+,- .,. /0 ,1*+
2
)
3 4 3
These surface-based constraints can be used in the following applications: •
To apply loads and boundary conditions to the pilot node (such as torque load or drill rotation). Example: a bolt head submitted to a torque force using a force-distributed surface constraint.
•
To model rigid end conditions. Example: using a rigid constraint surface to model a rigid end plate or rigid plane section of 3-D solid elements.
•
To define transitions between solid and structure elements. Example: a beam element connected to a solid element face.
11.7.3.1. Defining Surface-based Constraints The contact surface can be generated via the ESURF command. The contact nodes on the contact surface are the slave nodes of the MPC equations. The pilot node is the only target segment on the target surface side. It is the master node of the MPC equations. Forces and displacements can be applied on the pilot node. For a force-distributed surface constraint, use the following contact element key options: KEYOPT(2) = 2 - MPC based approach KEYOPT(12) = 5 or 6 - Bonded always or bonded initial (the two cases are the same) KEYOPT(4) = 1 - Nodal detection for CONTA171, CONTA172, CONTA173, CONTA174; Contact normal direction for CONTA175 For a rigid constraint surface, use the following contact element key options: KEYOPT(2) = 2 - MPC based approach KEYOPT(12) = 5 or 6 - Bonded always or bonded initial (the two cases are the same) KEYOPT(4) = 2 - Nodal detection for CONTA171, CONTA172, CONTA173, CONTA174 KEYOPT(4) = 0 - Contact normal direction for CONTA175 The following key options are ignored for surface-based constraints: KEYOPT(8), KEYOPT(5), KEYOPT(7), KEYOPT(10). Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–67
Chapter 11: Contact None of the standard contact real constants are used for surface-based constraints using internal MPC. KEYOPT(1) > 0 is ignored for a force-distributed surface constraint since only structural degree-of-freedom constraints are included. However, for a rigid constraint surface, you can use KEYOPT(1) to include other field degrees of freedom (in addition to the structural DOFs) in the constraint sets. You can specify the surface-based constraint in a local coordinate system. For the rigid constraint surface, rotate the contact nodes into a local coordinate system. For the force-distributed constraint, rotate the pilot node into a local coordinate system. You can apply the surface based constraint to a user-defined DOF set with respect to the global or the local coordinate system by using KEYOPT(4) of the target element (TARGE169 or TARGE170). For example, for the 3-D case (TARGE170), you might specify that only UX, UY, and ROTZ be used in the constraint. You can do this by entering a six digit value for KEYOPT(4). The first to sixth digits represent ROTZ, ROTY, ROTX, UZ, UY, UX, respectively. The number 1 (one) indicates the DOF is active, and the number 0 (zero) indicates the DOF is not active. Therefore, to specify that UX, UY, and ROTZ be used in the constraint, you would enter 100011 as the KEYOPT(4) value. For a force-distributed surface constraint, these additional guidelines apply: •
The pilot node is a dependent node (meaning the degrees of freedom for this node are removed). The contact nodes are independent nodes (the degrees of freedom are retained). If the pilot node has constraints applied to it, internally-generated MPCs are rewritten so that the degrees of freedom of the pilot node are no longer dependent DOF.
•
The pilot node has up to 3 degrees of freedom (2-D) or up to 6 degrees of freedom (3-D).
•
KEYOPT(4) of TARGE169 and TARGE170 controls the number of degrees of freedom of the pilot node.
•
The number of internally-generated MPCs is equal to the number of degrees of freedom defined by KEYOPT(4) of TARGE169 and TARGE170.
For a rigid constraint surface, these additional guidelines apply: •
The pilot node is an independent (retained) node in the constraint equation. The contact nodes are the dependent (removed) nodes. You should not apply any displacement constraints, coupling (CP command), or constraint equations (CE command) on the contact nodes.
•
The pilot node has 6 degrees of freedom (3-D) or 3 degrees of freedom (2-D).
•
KEYOPT(4) of TARGE169 and TARGE170 controls the DOF set (the number of DOF) of the contact (dependent) nodes used in the internally-generated MPCs.
•
The number of internally-generated MPCs is equal to (number of contact nodes) x (number of DOF).
11.7.3.2. Modeling a Beam-solid Assembly The surface-based constraint technique can be used to apply transitions between solid and structure elements; for example, a beam element connected to the solid or shell element face. One beam end node must be the pilot node and the solid/shell nodes must be the contact nodes. Generally speaking, the rigid constraint surface is well suited for the solid beam to solid surface case (see Figure 11.34: “Beam-solid Assembly Defined by Rigid Constraint Surface”) and the force-distributed constraint surface is well suited for the flexible beam (such as a thin wall beam) to solid/shell surface case (see Figure 11.35: “Beam-solid Assembly Defined by Force-distributed Surface”).
11–68
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.7: Using the Internal MPC Approach for Assemblies and Kinematic Constraints
Figure 11.34 Beam-solid Assembly Defined by Rigid Constraint Surface
!
Figure 11.35 Beam-solid Assembly Defined by Force-distributed Surface
"$# %& &'%& %( %)*!+ ./ & 0*) 0 1 %
, %-(%& %( %)*+
230)* - 4 *%& %( %)5*!+
11.7.4. Restrictions and Recommendations for Internal MPC The following restrictions apply when using the internal MPC approach.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–69
Chapter 11: Contact Generally speaking, displacement boundary conditions and other constraint equations or coupling equations should not be applied on the contact nodes for solid-solid, shell-shell, and shell-solid assemblies, and also for the rigid constraint surface MPC. Otherwise, over-constraint can occur since the degrees of freedom of contact nodes are eliminated through internal MPC equations. Sparse, PCG, and AMG solvers are recommended to solve models with constraint equations. In certain cases, the frontal solver may not solve problems containing constraint equations. The MPC based algorithm must work with nodal detection (KEYOPT(4) = 1 or 2) for CONTA171, CONTA172, CONTA173, and CONTA174. If nodal detection is not set, ANSYS will issue a warning message and automatically set KEYOPT(4) = 2. The internal MPC option does not support rigid-flexible contact when rigid surfaces are modeled by any primitive segments (such as circle, cylinder, cone, or sphere). The shell-solid assembly is usually used for the case where the solid mesh is fine with respect to the shell thickness. The shell-solid interface should be located in a region of the structure where shell theory is valid for an approximation. The accuracy of local stresses near the shell-solid interface (at least within the shell thickness range) is not guaranteed. We recommend you include at least two solid elements along the layer of the shell-solid interface. Using the force-distributed constraint type of MPC with a large number of contact nodes can result in a large wavefront for the global stiffness matrix. This may significantly increase the peak memory required during of element stiffness assembly. Consider reducing the number of contact nodes if real memory or virtual memory is limited. The contact related postprocessing items (ETABLE items, PRESOL,CONT, etc.) are not supported for the internal MPC option.
11.8. Performing a Node-to-Node Contact Analysis You can use node-to-node contact elements to model point-to-point contact (flexible-flexible or rigid-flexible). Additionally, you can use these elements to represent contact between two surfaces by specifying individual node-to-node contact between the opposing nodes of each surface. This use requires that the nodes of the two opposing surfaces match up geometrically and that the relative sliding between the two surfaces will be negligible. In addition, the deflections (rotations) of the two surfaces must remain small. The most commonly used node-to-node elements are shown in the following figure.
Figure 11.36 Node-to-Node Contact Elements
! " #
11–70
! %$ &
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.8: Performing a Node-to-Node Contact Analysis In terms of solution CPU time, the elements shown are the simplest and least expensive of all contact element types. When modeling conditions warrant their use, they can be an effective tool for modeling a variety of contact situations. CONTA178 offers more features and flexibility than CONTAC12 and CONTAC52. The following lists the features available with CONTA178: •
More contact algorithms, including the Lagrange method (KEYOPT(2))
•
Semiautomatic contact stiffness (real constants FKN-FKS)
•
More flexibility for defining contact normal
•
More contact behaviors (KEYOPT(10))
•
Cylindrical gap with friction (KEYOPT(4) = 4)
•
Damper (real constants CV1, CV2) Note — CONTA178 supports only elastic Coulomb friction behavior. For rigid Coulomb friction models, use CONTAC12 and CONTAC52
The procedure for performing a node-to-node contact analysis is similar to that described for the node-to-surface contact elements in Section 11.6: Performing a Node-to-Surface Contact Analysis. The following describes the typical steps in a node-to-node contact analysis. Each of these steps is explained in detail. 1.
Create the geometry and mesh the model.
2.
Generate the contact elements.
3.
Define the contact normal.
4.
Define the initial interference or gap.
5.
Select the contact algorithm.
6.
Apply the necessary boundary conditions.
7.
Define the solution options.
8.
Solve the problem.
9.
Review the results.
11.8.1. Creating Geometry and Meshing the Model Node-to-node contact elements transmit forces at the nodes (compared to surface-to-surface contact elements which transmit pressures at Gauss points). This feature limits their use to low order elements only. You must identify where contact might occur during the deformation of your model. The nodes on the two surfaces of potential contact must line up. Once you've identified potential contact surfaces and created an adequate mesh you can create the contact elements.
11.8.2. Generating Contact Elements You can generate node-to-node contact element in one of two ways: 1.
Use the direct generation method: Command(s): E GUI: Main Menu> Preprocessor> Modeling> Create> Elements> User Numbered> Thru Nodes
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–71
Chapter 11: Contact 2.
Use the EINTF command to generate the contact elements automatically at coincident nodes or offset nodes. This is discussed in detail in the following subsections.
11.8.2.1. Generating Contact Elements Automatically at Coincident Nodes If the two bodies are in the “just touching” position, you can use the EINTF command to automatically generate the contact elements. In this case, the menu path is Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> At Coincident Nodes. Only nodes within the tolerance value set in the first argument (TOLER) are considered as coincident. If you wish to check a subset of nodes for coincidence, first select all the nodes you wish to check using the NSEL command.
11.8.2.2. Generating Contact Elements Automatically at Offset Nodes If the two bodies are separated by a gap, the EINTF command can be used to create elements between offset nodes by specifying the node location increments (DX, DY, DZ) in the coordinate system KCN. The GUI path is Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Offset Nodes. If KOPT is set to 1, the nodes belonging to the contact elements created are rotated into the coordinate system KCN. For example, the following figure shows contact between two concentric pipes separated by a gap. In this example, KCN would be a cylindrical coordinate system centered in O, and DX would be set in ∆ (∆± TOLER).
Figure 11.37 Contact Between Two Concentric Pipes
11.8.2.3. Node Ordering Node ordering can be critical in determining the contact normal. You can use EINTF,,,LOW or EINTF,,,HIGH to control node ordering. When using the LOW argument, the 2-node elements are generated from the lowest numbered node to the highest numbered node. When using HIGH, 2-node elements are generated from the highest to the lowest. To check the contact normal, use /PSYMB,ESYS. If you discover that the ordering is incorrect, you can reverse it using EINTF,,,REVE. To determine which side of the interface contains the I nodes, use the following commands: ESEL,,ENAME,,178 NSLE,,POS,1 ESLN
11–72
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.8: Performing a Node-to-Node Contact Analysis NSLE EPLOT
11.8.3. Defining the Contact Normal The contact normal direction is of primary importance in a contact analysis with CONTA178. By default [KEYOPT(5) = 0 and NX, NY, NZ = 0], ANSYS will calculate the contact normal direction based on the initial positions of the I and J nodes, such that a positive displacement (in the element coordinate system) of node J relative to node I opens the gap. However, you must specify the contact normal direction for any of the following conditions: •
If nodes I and J have the same initial coordinates.
•
If the model has an initial interference condition in which the underlying elements' geometry overlaps.
•
If the initial open gap distance is very small.
In the above cases, the ordering of nodes I and J is critical. The correct contact normal usually points from node I toward node J unless contact is initially overlapped. You can specify the contact normal by means of real constants NX, NY, NZ (direction cosines related to the global Cartesian system) or element KEYOPT(5). The following lists the various options for KEYOPT(5): KEYOPT(5) = 0 The contact normal is either based on the real constant values of NX, NY, NZ or on node locations when NX, NY, NZ are not defined. For two dimensional contact, NZ = 0. KEYOPT(5) = 1 (2,3) The contact normal points in a direction which averages the direction cosines of the X (Y, Z) axis of the nodal coordinates on both nodes I and J. The direction cosines on nodes I and J should be very close. This option may be supported by the NORA and NORL commands, which rotate the X axis of the nodal coordinate system to point to the surface normal of solid models. The GUI paths for these commands are, respectively: Main Menu> Preprocessor> Modeling> Move/Modify> Rotate Node CS> To Surf Normal> On Areas Main Menu> Preprocessor> Modeling> Move/Modify> Rotate Node CS> To Surf Normal> On Lines Main Menu> Preprocessor> Modeling> Move/Modify> Rotate Node CS> To Surf Normal> With Area
Figure 11.38 Two Concentric Pipes, Normals Rotated Properly
For a pipe-within-a-pipe, this portrays the normals rotated properly. KEYOPT(5) = 4 (5,6) The contact normal points to X (Y, Z) of the element coordinate system issued by the ESYS command. If you use this option, make sure that the element coordinate system specified by ESYS is the Cartesian system. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–73
Chapter 11: Contact Note — For CONTAC12 you can define the orientation of the contact surface with real constant THETA. For CONTAC52, you can use real constants NX, NY, NZ.
11.8.4. Defining the Initial Interference or Gap With CONTA178, the gap size can be automatically calculated from the GAP real constant plus the node locations (projection of vector points from node I to J on the contact normal). This is the default (KEYOPT(4) = 0) This means that if you want the initial gap to be determined by the node locations only, set KEYOPT(4) = 0 and the real constant GAP to 0. If KEYOPT(4) = 1, the initial gap size is only based on the real constant GAP (it ignores the node location). A negative value for the gap size can be used to model initial interference. You can ramp initial interference using KEYOPT(9) = 1. This option isn't supported by CONTAC12 and CONTAC52. Note that CONTAC52's real constant GAP is the opposite of CONTAC12's real constant INTF, which defines an interference. KEYOPT(4) for CONTAC12 and CONTAC52 is also different from CONTA178.
11.8.5. Selecting the Contact Algorithm You can choose among the following four different contact algorithms for CONTA178: •
Pure Lagrange Multiplier
•
Lagrange multiplier on the contact normal, penalty on the frictional (tangential) direction.
•
Augmented Lagrange method
•
Pure penalty method.
CONTAC12 and CONTAC52 offer only the pure penalty method, in which you must specify the contact stiffness. The normal stiffness KN should be based upon the stiffness of the surface in contact. However, if you choose to use CONTA178 with the pure penalty method or the augmented Lagrange method, a “semiautomatic” setting is provided for the contact normal and tangential stiffnesses. ANSYS provides a default normal contact stiffness FKN, which is based on Young's modulus E and the size of the underlying elements. FKN and FKS are factors. If you want to import absolute values for FKN and FKS, use negative values.
11.8.6. Applying Necessary Boundary Conditions You can now apply necessary boundary conditions as you would do for any ANSYS analysis. For more information on applying boundary conditions, see the appropriate analysis description in earlier chapters of this guide. When using the Lagrange multiplier method, be careful not to overconstrain the model. The model is overconstrained when a contact constraint at a node conflicts with a prescribed boundary condition on that degree of freedom at the same node. The following figure illustrates this issue:
11–74
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 11.8: Performing a Node-to-Node Contact Analysis
Figure 11.39 Example of Overconstrained Contact Problem
Both nodes I and J are fixed in the X direction. The model is overconstrained only when the two bodies are in contact and bonded contact or rough friction has been defined. It can also occur if the contact status is “sticking,” In these cases, the constraint in the X-direction is duplicated which causes an overconstrained model. “Zero Pivot” and “Numerical Singularity” warning messages indicate overcontraints in a model. Overconstraints can lead to convergence difficulties and/or inaccurate results. They can be easily avoided by changing the contact definition or the boundary conditions.
11.8.7. Defining the Solution Options Convergence behavior for contact problems depends strongly on the particular problem. The options listed below are either typical or recommended for most node-to-node contact analyses. •
Set the appropriate auto time step behavior using KEYOPT(7). The SOLCONTROL command turns this off by default.
•
The time step size must be small enough to capture the proper contact zone. The smooth transfer of contact forces is disrupted if the time step size is too large. A reliable way to set an accurate time step size is to turn automatic time stepping on. The SOLCONTROL command turns this on by default. Command(s): AUTOTS,ON GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Basic Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Time-Time Step Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Time and Substps
•
Set the number of equilibrium equations to a number that is appropriate for a reasonable time step size. With SOLCONTROL,ON, this command defaults to between 15 and 26 iterations, depending upon the physics of the problem. Command(s): NEQIT GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Nonlinear Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Equilibrium Iter
•
Turn the predictor-corrector option on, unless you expect large rotations. Command(s): PRED GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Nonlinear Tab) Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Predictor
•
Set the Newton-Raphson option to FULL, with adaptive descent on. Command(s): NROPT,FULL,,ON Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
11–75
Chapter 11: Contact GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options •
For analysis involving friction, using NROPT, UNSYM is useful (and sometimes required if the coefficient of friction µ is > 0.2) for problems where the normal and tangential (sliding) motions are strongly coupled.
•
NLGEOM, ON is supported but the contact normal is not updated during the analysis. Make sure that only small rotations occur along the contact surfaces (except for the cylindrical gap option).
•
Many convergence failures in contact analysis are the result of using too large a value for contact stiffness (real constant KN). Be sure to follow the recommendations given previously in this section for an initial estimate for contact stiffness. If such estimated values lead to a convergence failure, reduce the contact stiffness and restart. (You must also explicitly define the tangent stiffness - see the Note below.)
•
Conversely, if overpenetration occurred in your contact analysis, you probably used a value of KN that was too small. In this case, gradually increase the contact stiffness value to an appropriate level by redefining it using new R commands over several load steps in a restart. (You must also explicitly define the tangent stiffness - see the Note statement below.) Note — Although you can change the contact stiffness value (real constant KN), you cannot change any other real constants between load steps. Therefore, if you plan to change KN in a restart (or from one load step to the next), you cannot allow the value of the tangent (or "sticking") contact stiffness (real constant KT) to be defined by default, because the program would then attempt to redefine the tangent stiffness as the contact stiffness changed. You must explicitly define the tangent stiffness whenever you change the contact stiffness to maintain a consistent value for the tangent stiffness throughout all load steps.
11.8.8. Solving the Problem You can now solve the analysis the same as you would for any linear or nonlinear analysis. See Section 2.3.5: Solve the Analysis in Chapter 2, “Structural Static Analysis”.
11.8.9. Reviewing the Results Postprocessing of contact result items for these elements requires the use of ETABLE commands. The steps for reviewing results in POST26 are the same as those for a typical nonlinear analysis See Section 8.5.6.3: Reviewing Results in POST26 in Chapter 8, “Nonlinear Structural Analysis”. For general information on post processing, refer to the ANSYS Basic Analysis Guide.
11–76
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 12: Fracture Mechanics 12.1. Definition of Fracture Mechanics Cracks and flaws occur in many structures and components, sometimes leading to disastrous results. The engineering field of fracture mechanics was established to develop a basic understanding of such crack propagation problems. Fracture mechanics deals with the study of how a crack or flaw in a structure propagates under applied loads. It involves correlating analytical predictions of crack propagation and failure with experimental results. The analytical predictions are made by calculating fracture parameters such as stress intensity factors in the crack region, which you can use to estimate crack growth rate. Typically, the crack length increases with each application of some cyclic load, such as cabin pressurization-depressurization in an airplane. Further, environmental conditions such as temperature or extensive exposure to irradiation can affect the fracture propensity of a given material. Some typical fracture parameters of interest are: •
Stress intensity factors (KI, KII, KIII) associated with the three basic modes of fracture (see Figure 19.13: “The Three Basic Modes of Fracture” in the ANSYS, Inc. Theory Reference).
•
J-integral, which may be defined as a path-independent line integral that measures the strength of the singular stresses and strains near a crack tip
•
Energy release rate (G), which represents the amount of work associated with a crack opening or closure
12.2. Solving Fracture Mechanics Problems Solving a fracture mechanics problem involves performing a linear elastic or elastic-plastic static analysis and then using specialized postprocessing commands or macros to calculate desired fracture parameters. In this section, we will concentrate on two main aspects of this procedure: •
Modeling the Crack Region
•
Calculating Fracture Parameters
See Chapter 2, “Structural Static Analysis” for details about the general static analysis procedure. Also see Chapter 8, “Nonlinear Structural Analysis” for a discussion of structural nonlinearities.
12.2.1. Modeling the Crack Region The most important region in a fracture model is the region around the edge of the crack. We will refer to the edge of the crack as a crack tip in a 2-D model and crack front in a 3-D model. This is illustrated in Figure 12.1: “Crack Tip and Crack Front”.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 12: Fracture Mechanics
Figure 12.1 Crack Tip and Crack Front
In linear elastic problems, it has been shown that the displacements near the crack tip (or crack front) vary as
r , where r is the distance from the crack tip. The stresses and strains are singular at the crack tip, varying as r
. To pick up the singularity in the strain, the crack faces should be coincident, and the elements around 1/ the crack tip (or crack front) should be quadratic, with the midside nodes placed at the quarter points. Such elements are called singular elements. Figure 12.2: “Examples of Singular Elements” shows examples of singular elements for 2-D and 3-D models.
12–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 12.2: Solving Fracture Mechanics Problems
Figure 12.2 Examples of Singular Elements
(a) 2-D models and (b) 3-D models
12.2.1.1. 2-D Fracture Models The recommended element type for a 2-D fracture model is PLANE2, the 6-node triangular solid. The first row of elements around the crack tip should be singular, as illustrated in Figure 12.2: “Examples of Singular Elements” (a). The PREP7 KSCON command (Main Menu> Preprocessor> Meshing> Size Cntrls> Concentrat KPs> Create), which assigns element division sizes around a keypoint, is particularly useful in a fracture model. It automatically generates singular elements around the specified keypoint. Other fields on the command allow you to control
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
12–3
Chapter 12: Fracture Mechanics the radius of the first row of elements, number of elements in the circumferential direction, etc. Figure 12.3: “A Fracture Specimen and 2-D FE Model” shows a fracture model generated with the help of KSCON.
Figure 12.3 A Fracture Specimen and 2-D FE Model
Other modeling guidelines for 2-D models are as follows: •
Take advantage of symmetry where possible. In many cases, you need to model only one half of the crack region, with symmetry or antisymmetry boundary conditions, as shown below.
Figure 12.4 Taking Advantage of Symmetry
•
For reasonable results, the first row of elements around the crack tip should have a radius of approximately a/8 or smaller, where a is the crack length. In the circumferential direction, roughly one element every 30° or 40° is recommended.
•
The crack tip elements should not be distorted, and should take the shape of isosceles triangles.
12.2.1.2. 3-D Fracture Models The recommended element type for 3-D models is SOLID95, the 20-node brick element. As shown in Figure 12.2: “Examples of Singular Elements” (b), the first row of elements around the crack front should be singular elements. Notice that the element is wedge-shaped, with the KLPO face collapsed into the line KO.
12–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 12.2: Solving Fracture Mechanics Problems Generating a 3-D fracture model is considerably more involved than a 2-D model. The KSCON command is not available, and you need to make sure that the crack front is along edge KO of the elements. Other meshing guidelines for 3-D models are as follows: •
Element size recommendations are the same as for 2-D models. In addition, aspect ratios should not exceed approximately 4 to 1 in all directions.
•
For curved crack fronts, the element size along the crack front will depend on the amount of local curvature. As a rough guide, you should have at least one element every 15° to 30° along a circular crack front.
•
All element edges should be straight, including the edge on the crack front.
12.2.2. Calculating Fracture Parameters Once the static analysis is completed, you can use POST1, the general postprocessor, to calculate fracture parameters. As mentioned earlier, typical fracture parameters of interest are stress intensity factors, the J-integral, and the energy release rate.
12.2.2.1. Stress Intensity Factors The POST1 KCALC command (Main Menu> General Postproc> Nodal Calcs> Stress Int Factr) calculates the mixed-mode stress intensity factors KI, KII, and KIII. This command is limited to linear elastic problems with a homogeneous, isotropic material near the crack region. To use KCALC properly, follow these steps in POST1: 1.
Define a local crack-tip or crack-front coordinate system, with X parallel to the crack face (perpendicular to the crack front in 3-D models) and Y perpendicular to the crack face, as shown in the following figure. Note — This coordinate system must be the active model coordinate system [CSYS] and results coordinate system [RSYS] when KCALC is issued. Command(s): LOCAL (or CLOCAL, CS, CSKP, etc.) GUI: Utility Menu> WorkPlane> Local Coordinate Systems> Create Local CS> At Specified Loc
Figure 12.5 Crack Coordinate Systems
(a) 2-D Models and (b) 3-D Models 2.
Define a path along the crack face. The first node on the path should be the crack-tip node. For a halfcrack model, two additional nodes are required, both along the crack face. For a full-crack model, where
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
12–5
Chapter 12: Fracture Mechanics both crack faces are included, four additional nodes are required: two along one crack face and two along the other. The following figure illustrates the two cases for a 2-D model. Command(s): PATH, PPATH GUI: Main Menu> General Postproc> Path Operations> Define Path
Figure 12.6 Typical Path Definitions
(a) a half-crack model and (b) a full-crack model 3.
Calculate KI, KII, and KIII. The KPLAN field on the KCALC command specifies whether the model is planestrain or plane stress. Except for the analysis of thin plates, the asymptotic or near-crack-tip behavior of stress is usually thought to be that of plane strain. The KCSYM field specifies whether the model is a halfcrack model with symmetry boundary conditions, a half-crack model with antisymmetry boundary conditions, or a full-crack model. Command(s): KCALC GUI: Main Menu> General Postproc> Nodal Calcs> Stress Int Factr
12.2.2.2. J-Integral In its simplest form, the J-integral can be defined as a path-independent line integral that measures the strength of the singular stresses and strains near a crack tip. The following equation shows an expression for J in its 2-D form is shown below. It assumes that the crack lies in the global Cartesian X-Y plane, with X parallel to the crack (see Figure 12.7: “J-Integral Contour Path Surrounding a Crack-Tip”).
∂uy ∂u J = ∫r Wdy − ∫r t x x + t y ds ∂ y ∂ x where: γ = any path surrounding the crack tip W = strain energy density (that is, strain energy per unit volume) tx = traction vector along x axis = σxnx + σxy ny ty = traction vector along y axis = σyny + σxy nx σ = component stress n = unit outer normal vector to path γ u = displacement vector s = distance along the path γ
12–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 12.2: Solving Fracture Mechanics Problems
Figure 12.7 J-Integral Contour Path Surrounding a Crack-Tip
Follow these steps to calculate J for a 2-D model: 1.
Read in the desired set of results. Command(s): SET GUI: Main Menu> General Postproc> Read Results> First Set
2.
Store the volume and strain energy per element. Command(s): ETABLE GUI: Main Menu> General Postproc> Element Table> Define Table
3.
Calculate the strain energy density per element. Command(s): SEXP GUI: Main Menu> General Postproc> Element Table> Exponentiate
4.
Define a path for the line integral. Figure 12.8: “Examples of Paths for J-integral Calculation” shows examples of such paths. Command(s): PATH, PPATH GUI: Main Menu> General Postproc> Path Operations> Define Path
Figure 12.8 Examples of Paths for J-integral Calculation
5.
Map the strain energy density, which was stored in the element table in step 1, onto the path. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
12–7
Chapter 12: Fracture Mechanics Command(s): PDEF GUI: Main Menu> General Postproc> Path Operations> Map Onto Path 6.
Integrate it with respect to global Y. Command(s): PCALC GUI: Main Menu> General Postproc> Path Operations> Integrate
7.
Assign the final value of the integral to a parameter. This gives us the first term of equation 10.1. Command(s): *GET,Name,PATH,,LAST GUI: Utility Menu> Parameters> Get Scalar Data
8.
Map the component stresses SX, SY, and SXY onto the path. Command(s): PDEF GUI: Main Menu> General Postproc> Path Operations> Map Onto Path
9.
Define the path unit normal vector. Command(s): PVECT GUI: Main Menu> General Postproc> Path Operations> Unit Vector
10. Calculate TX and TY using the expressions shown with equation 10.1. Command(s): PCALC GUI: Main Menu> General Postproc> Path Operations> operation 11. Shift the path a small distance in the positive and negative X directions to calculate the derivatives of the displacement vector (δux/δx and δuy/δy). The following steps are involved (see Figure 19.13: “The Three Basic Modes of Fracture” in the ANSYS, Inc. Theory Reference): •
Calculate the distance by which the path is to be shifted, say DX. A rule of thumb is to use one percent of the total length of the path. You can obtain the total path length as a parameter using *GET,Name,PATH,,LAST,S.
•
Shift the path a distance of DX/2 in the negative X direction [PCALC,ADD,XG,XG,,,,-DX/2] and map the displacements UX and UY onto the path [PDEF], giving them labels UX1 and UY1, for example.
•
Shift the path a distance of DX in the positive X direction (that is, +DX/2 from its original position) and map UX and UY onto the path, giving them labels UX2 and UY2, for example.
•
Shift the path back to its original location (a distance of -DX/2) and calculate the quantities (UX2UX1)/DX and (UY2-UY1)/DX using PCALC. These quantities represent δux/δx and δuy/δy, respectively.
See the ANSYS Coupled-Field Analysis Guide for a discussion of the *GET, PCALC and PDEF commands. 12. Using the quantities calculated in steps 10 and 11, calculate the integrand in the second term of J [PCALC] and integrate it with respect to the path distance S [PCALC]. This gives the second term of equation 10.1. 13. Calculate J according to equation 10.1, using the quantities calculated in steps 5-7 and 12. You can simplify the J-integral calculations by writing a macro that performs the above operations. (Macros are described in the ANSYS APDL Programmer's Guide.)
12.2.2.3. Energy Release Rate Energy release rate is a concept used to determine the amount of work (change of energy) associated with a crack opening or closure. One method to calculate the energy release rate is the virtual crack extension method, outlined below. In the virtual crack extension method, you perform two analyses, one with crack length a and the other with crack length a +∆a. If the potential energy U (strain energy) for both cases is stored, the energy release rate can be calculated from 12–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 12.2: Solving Fracture Mechanics Problems U − Ua G = − a +∆a B∆a where B is the thickness of the fracture model. Extend the crack length by ∆a for the second analysis by selecting all nodes in the vicinity of the crack and scaling them in the X direction [NSCALE] (Main Menu> Preprocessor> Modeling> Operate> Scale) by the factor ∆a. Note — If you used solid modeling, you will first need to detach the solid model from the finite element model [MODMSH,DETACH] (Main Menu> Preprocessor> Checking Ctrls) before scaling the nodes. The "vicinity of the crack" is usually taken to mean all nodes within a radius of a/2 from the crack tip. Also, the factor ∆a for node scaling is usually in the range of 1/2 to 2 percent of the crack length.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
12–9
12–10
Chapter 13: Composites 13.1. Definition of Composites Composite materials have been used in structures for a long time. In recent times composite parts have been used extensively in aircraft structures, automobiles, sporting goods, and many consumer products. Composite materials are those containing more than one bonded material, each with different structural properties. The main advantage of composite materials is the potential for a high ratio of stiffness to weight. Composites used for typical engineering applications are advanced fiber or laminated composites, such as fiberglass, glass epoxy, graphite epoxy, and boron epoxy. ANSYS allows you to model composite materials with specialized elements called layered elements. Once you build your model using these elements, you can do any structural analysis (including nonlinearities such as large deflection and stress stiffening).
13.2. Modeling Composites Composites are somewhat more difficult to model than an isotropic material such as iron or steel. You need to take special care in defining the properties and orientations of the various layers since each layer may have different orthotropic material properties. In this section, we will concentrate on the following aspects of building a composite model: •
Choosing the proper element type
•
Defining the layered configuration
•
Specifying failure criteria
•
Following modeling and postprocessing guidelines
13.2.1. Choosing the Proper Element Type The following element types are available to model layered composite materials: SHELL99, SHELL91, SHELL181, SOLID46, and SOLID191. Which element you choose depends on the application, the type of results that need to be calculated, and so on. Check the individual element descriptions to determine if a specific element can be used in your ANSYS product. All layered elements allow failure criterion calculations. SHELL99 - Linear Layered Structural Shell Element SHELL99 is an 8-node, 3-D shell element with six degrees of freedom at each node. It is designed to model thin to moderately thick plate and shell structures with a side-to-thickness ratio of roughly 10 or greater. For structures with smaller ratios, you may consider using SOLID46. The SHELL99 element allows a total of 250 uniform-thickness layers. Alternately, the element allows 125 layers with thicknesses that may vary bilinearly over the area of the layer. If more than 250 layers are required, you can input your own material matrix. It also has an option to offset the nodes to the top or bottom surface. SHELL91 - Nonlinear Layered Structural Shell Element SHELL91 is similar to SHELL99 except that it allows only up to 100 layers and does not allow you to input a material property matrix. However, SHELL91 supports plasticity, large-strain behavior and a special sandwich option, whereas SHELL99 does not. SHELL91 is also more robust for large deflection behavior. SHELL181 - Finite Strain Shell Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 13: Composites SHELL181 is a 4-node 3-D shell element with 6 degrees of freedom at each node. The element has full nonlinear capabilities including large strain and allows 255 layers. The layer information is input using the section commands rather than real constants. Failure criteria is available using the FC commands. SOLID46 - 3-D Layered Structural Solid Element SOLID46 is a layered version of the 8-node, 3-D solid element, SOLID45, with three degrees of freedom per node (UX, UY, UZ). It is designed to model thick layered shells or layered solids and allows up to 250 uniform-thickness layers per element. Alternately, the element allows 125 layers with thicknesses that may vary bilinearly over the area of the layer. An advantage with this element type is that you can stack several elements to model more than 250 layers to allow through-the-thickness deformation slope discontinuities. The user-input constitutive matrix option is also available. SOLID46 adjusts the material properties in the transverse direction permitting constant stresses in the transverse direction. In comparison to the 8-node shells, SOLID46 is a lower order element and finer meshes may be required for shell applications to provide the same accuracy as SHELL91 or SHELL99 . SOLID191 - Layered Structural Solid Element SOLID191 is a layered version of the 20-node 3-D solid element SOLID95, with three degrees of freedom per node (UX, UY, UZ). It is designed to model thick layered shells or layered solids and allows up to 100 layers per element. As with SOLID46, SOLID191 can be stacked to model through-the-thickness discontinuities. SOLID191 has an option to adjust the material properties in the transverse direction permitting constant stresses in the transverse direction. In spite of its name, the element does not support nonlinear materials or large deflections. In addition to the layered elements mentioned above, other composite element capabilities exist in ANSYS, but will not be considered further in the chapter: •
SOLID95, the 20-node structural solid element, with KEYOPT(1) = 1 functions similarly to a single layered SOLID191 including the use of an orientation angle and failure criterion. It allows nonlinear materials and large deflections.
•
SHELL63, the 4-node shell element, can be used for rough, approximate studies of sandwich shell models. A typical application would be a polymer between two metal plates, where the bending stiffness of the polymer would be small relative to the bending stiffness of the metal plates. The bending stiffness can be adjusted by the real constant RMI to represent the bending stiffness due to the metal plates, and distances from the middle surface to extreme fibers (real constants CTOP, CBOT) can be used to obtain output stress estimates on the outer surfaces of the sandwich shell. It is not used as frequently as SHELL91, SHELL99, or SHELL181, and will not be considered for anything other than sandwich structures in this section.
•
SOLID65, the 3–D Reinforced Concrete Solid Element, models an isotropic medium with optional reinforcing in 3 different user-defined orientations.
•
BEAM188 and BEAM189, the 3–D finite strain beam elements, can have their sections built up with multiple materials.
13.2.2. Defining the Layered Configuration The most important characteristic of a composite material is its layered configuration. Each layer may be made of a different orthotropic material and may have its principal directions oriented differently. For laminated composites, the fiber directions determine layer orientation. Two methods are available to define the layered configuration: •
13–2
By specifying individual layer properties
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 13.2: Modeling Composites •
By defining constitutive matrices that relate generalized forces and moments to generalized strains and curvatures (available only for SOLID46 and SHELL99 )
13.2.2.1. Specifying Individual Layer Properties With this method, the layer configuration is defined layer-by-layer from bottom to top. The bottom layer is designated as layer 1, and additional layers are stacked from bottom to top in the positive Z (normal) direction of the element coordinate system. You need to define only half of the layers if stacking symmetry exists. At times, a physical layer will extend over only part of the model. In order to model continuous layers, these dropped layers may be modeled with zero thickness. Figure 13.1: “Layered Model Showing Dropped Layer” shows a model with four layers, the second of which is dropped over part of the model.
Figure 13.1 Layered Model Showing Dropped Layer
For each layer, the following properties are specified in the element real constant table [R, RMORE, RMODIF] (Main Menu> Preprocessor> Real Constants) (accessed with REAL attributes). •
Material properties (via a material reference number MAT)
•
Layer orientation angle commands (THETA)
•
Layer thickness (TK)
Layered sections may also be defined through the Section Tool (Prep>Sections>Shell — Add/edit). For each layer, the following are specified in the section definition through the section commands; or through the Section Tool (SECTYPE, SECDATA) (accessed with the SECNUM attributes). •
Material properties (via a material reference number MAT)
•
Layer orientation angle commands (THETA)
•
Layer thickness (TK)
•
Number of integration points per layer (NUMPT)
Material Properties - As with any other element, the MP command (Main Menu> Preprocessor> Material Props> Material Models> Structural> Linear> Elastic> Isotropic or Orthotropic) is used to define the linear material properties, and the TB command is used to define the nonlinear material data tables (plasticity is only available for elements SOLID191 and SHELL91). The only difference is that the material attribute number for each layer of an element is specified in the element's real constant table. For the layered elements, the MAT command (Main Menu> Preprocessor> Meshing> Mesh Attributes> Default Attribs) attribute is only used for the DAMP and REFT arguments of the MP command. The linear material properties for each layer may be either isotropic or orthotropic (see Linear Material Properties in the ANSYS Elements Reference). Typical fiber-reinforced composites contain orthotropic materials and these properties are most often supplied in the major Poisson's ratio form (see the ANSYS, Inc. Theory Reference). Material property directions are parallel to the layer coordinate system, which is defined by the element coordinate system and the layer orientation angle (described below). Layer Orientation Angle- This defines the orientation of the layer coordinate system with respect to the element coordinate system. It is the angle (in degrees) between X-axes of the two systems. By default, the layer coordinate system is parallel to the element coordinate system. All elements have a default coordinate system which you Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
13–3
Chapter 13: Composites can change using the ESYS element attribute [ESYS] (Main Menu> Preprocessor> Meshing> Mesh Attributes> Default Attribs). You may also write your own subroutines to define the element and layer coordinate systems (USERAN and USANLY); see the Guide to ANSYS User Programmable Features for details. Layer Thickness- If the layer thickness is constant, you only need to specify TK(I), the thickness at node I. Otherwise, the thicknesses at the four corner nodes must be input. Dropped layers may be represented with zero thickness. Number of integration points per layer- This allows you to determine in how much detail the program should compute the results. For very thin layers, when used with many other layers, one point would be appropriate. But for laminates with few layers, more would be needed. The default is 3 points. This feature applies only to sections defined through the section commands. Note — Currently, the GUI only allows layer real constant input of up to 100 layers. If more layers are needed for SHELL99 or SOLID46, the R and RMORE commands must be used.
13.2.2.2. Defining the Constitutive Matrices This is an alternative to specifying the individual layer properties and is available as an option [KEYOPT(2)] for SOLID46 and SHELL99. The matrices, which represent the force-moment and strain-curvature relationships for the element, must be calculated outside the ANSYS program as outlined in the ANSYS, Inc. Theory Reference. They can be included as part of the solution printout with KEYOPT(10). The main advantages of the matrix approach are: •
It allows you to incorporate an aggregate composite material behavior.
•
A thermal load vector may be supplied.
•
The matrices may represent an unlimited number of layers.
The terms of the matrices are defined as real constants. Mass effects are incorporated by specifying an average density (real constants AVDENS) for the element. If the matrix approach is used, detailed results in each layer cannot be obtained since individual layer information is not input.
13.2.2.3. Sandwich and Multiple-Layered Structures Sandwich structures have two thin faceplates and a thick, but relatively weak, core. Figure 13.2: “Sandwich Construction” illustrates sandwich construction.
Figure 13.2 Sandwich Construction
You can model sandwich structures with SHELL63, SHELL91, or SHELL181. SHELL63 has one layer but permits sandwich modeling through the use of real constants. You can modify the effective bending moment of inertia and the distance from the middle surface to the extreme fibers to account for the weak core. KEYOPT(9) = 1 of SHELL91 specifies the sandwich option. The core is assumed to carry all of the transverse shear; the faceplates carry none. Conversely, the faceplates are assumed to carry all (or almost all) of the bending load. Only SHELL91 has this sandwich option.
13–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 13.2: Modeling Composites SHELL181 models the transverse shear deflection using as energy equivalence method that makes the need for a sandwich option unnecessary
13.2.2.4. Node Offset For SHELL181 using sections defined through the section commands, nodes can be offset during the definition of the section, using the SECOFFSET command. For SHELL91, and SHELL99 the node offset option (KEYOPT(11)) locates the element nodes at the bottom, middle or top surface of the shell. The figures below illustrate how you can conveniently model ply drop off in shell elements that are adjacent to each other. In Figure 13.3: “Layered Shell With Nodes at Midplane”, the nodes are located at the middle surfaces (KEYOPT(11) = 0) and these surfaces are aligned. In Figure 13.4: “Layered Shell With Nodes at Bottom Surface”, the nodes are located at the bottom surfaces (KEYOPT(11) = 1) and these surfaces are aligned.
Figure 13.3 Layered Shell With Nodes at Midplane
Figure 13.4 Layered Shell With Nodes at Bottom Surface
13.2.3. Specifying Failure Criteria Failure criteria are used to learn if a layer has failed due to the applied loads. You can choose from three predefined failure criteria or specify up to six failure criteria of your own (user-written criteria). The three predefined criteria are: •
Maximum Strain Failure Criterion, which allows nine failure strains.
•
Maximum Stress Failure Criterion, which allows nine failure stresses.
•
Tsai-Wu Failure Criterion, which allows nine failure stresses and three additional coupling coefficients. You have a choice of two methods of calculating this criterion. The methods are defined in the ANSYS, Inc. Theory Reference.
The failure strains, stresses, and coupling coefficients may be temperature-dependent. See the ANSYS Elements Reference for details about the data required for each criterion. To specify a failure criterion, use either the family of TB commands or the family of FC commands. The TB commands areTB, TBTEMP, and TBDATA. (Main Menu> Preprocessor> Material Props> Failure Criteria). A typical sequence of commands to specify a failure criterion using these commands is shown below. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
13–5
Chapter 13: Composites TB,FAIL,1,2 ! Data table for failure criterion, material 1, ! no. of temperatures = 2 TBTEMP,,CRIT ! Failure criterion key TBDATA,2,1 ! Maximum Stress Failure Criterion (Const. 2 = 1) TBTEMP,100 ! Temperature for subsequent failure properties TBDATA,10,1500,,400,,10000 ! X, Y, and Z failure tensile stresses (Z value ! set to a large number) TBDATA,16,200,10000,10000 ! XY, YZ, and XZ failure shear stresses TBLIST TBTEMP,200 ! Second temperature TBDATA,...
The FC commands are FC, FCDELE, and FCLIST commands (Main Menu> Preprocessor> Material Props> Material Models> Structural> Nonlinear> Inelastic> Non-Metal Plasticity> Failure Criteria) and (Main Menu> General Postproc> Failure Criteria). A typical sequence of commands to specify a failure criterion using these commands is shown below. FC,1,TEMP,, 100, FC,1,S,XTEN, 1500, FC,1,S,YTEN, 400, FC,1,S,ZTEN,10000, FC,1,S,XY , 200, FC,1,S,YZ ,10000, FC,1,S,XZ ,10000, FCLIST, ,100 FCLIST, ,150 FCLIST, ,200 PRNSOL,S,FAIL
200 1200 500 8000 200 8000 8000
! Temperatures ! Maximum stress components
! ! ! !
List status List status List status Use Failure
of Failure Criteria at 100.0 degrees of Failure Criteria at 150.0 degrees of Failure Criteria at 200.0 degrees Criteria
Note — The TB commands (TB, TBTEMP, and TBDATA) can be used only for SHELL91, SHELL99, SOLID46, or SOLID191, but the FC and FCLIST commands can be used for any 2-D or 3-D structural solid element or any 3-D structural shell element. See the ANSYS Commands Reference for a discussion of the TB, TBTEMP, TBDATA, TBLIST, FC, FCDELE, and FCLIST commands. Some notes about specifying failure criteria: •
The criteria are orthotropic, so you must input the failure stress or failure strain values for all directions. (The exception is that compressive values default to tensile values.)
•
If you don't want the failure stress or strain to be checked in a particular direction, specify a large number in that direction (as shown in the previous example).
User-written failure criteria may be specified via user subroutines USRFC1 through USRFC6. These subroutines should be linked with the ANSYS program beforehand; see the ANSYS Advanced Analysis Techniques Guide for a brief description of user-programmable features.
13.2.4. Additional Modeling and Postprocessing Guidelines Some additional guidelines for modeling and postprocessing of composite elements are presented below. 1.
Composites exhibit several types of coupling effects, such as coupling between bending and twisting, coupling between extension and bending, etc. This is due to stacking of layers of differing material properties. As a result, if the layer stacking sequence is not symmetric, you may not be able to use model symmetry even if the geometry and loading are symmetric, because the displacements and stresses may not be symmetric.
2.
Interlaminar shear stresses are usually important at the free edges of a model. For relatively accurate interlaminar shear stresses at these locations, the element size at the boundaries of the model should be approximately equal to the total laminate thickness. For shells, increasing the number of layers per actual
13–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 13.2: Modeling Composites material layer does not necessarily improve the accuracy of interlaminar shear stresses. With elements SOLID46, SOLID95, and SOLID191, however, stacking elements in the thickness direction should result in more accurate interlaminar stresses through the thickness. Interlaminar transverse shear stresses in shell elements are based on the assumption that no shear is carried at the top and bottom surfaces of the element. These interlaminar shear stresses are only computed in the interior and are not valid along the shell element boundaries. Use of shell-to-solid submodeling is recommended to accurately compute all of the free edge interlaminar stresses. 3.
Because a large amount of input data is required for composites, you should verify the data before proceeding with the solution. Several commands are available for this purpose: •
ELIST (Utility Menu> List> Elements) lists the nodes and attributes of all selected elements.
•
EPLOT (Utility Menu> Plot> Elements) displays all selected elements. Using the /ESHAPE,1 command (Utility Menu> PlotCtrls> Style> Size and Shape) before EPLOT causes shell elements to be displayed as solids with the layer thicknesses obtained from real constants or section definition (see Figure 13.5: “Example of an Element Display”. This example uses element SHELL99 with /ESHAPE turned on). It also causes SOLID46 elements to be displayed with layers.
•
/PSYMB,LAYR,n (Utility Menu> PlotCrls> Symbols) followed by EPLOT displays layer number n for all selected layered elements. This can be used to display and verify each individual layer across the entire model.
•
/PSYMB,ESYS,1 followed by EPLOT displays the element coordinate system triad for those elements whose default coordinate system has been changed.
Figure 13.5 Example of an Element Display
•
LAYLIST (Utility Menu> List> Elements> Layered Elements) lists the layer stacking sequence from real constants and any two material properties for SHELL99, SHELL91, SOLID46, and SOLID191 elements. You can specify a range of layer numbers for the listing. LIST LAYERS 1 TO 4 IN REAL SET TOTAL LAYERS = 4 LSYM = 1 LP1 =
1 FOR ELEMENT TYPE 1 0 LP2 = 0 EFS = .000E+00
NO. ANGLE THICKNESS MAT --- ----- ---------- --1 45.0 0.250 1 2 -45.0 0.250 2 3 -45.0 0.250 2 4 45.0 0.250 1 -----------------------SUM OF THK 1.00
•
LAYPLOT (Utility Menu> Plot> Layered Elements) displays the layer stacking sequence from real constants in the form of a sheared deck of cards (see Figure 13.6: “Sample LAYPLOT Display for [45/Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
13–7
Chapter 13: Composites 45/ - 45/45] Sequence”). The layers are crosshatched and color coded for clarity. The hatch lines indicate the layer angle (real constant THETA) and the color indicates layer material number (MAT). You can specify a range of layer numbers for the display. •
4.
SECPLOT (Main Menu> Preprocessor> Sections> Shell> Plot Section) displays the section stacking sequence from sections in the form of a sheared deck of cards (see Figure 13.6: “Sample LAYPLOT Display for [45/-45/ - 45/45] Sequence”). The sections are crosshatched and color coded for clarity. The hatch lines indicate the layer angle (THETA) and the color indicates layer material number (MAT) defined by the SECDATA command. You can specify a range of layer numbers for the display.
By default, only data for the bottom of the first (bottom) layer, top of the last (top) layer, and the layer with the maximum failure criterion value are written to the results file. If you are interested in data for all layers, set KEYOPT(8) = 1. Be aware, though, that this may result in a large results file.
Figure 13.6 Sample LAYPLOT Display for [45/-45/ - 45/45] Sequence
5.
Use the ESEL,S,LAYER command to select elements that have a certain layer number. If an element has a zero thickness for the requested layer, the element is not selected. Note — For energy output, the results are applicable only to the entire element; you cannot get output results for individual layers.
6.
13–8
Use the LAYER command (Main Menu> General Postproc> Options for Outp) in POST1 (or LAYERP26 (Main Menu> TimeHist Postpro> Define Variables) in POST26) to specify the layer number for which results are to be processed. The SHELL command (Main Menu> General Postproc> Options for Outp or Main Menu> TimeHist Prostpro> Define Variables) specifies a TOP, MID, or BOT location within the layer. The default in POST1 is to store results for the bottom of the bottom layer, and the top of the top layer, and the layer with the maximum failure criterion value. In POST26, the default is layer 1. If KEYOPT(8) = 1 (that is, data stored for all layers), the LAYER and LAYERP26 commands store the TOP and BOT results for the specified layer number. MID values are then calculated by average TOP and BOT values. If KEYOPT (8) = 2 is set for SHELL181 during SOLUTION, then LAYER and LAYERP26 commands store the TOP,
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 13.2: Modeling Composites BOTTOM, and MID results for the specified layer number. In this case, MID values are directly retrieved from the results file. For transverse shear stresses with KEYOPT(8) = 0, therefore, POST1 can only show a linear variation, whereas the element solution printout or KEYOPT(8) = 2 can show a parabolic variation. 7.
By default, POST1 displays all results in the global Cartesian coordinate system. Use the RSYS command (Main Menu> General Postproc> Options for Outp) to transform the results to a different coordinate system. In particular, RSYS,SOLU allows you to display results in the layer coordinate system if LAYER is issued with a nonzero layer number.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
13–9
13–10
Chapter 14: Fatigue 14.1. Definition of Fatigue Fatigue is the phenomenon in which a repetitively loaded structure fractures at a load level less than its ultimate static strength. For instance, a steel bar might successfully resist a single static application of a 300 kN tensile load, but might fail after 1,000,000 repetitions of a 200 kN load. The main factors that contribute to fatigue failures include: •
Number of load cycles experienced
•
Range of stress experienced in each load cycle
•
Mean stress experienced in each load cycle
•
Presence of local stress concentrations
A formal fatigue evaluation accounts for each of these factors as it calculates how "used up" a certain component will become during its anticipated life cycle.
14.1.1. What the ANSYS Program Does The ANSYS fatigue calculations rely on the ASME Boiler and Pressure Vessel Code, Section III (and Section VIII, Division 2) for guidelines on range counting, simplified elastic-plastic adaptations, and cumulative fatigue summation by Miner's rule. For fatigue evaluations based on criteria other than those of the ASME Code, you can either write your own macro, or else interface your ANSYS results with an appropriate third-party program (see the ANSYS APDL Programmer's Guide for more information on these two features). The ANSYS program features the following fatigue-calculation capabilities: •
You can postprocess existing stress results to determine the fatigue usage factors for any solid-element or shell-element model. (You can also manually input stresses for fatigue evaluation of line-element models.)
•
You can store stresses at a preselected number of locations for a preselected number of events and loadings within the event.
•
You can define stress concentration factors for each location and scale factors for each event.
14.1.2. Basic Terminology A location is a node in your model for which fatigue stresses are to be stored. You would typically choose locations that represent points on the structure that would be susceptible to fatigue damage. An event is a set of stress conditions that occur at different times during a unique stress cycle. See Section 14.2.3.4: Guidelines for Obtaining Accurate Usage Factors later in this chapter for more information. A loading is one of the stress conditions that is part of an event. The alternating stress intensity is a measure of the difference in stress state between any two loadings. The program does not adjust the alternating stress intensity for mean-stress effects.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 14: Fatigue
14.2. Doing a Fatigue Evaluation You do a fatigue evaluation in POST1, the general postprocessor, after you have completed a stress solution. The procedure normally consists of five main steps: 1.
Enter POST1 and resume your database.
2.
Establish the size (the number of locations, events, and loadings), define the fatigue material properties, identify stress locations, and define stress concentration factors.
3.
Store stresses at locations of interest for various events and loadings; assign event repetitions and scale factors.
4.
Activate the fatigue calculations.
5.
Review the results.
14.2.1. Enter POST1 and Resume Your Database In order to perform a fatigue evaluation, you need to follow these steps: 1.
Enter POST1. Command(s): /POST1 GUI: Main Menu> General Postproc
2.
Read your database file (Jobname.DB) into active memory. (If your intended fatigue evaluation is a continuation of an ongoing ANSYS session, then Jobname.DB will already be in memory.) A results file (Jobname.RST) with nodal stress results should also be available; you will read results data into memory later. Command(s): RESUME GUI: Utility Menu> File> Resume from
14.2.2. Establish the Size, Fatigue Material Properties, and Locations Define the following data: •
Maximum number of locations, events, and loadings
•
Fatigue material properties
•
Stress locations and stress concentration factors (SCFs)
1.
Define the maximum number of stress locations, events, and loadings. By default, your fatigue evaluation can consider up to five nodal locations, ten events, and three loadings within an event. You can use the following option to establish larger dimensions (that is, allow more locations, events, or loadings), if necessary. Command(s): FTSIZE GUI: Main Menu> General Postproc> Fatigue> Size Settings
2.
Define material fatigue properties. In order to calculate usage factors, and to include the effect of simplified elastic-plastic computations, you must define material fatigue properties. The material properties of interest in a fatigue evaluation are: •
14–2
The S-N curve, a curve of alternating stress intensity ((Smax - Smin)/2) versus allowable number of cycles. The ASME S-N curves already account for maximum mean stress effects. You should adjust your S-N Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 14.2: Doing a Fatigue Evaluation curve to account for mean-stress effects, if necessary. If you do not input an S-N curve, alternating stress intensities will be listed in decreasing order for all possible combinations of stress conditions, but no usage factors will be calculated. Command(s): FP GUI: Main Menu> General Postproc> Fatigue> Property Table> S-N Table •
The Sm-T curve, a curve of design stress-intensity value versus temperature. This curve is needed if you want the program to detect whether or not the nominal stress range has gone plastic. Command(s): FP GUI: Main Menu> General Postproc> Fatigue> Property Table> Sm_T Table
•
Elastic-plastic material parameters M and N (strain hardening exponents). These parameters are required only if you desire simplified elastic-plastic code calculations. These parameters' values can be obtained from the ASME Code. Command(s): FP GUI: Main Menu> General Postproc> Fatigue> Property Table> Elas-plas Par The following example illustrates the use of the FP command to input material fatigue properties: ! Define the S-N table: FP,1,10,30,100,300,1000,10000 FP,7,100000,1000000 FP,21,650,390,240,161,109,59 FP,27,37,26 ! Define the Sm-T table: FP,41,100,200,300,400,500,600 FP,47,650,700,750,800 FP,51,20,20,20,18.7,17.4,16.4 FP,57,16.1,15.9.15.5,15.1
! Allowable Cycles, N ! " ! Alternating Stress! Intensity Range, S, ksi
! Temperature,°F ! " ! "Design Stress-Intensity ! Value", Sm (=2/3*Sy or ! 1/3 *Su), ksi ! Define the elastic-plastic material parameters: FP,61,1.7,.3 ! M and N
3.
Define stress locations and stress concentration factors. The following option allows you to explicitly define a nodal location of interest to your fatigue evaluation, define stress concentration factors (SCFs) for that location, and assign a short (20 character) title to that location. Command(s): FL GUI: Main Menu> General Postproc> Fatigue> Stress Locations
Note — Not all fatigue analyses will require the FL command. Locations are automatically defined for nodes when FS, FSNODE, or FSSECT are issued (see below). If your model contains sufficient grid detail, your stresses could be accurate enough that you would not need to apply calculated SCFs. (Supplemental SCFs for surface, size, or corrosion effects might still be required, however.) Where only one location is being examined, you could omit a title. If explicit definition of locations, SCFs, or titles are not required, you could forgo the FL command entirely. Here is an example of some FL commands for a cylinder with a global Y axis, having two wall thicknesses of interest, where SCFs are to be applied (to the axial linearized stresses) at the outside wall. FL,1,281,,,,Line 1 at inside FL,2,285,,1.85,,Line 1 at outside FL,3,311,,,,Line 2 at inside FL,4,315,,2.11,,Line 2 at outside
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
14–3
Chapter 14: Fatigue
Figure 14.1 Cylinder Wall with Stress Concentration Factors (SCFs)
14.2.3. Store Stresses and Assign Event Repetitions and Scale Factors 14.2.3.1. Storing Stresses In order to perform a fatigue evaluation, the program must know the stresses at different events and loadings for each location, as well as the number of repetitions of each event. You can store stresses for each combination of location, event, and loading, using the following options: •
Manually stored stresses
•
Nodal stresses from Jobname.RST
•
Stresses at a cross-section Caution: The program never assumes that a "zero" stress condition exists. If zero stress is one of the conditions to be considered, it must be explicitly input for each event in which it may occur.
The following command sequences schematically illustrate how to store stresses. In some situations, you might prefer to use LCASE instead of SET. Manually stored stresses:
FS
Nodal stresses retrieved from Jobname.RST:
SET, FSNODE
Stresses at a cross-section:
PATH, PPATH, SET, FSSECT
(Cross-section calculations also require data from Jobname.RST.)
You can use more than one method of storing stresses in an event. Each of these methods is explained in detail below.
14.2.3.1.1. Manually Stored Stresses You can use this option to store stresses and the temperature "manually" (without direct access to the results file Jobname.RST). In such cases, you are not using the fatigue module in POST1 as a postprocessor, but simply as a fatigue calculator. Line elements, such as beams, must be handled in this way since the fatigue module is not able to access data from a results file other than for solid elements or shell elements. Command(s): FS GUI: Main Menu> General Postproc> Fatigue> Store Stresses> Specified Val Command input for this option is demonstrated by the following example: FS,201,1,2,1,-2.0,21.6,15.2,4.5,0.0,0.0 FS,201,1,2,7,450.3
14–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 14.2: Doing a Fatigue Evaluation In this example, only the total stresses (items 1-6) and the temperature (item 7) are input. If the linearized stresses were also to be input, they would follow the temperatures as items 8 through 13. Note — In the special case of a beam element having only axial stress, you would input only one stress component (SX), leaving the rest of the stress fields blank.
14.2.3.1.2. Nodal Stresses from Jobname.RST When you use this option, you cause a nodal stress vector containing six stress components to be stored directly from the results database. Stress components stored with this option can be modified with a subsequent FS command. Note — You must issue a SET command, and possibly a SHELL command, before executing FSNODE. SET will read results for a particular load substep from the results file (Jobname.RST) into the database. SHELL allows you to select results from the top, middle, or bottom surfaces for shell elements (default is the top surface). Command(s): FSNODE GUI: Main Menu> General Postproc> Fatigue> Store Stresses> From rst File Input by means of FSNODE is demonstrated by the following example for an event at one nodal location: SET,1 FSNODE,123,1,1 SET,2 FSNODE,123,1,2 SET,3 FSNODE,123,1,3
! ! ! ! ! ! !
Define data set for load step 1 Stress vector at node 123 assigned to event 1, loading 1. Define data set for load step 2 ...event 1, loading 2 ...load step 3 ...event 1, loading 3
Figure 14.2 Three Loadings in One Event
14.2.3.1.3. Stresses at a Cross-Section This option calculates and stores total linearized stresses at the ends of a section path (as defined by a preceding PATH and PPATH command). Because you will normally want the linearization to take place over a thickness representing the shortest distance between the two surfaces, use only the two surface nodes to describe the path in the PPATH command. This option retrieves stress information from the results database; therefore
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
14–5
Chapter 14: Fatigue FSSECT must also be preceded by a SET command. Stress components stored with an FSSECT command can be modified with a subsequent FS command. Command(s): FSSECT GUI: Main Menu> General Postproc> Fatigue> Store Stresses> At Cross Sect Input by means of FSSECT is demonstrated in the following example. If node locations are not assigned with an FL command, the FSSECT commands in this example will automatically assign location numbers to the two path nodes, 391 and 395. (See Figure 14.3: “Surface Nodes are Identified by PPATH Prior to Executing FSSECT”.) PATH,Name,2 PPATH,1,391 PPATH,2,395 SET,1 FSSECT,,1,1
! Define the path using the two surface nodes
! Store stresses at nodes 391 and 395
Figure 14.3 Surface Nodes are Identified by PPATH Prior to Executing FSSECT
14.2.3.2. Listing, Plotting, or Deleting Stored Stresses Use the following options to list, plot, or delete stored stresses. •
List the stored stresses per location, per event, per loading, or per stress condition: Command(s): FSLIST GUI: Main Menu> General Postproc> Fatigue> Store Stresses> List Stresses
•
Display a stress item as a function of loading number for a particular location and event: Command(s): FSPLOT GUI: Main Menu> General Postproc> Fatigue> Store Stresses> Plot Stresses
•
Delete a stress condition stored for a particular location, event, and loading: Command(s): FSDELE GUI: Main Menu> General Postproc> Fatigue> Store Stresses> Dele Stresses
•
Delete all stresses at a particular location: Command(s): FL GUI: Main Menu> General Postproc> Fatigue> Stress Locations
•
Delete all stresses for all loadings in a particular event: Command(s): FE GUI: Main Menu> General Postproc> Fatigue> Erase Event Data
14.2.3.3. Assigning Event Repetitions and Scale Factors This option assigns the number of occurrences to the event numbers (for all loadings at all locations of the event). It can also be used to apply scale factors to all of the stresses that make up its loadings. Command(s): FE GUI: Main Menu> General Postproc> Fatigue> Assign Events
14–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 14.2: Doing a Fatigue Evaluation An example of this command usage is given below: FE,1,-1 FE,2,100,1.2 *REPEAT,3,1 FE,5,500
! Erase all parameters and fatigue stresses formerly ! used for event 1. ! Assign 100 occurrences to events 2, 3 and 4, ! and scale by 1.2. ! Assign 500 occurrences to event 5.
14.2.3.4. Guidelines for Obtaining Accurate Usage Factors Structures are usually subjected to a variety of maximum and minimum stresses, which occur in unknown (or even random) order. Therefore, you must take care to achieve an accurate count of the number of repetitions of all possible stress ranges, in order to obtain a valid fatigue usage factor. The ANSYS program automatically calculates all possible stress ranges and keeps track of their number of occurrences, using a technique commonly known as the "rain flow" range-counting method. At a selected nodal location, a search is made throughout all of the events for the pair of loadings (stress vectors) that produces the most severe stress-intensity range. The number of repetitions possible for this range is recorded, and the remaining number of repetitions for the events containing these loadings is decreased accordingly. At least one of the source events will be "used up" at this point; remaining occurrences of stress conditions belonging to that event will subsequently be ignored. This process continues until all ranges and numbers of occurrences have been considered. Caution: It can be surprisingly easy to misuse the range-counting feature of the fatigue module. You must take pains to assemble events carefully if you want your fatigue evaluation to yield accurate usage factors. Consider the following guidelines when assembling events: •
Understand the internal logic of the ANSYS range-counting algorithm. See the ANSYS, Inc. Theory Reference for more details on how the ANSYS program performs range counting.
•
Because it can be difficult to predict the exact load step at which a maximum (or minimum) 3-D stress state occurs, good practice often requires that you include several clustered loadings in each event, in order to successfully capture the extreme stress state. (See Figure 14.2: “Three Loadings in One Event”.)
•
You will obtain consistently conservative results if you include only one extreme stress condition (either a local maximum or a local minimum) in any given event. If you group more than one extreme condition in a single event, you will sometimes generate unconservative results, as illustrated by the following example:
Consider a load history made up of two slightly different cycles: Load Cycle 1: 500 repetitions of Sx = +50.0 to -50.1 ksi Load Cycle 2: 1000 repetitions of Sx = +50.1 to -50.0 ksi These load cycles will obviously sum to 1500 repetitions having an alternating stress intensity of about 50 ksi. However, carelessly grouping these loadings into only two events will result in an inaccurate range count. Let's see how this would happen: Event 1,
loading 1: Sx = 50.0 loading 2: Sx = -50.1
500 repetitions
Event 2,
loading 1: Sx = 50.1 loading 2: Sx = -50.0
1000 repetitions
The possible alternating stress intensities are: a.
From E1,L1 to E1,L2:
50.05 ksi Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
14–7
Chapter 14: Fatigue b.
From E1,L1 to E2,L1:
0.05 ksi
c.
From E1,L1 to E2,L2:
50.00 ksi
d.
From E1,L2 to E2,L1:
50.10 ksi
e.
From E1,L2 to E2,L2:
0.05 ksi
f.
From E2,L1 to E2,L2:
50.05 ksi
Sorting these combinations by decreasing alternating stress intensity gives: d.
From E1,L2 to E2,L1:
50.10 ksi
a.
From E1,L1 to E1,L2:
50.05 ksi
f.
From E2,L1 to E2,L2:
50.05 ksi
c.
From E1,L1 to E2,L2:
50.00 ksi
b.
From E1,L1 to E2,L1:
0.05 ksi
e.
From E1,L2 to E2,L2:
0.05 ksi
The range counting then proceeds as follows: d.
500 cycles of E1,L2 to E2,L1
- this uses up 500 cycles of E1 and E2
a.
0 cycles of E1,L1 to E1,L2
- E1 is all used up
f.
500 cycles of E2,L1 to E2,L2
- this uses up 500 more cycles of E2
c.
0 cycles of E1,L1 to E2,L2
- both events are all used up
b.
0 cycles of E1,L1 to E2,L1
- both events are all used up
e
0 cycles of E1,L2 to E2,L2
- both events are all used up
Thus, only 1000 repetitions of about 50 ksi range would be counted, instead of the known 1500 cycles. This error results solely from improper assembly of events. If the loadings had each been described as separate events (such that E1,L1 ≥ E1; E1,L2 ≥ E2; E2,L1 ≥ E3; and E2,L2 ≥ E4), then the following range counts would be obtained: d.
500 cycles of E2 to E3
- this uses up 500 cycles of E2 and E3
a.
0 cycles of E1 to E2
- E2 is all used up
f.
500 cycles of E3 to E4
- uses up 500 more cycles of E3, and 500 of E4
c.
500 cycles of E1 to E4
- uses up 500 more cycles of E4
b.
0 cycles of E1 to E3
- E3 is all used up
e.
0 cycles of E2 to E4
- E2 and E4 are both all used up
Cumulative fatigue damage in this case would properly be calculated for 1500 repetitions of about 50 ksi range. •
Conversely, using separate events for each maximum and each minimum stress condition could sometimes become too conservative. In such cases, carefully choose those loadings that should be counted together, and group them into the same events. The following example illustrates how some events can appropriately contain multiple extreme stress conditions:
Consider a load history made up of these two load cycles: •
Load Cycle 1: 500 repetitions of Sx = +100.1 to +100.0 ksi
•
Load Cycle 2: 1000 repetitions of Sx = +50.1 to +50.0 ksi
14–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 14.2: Doing a Fatigue Evaluation It is readily apparent that the worst possible combination of these cycles would yield 500 repetitions having alternating stress intensity of about 25 ksi range. Proceeding as in the above example, grouping these loadings into two events would produce an accurate count of 500 repetitions of about 25 ksi range. Treating each loading as a separate event would yield an over-conservative count of 1000 repetitions of about 25 ksi range.
14.2.4. Activate the Fatigue Calculations Now that you have locations, stresses, events, and material parameters all specified, you can execute the fatigue calculations at a specified location. The location is specified by either the location number or the node itself. Command(s): FTCALC GUI: Main Menu> General Postproc> Fatigue> Calculate Fatig
14.2.5. Review the Results Fatigue calculation results are printed in the output. If you have routed your output [/OUTPUT] to a file (for example Jobname.OUT), then you can review the results by listing that file. Command(s): *LIST GUI: Utility Menu> List> Files> Other> Jobname.OUT If you have input an S-N curve, output is in the form of a table of alternating stress intensities (listed in decreasing order) with corresponding pairs of event/loadings, as well as cycles used, cycles allowed, temperature, and partial usage factor. Following that, the cumulative usage factor is shown for that particular location. This information is repeated for all locations. As has been just mentioned, FTCALC output shows the contributing pairs of events and loadings for any given alternating stress-intensity range. This information can help you isolate the transients (events/loadings) causing the most fatigue damage. A convenient way to modify your events would be to write all stored fatigue data on Jobname.FATG. (This option could be executed either before or after FTCALC.) Data are written to Jobname.FATG in terms of equivalent fatigue module commands. You can modify your events by editing Jobname.FATG; then use the /INPUT command to reread the modified fatigue commands. Command(s): FTWRITE GUI: Main Menu> General Postproc> Fatigue> Write Fatig Data
14.2.6. Other Approaches to Range Counting Earlier, we discussed the "rain flow" range-counting method. This technique is useful whenever the exact timehistory of various loadings is not known. However, if in your fatigue analysis the time-history is known, you can avoid the undue conservatism of this procedure simply by running a separate fatigue analysis [FTCALC] for each sequential event and then adding the usage factors manually.
14.2.7. Sample Input A sample input listing for a fatigue evaluation is shown below: ! Enter POST1 and Resume the Database: /POST1 RESUME,... ! Number of Locations, Events, and Loadings FTSIZE,... ! Material Fatigue Properties: FP,1,.... ! N values
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
14–9
Chapter 14: Fatigue FP,21,... ! S values FP,41,... ! T values FP,51,... ! Sm values FP,61,... ! Elastic-plastic material parameters ! Locations, Stress Concentration Factors, and Location Titles FL,... ! Store Stresses (3 Different Methods) ! Store Stresses Manually: FS,... ! Retrieve Stresses from the Results File: SET,... FSNODE,... ! Store Stresses at a Cross-Section: PPATH,... SET,... FSSECT,... ! Event Repetitions and Scale Factors FE,... ! Activate the Fatigue Calculations FTCALC,... ! Review the Results (List the output file) FINISH
See the ANSYS Commands Reference for a discussion of the FTSIZE, FP, FL, FS, FSNODE, PPATH, FSSECT, FE, and FTCALC commands.
14–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 15: p-Method Structural Static Analysis 15.1. Definition of p-Method Analysis The p-method obtains results such as displacements, stresses, or strains to a user-specified degree of accuracy. To calculate these results, the p-method manipulates the polynomial level (p-level) of the finite element shape functions which are used to approximate the real solution. This feature works by taking a finite element mesh, solving it at a given p-level, increasing the p-level selectively, and then solving the mesh again. After each iteration the results are compared for convergence against a set of convergence criteria. You can specify the convergence criteria to include displacement, rotation, stress or strain at a point (or points) in the model, and global strain energy. The higher the p-level, the better the finite element approximation to the real solution. In order to capitalize on the p-method functionality, you don't have to work only within the confines of p-generated meshes. The p-method is most efficient when meshes are generated considering that p-elements will be used, but this is not a requirement. Of course, you might want to create and mesh your model using p-elements, but you can also perform a p-method solution using meshes that have been generated with h-elements (generated by ANSYS or your CAD package), if the elements are at least mid-noded. This provides you with the flexibility of taking advantage of the p-method solution option independently of how the mesh was created. The p-method can improve the results for any mesh automatically.
15.2. Benefits of Using the p-Method The p-method solution option offers many benefits for linear structural static analyses that are not available with the more traditional h-method, discussed in the preceding chapters. The most convenient benefit is the ability to obtain good results to a desired level of accuracy without rigorous user-defined meshing controls. If you are new to finite element analysis or do not have a solid background in mesh design, you might prefer this method since it relieves you of the task of manually designing an accurate mesh. In addition, the p-method adaptive refinement procedure offers error estimates that are more precise than those of the h-method, and can be calculated locally as well as globally (for example, stress at a point rather than strain energy). For example, if you need to obtain highly accurate solutions at a point, such as for fracture or fatigue assessments, the p-method offers an excellent means of obtaining these results to the required accuracy.
15.3. Using the p-Method The procedure for a p-method static analysis consists of four main steps: 1.
Select the p-method procedure.
2.
Build the model.
3.
Apply loads and obtain the solution.
4.
Review the results.
Each step is discussed in detail in the following sections.
15.3.1. Select the p-Method Procedure You can activate the p-method solution procedure in two ways: through the GUI or by defining a p-element [ET].
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 15: p-Method Structural Static Analysis •
Activating p-method through the GUI: Command(s): /PMETH GUI: Main Menu> Preferences> p-method
•
Defining a p-element: The p-method solution procedure can also be activated by defining a p-element. If you are working outside of the GUI, the definition of a p-element lets the program know that a p-method solution is to be done; no other commands are necessary to initiate p-method. From within the GUI, you can also issue the ET command in the "Input Window" to activate the p-method procedure. (Remember, the ET command must be entered in the "Input Window," since, by default, only h-elements are displayed in the GUI unless p-method is active.) Command(s): ET GUI: Main Menu> Preprocessor> Element Type> Add/Edit/Delete
15.3.2. Build the Model In order to build a model with p-elements, you must follow the procedure listed below. 1.
Define the element types.
2.
Specify material properties and/or real constants.
3.
Define the model geometry.
4.
Mesh the model into solid or shell elements.
The above steps are common to most analyses. The ANSYS Modeling and Meshing Guide explains those steps in detail. In this section we will explain the techniques that are unique to a p-analysis.
15.3.2.1. Define the Element Types You can use the following five p-elements to build your model: •
2-D Quadrilateral (PLANE145)
•
2-D Triangle (PLANE146)
•
3-D Brick (SOLID147)
•
3-D Tetrahedron (SOLID148)
•
3-D Shell (SHELL150) Note — H-elements and p-elements cannot be active at the same time in your model.
15.3.2.1.1. Specifying a p-Level Range Various options are available for use with p-elements. One important option is the ability to specify, either locally or globally, a range in which the p-level may vary. The range within which the p-level may vary can be controlled locally through the p-element KEYOPT settings (KEYOPT(1) and KEYOPT(2)), or globally across the entire model with PPRANGE. By default, the p-level range is 2 to 8. When both KEYOPT values and PPRANGE have been used to specify p-level ranges, the local p-level range [ET] will take precedence over the global p-level range [PPRANGE].
15–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.3: Using the p-Method For example, if you set a global p-level range between 3 and 8 with PPRANGE, then define a local p-level range of 4 to 6 for PLANE145 elements (ET,1,145,4,6), the p-level for the PLANE145 elements may only vary between 4 and 6, while the rest of the model may vary between 3 and 8. At the (default) starting p-level of 2, convergence checking is performed to determine those elements which are converged and may have their p-level fixed at 2. That is, these elements will remain at a p-level of 2, and will be eliminated from any further convergence checking. Additional checking is performed at each iteration to fix the p-levels of the elements which are converged. Note — Convergence checking for SHELL150 begins at a p-level of 3 instead of a p-level of 2. Use local p-range control to eliminate regions of little importance from high p-escalation. Use global p-range control for overall control of the p-level. These range controls are not necessary, but p-escalations to high plevels increase CPU time. Therefore, it is advantageous to have such controls available. •
Defining a local p-level range: Command(s): ET GUI: Main Menu> Preprocessor> Element Type> Add/Edit/Delete
•
Defining a global p-level range: Command(s): PPRANGE GUI: Main Menu> Preprocessor> Loads> Load Step Opts> p-Method> Set p-range
See the ANSYS Elements Reference for complete descriptions of each of the above element types.
15.3.2.2. Specify Material Properties and/or Real Constants 15.3.2.2.1. Material Properties Material properties for p-elements may be either constant or temperature-dependent, and isotropic or orthotropic. As with other structural analyses, if you plan to apply inertia loads (such as gravity or rotational velocity), you must also specify the density (DENS) that is required for mass calculations. Young's modulus (EX) must be defined, and if thermal loads (temperatures) are to be applied, a coefficient of thermal expansion (ALPX) must be specified. Command(s): MP GUI: Main Menu> Preprocessor> Material Props> Material Models> Structural> Density Main Menu> Preprocessor> Material Props> Material Models> Structural> Linear> Elastic> Isotropic Main Menu> Preprocessor> Material Props> Material Models> Structural> Thermal Expansion Coef> Isotropic Caution: Element coordinate systems [ESYS] used for orthotropic material directions are not supported by p-elements. All element coordinate systems are parallel to the global Cartesian coordinate system.
15.3.2.2.2. Real Constants You may define optional thicknesses for 2-D elements and thicknesses for SHELL150 as real constants. Thicknesses must be defined for SHELL150. Command(s): R GUI: Main Menu> Preprocessor> Real Constants
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–3
Chapter 15: p-Method Structural Static Analysis
15.3.2.3. Define the Model Geometry You can create your model using any of the various techniques outlined in the ANSYS Modeling and Meshing Guide, or you can import it from a CAD system using ANSYS Connection product. If you are generating your model from within ANSYS, you can use either solid modeling or direct generation techniques. Note — Using direct generation is not recommended when you plan to create a p-mesh since all p-elements require that midside nodes be included in their geometric definition. In cases where surface curvature is important, it would not only be tedious, but possibly imprecise to manually define each midside node. In addition, the EMID command does not place nodes on a curved line. It is much more convenient to let the program generate the midside nodes using solid modeling. You may not drop any midside nodes from p-elements. If you use direct generation or import your mesh from an outside source, keep the following guidelines in mind: •
A curved element edge should not cover more than a 30° arc.
•
The angles between adjacent edges should be between 10° and 170°. Element shape checking will warn that adjacent edges should be between 30° and 150°, but it is usually acceptable to have angles in the range of 10° to 170° for p-elements.
•
A good rule of thumb is to keep the aspect ratio (ratio of element length to width) less than 20:1.
15.3.2.4. Mesh the Model into Solid or Shell Elements 15.3.2.4.1. Using Program Defaults After you have generated your solid model, you are ready to mesh it with p-elements. The general procedure for meshing your solid model is outlined in Chapter 7, “Generating the Mesh” in the ANSYS Modeling and Meshing Guide. Compared to h-elements, the program will generate a coarser mesh under default settings for p-elements. Normally, you will not need to specify any meshing size controls because the program defaults will give you an adequate mesh. In addition, each element's p-level will be manipulated during solution to obtain accurate and efficient results. For engineering design studies, the accuracy obtained with a relatively coarse, ungraded mesh is usually sufficient. (A graded mesh is one where there are more elements near an area of interest. These elements are smaller relative to the other areas of the model, and a transition region occurs from the large to the smaller elements.) Note — Adaptive meshing is not valid with a p-method analysis.
15.3.2.4.2. Specifying Mesh Controls By default, the DESIZE command controls automatic element sizing. For free meshing, you have the option of using the SmartSize feature [SMRTSIZE] to control element sizing. SmartSizing generally produces a better quality mesh and is recommended for meshing a p-element model. (SmartSizing is not available for mapped meshing.) Command(s): SMRTSIZE GUI: Main Menu> Preprocessor> Meshing> Size Cntrls> SmartSize> Basic or Command(s): DESIZE GUI: Main Menu> Preprocessor> Meshing> Size Cntrls> Manual Size> Global> Other
15–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.3: Using the p-Method Note — Since p-method prefers a coarser mesh, the default element size values for a p-method analysis are different than those used for h-elements. See the SMRTSIZE and DESIZE commands for details. For fracture or fatigue assessments, you may still need to specify meshing controls because the mesh must be fine enough to obtain the desired accuracy near the areas of interest. In certain cases, such as when there are severe geometric transition regions, you may also need to specify mesh controls to avoid a meshing failure. You may also want to specify meshing controls for curved geometries, where successful meshes are more difficult to achieve with the default size settings. Under default conditions, badly shaped elements may be produced because of the difficulty of filling a curved domain with as few elements as possible. User-defined meshing controls can make the task less difficult.
15.3.2.4.3. Guidelines for Creating a Good Mesh •
Subdivide complex geometries, or build them as separate geometries. As a general rule, if you were to stand inside a volume, you should be able to see all of its vertices. If this is not possible, you might wish to consider subdividing the volume into more manageable pieces.
•
The number of divisions on lines "parallel" and near to each other should be fairly equivalent. The SmartSizing method of meshing [SMRTSIZE] handles this situation well. However, if the DESIZE method of element sizing is used, you should set local mesh controls to achieve a good mesh in these areas.
•
For beam-like or shell-like models, use one element through the thickness in the meshed model. SmartSizing will do this automatically. However, if you are using DESIZE for meshing, set the default element size [MINH] to 1 [DESIZE,,1].
Figure 15.1 Fan Model Showing p-Element vs. h-Element Meshes
15.3.3. Additional Information for Building Your Model 15.3.3.1. Viewing your element model A subgrid approach is used for plotting the model in which the amount of displayed element curvature can be controlled. You may display varying degrees of curvature in your model by specifying the number of facets to be used for element display. Facets are piecewise linear approximations of the actual curve represented by the element face or edge. A greater number of facets will result in a smoother representation of the element surface Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–5
Chapter 15: p-Method Structural Static Analysis for p-element plots. PowerGraphics is the default graphics display method used for p-method plots. This method will display the plot at a much faster speed than the Full Model method. See Chapter 10, “PowerGraphics” in the ANSYS Basic Analysis Guide for more information on PowerGraphics. For more information on /EFACET, see the discussion on the p-Element Subgrid later in this section. Command(s): /EFACET GUI: Utility Menu> PlotCtrls> Style> Size and Shape
15.3.3.2. Coupling You may couple degrees of freedom (DOFs) between nodes on p-elements to control nodal solution behavior. All coupled nodes are forced to assume the same displacement values in the specified nodal coordinate direction. The amount of this displacement is unknown until the analysis has been completed. Command(s): CP GUI: Main Menu> Preprocessor> Coupling/Ceqn> Couple DOFs The first degree of freedom defined on the coupled set is the "prime" degree of freedom. All other degrees of freedom in the coupled set are eliminated from the solution matrices as a result of their relationship to the prime degree of freedom. Note — For p-elements, only the corner nodes may be defined as prime degrees of freedom if midside nodes are also part of the same coupled set. For a p-method analysis, only the nodal combinations described below are permitted when coupling, and any deviation from these combinations will most likely result in singularities.
15.3.3.2.1. Coupling of Corner Nodes 1.
Two nodes are coupled within the same element.
Figure 15.2 Coupled Nodes on One Element
2.
Two nodes are coupled between adjacent element edges/faces.
Figure 15.3 Nodes Coupled Between Adjacent Elements
15–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.3: Using the p-Method
15.3.3.2.2. Midside Node Coupling 1.
Both corner nodes on the element's edge or face are part of the same coupled set. Only the corner nodes may be defined as prime degrees of freedom.
Figure 15.4 Both Corner Nodes are Coupled
2.
All nodes in the coupled set are midside nodes. In this case, a midside node must be defined as the prime degree of freedom, but this is only valid as long as there are no corner nodes defined as part of the same coupled set.
Figure 15.5 All Coupled Nodes are Midside Nodes
Note — If you have coupled faces or edges on a p-element (that is, all edges of the element's face or all nodes of the element's edge are coupled), the p-level of that edge or face will be held to 2. In addition, constraint equations (used to represent relatively rigid parts) are not available in a p-method analysis.
15.3.4. Apply Loads and Obtain the Solution In this section you will take the following steps to obtain a solution for your model: 1.
Enter SOLUTION. Command(s): /SOLU GUI: Main Menu> Solution
2.
Define the analysis options. Choose any of three options to solve the simultaneous equations generated by a p-method analysis. These solvers are discussed at length in Chapter 3, “Solution” in the ANSYS Basic Analysis Guide. •
Frontal equation solver
•
Jacobian Conjugate Gradient equation solver (JCG)
•
Preconditioned Conjugate Gradient equation solver (PCG) (recommended) Command(s): EQSLV Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–7
Chapter 15: p-Method Structural Static Analysis GUI: Main Menu> Solution> Analysis Type> Sol'n Control ( : Sol'n Options Tab) Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options We generally recommend that you use the PCG solver for a p-element analysis. For most 3-D solid models and for very large 2-D models (usually greater than 40,000 DOF), the PCG solver is usually faster than the JCG and frontal solvers: •
The PCG solver is about 5 to 10 times faster than the frontal solver for p-elements.
•
The PCG solver is significantly faster than JCG for p-elements.
•
Computer-time savings will be greater with the PCG solver when p-levels of 4 and higher are active.
In certain cases, such as when your model contains elements with high aspect ratios or material type discontinuities, a greater number of iterations may be required to achieve convergence for the PCG solver. You may increase the maximum number of iterations by using the MULT option on the EQSLV command. This option is only valid when solving with the PCG solver. See the EQSLV command description in the ANSYS Commands Reference for more information on this capability. The PCG solver is not available for p-element shells. For more information on the general use of the PCG solver, refer to Chapter 3, “Solution” in the ANSYS Basic Analysis Guide. 3.
Apply the loads to the solid model (keypoints, lines, areas, etc.) or to the finite element model (nodes and elements), except for inertia loads (gravity, rotational velocity, etc.), which are independent of the model. For a general discussion of solid model loads versus finite element loads, see Chapter 2, “Loading” in the ANSYS Basic Analysis Guide. Internal Degrees of Freedom and Nodal Coordinate Systems In order to correctly apply boundary conditions, you need to understand nodal coordinate systems, and how degrees of freedom (DOFs) which are not attached to a node are handled. DOFs are the allowed motions or deformations of the elements. Those DOFs which are not attached to a node are referred to as internal degrees of freedom. •
Internal DOFs allow the elements to form a better approximation to the real solution. As the p-level is increased for each loop, more DOFs are added to the elements. Some of these DOFs act on the element boundary (edges and interior faces) resulting in deformations that vary from a polynomial order of 2 to 8. In many cases, the higher the p-level, the more complex the deformation, and the better the approximation to the real solution.
•
Nodal coordinate systems orient the degree of freedom directions at each node. Each node has its own nodal coordinate system, which, by default, is parallel to the global Cartesian system (regardless of the coordinate system in which the node was defined). Nodes may be rotated into a nodal coordinate system [NROTAT] (Main Menu> Preprocessor> Modeling> Move/Modify> Rotate Node CS> To Active CS). The constraints and forces are then applied to the nodes in the nodal coordinate systems. See the ANSYS Modeling and Meshing Guide for more details about nodal coordinate systems.
The program aligns the internal DOFs with the nodal coordinate systems as defined by the nodes on the element face or edge. Displacement constraints applied to nodes with rotated nodal coordinate systems are applied to the internal DOFs on an element edge or face only if ALL the nodes defining that edge or face are also rotated into that same coordinate system (see Figure 15.6: “Constraints on Rotated Nodes”). Therefore any symmetry/antisymmetry displacement boundary conditions applied to the nodes on adjoining surfaces 15–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.3: Using the p-Method should reference the same coordinate system. If you apply the symmetry/antisymmetry displacement boundary conditions to areas or lines, you should verify that the constraints all "point" in the same direction on each surface. If they do not, apply the boundary conditions to the individual nodes. Caution: If all of the DOFs of the nodes on an edge (or face) are not fully constrained (are only partially constrained, e.g. only UX is constrained) and the nodal rotations of these nodes are not the same, the stress results at these nodes may be inaccurate if the p-level of the attached elements exceeds 3. Nodal coordinate systems which are not necessarily parallel to the global Cartesian system are formed when you invoke symmetry or antisymmetry displacement constraints on model surfaces.
Figure 15.6 Constraints on Rotated Nodes
Loads Applicable to a p-Method Analysis Table 2.5: “Loads Applicable in a Static Analysis” of this manual describes the loads applicable to a static analysis. The following is a brief discussion of each type of loading. Displacements (UX, UY, UZ, ROTX, ROTY, ROTZ) are DOF constraints usually specified at model boundaries to define rigid support points. They are also used to indicate symmetry boundary conditions and points of known motion. The directions implied by the labels are in the nodal coordinate system. Displacement boundary conditions that are applied to all nodes on an element edge or face will also constrain the higher-order deformations along that edge or face. Conversely, if all of the nodes are not constrained in that direction, then those lower-order deformations will be constrained but not the higher-order ones. Never apply a displacement only at a midside node on an edge. (You may, however, apply a single constraint at a corner node.) Imposed motions may only vary linearly over an element edge or face. The program will ignore an imposed quadratic variation. Forces (FX, FY, FZ) are concentrated loads usually specified on the model exterior. The directions implied by the labels are in the nodal coordinate system. Moments (MX, MY, MZ) are concentrated loads usually specified on the model exterior. The directions implied by the labels are in the nodal coordinate system.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–9
Chapter 15: p-Method Structural Static Analysis Caution: Observe the following cautions: •
You should avoid applying single-point loads or constraints, since they cause stress singularities. If these loads or constraints are applied, exclude the elements attached to these nodes from the convergence computations. See the "Accounting for Stress Singularities" section later in this chapter.
•
Do not apply forces and moments to the midside nodes. You may only apply these loads at the corner nodes. In addition, out-of-plane (element ROTZ) moments may not be applied to SHELL150.
Pressures (PRES) are surface loads, also usually applied on the model exterior. Positive values of pressure act towards the element face (resulting in a compressive effect). Temperatures (TEMP) are applied to study the effects of thermal expansion or contraction (that is, thermal stresses). The coefficient of thermal expansion must be defined if thermal strains are to be calculated. You can read in temperatures from a thermal analysis, or you can specify temperatures directly on the nodes or the solid model keypoints. To obtain temperatures from a thermal analysis: •
Mesh the p-element model.
•
Convert the p-element types to the following thermal element types: PLANE145 to PLANE77, PLANE146 to PLANE35, SOLID147 to SOLID90, and SOLID148 to SOLID87. There is no thermal equivalent for SHELL150.
•
Run the thermal analysis.
•
Change the element types back to the p-element types in order to perform the p-method structural analysis.
•
For the remainder of the analysis, continue with the same procedure as defined for h-elements (see the ANSYS Thermal Analysis Guide).
Gravity, spinning, etc. are inertia loads that affect the entire structure. Density must be defined if inertia effects are to be included. 4.
Specify load step options. The following solution options are available to aid in solving a p-Method analysis: •
Convergence criteria specifications
•
Specifications for controlling p-levels
•
Accounting for stress singularities
As mentioned earlier in this section, a p-method analysis works with a series of iterations, or loops, checking for convergence each time. The PPRANGE command is used to specify the overall range where the p-level may vary (somewhere between 2 and 8). For analyses beginning at p=2, each element will have its solution checked for convergence against established criteria [PCONV]. If the solution is within the requested tolerance [PMOPTS], that element will have its p-level held to 2. Those elements that did not converge within the specified criteria (that is, not fixed at p=2 for the first iteration), will have their p-level increased, and another solution (iteration) will then be performed. At each iteration the convergence criteria (strain energy, displacement, stress, etc.) is checked, and if converged, the solution stops. Also, those elements whose individual solutions are considered to be converged will have their p-level held at the current p-level. This process is continued until all specified convergence criteria are met, or the maximum p-range has been reached. 15–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.3: Using the p-Method Convergence Criteria Specifications Convergence criteria may be global (for strain energy) or local. If you are specifically interested in the results at certain points in the model, then you should use local convergence criteria. Use this option to specify which areas of your model you would like to monitor for analysis convergence, as well as the type of criteria you would like to use to control convergence. Typically, you should select a few points of interest (nodes), at which to specify the convergence criteria (deflection, stress, strain, etc.). In most cases, the default convergence tolerance (5%) is sufficient for generally good results. You may want to lower this tolerance if you require a more accurate solution, such as for a fatigue evaluation. For a design study or optimization analysis, a higher tolerance will cut down on run times. Command(s): PCONV GUI: Main Menu> Preprocessor> Loads> Load Step Opts> p-Method> Convergence Crit For SHELL150, you also have the option to choose a layer (TOP, MID, or BOT) for stress or strain convergence criteria. If you are working with intersecting shells, it is recommended that you choose MID as the layer for convergence checking. Caution: Do not specify stress or strain criteria at nodes where there are singularities or at nodes along material interfaces. These locations will not converge due to the singularity. When choosing locations for specifying convergence criteria, you should concentrate your monitoring in the areas of high stress or at the point of maximum displacement rather than where stresses, strains, or displacements are relatively insignificant. Specifications for Controlling p-levels You may specify the starting (defaults to 2) and maximum (defaults to 8) p-levels that you wish to allow for your analysis [PPRANGE]. You may wish to start at a higher p-level if you have already completed an analysis and you want to perform a re-analysis (for a design change, for instance) and you know the final p-level where convergence will occur for most elements. You may also want to restrict the maximum plevel to less than 8 if conserving disk space or run time. Adjust the starting and maximum p-level in portions of your model using element KEYOPT selections. Accounting for Stress Singularities If the model contains any re-entrant (internal or concave) corners that are not modeled with a fillet radius, or contains point loads or any other areas of stress singularities, you should consider excluding these areas from the convergence computations. All elements that have a node at the singularity should be excluded. One exception applies to fracture mechanics. In that situation, you should not exclude elements at or near the crack tip. Command(s): PEXCLUDE GUI: Main Menu> Solution> Load Step Opts> p-Method> Strain Energy> Exclude Elems You can reassign, or re-include, elements for convergence checking. You may determine which elements have been included or excluded by listing [PINCLUDE,STAT; PEXCLUDE,STAT; or *GET] or plotting elements [EPLOT]. Excluded elements will appear `whited-out' in the plot. You may also select included or excluded elements by issuing the ESEL command directly [ESEL,,PEXC or ESEL,,PINC] (no GUI equivalent). This facilitates using these elements as a component [CM]. Command(s): PINCLUDE GUI: Main Menu> Solution> Load Step Opts> p-Method> Strain Energy> Include Elems 5.
Save a backup copy of the database. Command(s): SAVE Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–11
Chapter 15: p-Method Structural Static Analysis GUI: Utility Menu> File> Save As 6.
Start the p-level iterations and solution process. The output will provide a summary of each loop, indicating the current p-level, the convergence statistics, and the status of how many elements have converged. Command(s): SOLVE GUI: Main Menu> Solution> Solve> Current LS
15.3.5. Helpful Hints for Common Problems If the analysis is not successful, try the following steps to identify and correct the cause for failure: Problem: "Negative Pivot" error encountered. Possible Cause: Insufficient constraints to prevent rigid-body motion (the component can slide or rotate in one direction because there are no constraints to prevent it from doing so). Solution: Add enough displacement constraints to prevent any rigid-body motion. Problem: Solution does not converge to within the requested tolerance. Possible Causes: There are several possible causes. You may use the general postprocessor [/POST1] to look at this solution in order to determine the difficulty. Possible Causes The convergence criteria is too tight for the maximum allowable plevel and the mesh.
Solution Relax the convergence criteria.
The convergence criterion was specified at a singularity (infinite stress Do not monitor a singularity point. or strain value, such as under a point load) or the elements near the singularity were not excluded. The mesh is too coarse, especially in the area where the stress is high. Refine the mesh. The maximum p-level was restricted lower than that required for convergence.
Allow the maximum p-level to go higher.
The convergence criterion is at a location where the angle made by Refine the mesh in that region. adjacent element edges is greater than 55° on a curved boundary.
Caution: You may not restart a p-method analysis.
15.3.6. Review the Results The fundamental procedures for general postprocessing of results [/POST1] in the ANSYS program are discussed in Chapter 4, “An Overview of Postprocessing” in the ANSYS Basic Analysis Guide. Although most of these capabilities are directly applicable to p-method analyses, some techniques for reviewing results are unique to pmethod, such as •
The p-Element Subgrid
•
Querying Subgrid Results
•
Printing and Plotting Node and Element Results
•
Specialized p-Method Displays and Listings
The results from a p-method analysis are written to the results file, Jobname.RST. They consist of the following data:
15–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.3: Using the p-Method Primary data Nodal displacements (UX, UY, ROTX, etc.) Derived data Nodal and element stresses, nodal and element strains, element forces Note — You must read the results data from the results file (Jobname.RST) into the database [SET] before displacements may be reviewed during postprocessing. Thermal strains are not available on the results file. The tools used for time-history postprocessing [/POST26] are also applicable to p-method analyses, but have limited functionality, since p-element technology is restricted to linear static analyses. In this section we will explain those procedures that deviate from standard postprocessing, such as some plotting and printing operations, etc. Before reading this section, it would be a good idea to review the chapters on postprocessing in the ANSYS Basic Analysis Guide for more details on postprocessing, in general.
15.3.6.1. The p-Element Subgrid As mentioned previously, p-method finite element models generally contain fewer elements than do models meshed with h-elements. Since fewer elements correspond to a coarser mesh, a subgrid approach has been devised for viewing results in POST1. In this approach, each element is divided into smaller, "h-like" elements. Both the display of geometric curvature and the display and printout of field quantities (displacements, stresses, etc.) are affected by this approach. In most cases, a greater number of facets will result in a smoother representation of the element surface and results contours for p-element plots. The key command involved in the subgrid approach is /EFACET,NUM where NUM represents the number of facets per element edge (GUI path Utility Menu> PlotCtrls> Style> Size and Shape). The example below illustrates how /EFACET subdivides a quadrilateral element. If NUM = 2, the element has 2 facets per edge and is divided into 4 subgrid facets by adding a pseudo node at the "center". If NUM = 4, the element has 4 facets per edge which means two pseudo nodes per edge and 9 interior pseudo nodes are added for each p-element, dividing the quadrilateral into 16 subgrid facets.
Figure 15.7 p-Element Subgrids for Quadrilateral Elements
As a general rule, for a model with a very coarse mesh or any model in which the p-levels are high (p>3) you should consider using NUM = 4 to view your field quantities. Since results are available at each subgrid location, more information will be available at NUM = 4.
15.3.7. Querying Subgrid Results You have the ability to directly and interactively query subgrid results. You can obtain all subgrid point results (or element results). Command(s): No command equivalent. GUI: Main Menu> General Postproc> Query Results Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–13
Chapter 15: p-Method Structural Static Analysis You may query stresses, strains, and displacements at all subgrid locations that have previously been activated by the /EFACET command.
15.3.8. Printing and Plotting Node and Element Results For elements PLANE145, PLANE146, SOLID147, and SOLID148, displacements, stresses, and strains can be listed [PRNSOL] at all node locations (both corner and midside nodes). For SHELL150, results can be listed (as controlled by the SHELL command) and plotted at the top/bottom and middle layer locations. Likewise, these nodal values can be contoured for display purposes [PLNSOL], with the contour resolutions being controlled by the/EFACET command. Note — Results values for SHELL150 are displayed for the top and bottom layer simultaneously. When viewing nodal field values across p-element boundaries ([PRNSOL, PLNSOL], or when using the Query function), results may be displayed in various ways. The results data may be averaged along element boundaries with the AVRES command. You can average results at all boundaries (the default), or at all boundaries except where real constant, and/or material type discontinuities exist. If a geometric discontinuity exists, results will not be averaged at those locations. Note — AVRES has no effect on the nodal degree of freedom solution values (UX, UY, UZ, ROTX, ROTY, ROTZ, etc.). For all of the p-elements, displacement plots are available with both undisplaced structure and undisplaced edge options [PLDISP]. When using PowerGraphics [/GRAPHICS,POWER], displaced shape plots reflect each calculated element subgrid [/EFACET] displacement. For PLANE145, PLANE146, SOLID147, and SOLID148, stresses and strains can be listed [PRESOL] at all node locations for each element. Results for SHELL150 are listed for the top, middle, and bottom layers with results for the bottom layer listed first. Printout is similar to that for h-elements, with nodal results being unaveraged and sorted by element number. Unlike higher order h-element printout, results are for all nodal locations (corner and midside nodes). Results may be printed or plotted for the entire model [/GRAPHICS,FULL] or for the model surface only [/GRAPHICS,POWER]. Note — Issuing the /PMETH,ON command or defining a p-element [ET] will activate PowerGraphics unless a prior /GRAPHICS,FULL command has been issued. Similarly, /PMETH,OFF will deactivate PowerGraphics unless /GRAPHICS,POWER has been issued previously.
15.3.8.1. Specialized p-Method Displays and Listings There are three commands specifically designed for listing or plotting p-element results data [PRCONV, PLCONV, PPLOT]. You may print [PRCONV] or plot [PLCONV] the previously-specified convergence values [PCONV] versus characteristic p-levels. The characteristic p-level refers to the p-level range from the minimum specified [PPRANGE] to the maximum p-level reached during SOLUTION. Final p-levels that were assigned to individual elements can be viewed by means of the PPLOT command. A convenient way to visualize local convergence criteria at specified locations in the model is to display a symbol at the location of interest, [/PSYMB,PCON], then issue an element or node plot.
15.4. Sample p-Method Analysis (GUI Method) Follow the steps below to perform a p-method analysis using the GUI.
15–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.4: Sample p-Method Analysis (GUI Method)
15.4.1. Problem Description In this sample problem, you will perform a p-method analysis on a steel plate with a hole.
15.4.2. Problem Specifications For this problem, you will use symmetry boundary conditions to constrain the left side and bottom of the model. This problem uses element type PLANE145. The material is 1/4" thick steel. Loading for this problem is: P = (100) (10) (.25) = 250 lbs (total force applied on the right side).
15.4.3. Problem Diagram Figure 15.8 Steel Plate With a Hole
15.4.3.1. Set the Analysis Title After you enter the ANSYS program, follow these steps to set the title. 1.
Choose menu path Utility Menu> File> Change Title.
2.
Type the text "p-Method Plate with Hole" and click on OK.
15.4.3.2. Select p-Method 1.
Choose menu path Main Menu> Preferences. The Preferences for GUI Filtering dialog box appears.
2.
Click the Structural method on. Click the p-Method Struct. option on.
3.
Click on OK.
15.4.3.3. Define the Element Type and Options 1.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete.
2.
Click on Add. The Library of Element Types dialog box appears.
3.
Click on OK to accept the default of "2D Quad 145."
4.
Click on Options. The PLANE145 element type options dialog box appears. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–15
Chapter 15: p-Method Structural Static Analysis 5.
In the scroll box for Analysis type, scroll down to "Plane Stress+TK" to select it.
6.
Click on OK.
7.
Click on Close in the Element Types dialog box.
15.4.3.4. Define the Real Constants 1.
Choose menu path Main Menu> Preprocessor> Real Constants> Add/Edit/Delete.
2.
Click on Add. The Element Type for Real Constants dialog box appears.
3.
Click on OK. The Real Constants for PLANE145 dialog box appears.
4.
Enter .25 for thickness and click on OK.
5.
Click on Close to close the Real Constants dialog box.
15.4.3.5. Define Material Properties 1.
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.
2.
In the Material Models Available window, double-click on the icons next to the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
3.
Enter 30e6 for EX (Young's modulus).
4.
Enter 0.29 for PRXY and click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
5.
Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.
15.4.3.6. Create Plate with Hole 1.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Areas> Rectangle> By Dimensions. The Create Rectangle by Dimensions dialog box appears.
2.
Enter 0,20 for the X-coordinates and 0,10 for the Y-coordinates. Use the TAB key to move between fields.
3.
Click on OK. The rectangle appears in the ANSYS Graphics window.
4.
Choose menu path Main Menu> Preprocessor> Modeling> Create> Areas> Circle> By Dimensions. The Circular Area by Dimensions dialog box appears.
5.
Enter 5 for outer radius.
6.
Click on OK. The circle appears on the ANSYS Graphics window, on the lower left corner of the rectangle.
7.
Choose menu path Main Menu> Preprocessor> Modeling> Operate> Booleans> Subtract> Areas. The Subtract Areas picking menu appears.
8.
Click once on the rectangle to select it.
9.
Click on OK in the picking menu. Another Subtract Areas picking menu appears.
10. Click once on the circle to select it. 11. Click on OK in the picking menu. A semicircle is removed from the lower left-hand corner of the plate.
15.4.3.7. Mesh the Areas 1.
Choose menu path Main Menu> Preprocessor> Meshing> MeshTool. The MeshTool appears.
2.
Click the SmartSize check box on. Set the SmartSize slider to 5.
15–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 15.4: Sample p-Method Analysis (GUI Method) 3.
In the Mesh section of the MeshTool, choose Areas and Free. Then click the MESH button. The Mesh Areas picking menu appears.
4.
Click on Pick All. A mesh for the plate is created.
5.
Click Close to close the MeshTool.
6.
Click on SAVE_DB on the ANSYS Toolbar.
15.4.3.8. Define Symmetry Boundary Conditions 1.
Choose menu path Utility Menu> Select> Entities.
2.
In the top two menus, pick "Nodes" and "By Location."
3.
Enter 0 for Min, Max and click on OK.
4.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> Symmetry B.C.> On Nodes. The Apply SYMM on Nodes dialog box appears.
5.
Click on OK to accept the default of symmetric surface normal to X-axis. The displacement symbols appear down the left edge of the drawing.
6.
Choose menu path Utility Menu> Select> Entities.
7.
Click the "Y coordinates" option on. Click OK.
8.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> Symmetry B.C.> On Nodes. The Apply SYMM on Nodes dialog box appears.
9.
In the drop down menu for Symm surface is normal to, select "Y-axis."
10. Click OK. The displacement symbols appear along the bottom of the drawing.
15.4.3.9. Define Pressure Load along Right Edge. 1.
Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears.
2.
Click the "X coordinates" option on.
3.
Enter 20 for Min, Max and click on OK.
4.
Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Pressure> On Nodes. The Apply PRES on Nodes picking menu appears.
5.
Click on Pick All. The Apply PRES on Nodes dialog box appears.
6.
Enter 100 for pressure value and click on OK.
7.
Choose menu path Utility Menu> Select> Everything.
15.4.3.10. Define Convergence Criteria 1.
Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.
2.
In the Selection field, enter NCVG = NODE(0,5,0) and click on Accept.
3.
Click on Close.
4.
In the ANSYS Input window, enter PCONV,1,S,X,NCVG and press ENTER.
15.4.3.11. Solve the Problem 1.
Choose menu path Main Menu> Solution> Solve> Current LS. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
15–17
Chapter 15: p-Method Structural Static Analysis 2.
Carefully review the information in the status window, and then close it.
3.
Click on OK in the Solve Current Load Step dialog box to begin the solution.
4.
Click on Close when the Solution is done window appears.
15.4.3.12. Review the Results and Exit ANSYS In this step, you will review results as deformed shape and SX contour plot. 1.
Choose menu path Main Menu> General Postproc> Read Results> First Set.
2.
Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears.
3.
Click the "Def + undeformed" option on. Click on OK. The deformed and undeformed shapes appear in the ANSYS Graphics window.
4.
Choose menu path Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu. The Contour Nodal Solution Data dialog box appears.
5.
In the scroll box on the left, click once on "Stress" to select it. In the scroll box on the right, click once on "X-direction SX" to select it.
6.
Click on OK. Review the graphic using the legend in the graphics window. Expected results are: Max displacement = .97x10-4 in, and Max stress in X direction = 437 psi.
7.
Click on QUIT on the ANSYS Toolbar.
8.
Choose a save option and click on OK.
15.5. Sample p-Method Analysis (Command or Batch Method) You can perform the example p-method analysis of a plate with a hole using the ANSYS commands shown below instead of GUI choices. All items prefaced by an exclamation point (!) are comments. /TITLE, p-method plate with hole problem /PREP7 ET,1,PLANE145,,,3 R,1,.25 MP,EX,1,30e6 MP,PRXY,1,0.29 RECTNG,0,20,0,10 PCIRC,5,,0,360 ASBA,1,2 SMRTSIZ,5 AMESH,3 SAVE FINISH /SOLU NSEL,S,LOC,X,0 DSYM,SYMM,X NSEL,S,LOC,Y,0 DSYM,SYMM,Y NSEL,S,LOC,X,20 SF,ALL,PRES,-100 ALLSEL NCVG=NODE(0,5,0) PCONV,1,S,X,NCVG SOLVE /POST1 SET,1 PLNSOL,S,X PLDISP,1 FINISH
15–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 16: Beam Analysis and Cross Sections 16.1. An Overview of Beams Beam elements are used to create a mathematical one-dimensional idealization of a 3-D structure. They offer computationally efficient solutions when compared to solid and shell elements. The discussion in this chapter applies only to BEAM44, which is a 3-D tapered unsymmetric beam; and BEAM188 and BEAM189, which are 3-D finite strain beams. These beams provide more robust nonlinear analysis capabilities, and significant improvements in cross section data definition, analysis, and visualization, as compared to other ANSYS beams. See the descriptions of the BEAM44, BEAM188, and BEAM189 elements in the ANSYS Elements Reference for more information. Note — If you are using the cross section capabilities described in this chapter with BEAM44 elements, be aware that you cannot use these capabilities to define tapered sections. In addition, the postprocessing visualization capabilities described in this chapter are not applicable to BEAM44 elements. Note — Custom cross sections may not be used with the CDWRITE command.
16.2. What Are Cross Sections? A cross section defines the geometry of the beam in a plane perpendicular to the beam axial direction. ANSYS supplies a library of eleven commonly-used beam cross section shapes, and permits user-defined cross section shapes. When a cross section is defined, ANSYS builds a numeric model using a nine node cell for determining the properties (Iyy, Izz, etc.) of the section and for the solution to the Poisson's equation for torsional behavior. Figure 16.1: “Plot of a Z Cross Section” shows the centroid and shear center of the cross section and the calculated section properties:
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 16: Beam Analysis and Cross Sections
Figure 16.1 Plot of a Z Cross Section
Cross sections and user section meshes may be saved and stored in cross section library files. You may assign beam cross sections as attributes of a line using the LATT command. These section definitions will be incorporated into the generated beam elements when the line is meshed with BEAM44, BEAM188, or BEAM189.
16.3. How to Create Cross Sections The general procedure for creating cross sections consists of the following steps: 1.
Define the section and associate a section ID number with the section subtype.
2.
Define the geometry data for the section.
ANSYS supplies the following commands for creating, viewing, and listing cross sections, and for managing cross section libraries:
Table 16.1 ANSYS Cross Section Commands Command
GUI Menu Path
Purpose
PRSSOL
Main Menu> General Postproc> List Results> Section Solution Utility Menu> List> Results> Section Solution
Prints beam section results (not supported for BEAM44)
SECTYPE
Main Menu> Preprocessor> Sections> Beam> Common Sectns Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Read Sect Mesh
Associates section Subtype with
16–2
SECID
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.3: How to Create Cross Sections Command
GUI Menu Path
Purpose
SECDATA
Main Menu> Preprocessor> Sections> Beam> Common Sectns
Defines section geometry data
SECOFFSET
Main Menu> Preprocessor> Sections> Beam> Common Sectns Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Read Sect Mesh
Defines section offset for beam cross sections
SECCONTROLS
Main Menu> Preprocessor> Sections> Beam> Sect Control
Overrides program calculated properties.
SECNUM
Main Menu> Preprocessor> Meshing> Mesh At- Identifies the SECID to be assigned to an element tributes> Default Attribs Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes
SECPLOT
Main Menu> Preprocessor> Sections> Beam> Plot Section
Plots geometry of a beam section to scale
SECWRITE
Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Write From Areas
Creates an ASCII file containing user mesh or a custom cross section
/SECLIB
Main Menu> Preprocessor> Sections> Section Library> Library Path
Sets default section library path for SECREAD
SECREAD
Main Menu> Preprocessor> Sections> Section Library> Import Library Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Read Sect Mesh
Reads a user defined section library, mesh, or custom cross section
SLIST
Main Menu> Preprocessor> Sections> List Sec- Summarizes section properties tions Utility Menu> List> Properties> Section Properties Utility Menu> List> Properties> Specified Section Properties
SDELETE
Main Menu> Preprocessor> Sections> Delete Section
Deletes a cross section
For complete documentation of the cross section commands, see the ANSYS Commands Reference.
16.3.1. Defining a Section and Associating a Section ID Number Use the SECTYPE command to define a section and associate it with a section ID number. For example, the following command assigns a section identification number (2) to a predefined cross section shape (circular solid): Command(s): SECTYPE, 2, BEAM, CSOLID GUI: Main Menu> Preprocessor> Sections> Beam> Common Sectns To define your own cross sections, use the subtype MESH. To define a cross section with integrated properties such as Iyy and Izz, use the subtype ASEC.
16.3.2. Defining Cross Section Geometry and Setting the Section Attribute Pointer Use the SECDATA command to define the geometry of a cross section. Continuing with the example SECTYPE command shown above, note that the CSOLID subtype has two dimensions: the radius and the number of cells along its circumference. Thus, the SECDATA command shown below specifies 5 as the radius of the circular Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–3
Chapter 16: Beam Analysis and Cross Sections solid beam, and 8 as the number of cells along its circumference. The SECNUM command sets the element section attribute pointer to 2. Command(s): SECDATA, 5, 8 and SECNUM, 2 GUI: Main Menu> Preprocessor> Sections> Beam> Common Sectns Main Menu> Preprocessor> Meshing> Mesh> Attributes> Default Attribs
16.3.2.1. Determining the Number of Cells to Define In general, you do not need to set the number of cells when building a cross section. ANSYS will calculate values for the cross section such as the area of the section and the moments of inertia about the coordinate axes using default integration rules and will produce results that are numerically exact. Since the torsion constant is derived from the mesh, the accuracy of the torsion constant is directly proportional to the mesh size of the cross section. The default mesh used by ANSYS yields acceptable engineering accuracy. There are two ways to specify the mesh size for common sections: •
invoking SECTYPE,,,,,REFINEKEY to set the level of mesh refinement for thin-walled sections (CTUBE, CHAN, I, Z, L, T, HATS, and HREC)
•
specifying the number of divisions using SECDATA for solid sections (RECT, QUAD, and CSOLID)
The thin wall sections have a minimum of two integration points through thickness, so results produced using thin wall sections should be acceptable for materially nonlinear analysis. However, when doing a plasticity analysis, the cell defaults may need to be changed for the solid sections. Here are examples of ANSYS-generated solid section cell meshes and the type of analysis you may wish to use them with.
Figure 16.2 Types of Solid Section Cell Mesh
16.3.3. Meshing a Line Model with BEAM44, BEAM188, or BEAM189 Elements Before you mesh a line with BEAM44, BEAM188, or BEAM189 elements, some of its attributes must be defined. These attributes include: •
The material set attribute pointer to be associated with the generated beam elements.
•
The beam element type to be used in meshing the line.
•
The orientation of the cross section with respect to the beam element axis. For detailed information about orientation nodes and beams, see Section 7.5.2: Generating a Beam Mesh With Orientation Nodes in the ANSYS Modeling and Meshing Guide.
16–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.4: Creating Cross Sections •
The cross section ID to be assigned to the generated beam elements.
Issue the LATT command to associate these attributes with the selected, unmeshed line: Command(s): LATT, MAT, , TYPE, , KB, KE, SECNUM GUI: Main Menu> Preprocessor> Meshing> Mesh Attributes> Picked Lines See the LATT command description for the meaning of MAT and TYPE. The following arguments are described here in terms of their applicability to beams. KB
Corresponds to any keypoint number in the model. All beam elements generated will have their beam section oriented such that the beam z-axis will lie in the plane defined by two line end keypoints and this keypoint number. KE
Corresponds to any keypoint number in the model (optional). This keypoint determines the beam orientation at the end of the line as described above. If KE is given, KB determines the beam orientation at the beginning of the line. This is useful for creating twisted beams. SECNUM
Corresponds to the beam section defined by the SECTYPE command with the section ID number as given by the SECNUM.
16.4. Creating Cross Sections There are two main types of beam cross sections: •
common sections
•
custom sections
Common sections are described by a standard geometry and a single material. Custom sections are defined by an arbitrary geometry and may consist of several isotropic materials. In addition, you can use defined sections to create tapered beams (for BEAM188 and BEAM189 only). See Section 16.4.5: Defining a Tapered Beam for more information.
16.4.1. Using the Beam Tool to Create Common Cross Sections The SECTYPE, SECDATA, and SECOFFSET commands (Main Menu> Preprocessor> Sections> Beam> Common Sectns) are all associated with the BeamTool in the GUI. The appearance of the BeamTool varies depending on the cross section subtype you select:
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–5
Chapter 16: Beam Analysis and Cross Sections
Figure 16.3 BeamTool with Subtypes Drop Down List Displayed
The top part of the BeamTool relates a section ID number to a subtype (and, optionally, a section name) [SECTYPE]. The middle of the BeamTool defines the section offset information, if needed [SECOFFSET]. The bottom contains the fields for section geometry information [SECDATA]. The dimensions defined by the SECDATA command are determined by the subtype selected. For documentation about a particular variant of the BeamTool, select the subtype that you want information about, and then click on the Help button on the BeamTool. The subtype dimensions are also documented in the SECDATA command description.
16.4.2. Creating Custom Cross Sections with a User-defined Mesh If you need to define a cross section that is not common, you must create a user mesh file. To create a user mesh file, create a 2-D solid model and save it using the SECWRITE command (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Write From Areas). This procedure is outlined in greater detail below: 1.
Create all areas (Main Menu> Preprocessor> Modeling> Create> Areas).
2.
Overlap the areas (Main Menu> Preprocessor> Modeling> Operate> Booleans> Overlap> Areas) or glue them (Main Menu> Preprocessor> Modeling> Operate> Booleans> Glue> Areas) where appropriate.
3.
Save the model.
16–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.4: Creating Cross Sections 4.
Set the number of line divisions for all lines (Main Menu> Preprocessor> Meshing> Size Cntrls> ManualSize> Lines> Picked Lines or use the MeshTool).
5.
Select Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Write From Areas. A picker appears. Pick the area(s) of the cells.
6.
ANSYS creates cells on the areas. ANSYS may display bad shape messages during the mesh - these messages can be ignored. However, you may see an "Unable to mesh area ...." message. If you do, clear the elements from all areas (Main Menu> Preprocessor> Meshing> Clear> Areas) and repeat steps 4 and 5.
7.
Write the .SECT file out to a unique name in the Write Section Library File dialog box and click on OK.
8.
Read in the user mesh file (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Read Sect Mesh) to calculate the section properties. Material properties must be defined to calculate the cross section shear correction factors, material-weighted centroids and the shear centers.
Note — Even if you have already set LESIZE, you will see the following message: Line element sizes may need to be specified for desired cross-section mesh. Please refer to the LESIZE command. If you have already set the line element size, click on the Close button to continue. If you have not already set it, issue LESIZE with the appropriate information. When creating cells on the area using the GUI, you do not need to define a plane element type. On the other hand, a plane element type must be defined if the user issues the SECWRITE command explicitly. MESH200 with KEYOPT(1) = 7 and PLANE82 are the only valid plane element types.
16.4.3. Creating Custom Cross Sections with Mesh Refinement and Multiple Materials When doing a plasticity analysis, you may need to refine the cross section mesh. A cross section consisting of more than one material may be defined to represent layers, reinforcements or sensors. When defining a multiplematerial cross section, you will need to specify the material that each cross section cell is made of. You may take a previously-created cross section and modify it. To create a custom cross section with a refined mesh and/or multiple materials, perform the following tasks: 1.
Either read a common section (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Built-up> Edit Common) from the ANSYS database or read a custom section from a .SECT file. (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Built-up> Edit Custom)
2.
ANSYS displays a MESH200 plot in the Graphics Window.
3.
Refine the section mesh. (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Builtup> Refine Mesh)
4.
Modify the cell materials. (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Builtup> Modify Material) If you want to create a multiple-material section, define the materials. This is necessary to calculate the shear correction factors and material-weighted centroids.
5.
Save the section to a .SECT file using SECWRITE (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Built-up> Save).
6.
To calculate the section properties and use a custom section in the analysis, read in the user mesh file (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Read Sect Mesh).
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–7
Chapter 16: Beam Analysis and Cross Sections Note — If you redefine a material after creating the section, you must reissue the SECTYPE and SECREAD commands to recompute the cross section. When a cross section has multiple materials, and /ESHAPE is used to produce contour plots of stresses (and other quantities), the element averages the stresses across material boundaries. To limit this behavior, use small cross section cells around the material boundaries. When a cross section has multiple materials, the multiple materials will not be displayed in an element plot with /ESHAPE,1. The multiple materials can be verified by viewing the cross section in the Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Built-up> Edit Custom submenu. When using the SECWRITE command explicitly, a section with multiple materials can be created by assigning material attributes to the areas. During meshing, the elements inherit the material attribute from the area and this attribute is written to the .SECT file.
16.4.4. Defining Composite Cross Sections A composite cross section is a cross section consisting of at least two materials and meshed with a user-defined mesh. When creating a composite section, define the materials before running the SECREAD command. This is necessary to calculate the shear correction factors, material-weighted centroids and the shear centers. Note — If you redefine a material after creating the section, you must reissue the SECREAD command to recompute the cross section. You can save composite cross sections as custom cross sections. For information on custom cross sections, see Section 16.4.1: Using the Beam Tool to Create Common Cross Sections
16.4.5. Defining a Tapered Beam For BEAM188 and BEAM189, you can define tapered beams using the TAPER option on the SECTYPE command (Main Menu> Preprocessor> Sections> Beam> Taper Sections). The tapered section varies linearly between two specified locations, (x1, y1, z1) and (x2, y2, z2). Thus, two SECDATA commands are required to define the taper as shown below. At each of these end points, a valid beam section ID must be input (station-1 and station2 in the example below). SECTYPE,SECID,TAPER SECDATA,station-1,x1,y1,z1 SECDATA,station-2,x2,y2,z2 The following is a typical command input stream used to create a tapered cross section: sectype,1,beam,rect secdata,.0001,0.5 sectype,2,beam,rect secdata,3,0.5 sectype,3,taper secdata,1,0.0,0.0 secdata,2,0.0,20.0
! define cross section at first end point ! define cross section at far end ! new Section ID for tapered beam analysis ! section 1 at location (0,0,0) ! section 2 at location (0,20,0)
Continuing with this example, you can then use 3 as the taper section ID when assigning mesh attributes with the SECNUM or LATT command. The resulting beam cross section is (0.0001*0.5) at end 1, and linearly tapers to (3*0.5) at end 2. The following assumptions apply to tapered beams defined with this method: •
The end sections must be defined prior to defining the taper.
•
Sections defined at the end points must be topologically identical.
16–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.6: Sample Lateral Torsional Buckling Analysis (GUI Method) •
A section cannot taper to a point (or zero area) at either end.
•
The arbitrary beam section type (ASEC on the SECTYPE command) is not supported for tapered beams.
The program performs a number of checks (although not completely comprehensive) to ensure topological equality. The following items are compared: •
number of section nodes
•
number of section elements
•
section type
If both end stations refer to custom cross sections with multiple materials, you must ensure that material IDs for the cells are the same for both ends. At a Gauss point of integration, the BEAM188 and BEAM189 elements will find the closest point on the line defined by station-1 and station-2. Using this information, a linear interpolation is performed for the cross section mesh. Therefore, it is very important that the Gauss point be located within the end points. ANSYS will produce error messages when this is not the case. The tapered section treatment is significantly more expensive than a constant cross section (since recomputation is necessary). If this is a concern, use KEYOPT(12) of the beam element to specify the tapered section treatment. •
KEYOPT(12) = 0 - Linear tapered section analysis (more accurate, but expensive)
•
KEYOPT(12) = 1 - Average cross section analysis (an approximation of the order of the mesh size, but faster)
16.5. Managing Cross Section and User Mesh Libraries Cross section data for common sections such as CHAN and RECT can be stored in cross section libraries. To create standard cross sections for later use, create one or more cross sections, edit the Jobname.LOG file, and copy the appropriate SECTYPE, SECDATA, and SECOFFSET commands into a separate file with a SECT extension. These predefined cross sections can later be read into a model using the /SECLIB command (Main Menu> Preprocessor> Sections> Section Library> Import Library).
16.6. Sample Lateral Torsional Buckling Analysis (GUI Method) You can use BEAM188 and BEAM189 elements to model not only straightforward beam bending and shear response but also to model beam response that involves lateral-torsional buckling. To create this type of model, you will need to create an adequately fine mesh of beam elements. You typically need to model a single beam member using a series of short beam elements, as shown in Figure 16.4: “Lateral-Torsional Buckling of a Cantilever I-Beam”.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–9
Chapter 16: Beam Analysis and Cross Sections
Figure 16.4 Lateral-Torsional Buckling of a Cantilever I-Beam
Lateral-Torsional Buckling of a Cantilever I-Beam, Modeled With 60 BEAM188 Elements (Displayed Using /ESHAPE) Chapter 7, “Buckling Analysis” in the ANSYS Structural Analysis Guide documents buckling analysis in detail. This sample problem shows what happens when a cantilever beam is subjected to a concentrated end load, which causes lateral-torsional buckling.
16.6.1. Problem Description A straight, slender cantilever beam has one fixed end and one free end. A load is applied to the free end. The model is analyzed using eigenvalue buckling calculations, followed by a nonlinear load versus deflection study. The objective is to determine the critical value of the end load (indicated by P in Figure 16.5: “Diagram of a Beam With Deformation Indicated”) at which the beam undergoes a bifurcation indicated by a large displacement in the lateral direction.
16.6.2. Problem Specifications The following material properties are used for this problem: Young's modulus = 1.0 X 104 psi Poisson's ratio = 0.0 16–10
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.6: Sample Lateral Torsional Buckling Analysis (GUI Method) The following geometric properties are used for this problem: L = 100 in H = 5 in B = .2 in Loading for this problem is: P = 1 lb.
16.6.3. Problem Sketch Figure 16.5 Diagram of a Beam With Deformation Indicated
16.6.4. Eigenvalue Buckling and Nonlinear Collapse Eigenvalue buckling calculation is a linearized calculation, and is generally valid only for elastic structures. The yielding of materials occurs usually at loads lesser than that predicted by eigenvalue buckling analysis. This type of analysis tends to need less computation time than a full nonlinear buckling analysis. You can also perform a nonlinear load versus deflection study, which employs an arc length solution strategy to identify critical loads. While the approach is more general, a collapse analysis may be computationally intensive. The nonlinear collapse analysis must be performed on a structure with imperfections built in to the model, since a perfect model will not show signs of buckling. You can add imperfections by using eigenvectors that result from an eigenvalue buckling analysis. The eigenvector determined is the closest estimate of the actual mode of buckling. The imperfections added should be small when compared to a typical thickness of the beam being analyzed. The imperfections remove the sharp discontinuity in the load-deflection response. It is customary to use one to ten percent of the beam/shell thickness as the maximum imperfection introduced. The UPGEOM command adds displacements from a previous analysis and updates the geometry to the deformed configuration.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–11
Chapter 16: Beam Analysis and Cross Sections
16.6.5. Set the Analysis Title and Define Model Geometry 1.
Choose menu path Utility Menu> File> Change Title.
2.
Enter the text "Lateral Torsional Buckling Analysis" and click on OK.
3.
Start the model creation preprocessor and define the keypoints for the beam. Choose menu path Main Menu> Preprocessor> Modeling> Create> Keypoints> In Active CS, and enter these keypoint numbers and the coordinates in the dialog box as indicated: Keypoint Number
X Location
Y Location
Z Location
Click This Button to Accept Values
1
0
0
0
Apply
2
100.0
0
0
Apply
3
50
5
0
OK
4.
Create a straight line through keypoints 1 and 2. Choose menu path Main Menu> Preprocessor> Modeling> Create> Lines> Lines> Straight Line. The Create Straight Line picker appears. Select keypoints 1 and 2 in the Graphics window and click on OK in the Create Straight Line picker.
5.
Save the model. Choose menu path Utility Menu> File> Save As. Enter buckle.db in the Save Database to box and click on OK.
16.6.6. Define Element Type and Cross Section Information 1.
Choose menu path Main Menu> Preferences and select the "Structural" check box. Click on OK to continue.
2.
Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete. The Element Types dialog box appears.
3.
Click on Add ... The Library of Element Types dialog box appears.
4.
In the scroll box on the left, click on "Structural Beam" to select it.
5.
In the scroll box on the right, click on "3D finite strain, 3 node 189" to select BEAM189.
6.
Click on OK, and then click on Close in the Element Types dialog box.
7.
Define a rectangular cross section for the beam. Choose menu path Main Menu> Preprocessor> Sections> Beam> Common Sectns. The BeamTool is displayed. ANSYS sets the section ID to 1, and the subtype to RECT (signified by a rectangle on the subtype button) by default. Since you will be creating a rectangular cross section, there is no need to change the subtype.
8.
In the lower half of the BeamTool, you will see a diagram of the cross section shape with dimension variables labeled. Enter the width of the cross section, 0.2, in the box labeled B. Enter the height of the cross section, 5.0, in the box labeled H. Click on Apply to set the cross section dimensions.
9.
Use the BeamTool to display information about the cross section. Click on the Preview button on the BeamTool. A diagram and data summary of the cross section appear in the Graphics window. You can also preview the mesh of the cross section by selecting the Meshview button. Click on the Close button in the BeamTool to continue.
16.6.7. Define the Material Properties and Orientation Node 1.
16–12
Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.6: Sample Lateral Torsional Buckling Analysis (GUI Method) 2.
In the Material Models Available window on the right, double-click on the following: Structural, Linear, Elastic, Isotropic. A dialog box appears.
3.
Enter 1E4 for EX (Young's modulus).
4.
Enter 0.0 for PRXY (Poisson's ratio), and click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
5.
Choose menu path Material> Exit to close the Define Material Model Behavior dialog box.
6.
Replot the line by choosing menu path Utility Menu> Plot> Lines.
7.
Select the line and define the orientation node of the line as an attribute. Choose menu path Main Menu> Preprocessor> Meshing> Mesh Attributes> Picked Lines. The Line Attributes picker appears. Select the line in the Graphics window and click on Apply in the Line Attributes picker.
8.
The Line Attributes dialog box appears. ANSYS includes the material attribute pointer to the material set 1, the element type attribute pointer to the local element type 1, and the section attribute pointer to the section ID 1 by default. Click on the radio button beside the Pick Orientation Keypoint(s) label to change it to Yes and click on OK.
9.
The Line Attributes picker reappears. Type 3 in the picker, press the Enter key, and click on OK.
10. Save the model. Choose menu path Utility Menu> File> Save As. If the buckle.db file is not already selected, select it. Select OK, and when ANSYS prompts you if you want to overwrite the existing file, click on OK.
16.6.8. Mesh the Line and Verify Beam Orientation 1.
Define the mesh size and number of divisions. Choose menu path Main Menu> Preprocessor> Meshing> Size Cntrls> ManualSize> Lines> All Lines. Enter 10 in the No. of Element Divisions box and click on OK.
2.
Mesh the line. Choose menu path Main Menu> Preprocessor> Meshing> MeshTool. Click on MESH on the MeshTool and the Mesh Lines picker appears. Pick the line in the Graphics window, and then click on OK in the Mesh Lines picker. Click on Close in the MeshTool to close it.
3.
Rotate the meshed line. Choose menu path Utility Menu> PlotCtrls> Pan, Zoom, Rotate. The Pan, Zoom, Rotate tool appears. Select ISO and click on Close. The beam is rotated in the Graphics window.
4.
Verify the beam orientation. Choose menu path Utility Menu> PlotCtrls> Style> Size and Shape. Select the radio button next to the /ESHAPE label to turn /ESHAPE on and click on OK.
16.6.9. Define the Boundary Conditions 1.
Define a boundary condition to the fixed end. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Keypoints. The Apply U,ROT on KPs picker appears.
2.
Define keypoint 1 as the fixed end. In the picker, type 1, press the Enter key, then click on OK. The Apply U,ROT on KPs dialog box appears.
3.
Click on "All DOF" to select it, and click on OK. The boundary condition information appears in the ANSYS Graphics window at keypoint 1.
4.
Apply a force to the free end. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment> On Keypoints. The Apply F/M on KPs picker appears.
5.
Identify keypoint 2 as the free end. Type 2 in the picker, press the Enter key, and then click on OK. The Apply F/M on KPs dialog box appears.
6.
In the drop down list for Direction of force/mom, select FY. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–13
Chapter 16: Beam Analysis and Cross Sections 7.
Enter 1 for the Force/moment value in the Apply F/M on KPs dialog box, and click on OK. The force symbol appears in the ANSYS Graphics window at keypoint 2.
8.
Save the model. Choose menu path Utility Menu> File> Save As. If the buckle.db file is not already selected, select it. Click on OK and when ANSYS prompts you if you want to overwrite the existing file, click on OK again.
16.6.10. Solve the Eigenvalue Buckling Analysis 1.
Set analysis options. Choose menu path Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options. The Static or Steady-State Analysis dialog box appears.
2.
Use the sparse solver for the solution. In the Static or Steady-State Analysis dialog box, make sure that Sparse solver is selected in the drop down box beside the Equation solver label.
3.
Include prestress effect, which will be stored for later use in the eigenvalue buckling calculation. In the drop down list labeled Stress stiffness or prestress, select "Prestress ON." Click on OK to close the Static or Steady-State Analysis dialog box.
4.
Choose menu path Main Menu> Solution> Solve> Current LS. Review the summary information in the /STAT command window, then select Close from its menu bar. Click on OK in the Solve Current Load Step window to begin the solution.
5.
When the Solution is Done! window appears, click on Close to close it.
6.
Choose menu path Main Menu> Finish.
7.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis.
8.
Select the "Eigen Buckling" option, then click on OK.
9.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. The Eigenvalue Buckling Options dialog box appears. Select the Block Lanczos option. Enter 4 in the No. of modes to extract box, then click on OK.
10. Set the element calculation key for the MXPAND command. Choose menu path Main Menu> Solution> Load Step Opts> ExpansionPass> Single Expand> Expand Modes. 11. In the Expand Modes dialog box, enter 4 in the No. of modes to expand box, change the No to Yes beside the Calculate elem results label, and click on OK. 12. Choose menu path Main Menu> Solution> Solve> Current LS. Review the summary information in the /STAT command window, then select Close from its menu bar. Click on OK in the Solve Current Load Step window to begin the solution. 13. When the Solution is Done! window appears, click on Close to close it. 14. Choose menu path Utility Menu> PlotCtrls> Style> Size and Shape. Be sure the radio button beside the label Display of element shapes ... (/ESHAPE) is set to On and click on OK. 15. Display the results summary. Choose menu path Main Menu> General Postproc> Results Summary. After you have reviewed the results, click on Close to close the window. 16. Choose menu path Main Menu> General Postproc> Read Results> First Set. 17. Plot the first mode shape of the beam. Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears. Select Def + undef edge and click on OK. 18. Choose menu path Main Menu> Finish.
16–14
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.6: Sample Lateral Torsional Buckling Analysis (GUI Method)
16.6.11. Solve the Nonlinear Buckling Analysis 1.
Introduce model imperfections calculated by the previous analysis. Choose menu path Main Menu> Preprocessor> Modeling> Update Geom. In the Update nodes using results file displacements dialog box, enter 0.002 in the Scaling factor box, 1 in the Load step box, 1 in the Substep box, and file.rst in the Selection box. Click on OK.
2.
Choose menu path Main Menu> Solution> Analysis Type> New Analysis.
3.
Select the "Static" option, then click on OK.
4.
Choose menu path Main Menu> Solution> Load Step Opts> Output Ctrls> DB/Results File and be sure the drop down lists display All Items and All entities respectively. Choose the Every substep for the File write frequency radio button and click on OK.
5.
Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. Select the radio button beside Large deform effects, then click on OK.
6.
Set the arc-length method, and set parameters for the termination of the solution. Choose menu path Main Menu> Solution> Load Step Opts> Nonlinear> Arc-Length Opts. Select the Arc-length method on/off radio button and set it to On. Choose the pull down menu next to the Lab label and select Displacement lim. Enter 1.0 in the Max desired U box. Enter 2 in the Node number for VAL box. Choose the pull down menu next to the Degree of freedom label and select UZ. Click on OK.
7.
Define the number of substeps to be run during this load step. Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Time and Substps. Enter 10000 in the Number of substeps box and click on OK.
8.
Solve the current model. Choose menu path Main Menu> Solution> Solve> Current LS. Review the summary information in the /STAT command window, then select Close from its menu bar. Click on OK in the Solve Current Load Step window to begin the solution. A Nonlinear Solution window with a Stop button appears. A convergence graph is built, and can take several minutes to complete.
9.
You may receive a warning message. You should review the information in the message but you do not need to close it. Continue waiting for the solution to complete. When the Solution is Done! window appears, click on Close to close it.
10. Choose menu path Main Menu> Finish.
16.6.12. Plot and Review the Results 1.
Replot the beam. Choose menu path Utility Menu> Plot> Elements.
2.
Define the load point deflection to be read from the results file. Choose menu path Main Menu> TimeHist PostPro> Define Variables. When the Defined Time-History Variables dialog box appears, select Add.
3.
When the Add Time-History Variable dialog box appears, be sure the Nodal DOF result option is selected. Click on OK.
4.
The Define Nodal Data picker appears. In the Graphics window, pick node 2 (the end node on the right side of the beam) and click on OK.
5.
The Define Nodal Data dialog box appears. Be sure the Ref number of variable and Node number are both set to 2. Enter TIPLATDI in the User-specified label box. Select Translation UZ from the menu and click on OK.
6.
Define the total reaction force to be read from the results file. Choose Add from the Defined Time-History Variables dialog box.
7.
When the Add Time-History Variable dialog box appears, choose the Reaction forces radio button and then click on OK. Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–15
Chapter 16: Beam Analysis and Cross Sections 8.
The Define Reaction Force picker appears. Pick the end node on the left side of the beam and click on OK.
9.
The Define Reaction Force Variable dialog box appears. Be sure the Ref number of variable is set to 3 and Node number is set to 1. Select Struct Force FY from the menu and click on OK. Click on Close to close the Defined Time-History Variables dialog box.
10. Choose menu path Main Menu> TimeHist Postpro> Math Operations> Multiply. In the Multiply TimeHistory Variables dialog box, enter 4 in the Reference number for result box, -1.0 in the 1st Factor box, and 3 in the 1st Variable box. Click on OK. 11. Display the X variable. Choose menu path Main Menu> TimeHist Postpro> Settings> Graph. Choose the single variable button, enter 2 in the Single variable no. box, and click on OK. 12. Plot the load versus deflection curve to confirm the critical load calculated by the eigenvalue method. Choose menu path Main Menu> TimeHist PostPro> Graph Variables. Enter 4 in the 1st variable to graph box. Click on OK. 13. List the variables versus time. Choose menu path Main Menu> TimeHist PostPro> List Variables. Enter 2 in the 1st variable to list box and 4 in the 2nd variable box and click on OK. 14. Check the values in the PRVAR Command window to see how they compare against the values generated by the eigenvalue buckling analysis. Expected results are: Critical buckling load, Pcr = 0.01892. Close the PRVAR Command window. 15. Choose menu path Main Menu> Finish. 16. In the ANSYS Toolbar, click on Quit. 17. Choose a save option and click on OK.
16.7. Sample Problem with Cantilever Beams, Command Method Here is the input file for the problem described in the previous section: /GRAPHICS,POWER /GST,ON /SHOW,BUCKLE,GRPH /PREP7 K,1,0,0,0 K,2,100.0,0,0 K,3,50,5,0 LSTR,1,2 ET,1,BEAM189 SECTYPE,1, BEAM, RECT SECDATA, 0.2, 5.0 SLIST, 1, 1 MP,EX,1,1E4 MP,NUXY,1,0.0 LSEL,S, , , 1, 1, 1 LATT,1, ,1,0, 3, ,1 LESIZE, all, , ,10 SECNUM,1 LMESH,all /VIEW,,1,1,1 /ESHAPE,1 EPLOT DK,1, , , ,0,ALL FK,2,FY,1.0 FINISH /SOLU PSTRES,ON EQSLV,SPARSE ! EQSLV,SPARSE is the default for static and full transient SOLVE FINISH /SOLU
16–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 16.8: Where to Find Other Examples ANTYPE,BUCKLE BUCOPT,LANB,4 MXPAND,4,,,YES SOLVE FINISH /POST1 /ESHAPE,1 /VIEW, 1 ,1,1,1 /ANG, 1 SET,LIST SET,1,1 PLDISP,2 FINISH /PREP7 UPGEOM,0.002,1,1,file,rst /SOLU ANTYPE,STATIC OUTRES,ALL,ALL NLGEOM,ON ARCLEN,ON,25,0.0001 ARCTRM,U,1.0,2,UZ NSUBST,10000 SOLVE FINISH /POST26 NSOL,2,2,U,Z,TIPLATDI RFORCE,3,1,F,Y PROD,4,3, , , , , ,-1.0,1,1 XVAR,2 PLVAR,4 PRVAR,2,4 FINISH
16.8. Where to Find Other Examples Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional beam analyses. The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS program. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as step-by-step examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments. The ANSYS Verification Manual contains one beam test case: VM222 - Warped Cantilever Beam
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
16–17
16–18
Chapter 17: Shell Analysis and Cross Sections 17.1. An Overview of Shells Shell elements are used to create a mathematical 2-D idealization of a 3-D structure. They offer computationally efficient solutions for modelling shell structures when compared to solid elements. The discussion in this chapter applies to SHELL181, which is a 3-D finite strain shell element. This shell element provides more robust nonlinear analysis capabilities, and significant improvements in cross section data definition, analysis, and visualization, as compared to other ANSYS shells. The method for defining shell sections described here can also be used to define the cross-sectional properties of the layered thermal shell elements, SHELL131 and SHELL132. Discussions in this chapter relating to integration points (NUMPT on the SECDATA command) and section properties (SECCONTROLS command) do not apply to SHELL131 and SHELL132.
17.2. What Are Cross Sections? A cross section defines the geometry of the shell in a plane parallel to the shell x-y plane. Through the section family of commands, you can describe the z direction of the element by defining consecutive layers. Each layer may vary in thickness, material type, orientation (from element x-axis), and number of integration points.
17.3. How to Create Cross Sections The general procedure for creating cross sections consists of the following steps: 1.
Define the section and associate a section ID number with the section.
2.
Define the geometry data for the section.
ANSYS supplies the following commands for creating, viewing, and listing cross sections, and for managing cross section libraries:
Table 17.1 ANSYS Cross Section Commands Command
Purpose
GUI Menu Path
SECTYPE
Associates section with SECID (section number)
Main Menu> Preprocessor> Sections> Shell> Add/Edit
SECDATA
Defines section geometry Main Menu> Preprocessor> Sections> Shell> Add/Edit data
SECCONTROLS Overrides program calcu- Main Menu> Preprocessor> Sections> Shell> Add/Edit lated properties. SECFUNCTION Specifies shell section thickness as a tabular function.
Main Menu> Preprocessor> Sections> Shell> Add/Edit
SECNUM
Identifies the SECID (sec- Main Menu> Preprocessor> Meshing> Mesh Attributes> Default tion number) to be asAttribs signed to an element Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes
SECOFFSET
Defines section offset for Main Menu> Preprocessor> Sections> Shell> Add/Edit shell cross sections
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Chapter 17: Shell Analysis and Cross Sections Command
Purpose
GUI Menu Path
SECPLOT
Plots geometry of a shell Main Menu> Preprocessor> Sections> Shell> Plot Section section to scale
SLIST
Summarizes section prop- Main Menu> Preprocessor> Sections> List Sections erties Utility Menu> List> Properties> Section Properties Utility Menu> List> Properties> Specified Section Properties
SDELETE
Deletes a cross section
Main Menu> Preprocessor> Sections> Delete Section
For complete documentation of the cross section commands, see the ANSYS Commands Reference. Figure 17.1: “Plot of a Shell Section” shows the layer stacking of a shell section. The layer order, along with material and orientation of each layer, is represented here:
Figure 17.1 Plot of a Shell Section
17.3.1. Defining a Section and Associating a Section ID Number Use the SECTYPE command to define a section and associate it with a section ID number. For example, the following command assigns a section identification number (2) to a shell section: Command(s): SECTYPE, 2, SHELL GUI: Main Menu> Preprocessor> Sections> Shell> Add/Edit
17.3.2. Defining Layer Data Use the SECDATA command to define the layers of a shell section. Each consecutive SECDATA command defines the next layer's thickness, material, orientation, and number of integration points. (The number of integration points input on SECDATA is not used by thermal shell elements.) The layer orientation angle is the angle between the layer coordinate system and the x-axis of the element coordinate system.
17–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 17.3: How to Create Cross Sections You may designate the number of integration points (1, 3, 5, 7, or 9) located thru the thickness of each layer. When only 1, the point is always located midway between the top and bottom surfaces. If 3 or more points, 2 points are located on the top and bottom surfaces respectively and the remaining points are distributed equal distance between the 2 points. An exception occurs when designating 5 points, where the quarter point locations are moved 5 percent toward their nearest layer surface to agree with the locations selected with real constant input. The default for each layer is 3. If a shell section has only one layer, and the number of section integration points is equal to one, then the shell does not have any bending stiffness. This may result in solver difficulties, and may affect convergence adversely. Command(s): SECDATA, 0.5, 1, 45, 3 SECDATA, 0.5, 2, -45, 3 SECDATA, 0.5, 1, 45, 3 GUI: Main Menu> Preprocessor> Sections> Shell> Add/Edit
17.3.3. Overriding Program Calculated Section Properties Use the SECCONTROLS command to override the program calculated section properties. By default, the program calculates shear correction factors and mass for each element based on the input section geometry and material properties. Any values input on the SECCONTROLS command will replace the defaults. (SECCONTROLS does not apply to thermal shell elements.) Command(s): SECCONTROLS, 0.8, 0.0, 0.8, 1.0 GUI: Main Menu> Preprocessor> Sections> Shell> Add/Edit
17.3.4. Specifying a Shell Thickness Variation (Tapered Shells) Use the SECFUNCTION command to associate a tabular thickness variation with the section. A table that describes thickness with respect to the global Cartesian coordinate system may be associated with a shell section. This thickness is interpreted as the total thickness of a shell. The total thickness of a layered shell, and all layer thickness values, will be scaled according to the tabular function. Command(s): SECFUNCTION, %table_name% GUI: Main Menu> Preprocessor> Sections> Shell> Add/Edit
17.3.5. Setting the Section Attribute Pointer Use the SECNUM command to associate an element with a particular section. Any element created after the SECNUM command will have this section identification number (2) as its section attribute. Command(s): SECNUM, 2 GUI: Main Menu> Preprocessor> Meshing> Mesh Attributes> Define> Default Attribs
17.3.6. Associating an Area with a Section Use the AATT command to associate an area with a shell section type. When the area is meshed, the new elements are associated with the section specified on the AATT command. The section specified by the SECNUM command is ignored. Command(s): AATT, , , , , 2 GUI: Main Menu> Preprocessor> Meshing> Mesh Attributes> All Areas Main Menu> Preprocessor> Meshing> Mesh Attributes> Picked Areas
17.3.7. Using the Shell Tool to Create Sections The SECTYPE, SECDATA, SECOFFSET, SECFUNCTION, and SECCONTROLS commands (Main Menu> Preprocessor> Sections> Shell> Add/Edit) are all associated with the ShellTool in the GUI.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
17–3
Chapter 17: Shell Analysis and Cross Sections
Figure 17.2 Shell Tool With Layup Page Displayed
The top part of the Layup page of the ShellTool relates a section ID number to a Shell section type (and, optionally, a section name) [SECTYPE]. The middle part of the page of the ShellTool defines each layer in the positive Z direction of the element [SECDATA]. Note that the order of the rows in the spreadsheet ascends up the page, resembling that stacking of the layers. (Integration point data for each layer is ignored by thermal shell elements.) The bottom contains the fields for section offset information, if needed [SECOFFSET]. You can define tapered shells by specifying a section function relating thickness to global coordinates [SECFUNCTION].
Figure 17.3 Shell Tool With Section Controls Page Displayed
The transverse shear stiffness, hourglass coefficients and drill stiffness of the sections are calculated from the section geometry and material properties. The default added mass per unit area of the section is always zero. On the Section Controls page, you can override the program calculated quantities [SECCONTROLS]. (The Section Controls page does not apply to thermal shell elements.)
17–4
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Section 17.3: How to Create Cross Sections
Figure 17.4 Shell Tool With Summary Page Displayed
On the Summary page, you can review the section properties.
17.3.8. Managing Cross Section Libraries Cross section data for shell sections can be stored in cross section libraries. To create standard cross sections for later use, create one or more cross sections, edit the Jobname.LOG file, and copy the appropriate SECCONTROLS, SECDATA, SECFUNCTION, SECOFFSET, and SECTYPE commands into a separate file with a SECT extension.
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
17–5
17–6
creep, 8–31 hyperelasticity, 8–21 large strain, 8–6 plasticity, 8–9
Index Symbols 2-D fracture models, 12–3 3-D fracture models, 12–4
B
A adaptive descent, 8–53 adequate mesh density, 8–64 alpha (mass) damping, 4–10, 5–36, 6–18 alternating stress intensity, 14–1 amplitude of harmonic loads, 4–5 analysis modal analysis options, 3–4 reduced transient dynamic, 5–19 analysis options harmonic response analysis, 4–25 mode superposition method, 4–25 modal analysis, 3–2, 4–4, 4–20 nonlinear static structural analysis, 8–49 single-point spectrum analysis, 6–3 transient dynamic analysis, 5–14, 5–20 mode superposition method, 5–14 reduced method, 5–20 analysis type buckling, 7–1 full transient, 5–7 harmonic response, 4–1 modal, 3–1 nonlinear structural, 8–1 p-method, 15–1 spectrum, 6–1 static structural, 2–1, 2–2 structural, 1–1 definition of, 1–1 transient dynamic, 5–1 animation gasket results, 10–19 anisotropic, 8–10 applying loads, 3–2, 4–4, 4–20, 8–56, 8–60 harmonic response analysis, 4–5 increments for buckling analysis, 7–2 modal analysis, 3–5 nonlinear analysis, 8–56 p-method, 15–7 structural static analysis, 2–8, 2–8 transient dynamic analysis, 5–9 using TABLE array parameters, 2–8 arc-length method, 2–5, 7–2, 7–3, 8–2, 8–68 automatic time stepping, 5–35, 7–2, 8–67
Bauschinger effect, 8–10 beam tool, 16–5 beams cross sections, 16–1 Besseling model, 8–10 beta (stiffness) damping, 4–10, 5–36, 6–3, 6–18 bilinear isotropic hardening, 8–10 bilinear kinematic hardening, 8–10 birth and death, 8–69, 8–70 element, 8–63 bisection, 8–5 Block Lanczos extraction method, 4–25 Block Lanczos method, 3–3, 3–17 bonlinear structural analysis restarts, 8–59 buckling analysis, 7–1, 7–1 eigenvalue, 7–3 procedure, 7–3 expand the solution, 7–6 expansion pass, 7–6 methods of solution, 7–1 nonlinear, 7–2 procedure, 7–2 obtain the eigenvalue buckling solution, 7–5 obtain the static solution, 7–4
C calculating covariance in POST26, 6–23 fracture parameters, 12–5 cast iron plasticity, 8–10 causes of nonlinear behavior, 8–1 changing status, 8–2 geometric nonlinearities, 8–2 material nonlinearities, 8–2 cells defining for a section, 16–4 Chaboche model, 8–10 changing status, 8–2 combinations material model, 8–35 composite cross section, 16–8 composites, 13–1 element types for, 13–1 guidelines, 13–6
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index how to model, 13–1 layer properties, 13–3 concrete, 8–10, 8–29, 8–63 constant damping ratio, 4–10, 5–36, 6–3, 6–18 constitutive matrices, 13–4 constraint equations, 15–7 with QR Damped method, 3–19 contact, 8–2 node-to-node, 8–63 contact analysis, 11–1 asymmetric vs. symmetric contact, 11–7 birth and death option, 11–42 boundary conditions for node-to-node contact, 11–74 boundary conditions for surface-to-surface contact, 11–51 chattering controls, 11–21 choosing surfaces, 11–6 conduction, 11–45 contact algorithm, 11–21, 11–74 contact direction, 11–13 contact location detection, 11–28 Contact Manager, 11–4, 11–54 contact pairs, 11–5, 11–56 contact status, 11–38, 11–44 contact stiffness, 11–21, 11–22 contact surface elements, 11–3 Contact Wizard, 11–55 convection, 11–46 deformable contact surface, 11–14 direct generation to create rigid target elements, 11–9 electric contact, 11–48 electrostatic elements, 11–48 emissivity, 11–46 explicit dynamics, 11–1 flexible-to-flexible, 11–1, 11–4 free surface convection, 11–44 free surface radiation, 11–44 free thermal surface, 11–44 friction model, 11–25 gap, 11–74 Gauss integration points, 11–28 generating node-to-node contact elements, 11–71 generating surface-to-surface contact elements, 11–16 heat flux, 11–44, 11–48 heat generation due to electric current, 11–49 heat generation due to friction, 11–47 initial contact conditions, 11–30 initial interference, 11–74 internal MPC, 11–60
Index–2
localized contact zone, 11–12 magnetic contact, 11–50 moving contact nodes, 11–37 node ordering in node-to-node analysis, 11–72 node-to-node, 11–2, 11–4, 11–70 node-to-surface, 11–2, 11–3, 11–57 node-to-surface KEYOPTS, 11–59 node-to-surface real constants, 11–60 normals, 11–13, 11–16, 11–54, 11–73 open far-field contact status, 11–38 open near-field contact status, 11–38 overall steps, 11–5 overconstrained contact problem, 11–74 penalty stiffness, 11–15 penetration, 11–21 piezoelectric elements, 11–48 pinball region, 11–38 point-to-point, 11–4 point-to-surface, 11–3 pseudo element technique, 11–57 radiation, 11–46 results, 11–53 rigid-to-flexible, 11–1, 11–4, 11–43 self contact, 11–7, 11–39 shells, 11–42 sliding contact status, 11–38 slippage, 11–28 solution options for node-to-node contact, 11–75 solution options for surface-to-surface contact, 11–51 solving, 11–52 spurious contact, 11–39 Stefan-Boltzmann constant, 11–46 sticking contact status, 11–38 summary of contact capabilities, 11–2 superelements, 11–41 surface interaction for electric contact, 11–48 surface interaction models, 11–40 surface-to-surface, 11–2, 11–3, 11–4, 11–14 surface-to-surface KEYOPTS, 11–20 surface-to-surface material properties, 11–15 surface-to-surface overview, 11–4 surface-to-surface real constants, 11–15, 11–17 symmetric/unsymmetric solver, 11–25 target element shapes, 11–9 target surface definition, 11–7 target surface element types and real constants, 11–8 target surface modeling and meshing tips, 11–12 target surface nodal number ordering, 11–13 target surface pilot node, 11–8, 11–43 target surface primitives, 11–8 temperature required, 11–45
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index thermal contact, 11–44 thickness effect, 11–42 time step control, 11–42 using meshing tools to create rigid target elements, 11–10 contour displays, 2–11, 3–11, 6–8, 7–7, 8–57, 10–19 control elements, 8–69 controlling cutbacks, 2–4 controlling p-levels, 15–7 controlling restarts, 2–4 convergence checking, 8–51 enhancements, 8–64 failure, 8–64 convergence criteria, 8–51 default value, 8–51 disjointed structures, 8–51 displacement checking, 8–51 force checking, 8–51 p-method, 15–7 vector norms, 8–51 convergence tolerances, 2–4 coupling, 13–6, 15–6 covariance calculating, 6–23 crack faces, 12–1 crack front, 12–1 crack region modeling, 12–1 crack tip, 12–1 creating sections, 16–2, 16–5, 17–1 beam tool, 16–5 creep, 8–8, 8–29 automatic time stepping, 8–31 explicit, 8–29, 8–55 explicit creep procedure, 8–31 implicit, 8–29, 8–55 implicit creep procedure, 8–30 material curve fitting, 9–7 ratio, 8–55 creep criteria, 2–7, 8–55 creep strain rate, 8–29 cross sections (see sections) (see Sections) composite, 16–8 custom convergence criteria, 8–51 cutback criteria, 2–4 CUTCONTROL command changes through SOLCONTROL, 8–53 cyclic hardening/softening, 8–10
D damped method modal analysis, 3–3, 3–18 damping, 5–9, 5–36, 8–60 harmonic response analysis, 4–10 spectrum analysis, 6–18 PSD, 6–18 table of options, 5–36 transient dynamic analysis, 5–7, 5–9, 5–14, 5–22 database output, 2–2, 3–8, 4–10, 4–21, 5–7, 5–14, 5–24, 7–6, 8–49 DDAM (see dynamic design analysis method) deep drawing, 8–32 deformed shape display, 2–11, 6–8, 7–7, 8–57 displaying, 10–19 deleting sections, 16–2, 17–1 deterministic analysis, 6–2 disjointed structures, 8–51 display deformed shape, 3–11, 4–12 displaying deformed shapes, 8–57 DOFs master, 3–4 Drucker-Prager, 8–10 dynamic analyses harmonic response, 4–1 spectrum, 6–1 transient, 5–1 dynamic design analysis method (DDAM), 6–2, 6–25
E eigenvalue analysis, 3–1 eigenvalue buckling, 7–1 eigenvalue buckling solution buckling analysis, 7–5 eigenvalue calculation shift point, 7–5 eigenvalue extraction methods, 7–5 eigenvalues, 3–1 number to be extracted, 7–5 eigenvectors, 3–1 elastomers, 8–17 element birth and death, 8–63 element damping, 5–36 element loads, 4–25 element types structural, 1–2 elements associating sec IDs with, 16–2, 17–1 energy release rate, 12–1, 12–8
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index–3
Index engineering strain, 8–7 engineering stress, 8–7 epoxy, 13–1 equation solvers, 2–4, 4–4, 8–50, 15–7 equilibrium iterations, 8–2, 8–52 number of, 2–4, 8–52 error estimation, 2–11 example problems beam analysis, 16–17 buckling analysis, 7–12 harmonic response analysis, 4–19 modal analysis, 3–14 nonlinear analysis, 8–82 reduced transient dynamic analysis, 5–40 single-point response spectrum analysis, 6–17 static analysis, 2–26 excitation direction, 6–3 expand single solution, 5–24 expand the modes single-point response spectrum analysis, 6–6 expand the solution buckling analysis, 7–6 reduced harmonic response analysis, 4–21 expanded modes number to use, 6–3 expanded solution review results, 5–25 expanding modes, 3–8 expansion frequency range, 3–8 expansion pass, 4–21 activating, 3–8, 4–21, 5–24 buckling analysis, 7–6 harmonic response analysis, 4–21, 4–27 mode superposition method, 4–27 reduced method, 4–21 transient dynamic analysis, 5–18, 5–24 mode superposition method, 5–18 reduced method, 5–24 expansion pass options harmonic response analysis (reduced), 4–21 modal analysis, 3–8 transient dynamic analysis (reduced), 5–24 explicit creep, 8–29 explicit creep procedure, 8–31 extra element shapes, 8–70 extracting modes, 3–1 extrapolation of results, 2–7, 4–10, 4–21, 5–24, 8–56
F failure criteria, 13–5 maximum strain, 13–5 Index–4
maximum stress, 13–5 Tsai-Wu, 13–5 failures convergence, 8–64 fatigue alternating stress intensity, 14–1 design stress-intensity value (Sm), 14–2 evaluation procedure, 14–2 event, 14–1 event repetitions, 14–6 fatigue data file (Jobname.FATG), 14–9 guidelines for assembling events, 14–7 loading, 14–1 location, 14–1 manually stored stresses, 14–4 material properties, 14–2 overview, 14–1 S-N curve, 14–2 sample input, 14–9 scale factors, 14–6 Sm-T curve, 14–2 strain hardening exponents, 14–2 stress concentration factors, 14–2 stress locations, 14–2 stresses at a cross-section, 14–5 stresses from results file, 14–5 with p-elements, 15–4 fatigue assessments, 15–4 fatigue calculations activating, 14–9 fiberglass, 13–1 files Jobname.FATG, 14–9 .SECT, 16–6 forced vibrations, 4–1 forcing frequency range, 4–10 fracture assessments, 15–4 fracture mechanics, 12–1, 12–1 solving problems, 12–1 fracture models 2-D, 12–3 3-D, 12–4 fracture parameters calculating, 12–5 free meshing, 15–4 free-body analysis (see inertia relief) frequency range for expansion, 3–8, 4–21 frequency vector, 6–23 frequency-dependent damping ratio, 6–18 full harmonic response analysis procedure, 4–3 full transient dynamic analysis
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index procedure, 5–3
Blatz-Ko foam model, 8–20 Gent model, 8–20 large strain, 8–17 material curve fitting, 9–1 Mooney-Rivlin model, 8–18, 8–21 neo-Hookean model, 8–19 Ogden compressible foam model, 8–20 Ogden model, 8–18 polynomial form model, 8–19 stability checks, 8–21 u-P formulation, 8–21 user-defined option, 8–21 Yeoh model, 8–20
G gap conditions, 5–14, 5–20 and QR Damped method, 5–14 gasket joints simulation, 10–1 applications, 10–3 element topologies, 10–2 elements, 10–3 formulation, 10–2 materials, 10–4 meshing, 10–12 output listing, 10–17 overview, 10–1 plotting data, 10–11 procedure, 10–1 results, 10–19 sample problem, 10–20 solution, 10–16 thickness, 10–2 gasket results animation, 10–19 POST1, 10–19 POST26, 10–20 reviewing, 10–19 tabular listing, 10–19 geometric nonlinearities, 8–2, 8–6 geometry data for sections, 16–2, 17–1 geometry data of a section, 16–3, 17–2 glass, 8–33 guyan reduction, 3–19
H harmonic forcing frequency, 4–5 harmonic response, 4–1 harmonic response analysis, 4–1 full method, 4–3, 4–3 procedure, 4–3 methods of solution, 4–2 mode superposition method, 4–25, 4–27 procedure, 4–25 sample input, 4–27 prestressed, 4–28 reduced method, 4–20, 4–24 sample input, 4–24 uses for, 4–1 harmonic solutions number of, 4–9 Hill anisotropy, 8–10 hyperelasticity, 8–8, 8–17 Arruda-Boyce model, 8–19 automatic time stepping, 8–21
I implicit creep, 8–29 implicit creep procedure, 8–30 inertia relief, 2–9 calculating, 2–9 output, 2–9 partial, 2–9 initial accelerations, 5–4 initial conditions transient dynamic analysis, 5–4, 5–14, 5–21 full method, 5–4 mode superposition method, 5–14 reduced method, 5–21 initial displacement, 5–4 initial velocity, 5–4 integration point, 8–56 integration time step, 5–1, 5–7, 5–14, 5–22 guidelines for, 5–33 interface material model, 1–2 internal MPC, 11–60
J J-integral, 12–1, 12–6
K kinematic analysis, 8–60, 8–67 KSPIN [OMEGA], 8–8
L large deflection and load direction, 8–6 large deformation effects, 2–2, 5–7, 7–2, 8–6, 8–8, 8–60 large strain analyses, 8–6, 8–10 automatic time stepping, 8–6 hyperelasticity, 8–17 logarithmic strain, 8–7
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index–5
Index true stress, 8–7 viscoplasticity, 8–32 layer orientation angle, 13–3 layer thickness, 13–3 layered elements, 13–1 libraries sections, 16–9, 17–5 library paths for cross sections, 16–2 line element results, 2–11, 3–11 line search option, 2–4, 8–53, 8–68 list master DOF, 3–11 listing section properties, 16–2, 17–1 section results, 16–2 load step options, 3–8, 4–21, 5–24 buckling analysis, 7–6 eigenvalue buckling, 7–5 harmonic response analysis, 4–9, 4–20, 4–25 full method, 4–9 mode superposition method, 4–25 reduced method, 4–20 modal analysis, 3–6 mode superposition transient dynamic analysis, 5–14 Newton-Raphson, 8–54 p-method, 15–7 reduced transient dynamic analysis, 5–21 spectrum analysis, 6–3, 6–18 PSD, 6–18 single-point, 6–3 time, 5–14 transient dynamic analysis, 5–10, 5–10, 5–14, 5–21 full method, 5–10 mode superposition method, 5–14 reduced method, 5–21 load steps, 8–2 applying for transient loading, 5–10 load types, 2–7, 3–5 harmonic response analysis, 4–5 p-method, 15–7 load vector, 4–25, 5–14, 5–14 load-versus-time curve, 5–4 loads applying, 2–8, 3–2, 3–5, 4–8, 4–20, 5–14, 7–2, 8–56, 8–60, 15–7 p-method, 15–7 applying for transient loading, 5–9 direction in a large-deflection analysis, 8–6 harmonic response analysis, 4–5, 4–20, 4–25 mode superposition method, 4–25 reduced method, 4–20 modal analysis, 3–5
Index–6
nonlinear analysis, 8–56 structural static analysis, 2–8, 2–8 transient dynamic analysis, 5–9, 5–9, 5–14, 5–21 full method, 5–9 mode superposition method, 5–14 reduced method, 5–21 Loads applying, 4–4 logarithmic strain, 8–7, 8–7
M macros, 2–10 magnetic analysis contact, 11–50 mass damping, 5–36 mass matrix formulation, 2–6, 3–4, 4–4, 5–9 master degrees of freedom selection of, 3–19 master DOF (MDOF), 3–19, 5–20 master DOFs definition of, 3–4 material curve fitting, 9–1 creep, 9–7 viscoelastic, 9–14 material model combinations, 8–35 material model interface, 1–2 material models shape memory alloy, 8–31 material nonlinearities, 8–2, 8–8 material properties, 15–3 fatigue, 14–2 material curve fitting, 9–1 nonlinear, 8–8 material-dependent damping, 5–36 matrix reduction, 3–19 theory of, 3–19 maximum strain failure criterion, 13–5 maximum stress failure criterion, 13–5 MDOF, 3–4 memory saving when generating stiffness matrix, 8–50 meshing a line for a section, 16–4 p-element, 15–4 metal forming, 8–32 midside nodes p-element, 15–4 MINREF [CNVTOL], 8–51 modal analysis, 3–1 applying loads, 3–5 mode-extraction methods, 3–3, 3–16
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index options for, 3–4 prestressed, 3–14 prestressed, large deflection, 3–15 procedure, 3–1 modal damping, 5–36, 6–3 modal solution obtaining, 5–13 single-point response spectrum analysis, 6–3 mode combination methods, 6–6 mode extraction methods QR Damped, 6–3 mode numbers, 2–7 mode superposition harmonic response analysis, 4–25 mode-extraction methods, 4–25 transient dynamic analysis, 5–13 mode superposition method, 4–3, 5–2 mode superposition transient dynamic analysis obtain the modal solution, 5–13 obtain the mode superposition transient solution, 5–14 mode-extraction methods, 3–3, 3–16 Block Lanczos, 3–3, 3–17, 4–25 damped, 3–3, 3–18 power dynamics, 3–3, 3–17 QR Damped, 3–3, 3–19, 4–25, 4–25, 5–13, 5–14 reduced, 3–3, 3–18 subspace, 3–3, 3–17 unsymmetric, 3–3, 3–18 mode-frequency analysis, 3–1 model geometry defining, 15–4 modeling the crack region, 12–1 modes expanding, 3–8 number of, 3–8 number to expand, 3–4 number to extract, 3–4 Mohr-Coulomb, 8–10 MONITOR command changes from SOLCONTROL, 8–55 Mooney-Rivlin constants, 8–21 MPRS analysis, 6–25 multi-point response spectrum, 6–1 multilinear elastic, 8–8 multilinear elasticity, 8–16 multilinear isotropic hardening, 8–10 multilinear kinematic hardening, 8–10 multipoint constraint, 11–60
N natural frequencies, 3–10
Newton-Raphson, 8–2 Newton-Raphson option, 2–6 Newton-Raphson options, 8–54 nodal coordinate systems p-method, 15–7 nodal forces and moments, 2–11 nodal solution listing format, 4–21 nonlinear analysis tips and guidelines, 8–63 nonlinear behavior causes, 8–1 nonlinear diagnostics, 8–64 nonlinear isotropic hardening, 8–10 nonlinear kinematic hardening, 8–10 nonlinear material properties material curve fitting, 9–1 nonlinear structural analysis automatic time stepping, 8–67 buckling, 7–2 conservative vs. nonconservative, 8–5 creep, 8–29 geometric nonlinearities, 8–6 hyperelasticity, 8–17 interpolation of results, 8–57 levels of operation, 8–2 load directions, 8–6 material nonlinearities, 8–8 nonlinear elements, 8–63 overview, 8–1 plasticity, 8–9 sample transient input, 8–61 swelling, 8–34 termination, 8–59 verifying results, 8–70 viscoelasticity, 8–33 viscoplasticity, 8–32 nonlinear transient analysis procedure, 8–59 number of eigenvalues to be extracted, 7–5 number of harmonic solutions, 4–9 number of integration points per layer, 13–3 number of solutions to expand, 4–21
O obtain the modal solution, 4–25 offsets for sections, 16–2, 17–1 OPNCONTROL command changes through SOLCONTROL, 8–55 output, 8–70 database and results file, 2–2, 3–8, 4–10, 4–21, 5–7, 5–14, 5–24, 7–6, 8–49
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index–7
Index printed, 2–7, 3–8, 4–10, 4–21, 5–14, 5–14, 5–23, 5–24, 7–6, 8–56 output control, 4–10, 5–14, 5–23, 7–6 output controls, 3–6, 3–8, 5–24, 7–5
P p-elements meshing, 15–4 real constants, 15–3 p-level error-estimation range, 15–2 error-estimation techniques, 15–2 p-method, 15–1 benefits of, 15–1 guidelines for meshing, 15–5 internal DOFs, 15–7 load step options, 15–7 loads, 15–7 meshing the model, 15–4 p-element subgrid, 15–12 printing and plotting results, 15–14 querying subgrid results, 15–12, 15–13 reviewing results, 15–12 solving common problems, 15–12 specialized displays and listings, 15–14 status of elements, 15–7 use of solvers, 15–7 using, 15–1 viewing the element model, 15–5 participation factor calculations, 3–6, 6–18 Peirce model, 8–32 penalty stiffness in contact analysis, 11–15 Perzyna model, 8–32 phase angle for expansion, 4–21 phase angle of harmonic loads, 4–5 pilot node in contact analysis, 11–8, 11–43 plastic, 8–8 plasticity, 8–9, 8–68 anisotropic, 8–10 automatic time stepping, 8–9 bilinear isotropic hardening, 8–10 bilinear kinematic hardening, 8–10 cast iron, 8–10 Drucker-Prager, 8–10 Hill anisotropic, 8–10 multilinear isotropic hardening, 8–10 multilinear kinematic hardening, 8–10 nonlinear isotropic hardening, 8–10 nonlinear kinematic hardening, 8–10 rate-dependent, 8–32 Index–8
plastics, 8–33 PLNSOL command with p-elements, 15–14 plotting sections, 16–2, 17–1 POST1, 2–11, 4–11, 4–23, 4–27, 5–11, 5–25, 6–8, 6–22, 7–7, 8–57, 12–5, 14–2 using, 4–12, 5–12 POST26, 2–11, 4–11, 4–21, 4–23, 4–27, 5–11, 5–23, 5–25, 6–23, 8–57 using, 4–12, 5–11 postprocessing fatigue, 14–1 for different analysis (see reviewing results) power dynamics method, 3–3, 3–17 power spectral density (PSD), 6–2 predictor, 8–52 predictor-corrector option, 2–4, 8–52 PRESOL command with p-elements, 15–14 pressure loads in a large-deflection analysis, 8–6 prestress effects calculation, 2–6, 3–4, 7–4 prestressed analysis harmonic response, 4–28 mode superposition harmonic response, 4–29 transient, 5–32 prestressed full transient dynamic analysis procedure, 5–32 prestressed harmonic response analysis procedure, 4–28 prestressed modal analysis, 3–14 prestressed modal analysis of a large deflection, 3–15 prestressed mode superposition harmonic response analysis procedure, 4–29 prestressed mode superposition transient dynamic analysis procedure, 5–33 prestressed reduced transient dynamic analysis procedure, 5–33 printed output, 2–7, 4–10, 4–21, 5–14, 5–14, 5–23, 5–24, 7–6, 8–56 printing and plotting node and element results p-method, 15–14 PRNSOL command with p-elements, 15–14 probabilistic analysis, 6–2 program-selected masters, 3–21 proportional limit, 8–9 PSD analysis, 6–18 PSD type, 6–18
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index PSD-versus-frequency table, 6–18
Q QR Damped extraction method harmonic analysis, 4–25 QR Damped method gap conditions, 5–14 harmonic analysis, 4–25 modal analysis, 3–3, 3–19 spectrum analysis, 6–3 transient analysis, 5–13, 5–14
R ramped loads, 4–9, 5–7, 5–14, 5–23, 8–60 random vibrations, 6–18 and power spectral density, 6–2 range counting, 14–9 ratcheting effect, 8–10 rate-dependent plasticity , 8–32 ratio creep, 8–55 Rayleigh damping constants, 5–36 reaction forces and moments, 2–11 reading user-defined mesh, 16–2 real constants for layered elements, 13–3 reduced (Householder) method, 3–3 reduced analysis (see matrix reduction) reduced harmonic response analysis expand the solution, 4–21 reduced method, 3–18, 4–2, 5–3 reduced transient dynamic analysis expansion pass, 5–24 load step options, 5–21 obtain the reduced solution, 5–19 review results of expanded solution, 5–25 reference temperature, 2–7 relative stress distributions buckling analysis, 7–7 response PSD calculating, 6–23 response spectrum multi-point, 6–1 single-point, 6–1 type, 6–3 restart control, 2–4 restarts, 8–62 results data from a PSD analysis, 6–22 extrapolation of, 2–7, 4–10, 4–21, 5–24, 8–56
results file output, 2–2, 3–8, 4–10, 4–21, 5–7, 5–14, 5–24, 7–6, 8–49 reviewing results eigenvalue buckling, 7–7 fatigue, 14–9 harmonic response analysis, 4–11, 4–21, 4–27 full method, 4–11 mode superposition method, 4–27 reduced method, 4–21 modal analysis, 3–10 nonlinear static structural, 8–57 nonlinear transient structural, 8–61 reduced harmonic analysis, 4–23 spectrum analysis, 6–8, 6–22 PSD, 6–22 single-point, 6–8 static structural analysis, 2–10 transient dynamic analysis, 5–11, 5–18, 5–23 full method, 5–11 mode superposition method, 5–18 reduced method, 5–23 Rice's model, 8–10 rock, 8–10 rolling, 8–32 rubber, 8–17
S sample buckling analysis command method, 7–12 GUI method, 7–8 sample harmonic response analysis command method, 4–18 GUI method, 4–13 sample input fatigue, 14–9 full transient dynamic analysis, 5–12 harmonic response analysis, 4–24, 4–27 mode superposition method, 4–27 reduced method, 4–24 mode superposition transient analysis, 5–18 nonlinear structural, 8–61 transient, 8–61 spectrum analysis, 6–24 PSD, 6–24 transient dynamic analysis, 5–18 mode superposition method, 5–18 sample modal analysis command method, 3–13 GUI method, 3–12 sample nonlinear analysis command method, 8–79 GUI method, 8–71
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index–9
Index sample p-method analysis command method, 15–18 GUI method, 15–14 sample spectrum analysis command method, 6–16 GUI method, 6–10 sample static analysis command method, 2–24 GUI method, 2–13 sample transient dynamic analysis command method, 5–31 GUI method, 5–26 sandwich structures, 13–4 scaling the load vector, 4–25 .SECT file, 16–6 sections, 16–1, 17–1 associating subtypes with IDs, 16–2, 17–1 creating, 16–2, 16–5, 17–1 beam tool, 16–5 defining dimensions, 16–2, 17–1 geometry data of, 16–3, 17–2 libraries of, 16–9, 17–5 meshing a line for, 16–4 solid, 16–4 thin wall, 16–4 shakedown effect, 8–10 shape memory alloy, 8–31 SHELL command with p-elements, 15–14 shells, 17–1 shift point for eigenvalue calculation, 7–5 significant modes expanding, 6–6 single solution to expand, 5–24 single-point response spectrum, 6–1 acceleration response, 6–6 CQC mode combination method, 6–6 displacement response, 6–6 DSUM mode combination method, 6–6 expanding significant modes, 6–6 GRP mode combination method, 6–6 mode combination methods, 6–6 NRLSUM mode combination method, 6–6 procedure, 6–2 SRSS mode combination method, 6–6 velocity response, 6–6 single-point spectrum analysis load step option for, 6–3 singular elements, 12–1 slave DOF, 3–19 small deflection, 8–6 small strain analyses, 8–6
Index–10
S-N curve, 14–2 soil, 8–10 solid sections, 16–4 solution obtain the mode superposition transient solution, 5–14 solution controls, 8–48 solution controls dialog box full transient analysis, 5–6, 5–6, 5–6 defining analysis type and options, 5–6 static analysis, 2–2 solution listing format, 4–4 solution method harmonic response, 4–4 solution methods, 4–2, 5–2 full, 4–2, 5–2 transient dynamic analysis, 4–2 mode superposition, 4–3, 5–2 reduced, 4–2, 5–3 solution termination, 2–5 solutions to be expanded, 5–24 solver, memory saving option, 8–50 solvers equation, 2–4, 8–50, 15–7 sparse direct solver, 4–4 specifying a p-level range, 15–2 specifying mesh controls, 15–4 spectral-value-versus-frequency curve, 6–3 spectrum, 6–1 spectrum analysis, 5–36, 6–1, 6–1 DDAM, 6–25 multi-point, 6–25 PSD, 6–18, 6–24 procedure, 6–18 sample input, 6–24 random vibration (PSD), 6–18 obtain the spectrum solution, 6–18 single-point, 6–2 procedure, 6–2 single-point response, 6–3, 6–3, 6–6 expand the modes, 6–6 obtain the modal solution, 6–3 obtain the spectrum solution, 6–3 spectrum data, 6–18 spectrum solution random vibration (PSD) analysis, 6–18 single-point response spectrum analysis, 6–3 spectrum type single-point response, 6–3 spin softening, 8–8 stability analysis, 7–1 static solution
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index buckling analysis, 7–4 static structural analysis, 2–1 loading, 2–8 procedure, 2–1 stepped loads, 4–9, 5–7, 5–14, 5–23, 8–60 stiffness matrix memory saving option, 8–50 strain creep, 8–29 strain energy, 12–6 strain rate creep, 8–29 strain rate effect, 2–4 stress calculations, 3–8, 4–21 stress concentration factors, 14–2 stress intensity factors, 12–1, 12–5 stress pass (see expansion pass) stress relaxation, 8–29 stress singularities accounting for in p-method, 15–7 PEXCLUDE command, 15–7 PINCLUDE command, 15–7 stress stiffening, 8–7 stress stiffening effects, 2–5, 5–32, 8–53 structural analyses buckling, 7–1 fatigue, 14–1 harmonic response, 4–1 modal, 3–1 nonlinear, 8–1 spectrum, 6–1 static, 2–1 transient dynamic, 5–1 structural analysis, 1–1 element types, 1–2 nonlinear, 8–1 structural energy error estimation, 2–11 STURM number, 3–7 subgrid results, 15–13 subspace method, 3–3, 3–17 substeps, 8–2, 8–5, 8–49 swelling, 8–8, 8–34 swelling subroutine, 8–34
T TABLE array parameters, 2–8 tabular listings, 2–11, 3–11, 4–12, 6–8, 8–57 tapered beams, 16–8 termination solution, 2–5 thin wall sections, 16–4 time, 5–23, 5–32
arc-length, 8–68 time integration effects, 5–7, 5–32, 8–60, 8–60 time step optimization thermal, 8–55 time steps, 8–2, 8–5, 8–6, 8–49 automatic, 2–2, 5–7, 5–35, 7–2, 8–51 number of, 2–2, 5–7, 8–67, 8–68 size of, 2–2, 5–7, 8–67 TOLER [CNVTOL], 8–51 transient dynamic analysis, 5–1 full method, 5–3 procedure, 5–3 load step options for, 5–10 methods of solution, 5–2 mode superposition method, 5–13 procedure, 5–13 preparing for, 5–1 prestressed, 5–32 reduced method, 5–19, 5–19 procedure, 5–19 reduced solution, 5–19 transient integration parameters, 5–7, 5–14, 5–22, 8–60 true strain, 8–7 true stress, 8–7, 8–7 Tsai-Wu failure criterion, 13–5
U unsymmetric method, 3–3, 3–18 user defined material, 8–16 user mesh files, 16–9 USERSW, 8–34
V vector displays, 2–11, 6–8 vector norms, 8–51 vector plots, 4–12 vibration analysis, 3–1 virtual crack extension method, 12–8 viscoelastic material curve fitting, 9–14 viscoelasticity, 8–8, 8–33 element types, 8–33 viscoplasticity, 8–8, 8–32, 8–32 element types, 8–32 large strain, 8–32 Voce hardening law, 8–10
W wave propagation effects, 5–33 writing user mesh, 16–2
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Index–11
Index
Y yield point, 8–9
Index–12
Structural Analysis Guide . ANSYS Release 8.1 . 001972 . © SAS IP, Inc.
Related Documents
Ansys 8.1 - Structural Analysis Guide
November 2019 19
7207839 Ansys Structural Analysis Guide
May 2020 3
Structural Analysis
June 2020 7
Structural Analysis
November 2019 18
Computer Aided Structural Analysis
December 2019 16
R5310105-structural Analysis - Ii
May 2020 10More Documents from ""
Ansys Example 0153 Offshore Structure
November 2019 17
Imo Circ 860 Guidelines For Offshore Containers
November 2019 8
Ansys 8.1 - Structural Analysis Guide
November 2019 19
Free.pdf
June 2020 11
