Docstoc

ans ctec

Document Sample
ans ctec Powered By Docstoc
					                       Contact Technology Guide




ANSYS, Inc.                                Release 12.0
Southpointe                                April 2009
275 Technology Drive                       ANSYS, Inc. is
Canonsburg, PA 15317                       certified to ISO
ansysinfo@ansys.com                        9001:2008.
http://www.ansys.com
(T) 724-746-3304
(F) 724-514-9494
Copyright and Trademark Information
© 2009 SAS IP, Inc. All rights reserved. Unauthorized use, distribution or duplication is prohibited.

ANSYS, ANSYS Workbench, Ansoft, AUTODYN, EKM, Engineering Knowledge Manager, CFX, FLUENT, HFSS and any and
all ANSYS, Inc. brand, product, service and feature names, logos and slogans are registered trademarks or trademarks
of ANSYS, Inc. or its subsidiaries in the United States or other countries. ICEM CFD is a trademark used by ANSYS, Inc.
under license. CFX is a trademark of Sony Corporation in Japan. All other brand, product, service and feature names
or trademarks are the property of their respective owners.

Disclaimer Notice
THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE SECRETS AND ARE CONFIDENTIAL
AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. The software products and document-
ation are furnished by ANSYS, Inc., its subsidiaries, or affiliates under a software license agreement that contains pro-
visions concerning non-disclosure, copying, length and nature of use, compliance with exporting laws, warranties,
disclaimers, limitations of liability, and remedies, and other provisions. The software products and documentation may
be used, disclosed, transferred, or copied only in accordance with the terms and conditions of that software license
agreement.
ANSYS, Inc. is certified to ISO 9001:2008.

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

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

Published in the U.S.A.
Table of Contents
1. Contact Overview .................................................................................................................................... 1
    1.1. General Contact Classification ........................................................................................................... 1
    1.2. ANSYS Contact Capabilities ............................................................................................................... 2
         1.2.1. Surface-to-Surface Contact Elements ........................................................................................ 3
         1.2.2. Node-to-Surface Contact Elements ........................................................................................... 4
         1.2.3. 3-D Line-to-Line Contact .......................................................................................................... 4
         1.2.4. Line-to-Surface Contact ............................................................................................................ 4
         1.2.5. Node-to-Node Contact Elements .............................................................................................. 4
2. GUI Aids for Contact Analyses ................................................................................................................ 7
    2.1. The Contact Manager ........................................................................................................................ 7
    2.2. The Contact Wizard ........................................................................................................................... 8
    2.3. Managing Contact Pairs .................................................................................................................... 9
3. Surface-to-Surface Contact ................................................................................................................... 11
    3.1. Using Surface-to-Surface Contact Elements ..................................................................................... 11
    3.2. Steps in a Contact Analysis .............................................................................................................. 11
    3.3. Creating the Model Geometry and Mesh ......................................................................................... 12
    3.4. Identifying Contact Pairs ................................................................................................................. 12
    3.5. Designating Contact and Target Surfaces ........................................................................................ 13
         3.5.1. Asymmetric Contact vs. Symmetric Contact ............................................................................ 14
             3.5.1.1. Background ................................................................................................................... 14
             3.5.1.2. Using KEYOPT(8) ............................................................................................................ 14
    3.6. Defining the Target Surface ............................................................................................................. 15
         3.6.1. Pilot Nodes ............................................................................................................................ 15
         3.6.2. Primitives ............................................................................................................................... 15
         3.6.3. Element Types and Real Constants .......................................................................................... 15
             3.6.3.1. Defining Target Element Geometry ................................................................................ 15
         3.6.4. Using Direct Generation to Create Rigid Target Elements ......................................................... 16
         3.6.5. Using ANSYS Meshing Tools to Create Rigid Target Elements ................................................... 17
             3.6.5.1. Some Modeling and Meshing Tips ................................................................................. 20
             3.6.5.2. Verifying Nodal Number Ordering (Contact Direction) of Target Surface .......................... 20
    3.7. Defining the Deformable Contact Surface ....................................................................................... 21
         3.7.1. Element Type ......................................................................................................................... 22
         3.7.2. Real Constants and Material Properties ................................................................................... 23
         3.7.3. Generating Contact Elements ................................................................................................. 23
    3.8. Set the Real Constants and Element KEYOPTS .................................................................................. 24
         3.8.1. Real Constants ....................................................................................................................... 25
             3.8.1.1. Positive and Negative Real Constant Values .................................................................... 27
         3.8.2. Element KEYOPTS ................................................................................................................... 28
         3.8.3. Selecting a Contact Algorithm (KEYOPT(2)) ............................................................................. 30
             3.8.3.1. Background ................................................................................................................... 30
         3.8.4. Determining Contact Stiffness and Allowable Penetration ....................................................... 31
             3.8.4.1. Background ................................................................................................................... 31
             3.8.4.2. Using FKN and FTOLN .................................................................................................... 32
             3.8.4.3. Using FKT and SLTO ....................................................................................................... 32
             3.8.4.4. Using KEYOPT(10) .......................................................................................................... 33
             3.8.4.5. Using KEYOPT(6) ............................................................................................................ 34
             3.8.4.6. Chattering Control Parameters ....................................................................................... 34
         3.8.5. Choosing a Friction Model ...................................................................................................... 35
             3.8.5.1. Background ................................................................................................................... 35
             3.8.5.2. Coefficient of Friction .................................................................................................... 36

                               Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                           of ANSYS, Inc. and its subsidiaries and affiliates.                                            iii
Contact Technology Guide

             3.8.5.3. Using TAUMAX, FACT, DC, and COHE ............................................................................... 36
             3.8.5.4. Static and Dynamic Friction Coefficients ......................................................................... 37
             3.8.5.5. Forced Frictional Sliding Using Velocity Input ................................................................. 38
             3.8.5.6. User-defined Friction ..................................................................................................... 39
         3.8.6. Selecting Location of Contact Detection ................................................................................. 39
             3.8.6.1. Background ................................................................................................................... 39
             3.8.6.2. Using KEYOPT(4) and TOLS ............................................................................................. 39
         3.8.7. Adjusting Initial Contact Conditions ........................................................................................ 41
             3.8.7.1. Background ................................................................................................................... 41
             3.8.7.2. Using PMIN, PMAX, CNOF, ICONT, KEYOPT(5), and KEYOPT(9) ........................................... 41
         3.8.8. Physically Moving Contact Nodes Towards the Target Surface .................................................. 47
         3.8.9. Determining Contact Status and the Pinball Region ................................................................ 48
             3.8.9.1. Background ................................................................................................................... 48
             3.8.9.2. Using PINB .................................................................................................................... 49
         3.8.10. Avoiding Spurious Contact in Self Contact Problems ............................................................. 49
         3.8.11. Selecting Surface Interaction Models .................................................................................... 50
             3.8.11.1. Background ................................................................................................................. 50
             3.8.11.2. Using KEYOPT(12) ........................................................................................................ 50
             3.8.11.3. Using FKOP .................................................................................................................. 51
             3.8.11.4. Bonded Contact for Shell-Shell Assemblies ................................................................... 52
         3.8.12. Modeling Contact with Superelements ................................................................................. 53
             3.8.12.1. Background ................................................................................................................. 53
             3.8.12.2. Using KEYOPT(3) .......................................................................................................... 53
         3.8.13. Accounting for Thickness Effect ............................................................................................ 54
             3.8.13.1. Background ................................................................................................................. 54
             3.8.13.2. Using KEYOPT(11) ........................................................................................................ 54
         3.8.14. Using Time Step Control and Impact Constraints ................................................................... 54
             3.8.14.1. Background ................................................................................................................. 54
             3.8.14.2. Using KEYOPT(7) .......................................................................................................... 54
         3.8.15. Using the Birth and Death Option ......................................................................................... 55
    3.9. Controlling the Motion of the Rigid Target Surface ........................................................................... 55
    3.10. Applying Necessary Boundary Conditions to the Deformable Elements .......................................... 56
    3.11. Applying Fluid Pressure-Penetration Loads .................................................................................... 56
         3.11.1. Applying Fluid Penetration Pressure ..................................................................................... 57
         3.11.2. Specifying Fluid Penetration Starting Points .......................................................................... 58
         3.11.3. Specifying a Pressure-Penetration Criterion ........................................................................... 59
         3.11.4. Specifying a Fluid Penetration Acting Time ........................................................................... 60
         3.11.5. Redefining or Modifying the Pressure-Penetration Loads ....................................................... 62
         3.11.6. Postprocessing Fluid Pressure-Penetration Loads .................................................................. 62
    3.12. Defining Solution and Load Step Options ...................................................................................... 63
    3.13. Solving the Problem ...................................................................................................................... 64
    3.14. Reviewing the Results ................................................................................................................... 65
         3.14.1. Points to Remember ............................................................................................................. 65
         3.14.2. Reviewing Results in POST1 .................................................................................................. 65
         3.14.3. Reviewing Results in POST26 ................................................................................................ 67
4. Node-to-Surface Contact ...................................................................................................................... 69
    4.1. The Node-to-Surface Contact Element ............................................................................................. 69
    4.2. Performing a Node-to-Surface Contact Analysis ............................................................................... 70
         4.2.1. CONTA175 KEYOPTS ............................................................................................................... 70
             4.2.1.1. KEYOPT(3) ..................................................................................................................... 70
             4.2.1.2. KEYOPT(4) ..................................................................................................................... 71
         4.2.2. CONTA175 Real Constants ...................................................................................................... 71


                              Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
iv                                                        of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                 Contact Technology Guide

    4.3. Using CONTA175 for Multiphysics Contact ....................................................................................... 71
5. 3-D Beam-to-Beam Contact .................................................................................................................. 73
    5.1. The 3-D Line-to-Line Contact Element ............................................................................................. 73
    5.2. Modeling Beam-to-Beam Contact ................................................................................................... 74
    5.3. Performing a 3-D Beam-to-Beam Contact Analysis ........................................................................... 75
         5.3.1. KEYOPTs and Real Constants ................................................................................................... 76
             5.3.1.1. Real Constants R1, R2 ..................................................................................................... 76
             5.3.1.2. KEYOPT(3) ..................................................................................................................... 77
             5.3.1.3. Real Constants FKN and FKT ........................................................................................... 77
             5.3.1.4. Real Constant TOLS ........................................................................................................ 77
             5.3.1.5. KEYOPT(4) ..................................................................................................................... 78
6. Line-to-Surface Contact ........................................................................................................................ 79
    6.1. The 3-D Line-to-Surface Contact Element ........................................................................................ 79
    6.2. Performing a 3-D Line-to-Surface Contact Analysis .......................................................................... 80
         6.2.1. KEYOPTs and Real Constants ................................................................................................... 80
             6.2.1.1. Real Constants FKN and FKT ........................................................................................... 81
             6.2.1.2. Accounting for Thickness Effect (CNOF and KEYOPT(11)) ................................................. 81
             6.2.1.3. Real Constant TOLS ........................................................................................................ 81
             6.2.1.4. KEYOPT(4) ..................................................................................................................... 81
7. Multiphysics Contact ............................................................................................................................. 83
    7.1. Modeling Thermal Contact .............................................................................................................. 83
         7.1.1. Thermal Contact Behavior vs. Contact Status ........................................................................... 83
         7.1.2. Free Thermal Surface .............................................................................................................. 84
         7.1.3. Temperature on Target Surface ............................................................................................... 84
         7.1.4. Modeling Conduction ............................................................................................................ 84
             7.1.4.1. Using TCC ...................................................................................................................... 84
             7.1.4.2. Using the Quasi Solver Option ....................................................................................... 85
         7.1.5. Modeling Convection ............................................................................................................. 85
         7.1.6. Modeling Radiation ................................................................................................................ 85
             7.1.6.1. Background ................................................................................................................... 85
             7.1.6.2. Using SBCT and RDVF .................................................................................................... 86
         7.1.7. Modeling Heat Generation Due to Friction .............................................................................. 86
             7.1.7.1. Background ................................................................................................................... 86
             7.1.7.2. Using FHTG and FWGT ................................................................................................... 87
         7.1.8. Modeling External Heat Flux ................................................................................................... 87
    7.2. Modeling Electric Contact ............................................................................................................... 87
         7.2.1. Modeling Surface Interaction ................................................................................................. 88
             7.2.1.1. Background ................................................................................................................... 88
             7.2.1.2. Using ECC ...................................................................................................................... 88
         7.2.2. Modeling Heat Generation Due to Electric Current .................................................................. 88
    7.3. Modeling Magnetic Contact ............................................................................................................ 89
         7.3.1. Using MCC ............................................................................................................................. 90
         7.3.2. Modeling Perfect Magnetic Contact ........................................................................................ 90
8. Node-to-Node Contact .......................................................................................................................... 91
    8.1. Node-to-Node Contact Elements ..................................................................................................... 91
    8.2. Performing a Node-to-Node Contact Analysis .................................................................................. 92
         8.2.1. Creating Geometry and Meshing the Model ............................................................................ 92
         8.2.2. Generating Contact Elements ................................................................................................. 92
             8.2.2.1. Generating Contact Elements Automatically at Coincident Nodes ................................... 92
             8.2.2.2. Generating Contact Elements Automatically at Offset Nodes .......................................... 93
             8.2.2.3. Node Ordering .............................................................................................................. 93
         8.2.3. Defining the Contact Normal .................................................................................................. 93


                              Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                          of ANSYS, Inc. and its subsidiaries and affiliates.                                           v
Contact Technology Guide

         8.2.4. Defining the Initial Interference or Gap ................................................................................... 95
         8.2.5. Selecting the Contact Algorithm ............................................................................................. 95
         8.2.6. Applying Necessary Boundary Conditions ............................................................................... 95
         8.2.7. Defining the Solution Options ................................................................................................ 96
         8.2.8. Solving the Problem ............................................................................................................... 97
         8.2.9. Reviewing the Results ............................................................................................................ 97
9. Multipoint Constraints and Assemblies ................................................................................................ 99
    9.1. Modeling Solid-Solid and Shell-Shell Assemblies ........................................................................... 100
    9.2. Modeling a Shell-Solid Assembly ................................................................................................... 102
    9.3. Surface-Based Constraints ............................................................................................................. 106
         9.3.1. Defining Surface-Based Constraints ...................................................................................... 108
         9.3.2. Defining Influence Range (PINB) ........................................................................................... 109
         9.3.3. Degrees of Freedom of Surface-Based Constraints ................................................................. 109
         9.3.4. Specifying a Local Coordinate System ................................................................................... 110
         9.3.5. Additional Guidelines for a Force-Distributed Constraint ....................................................... 111
         9.3.6. Additional Guidelines for A Rigid Surface Constraint ............................................................. 111
         9.3.7. Modeling a Beam-Solid Assembly ......................................................................................... 111
    9.4. Modeling Rigid Bodies .................................................................................................................. 112
         9.4.1. Modeling Contact between Rigid Bodies .............................................................................. 113
    9.5. Overconstraint Detection and Elimination ..................................................................................... 113
    9.6. Restrictions and Recommendations for Internal MPC ..................................................................... 114
10. Dynamic Contact and Impact Modeling ........................................................................................... 117
    10.1. Energy and Momentum Conserving Contact ............................................................................... 117
         10.1.1. Energy Conservation .......................................................................................................... 118
         10.1.2. Automatic Time Stepping ................................................................................................... 118
         10.1.3. Penetration and Relative Velocity ........................................................................................ 118
11. Spot Welds ......................................................................................................................................... 119
    11.1. Defining a Spot Weld Set ............................................................................................................. 120
         11.1.1. Creating a Basic Spot Weld Set with SWGEN ........................................................................ 120
         11.1.2. The Components of a Spot Weld ......................................................................................... 124
         11.1.3. Adding Surfaces to a Basic Set ............................................................................................ 126
    11.2. Listing and Deleting Spot Welds .................................................................................................. 129
12. Debonding ........................................................................................................................................ 131
    12.1. Including Debonding in a Contact Analysis .................................................................................. 131
         12.1.1. Cohesive Zone Materials Used for Debonding ..................................................................... 132
               12.1.1.1. Bilinear Material Behavior with Tractions and Separation Distances (TBOPT = CBDD) .... 132
               12.1.1.2. Bilinear Material Behavior with Tractions and Critical Fracture Energies (TBOPT =
               CBDE) ..................................................................................................................................... 132
         12.1.2. Debonding Modes ............................................................................................................. 133
         12.1.3. Other Considerations for Debonding .................................................................................. 133
         12.1.4. Postprocessing ................................................................................................................... 133
A. Example 2-D Contact Analysis with Fluid Pressure-Penetration Loading .................................................. 135
    A.1. Problem Description ..................................................................................................................... 135
    A.2. Input File ...................................................................................................................................... 138
Index ........................................................................................................................................................ 143



List of Figures
2.1. Contact Manager Toolbar ........................................................................................................................ 7
2.2. Example of a Contact Wizard Dialog ........................................................................................................ 9
3.1. Localized Contact Zones ....................................................................................................................... 13

                                Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
vi                                                          of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  Contact Technology Guide

3.2. ANSYS Geometric Entities and Their Corresponding Rigid Target Elements ............................................. 18
3.3. A Single Circular Target Segment Created From Arc Line Segments ........................................................ 18
3.4. Meshing Patterns for Arbitrary Target Surfaces ....................................................................................... 19
3.5. Smoothing Convex Corner .................................................................................................................... 20
3.6. Correct Node Ordering .......................................................................................................................... 20
3.7. Contact Element Types .......................................................................................................................... 22
3.8. Specification of the Contact Surface's Outward Normal .......................................................................... 24
3.9. Depth of the Underlying Element .......................................................................................................... 28
3.10. Sliding Contact Resistance .................................................................................................................. 36
3.11. Friction Decay ..................................................................................................................................... 38
3.12. Contact Detection Located at Gauss Point ........................................................................................... 39
3.13. Contact Detection Point Location at Nodal Point ................................................................................. 40
3.14. Node Slippage Using Nodal Integration KEYOPT(4) = 1 or 2 .................................................................. 40
3.15. Contact Surface Adjustment With ICONT ............................................................................................. 43
3.16. Contact Surface Adjustment (PMIN, PMAX) .......................................................................................... 44
3.17. A Scenario in Which Initial Adjustment Will Fail .................................................................................... 44
3.18. Ignoring Initial Penetration, KEYOPT(9) = 1 ........................................................................................... 46
3.19. Components of True Penetration ......................................................................................................... 46
3.20. Ramping Initial Interference ................................................................................................................ 47
3.21. Effect of Moving Contact Nodes .......................................................................................................... 48
3.22. Auto Spurious Prevention ................................................................................................................... 50
3.23. Penalty-Based Shell-Shell Assembly ..................................................................................................... 52
3.24. Path Dependent Fluid Penetration Loading ......................................................................................... 57
3.25. Free End Points (2-D) and Free Open Edges (3-D) ................................................................................. 59
3.26. Fluid Penetration Acting Time (FPAT) Greater Than Substep ................................................................. 61
3.27. Fluid Penetration Acting Time (FPAT) Less Than Substep ...................................................................... 62
4.1. Node-to-Surface Contact Elements ........................................................................................................ 69
5.1. Line-to-Line Contact Elements .............................................................................................................. 73
5.2. Internal Contact (One Beam Sliding Inside Another) ............................................................................... 74
5.3. External Contact (Two Beams Roughly Parallel) ...................................................................................... 74
5.4. External Contact (Two Beams Cross Each Other) .................................................................................... 75
5.5. Continuous Line Segments ................................................................................................................... 76
5.6. Equivalent Circular Cross Section ........................................................................................................... 77
6.1. Line-to-Surface Contact Elements ......................................................................................................... 79
6.2. Continuous Line Segments ................................................................................................................... 80
7.1. Target Temperature ............................................................................................................................... 84
8.1. Node-to-Node Contact Elements ........................................................................................................... 91
8.2. Contact Between Two Concentric Pipes ................................................................................................. 93
8.3.Two Concentric Pipes, Normals Rotated Properly .................................................................................... 94
8.4. Example of Overconstrained Contact Problem ....................................................................................... 96
9.1. Example of Shell-Solid Assembly ......................................................................................................... 102
9.2. Shell-Solid Assembly (Original Mesh) ................................................................................................... 103
9.3. Shell-Solid Assembly with Solid-Solid Constraint Option ...................................................................... 104
9.4. Shell-Solid Assembly with Shell-Shell Constraint Option ....................................................................... 104
9.5. Shell-Solid Assembly with Shell-Solid Constraint Option ...................................................................... 105
9.6. Shell-Solid Constraint - No Intersection (use KEYOPT(5) = 4 or 5) ........................................................... 106
9.7. Rigid Surface Constraint ...................................................................................................................... 107
9.8. Force-Distributed Constraint ............................................................................................................... 108
9.9. Slider Link ........................................................................................................................................... 110
9.10. Free Radial Expansion Under Torque Load .......................................................................................... 111
9.11. Beam-Solid Assembly Defined by Rigid Surface Constraint ................................................................. 112
9.12. Beam-Solid Assembly Defined by Force-distributed Constraint ........................................................... 112


                               Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                           of ANSYS, Inc. and its subsidiaries and affiliates.                                              vii
Contact Technology Guide

11.1. Example Spot Weld Configuration ..................................................................................................... 119
11.2. Default Projection Direction for Node 1 ............................................................................................. 121
11.3. Default Projection Direction for Nodes 1 and 2 ................................................................................... 122
11.4. User-specified Projection Direction, Node 1 ....................................................................................... 122
11.5. User-specified Projection Direction, Nodes 1 and 2 ............................................................................. 123
11.6. Search Radius for Spot Weld .............................................................................................................. 124
11.7. Nodes Included in Constraint Equations ............................................................................................ 125
11.8. Beam Element Created for Spot Weld ................................................................................................ 125
11.9. Surfaces Added to Basic Spot Weld Set .............................................................................................. 127
11.10. Node Reordering for Beam Elements ............................................................................................... 128
A.1. Diagram of Planar Seal Model ............................................................................................................. 135
A.2. Meshed Planar Seal Model .................................................................................................................. 136
A.3. Fluid Pressure Loading on Planar Seal .................................................................................................. 136
A.4. Intermediate Fluid Pressure Distribution ............................................................................................. 137
A.5. Final Fluid Pressure Distribution .......................................................................................................... 137
A.6. Time History of Fluid Pressure for Three Contact Elements ................................................................... 138



List of Tables
1.1. ANSYS Contact Capabilities ..................................................................................................................... 2
3.1. Summary of Real Constant Defaults in Different Environments ............................................................... 26
3.2. Summary of KEYOPT Defaults in Different Environments ........................................................................ 29




                              Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
viii                                                      of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 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 Chapter 9, Multipoint
Constraints and Assemblies (p. 99) for more information). Another alternative is to use constraint equations
or coupled degrees of freedom instead of contact to model these situations (see "Coupling and Constraint
Equations" in the Modeling and Meshing Guide for more information). The external constraint equations or
coupling equations are only suitable for small strain applications.

In addition to the implicit contact capabilities discussed in this guide, 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.

1.1. 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.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               1
Chapter 1: Contact Overview


1.2. ANSYS Contact Capabilities
ANSYS supports five contact models: node-to-node, node-to-surface, surface-to-surface, line-to-line, and line-
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 the table below.

Table 1.1 ANSYS Contact Capabilities
                        Node-to-Node                           Node-              Surface-to-Sur-                     Line-            Line-
                                                              to- Sur-                 face                            to-            to- Sur-
                                                                face                                                  Line              face
Contact Ele-       12              52            178              175              171,              173,              176             177
 ment No.                                                                          172               174
    Target Ele-                                                  169,              169               170               170             170
     ment No.                                                    170
2-D                 Y                              Y                Y                 Y
3-D                                 Y              Y                Y                                  Y                 Y               Y
Sliding           small          small          small            large             large            large             large            large
Cylindrical         Y                              Y
Gap
Pure Lag-                                          Y                Y                 Y                Y                 Y               Y
range Multipli-
er
Augmented                                          Y                Y                 Y                Y                 Y               Y
Lagrange Mul-
tiplier
Lagrange Mul-                                      Y                Y                 Y                Y                 Y               Y
tiplier on Nor-
mal and Pen-
alty on Tan-
gent
Internal Multi-                                                     Y                 Y                Y                 Y               Y
point Con-
straint (MPC)
Contact Stiff-    user-   user-   semi-                         semi-             semi-             semi-             semi-            semi-
ness              defined defined auto                          auto              auto              auto              auto             auto
Auto-meshing      EINTF         EINTF          EINTF           ESURF             ESURF             ESURF             ESURF            ESURF
Tools
Lower-Order         Y               Y              Y                Y                 Y                Y                 Y               Y
Higher-Order                                                    Y (2-D                Y                Y                 Y               Y
                                                                only)
Rigid-Flexible      Y               Y              Y                Y                 Y                Y                 Y               Y
Flexible-Flex-      Y               Y              Y                Y                 Y                Y                 Y               Y
ible
Thermal Con-                                                        Y                 Y                Y
tact


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
2                                                   of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                1.2.1. Surface-to-Surface Contact Elements

                        Node-to-Node                         Node-              Surface-to-Sur-                     Line-            Line-
                                                            to- Sur-                 face                            to-            to- Sur-
                                                              face                                                  Line              face
Contact Ele-       12            52            178              175              171,              173,              176             177
 ment No.                                                                        172               174
 Target Ele-                                                   169,              169               170               170             170
  ment No.                                                     170
Electric Con-                                                     Y                 Y                Y
tact
Magnetic                                                          Y                 Y                Y
Contact

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. 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 remaining chapters of this guide.

An overview of the ANSYS contact elements and their capabilities follows. For detailed information on any
of these elements, refer to the Element Reference and the Theory Reference for the Mechanical APDL and
Mechanical Applications.

1.2.1. 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 Chapter 3, Surface-
to-Surface Contact (p. 11).

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, corner-
     noded 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.
 •   Allow modeling of fluid pressure penetration loads.

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


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                          3
Chapter 1: Contact Overview

rigid forms or general deformable forms can be modeled using special preprocessing techniques (see Defining
the Target Surface (p. 15) for more information).

Surface-to-surface contact elements are not well-suited for point-to-point, point-to-surface, edge-to-surface,
or 3-D line-to-line contact applications, such as pipe whip or snap-fit assemblies. You should use the node-
to-surface, node-to-node, or line-to-line 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.

1.2.2. 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. Contact occurs when the element penetrates one of the target
segment elements (TARGE169, TARGE170) on a specified target surface. CONTA175 is typically used to
model point-to-surface contact applications, such as the corners of snap-fit parts sliding along the mating
surface.

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 discontinuous. No contour plots are available for contact results.

1.2.3. 3-D Line-to-Line Contact
The line-to-line contact element, CONTA176, is typically used to model 3-D beam-to-beam contact (crossing
beams or beams that are parallel to each other) or a pipe sliding inside another pipe. Some practical applic-
ations are woven fabric and tennis racquet strings.

CONTA176 can be attached to 3-D beam or pipe elements and supports both low-order and higher-order
elements on the contact surface. The target surface is modeled with 3-D line segments (TARGE170 straight
line or parabolic line elements). This element supports large sliding and large displacement applications.
For more information on how to use CONTA176, see Chapter 5, 3-D Beam-to-Beam Contact (p. 73).

1.2.4. Line-to-Surface Contact
The line-to-surface contact element, CONTA177, can be used to model a 3D beam or shell edge contacting
solid or shell elements. CONTA177 supports both low-order and higher-order elements on the contact surface.
The target surface is modeled with 3-D target segment elements (TARGE170). This element is also suitable
for large sliding and large displacement applications. For more information on how to use CONTA177, see
Chapter 6, Line-to-Surface Contact (p. 79).

1.2.5. Node-to-Node Contact Elements
Node-to-node contact elements are typically used to model point-to-point contact applications. To use node-
to-node contact elements, you need to know the location of contact beforehand. These types of contact


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
4                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                     1.2.5. Node-to-Node Contact Elements

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 suf-
ficient.

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.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                   5
    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
6                               of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 2: GUI Aids for Contact Analyses
Several GUI aids are available to help you create and manage contact pairs. The Contact Manager allows
you to define, view, and edit contact pairs. It provides a convenient way to manage all contact pairs for your
entire model. The Contact Wizard, which is accessed from the Contact Manager, leads you through the
process of creating contact pairs.

The following contact-related GUI topics are available:
 2.1.The Contact Manager
 2.2.The Contact Wizard
 2.3. Managing Contact Pairs

2.1. The Contact Manager
You can access the Contact Manager via the Contact Manager icon         in the ANSYS Standard Toolbar, or
via the menu path Preprocessor> Modeling> Create> Contact Pair. The Contact Manager is available at
the Begin level and in the following processors: preprocessor (PREP7), solution (SOLU), and general postpro-
cessor (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 2.1: Contact Manager Toolbar




 •   Contact Wizard - Accesses the Contact Wizard GUI described in The Contact Wizard (p. 8). Allows you
     to manually define target and contact surfaces. Supports both 2-D and 3-D geometries as well as rigid-
     flexible (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.
 •   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

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               7
Chapter 2: GUI Aids for Contact Analyses

 •   Flip Normals - Flips the element normals of the selected contact pair. This action is limited to the ele-
     ments 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 Physically Moving Contact Nodes Towards the Target Surface (p. 47).)
     –   Reset target element and contact element key options and real constants to their default values
         (CNCHECK,RESET command).
 •   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.

2.2. 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.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
8                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                        2.3. Managing Contact Pairs

Figure 2.2: 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.

2.3. Managing Contact Pairs
As discussed in Chapter 3, Surface-to-Surface Contact (p. 11) 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

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.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                            9
Chapter 2: GUI Aids for Contact Analyses

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 com-
     mands to read the results from the proper results file (see CNCHECK for details).




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
10                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 3: Surface-to-Surface Contact
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 Chapter 2,
GUI Aids for Contact Analyses (p. 7) for more information on using the Contact Manager.

This chapter explains how to set up a surface-to-surface contact analysis using both the command and GUI
approaches. The following topics are available:
 3.1. Using Surface-to-Surface Contact Elements
 3.2. Steps in a Contact Analysis
 3.3. Creating the Model Geometry and Mesh
 3.4. Identifying Contact Pairs
 3.5. Designating Contact and Target Surfaces
 3.6. Defining the Target Surface
 3.7. Defining the Deformable Contact Surface
 3.8. Set the Real Constants and Element KEYOPTS
 3.9. Controlling the Motion of the Rigid Target Surface
 3.10. Applying Necessary Boundary Conditions to the Deformable Elements
 3.11. Applying Fluid Pressure-Penetration Loads
 3.12. Defining Solution and Load Step Options
 3.13. Solving the Problem
 3.14. Reviewing the Results

     Note

     The procedures described in this chapter also apply to node-to-surface contact analyses using
     CONTA175, 3-D beam-to-beam contact analyses using CONTA176, and 3-D line-to-surface contact
     using CONTA177 unless otherwise noted.


3.1. 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 pairs, use TARGE170 with CONTA173, CONTA174, CONTA175, CONTA176, or CONTA177.
Each contact pair is identified via the same real constant number.

3.2. 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 sections.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               11
Chapter 3: Surface-to-Surface Contact

 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.    Apply fluid pressure-penetration loads
 10. Define solution options and load steps
 11. Solve the contact problem
 12. Review the results

Each contact-specific step also has a corresponding GUI approach where you use functions and features on
the Contact Toolbar.

3.3. 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
Modeling and Meshing Guide.

      Command(s): AMESH, VMESH
      GUI: Main Menu> Preprocessor> Meshing> Mesh

       Note

       You should avoid midside-noded elements for 3-D contact surfaces when using node-to-surface
       element CONTA175.


3.4. 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 kin-
ematics 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 ne-
cessary 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.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
12                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                            3.5. Designating Contact and Target Surfaces

Figure 3.1: 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 3.1: Loc-
alized Contact Zones (p. 13).

The geometry-based contact pair generation tools (see the Contact Wizard) may create unnecessary contact
and target elements which are never in contact during solution. For modeling small sliding contact or assembly
contact, you can issue CNCHECK,TRIM to remove contact and target elements which are initially in far-field
(that is, open and not near contact). The trimming is based on the contact pinball size; the smaller the pinball
radius, the greater the number of contact and target elements that will be deleted. The contact trimming
option is useful in Distributed ANSYS runs to achieve better performance.

3.5. 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.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                13
Chapter 3: Surface-to-Surface Contact

 •   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.
 •   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 ele-
     ments 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 sur-
     rounds the other surface, the larger surface should be the target surface.
 •   In the case of 3-D internal beam-to-beam contact modeled by CONTA176 (a beam or pipe sliding inside
     another hollow beam or pipe), the inner beam should be considered the contact surface and the outer
     beam should be the target surface. However, when the inner beam is much stiffer than the outer beam,
     the inner beam can 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.

3.5.1. Asymmetric Contact vs. Symmetric Contact
3.5.1.1. 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
surface-to-surface contact. However, under some circumstances asymmetric contact does not perform satis-
factorily. 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 circum-
stances, 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.

3.5.1.2. 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.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
14                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                    3.6.3. Element Types and Real Constants


     Note

     In any contact model, you can mix different types of contact pairs: rigid-to-flexible or flexible-to-
     flexible contact; symmetric contact or asymmetric contact. However, only one type can exist with
     a contact pair.


3.6. 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 Defining the Deform-
able Contact Surface (p. 21) for details). If you are modeling 3-D line-to-line contact and the underlying ele-
ments are a part of shell edges, issue ESURF,,,LINE to generate 3-D line or parabola segments along the
shell edges.

You should not use the following rigid target segments for a deformable target surface: ARC, CARC, CIRC,
CYL1, CONE, SPHE, POINT, 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, straight lines, parabolas, cylinders, cones, and spheres,
which can be represented with TARGE170. You can use any reasonable combination of low/high-order triangles
and quadrilaterals to model a target surface with a complex, arbitrary geometry.

3.6.1. 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 usually
should be prescribed on 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.

3.6.2. 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. The primitives do not support MPC based bonded or no-separation contact.

3.6.3. 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

3.6.3.1. Defining Target Element Geometry
You define characteristics of the target element geometry through real constants R1 and R2 as follows:

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                   15
Chapter 3: Surface-to-Surface Contact

 •   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, and to line-to-surface
     element CONTA177):
     –   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.
 •   For CONTA176, used to model 3-D beam-to-beam contact:
     –   R1 is the radius of circular beams on the target side (target radius). Use a positive value when
         modeling external beam-to-beam contact. Use a negative value to represent the inner radius of the
         outer beam (or pipe) when modeling internal beam-to-beam contact.
     –   R2 is the radius of circular beams on the contact side (contact radius). Use a positive value for both
         external and internal beam-to-beam contact.

To set the real constant number for the target elements:

     Command(s): REAL
     GUI: Main Menu> Preprocessor> Real Constants

For TARGE169 and TARGE170, you need only set real constants R1 and R2 (if required). For a complete de-
scription of the target elements, element shapes, and real constants, see the description of TARGE169 and
TARGE170 in the Element Reference.

      Note

      Specifying real constants (R1, R2) manually is necessary only if you use direct generation to create
      your target elements, or if you model 3-D beam-to-beam contact with CONTA176. You can also
      use the ANSYS meshing tools to create the elements, or use the Contact Manager Toolbar.


3.6.4. 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 and 3-D)
 •   Parabola (2-D and 3-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)

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
16                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                           3.6.5. Using ANSYS Meshing Tools to Create Rigid Target Elements

 •   Eight-node quadrilateral (3-D)
 •   Cylinder (3-D)
 •   Cone (3-D)
 •   Sphere (3-D)
 •   Point (2-D or 3-D)
 •   Pilot node (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 "Direct Generation" in the 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
     GUI: Utility Menu> List> Elements> Nodes + Attributes

3.6.5. 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 POINT segments, use the Direct Generation method or use ESURF,,,POINT command on selected
nodes.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               17
Chapter 3: Surface-to-Surface Contact

To generate 2-D rigid target elements or 3-D rigid line/parabola segments, 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 3.2: ANSYS Geometric Entities and Their Corresponding Rigid Target Ele-
ments (p. 18)). If all the arcs form a closed circle, ANSYS creates a single circular segment (see Figure 3.3: A
Single Circular Target Segment Created From Arc Line Segments (p. 18)). 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 cir-
cular segment.

     Command(s): LMESH
     GUI: Main Menu> Preprocessor> Meshing> Mesh> Lines

Figure 3.2: ANSYS Geometric Entities and Their Corresponding Rigid Target Elements




Figure 3.3: 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 automat-
ically 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.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
18                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                           3.6.5. Using ANSYS Meshing Tools to Create Rigid Target Elements

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 3.4: Meshing Patterns for Arbitrary Target
Surfaces (p. 19) 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 auto-
     matically.

Figure 3.4: Meshing Patterns for Arbitrary Target Surfaces




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               19
Chapter 3: Surface-to-Surface Contact

3.6.5.1. 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 3.5: Smoothing Convex
Corner (p. 20)).

Figure 3.5: Smoothing Convex Corner




3.6.5.2. 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 3.6: Correct Node Ordering (p. 20)).

Figure 3.6: Correct Node Ordering




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
20                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                           3.7. Defining the Deformable Contact Surface

For 3-D contact, the target 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.

For 3-D line segments, the target nodes must be numbered in a sequence that defines a continuous line.
The line can be made up of linear or parabolic segments, depending on whether the underlying beam is
made up of first order or second order elements.

To check the direction of the normals, turn on the element coordinate systems.

     Command(s): /PSYMB,ESYS,1
     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.


3.7. Defining the Deformable Contact Surface
To create the deformable contact surface, you must define that surface using one of the following contact
elements:

 •   CONTA171 or CONTA172 (for 2-D)
 •   CONTA173 or CONTA174 (for 3-D)
 •   CONTA175 (for 2- or 3-D)
 •   CONTA176 or CONTA177 (for 3-D line)

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, beam, or pipe 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.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               21
Chapter 3: Surface-to-Surface Contact

3.7.1. Element Type
The four surface-to-surface contact element types are shown in the figure below, followed by a brief descrip-
tion of each element. For complete information on these element types, see the Element Reference.

Figure 3.7: Contact Element Types




 •   CONTA171: This 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 SHELL208).
 •   CONTA172: This 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 PLANE183).
 •   CONTA173: This 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 trian-
     gular element.
 •   CONTA174: This 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 SHELL281). It can be
     degenerated to 3- to 7-node quadrilateral/triangular shapes.

The following elements can also be defined using the method described here.

 •   CONTA175: This is a 2- or 3-D, 1-node element that can be located on the surface of 2-D lower order
     and higher order solid or beam elements or 3-D lower order solid or shell elements. Use CONTA175 for
     node-to-surface contact.
 •   CONTA176: This is a 3-D line element that can be located on the surface of 3-D beam and pipe elements.
     The element can be a 2-node line or a 3-node parabola, depending on whether the underlying element
     is lower or higher order. Use CONTA176 to model 3-D beam-to-beam contact.
 •   CONTA177: This is a 3-D line element that can be located on the surface of 3-D beam and pipe elements
     or on the edge of 3-D shell elements. The element can be a 2-node line or a 3-node parabola, depending
     on whether the underlying element is lower or higher order. Use CONTA177 to model 3-D line-to-surface
     contact.

Use the following command to define the contact element type.

     Command(s): ET


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
22                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                             3.7.3. Generating Contact Elements

      GUI: Main Menu> Preprocessor> Element Type> Add/Edit/Delete

3.7.2. 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. ANSYS automatically defines a default value for tangent (sliding) contact stiffness that is propor-
tional 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.

3.7.3. Generating Contact Elements
You can generate contact elements either through direct generation or by generating the surface automat-
ically 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 ele-
       ments are solid elements, then the TOP or BOTTOM setting has no effect.
 3.    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 surface-to-surface contact
       elements CONTA173 and CONTA174, 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. For the 3-D line-to-
       line contact element CONTA176 and the 3-D line-to-surface contact element CONTA177, the contact

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                      23
Chapter 3: Surface-to-Surface Contact

     nodes must be ordered in a sequence that defines a continuous line. Figure 3.8: Specification of the
     Contact Surface's Outward Normal (p. 24) illustrates both proper and improper specification of the
     contact surface's outward normal.

         Command(s): /PSYMB,ESYS
         GUI: Utility Menu> PlotCtrls> Symbols

     Figure 3.8: 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, you can 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 node-
     to-surface contact (CONTA175) because it is a single-node element with no surface normal asso-
     ciated with it.


3.8. Set the Real Constants and Element KEYOPTS
ANSYS uses several real constants and KEYOPTs to control contact behavior using surface-to-surface contact
elements. For more information in addition to what is presented here, refer to the individual contact element
descriptions in the Element Reference.

If you decide the real constant and KEYOPT settings you have specified for a particular contact pair are not
appropriate, you can use the CNCHECK,RESET command to reset all values back to their default settings.
Some real constants and key options are not affected by this command; see CNCHECK for details.

In many cases, certain default settings may not be appropriate for your specific model. You can issue the
CNCHECK,AUTO command to obtain optimized KEYOPT and real constant settings in terms of robustness
and efficiency. Usually, only the undefined or default KEYOPT settings and real constants are changed. Refer
to the CNCHECK command description for details of which settings are typically changed. You should always

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
24                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    3.8.1. Real Constants

verify these changes by issuing the CNCHECK,DETAIL command to list current contact pair properties. If
necessary, you can overwrite the optimized settings by redefining specific KEYOPTs (KEYOPT command)
and real constants (RMODIF command).

3.8.1. 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.
 •   FKOP specifies the stiffness factor applied when contact opens or the damping coefficient for standard
     contact.
 •   FKT specifies the tangent contact stiffness factor.
 •   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) = 1 or 2) or when KEYOPT(2) = 3.
 •   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).
 •   PPCN specifies the pressure-penetration criterion (surface contact elements only).
 •   FPAT specifies the fluid penetration acting time (surface contact elements only).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                                 25
Chapter 3: Surface-to-Surface Contact

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 3.1 Summary of Real Constant Defaults in Different Environments
Real Constants          Description                                                     ANSYS De-                ANSYS
                                                                                        fault                    Work-
                                                                                                                 bench
                                                                                                                 Default
No.         Name
1           R1          Radius associated with target geo-                              0                        n/a
                        metry [5]
2           R2          Radius associated with target geo-                              0                        n/a
                        metry
                                                                                        1
                        Superelement thickness [5 (p. 27)]
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 or                                    1                        1
                        Damping coefficient                                             0                        0
12          FKT         Tangent penalty stiffness factor                                1                        1
13          COHE        Contact cohesion                                                0                        0
14          TCC         Thermal contact conductance                                     0                        [3]
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                        [7]
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          TNOP        Maximum allowable tensile contact                               [6]                      [6]
                        pressure
25          TOLS        Target edge extension factor                                    [4]                      [4]
26          MCC         Magnetic contact permeance                                      0                        n/a
27          PPCN        Pressure-penetration criterion                                  0                        n/a

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
26                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     3.8.1. Real Constants

Real Constants            Description                                                     ANSYS De-                ANSYS
                                                                                          fault                    Work-
                                                                                                                   bench
                                                                                                                   Default
No.          Name
28           FPAT         Fluid penetration acting time                                   0.01                     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 Using PINB (p. 49)).
 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.
 5.    R1 and R2 are used to define the target element geometry. See Defining Target Element Geometry (p. 15)
       and the target element descriptions (TARGE169 and TARGE170) for details on how they are used for
       different geometries.
 6.    TNOP defaults to the force convergence tolerance divided by contact area at contact nodes.
 7.    Calculated as a function of lowest resistivity and overall model size.

      Command(s): R
      GUI: Main Menu> Preprocessor> Real Constants

3.8.1.1. 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 3.9: Depth of the Underlying Element (p. 28) 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.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                                 27
Chapter 3: Surface-to-Surface Contact

Figure 3.9: 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.


3.8.2. 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 (see note
     below for other meanings of KEYOPT(3))
 •   Location of contact detection point (KEYOPT(4))
 •   CNOF Automated adjustment (KEYOPT(5))
 •   Contact stiffness variation range (KEYOPT(6))
 •   Time step control and impact constraints (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)) (not applicable to CONTA176 or CONTA177)
 •   Behavior of contact surface (rough, bonded, etc.) (KEYOPT(12))


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
28                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                              3.8.2. Element KEYOPTS

 •   Behavior of fluid penetration load (KEYOPT(14))

     Note

     For node-to-surface contact (CONTA175), KEYOPT(3) specifies the contact model. For line-to-line
     contact (CONTA176), KEYOPT(3) specifies the type of beam-to-beam contact. KEYOPT(3) is not
     used for line-to-surface contact (CONTA177).

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 3.2 Summary of KEYOPT Defaults in Different Environments
KEY-      Description                                ANSYS              ANSYS              ANSYS Work-                 ANSYS Work-
OPT                                                                     Contact            bench De-                   bench, De-
                                                                        Wizard             fault Linear                fault Nonlin-
                                                                                           (bonded, no                 ear (standard,
                                                                                           sep)                        rough)
1         Selects DOF*                               Manual             Auto               Auto                        Auto
2         Contact Algorithm                          Aug.               Aug.               Pure Penalty                Pure Penalty
                                                     Lagr.              Lagr.
3         Stress state when superele- no su-                            no su-             n/a                         n/a
          ment is present             per                               per
                                      elem                              elem
4         Location of contact detec-                 gauss              gauss              gauss                       gauss
          tion point
5         CNOF/ICONT adjustment                      No ad-             No ad-             No adjust                   No adjust
                                                     just               just
6         Contact stiffnes variation                 Use de-            Use de-            Use default                 Use default
                                                     fault              fault              range                       range
                                                     range              range
7         Element level time incre-                  No con-            No con-            No control                  No control
          ment control                               trol               trol
8         Asymmetric contact selec-                  No ac-             No ac-             No action                   No action
          tion                                       tion               tion
9         Effect of initial penetration Include                         Include            Exclude all                 Include all
          or gap                        all                             all
10        Contact stiffness update                   Between Between Between                                           Between load
                                                     load    itera-  load steps                                        steps
                                                     steps   tions
11        Beam/shell thickness effect                Exclude            Exclude            Exclude                     Exclude
12        Behavior of contact sur-                   Stand-             Stand-             Bonded                      n/a
          face                                       ard                ard
14        Behavior of fluid penetra-                 Itera-             Itera-             n/a                         n/a
          tion load                                  tion-              tion-
                                                     based              based


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                            29
Chapter 3: Surface-to-Surface Contact

*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

3.8.3. Selecting a Contact Algorithm (KEYOPT(2))
3.8.3.1. 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
FKT for all values of KEYOPT(10), plus FTOLN and SLTO if KEYOPT(10) = 1 or 2.

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 addi-
tional 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
FKT. 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 method 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(12) = 5 or 6) and no separation contact (KEYOPT(12) = 4) to model several types of contact
assemblies and kinematic constraints. See Chapter 9, Multipoint Constraints and Assemblies (p. 99) for more
information on how to use this feature.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
30                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                              3.8.4. Determining Contact Stiffness and Allowable Penetration


     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.


     Note

     If overconstraint occurs in bonded shell-shell assemblies when using the MPC algorithm, you can
     switch to the penalty method or the augmented Lagrangian method. See Bonded Contact for
     Shell-Shell Assemblies (p. 52) for more information.


     Note

     For 3-D higher order contact elements (CONTA174), the Lagrange multiplier method is applied
     at each contact node (including mid-side nodes), but the penalty method is applied on the center
     of the contact elements, even when KEYOPT(2)=3,4 is set.


3.8.4. Determining Contact Stiffness and Allowable Penetration
3.8.4.1. 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 conver-
gence 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) = 2 to allow the program to update the contact stiffness automatically.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               31
Chapter 3: Surface-to-Surface Contact

3.8.4.2. 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).

     Note

     The default contact normal stiffness is affected by defined material properties, element size, and
     the total number of degrees of freedom in the model. Many factors may be applied to the actual
     contact normal stiffness during the solution. The default contact stiffness listed in the Contact
     Manager or by the CNCHECK command may be different from the actual contact stiffness reported
     by the ETABLE command. You should check the value reported by ETABLE to confirm that the
     appropriate contact normal stiffness is used.

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 3.9: Depth of the Underlying Element (p. 28)). This factor is used to determine if penetration com-
patibility 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 guar-
     antee 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.

3.8.4.3. 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 (KT = 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 ac-
curacy. Based on the tolerance, current normal pressure, and friction coefficient, the tangential contact

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
32                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                3.8.4. Determining Contact Stiffness and Allowable Penetration

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).

     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 es-
            tablished).
      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 conver-
            gence 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 in-
            crease FKN.



     Note

     For bonded contact and rough contact, ANSYS uses MU = 1.0 to calculate tangential contact
     stiffness.


     Note

     Generally, the contact stiffness, FKN and FKT, has units of FORCE/LENGTH3. However, for contact
     force-based models the contact stiffness has units FORCE/LENGTH. This applies to CONTA175
     with KEYOPT(3) = 0, and to CONTA176 and CONTA177.

3.8.4.4. Using KEYOPT(10)
The normal and tangential contact stiffness can be updated during the course of an analysis, either automat-
ically (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)
= 2 to allow the program to update contact stiffnesses automatically. The possible settings for KEYOPT(10)
are outlined below.



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               33
Chapter 3: Surface-to-Surface Contact

 •   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.
 •   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.

3.8.4.5. Using KEYOPT(6)
The default method of updating normal contact stiffness is suitable for most applications. However, the
variational range of the contact stiffness may not be wide enough to handle certain contact situations. In
the case of a very small penetration tolerance (FTOLN), a larger normal contact stiffness is often needed.
Furthermore, to stabilize the initial contact condition and to prevent rigid body motion, a smaller normal
contact stiffness is required.

The allowed contact stiffness variation is intended to enhance stiffness updating when KEYOPT(10) > 0 by
calculating an optimal allowable range in stiffness for use in the updating shceme. To increase the stiffness
variational range, set KEYOPT(6) = 1 to make a nominal refinement to the allowable stiffness range, or KEY-
OPT(6) = 2 to make an aggressive refinement to the allowable stiffness range.

3.8.4.6. 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.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
34                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                 3.8.5. Choosing a Friction Model


     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. However, the sign of the contact pressure is switched during postprocessing.


     Note

     For contact force-based models, TNOP is the maximum allowable tensile contact force. This applies
     to CONTA175 with KEYOPT(3) = 0, and to CONTA176 and CONTA177.

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 iter-
     ation.

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.

3.8.5. Choosing a Friction Model
3.8.5.1. 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.

As an alternative to the program-supplied friction model, you can define your own friction model with the
USERFRIC subroutine (see User-defined Friction (p. 39)).

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 compu-
tationally expensive than a symmetric solver for each iteration. For this reason, ANSYS uses a symmetrization

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                         35
Chapter 3: Surface-to-Surface Contact

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.

3.8.5.2. Coefficient of Friction
The interface coefficient of friction, MU, is used for the Coulomb friction model. You can input MU as a ma-
terial property for the contact elements. 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 res-
istance regardless of the specified value of MU. MU can have dependence on temperature, time, normal
pressure, sliding distance, or sliding relative velocity. Suitable combinations of up to two fields can be used
to define dependency; for example, temperature only, temperature and sliding distance, or sliding relative
velocity and normal pressure. 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 two models for Coulomb friction: isotropic friction (2-D and 3-D contact) and orthotropic
friction (3-D contact). The isotropic friction model is based on a single coefficient of friction, MU. You can
use either TB command input (recommended method) or the MP command to specify MU. The orthotropic
friction model is based on two coefficients of friction, MU1 and MU2. Use TB command input to specify MU1
and MU2 in two principal directions (see the element descriptions for CONTA173, CONTA174, CONTA175,
CONTA176, and CONTA177 for a description of the principal directions for each individual element). See
Contact Friction (TB,FRIC) in the Element Reference for details on how to specify the coefficients of friction.

3.8.5.3. Using TAUMAX, FACT, DC, and COHE
ANSYS provides one extension of classical Coulomb friction: real constant 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. Empirical data is often the best source for TAUMAX. Its value may be close to
 σy
  3
      , where σy is the yield stress of the material being deformed.

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 3.10: Sliding Contact Resist-
ance (p. 36)).

Figure 3.10: 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.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
36                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                  3.8.5. Choosing a Friction Model

3.8.5.4. 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:

     µ = coefficient of friction.
     MU = dynamic coefficient of friction.
     FACT = ratio of static to dynamic coefficients of friction. It defaults to the minimum value of 1.0
     DC = decay coefficient, which has units of time/length. Therefore, time has some meaning in a static
     analysis. DC defaults to zero. When DC is zero, the equation is rewritten to be µ = MU for the case of
     sliding and µ = FACT*MU for the case of sticking.
     Vrel = slip rate calculated by ANSYS.

For the isotropic friction model, MU is input using the MP command or the TB command as explained above.
For orthotropic friction, MU is the equivalent coefficient of friction computed from MU1 and MU2 which are
specified with TB command input:

           2
         (µ1 + µ2 )
                2
µ=
             2

Figure 3.11: Friction Decay (p. 38) shows the exponential decay curve where the static coefficient of friction
is given by:

µs   =   FACT × MU




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                         37
Chapter 3: Surface-to-Surface Contact

Figure 3.11: Friction Decay


      µ


  µ
      s




  MU

                                                                                                                              V rel
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:

           1             µ1 − MU      
DC = −          × ℓn                  
          Vrel1       (FACT − 1) × MU 

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.

3.8.5.5. Forced Frictional Sliding Using Velocity Input
In a static analysis, you can model steady-state frictional sliding between two flexible bodies or between a
flexible and a rigid body with different velocities. In this case the sliding velocities no longer follow the
nodal displacements, and they are predefined through the CMROTATE command. This command sets the
velocities on the nodes of the element component as an initial condition at the start of a load step. ANSYS
determines the sliding direction based on the direction of the sliding velocities. The amplitude of the velo-
cities does not affect the solution.

This feature is primarily useful for generating sliding contact at frictional contact interfaces in a brake squeal
analysis. In this case, the contact pair elements (either the contact elements or the target elements) on the
brake rotor need to be included in the rotating element component (CM command) that is specified on the
CMROTATE command. We recommend that you include only the contact elements or only the target elements
in the element component.

Velocities defined by CMROTATE will be ignored for the following contact definitions:

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
38                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                          3.8.6. Selecting Location of Contact Detection

   Frictionless contact
   Rough contact (KEYOPT(12) = 1)
   Bonded contact (KEYOPT(12) = 2, 5, 6)
   MPC contact (KEYOPT(12) = 2)

     Note

     You should always verify the sliding direction when the velocities defined by CMROTATE are
     applied on nodes that are shared by more than one frictional contact pair. In this situation, you
     can redefine any contact elements that have a potentially incorrect sliding direction as frictionless
     contact.

3.8.5.6. User-defined Friction
You can write a USERFRIC subroutine to program your own friction model for 2-D and 3-D contact elements
(CONTA171, CONTA172, CONTA173, CONTA174, CONTA175, CONTA176, CONTA177, and CONTA178). See
User-defined Friction in the Element Reference for more information on how to use this feature. See also the
Guide to ANSYS User Programmable Features for a detailed description of the USERFRIC subroutine.

3.8.6. Selecting Location of Contact Detection
3.8.6.1. 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 3.12: Contact Detection Located at Gauss Point (p. 39).

Figure 3.12: 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, the line-to-line contact element, CONTA176, and
the line-to-surface contact element, CONTA177, always use the nodal detection scheme.

3.8.6.2. 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

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                 39
Chapter 3: Surface-to-Surface Contact

only to deal with corner, point-surface, or edge-surface contact (see Figure 3.13: Contact Detection Point Loc-
ation at Nodal Point (p. 40)). 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.

Figure 3.13: 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 3.14: Node Slippage
Using Nodal Integration KEYOPT(4) = 1 or 2 (p. 40). 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 Chapter 4, Node-to-Surface Contact (p. 69)
later in this guide.

Figure 3.14: 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.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
40                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                  3.8.7. Adjusting Initial Contact Conditions

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 node-to-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 KEYOPT(4) (p. 71). For the 3-D line-to-line contact element CONTA176 and
     the 3-D line-to-surface contact element CONTA177, KEYOPT(4) is not used to select the location
     of contact detection, and the contact normal is always perpendicular to both the contact and
     target surfaces. For CONTA176 and CONTA177, KEYOPT(4) is used to specify a surface-based
     constraint type.


3.8.7. Adjusting Initial Contact Conditions
3.8.7.1. 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.

3.8.7.2. 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


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                     41
Chapter 3: Surface-to-Surface Contact

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.

           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.


           Note

           For the CONTA177 line-to-surface element, CNOF can be used to model thickness of the
           underlying beam elements. Input half of the beam thickness for CNOF to properly model
           the thickness effects. See Accounting for Thickness Effect (CNOF and KEYOPT(11)) (p. 81) for
           more information.

      ANSYS can automatically provide the CNOF value to either just close the gap or reduce initial penetra-
      tion. 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 KEY-
      OPT(12) = 6 for bonded-initial contact; see Selecting Surface Interaction Models (p. 50) for more inform-
      ation). 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 3.15: Contact Surface Adjustment With ICONT (p. 43)(a)). Only a very small correction is sug-
      gested; 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.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
42                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                 3.8.7. Adjusting Initial Contact Conditions

     Figure 3.15: Contact Surface Adjustment With ICONT


                       (a) before adjustment




                                                                                                                                   Contact
                                                                                                                                   Surface
                       Target Surface




                                                                                                                              ICONT
                                                                                                                              Contact
                (b) after adjustment                                                                                          Surface




                                                                                                                                   Contact
     Potential
                                                                                                                                   Surface
     discontinuity
                     Target Surface




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 3.16: Contact Surface Adjustment (PMIN, PMAX) (p. 44)). 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 dir-
     ections.

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                         43
Chapter 3: Surface-to-Surface Contact

      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 3.17: A Scenario in Which Initial Adjustment Will Fail (p. 44) 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 3.16: Contact Surface Adjustment (PMIN, PMAX)




      Figure 3.17: A Scenario in Which Initial Adjustment Will Fail




 4.   Set KEYOPT(9) to adjust initial penetration or gap; see Figure 3.18: Ignoring Initial Penetration, KEYOPT(9)
      = 1 (p. 46).

      True initial penetration includes two parts:
      •   Penetration or gap due to geometry

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
44                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                  3.8.7. Adjusting Initial Contact Conditions

      • Penetration or gap due to user-defined contact surface offset (CNOF).
      See Figure 3.19: Components of True Penetration (p. 46).

      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 3.20: Ramp-
      ing Initial Interference (p. 47). The following KEYOPT(9) settings provide ramped capabilities:
      •   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.

      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 interfer-
      ence.

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).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                     45
Chapter 3: Surface-to-Surface Contact

Figure 3.18: Ignoring Initial Penetration, KEYOPT(9) = 1




Figure 3.19: Components of True Penetration




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
46                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                         3.8.8. Physically Moving Contact Nodes Towards the Target Surface

Figure 3.20: 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.

3.8.8. Physically Moving Contact Nodes Towards the Target Surface
You can adjust the initial contact status in order to close the gap by doing one of the following:

   (a) Define an initial contact adjustment via real constant ICONT. (ICONT may change the shape of the
   contact detection surface.)
   (b) Define a contact offset via real constant CNOF. (CNOF does not change the shape of the contact de-
   tection surface.)
   (c) Ignore the penetration by setting KEYOPT(9) = 1. (KEYOPT(9) = 1 does change the shape of the contact
   detection surface.)

However, these adjustment methods do not truly change the physical locations of contact nodes; rather,
the contact detection locations are adjusted.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               47
Chapter 3: Surface-to-Surface Contact

The initial adjustment due to (a) is applied only once in the beginning of the contact analysis, where each
contact detection point within the ICONT range is made to be in initial contact with the target surface. The
contact adjustments due to (b) and (c) offset the entire contact detection surface to close any gap that is
present. In doing so, methods (b) and (c) introduce a "rigid region" between the contact and target surfaces
during the entire analysis, which 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:

 •   Only when using the nodal detection option (KEYOPT(4) = 1 or 2), or when using CONTA175 or CONTA177,
     or when using CONTA176 with KEYOPT(3) = 0 (parallel beams).
 •   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 3.21: Effect of Moving Contact Nodes (p. 48). You can change other contact related
settings in PREP7 (for example, set KEYOPT(4) = 0 to use the Gauss detection option) and save the Job-
name.DB file. Issuing the SAVE command before issuing the CNCHECK,ADJUST command is recommended
in order to resume the Jobname.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 3.21: Effect of Moving Contact Nodes




3.8.9. Determining Contact Status and the Pinball Region
3.8.9.1. 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 (open and not near 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.

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
48                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                      3.8.10. Avoiding Spurious Contact in Self Contact Problems

This distance 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.

3.8.9.2. 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 flexible-to-flexible contact) of the underlying element. (See the discussion of element depth
in Positive and Negative Real Constant Values (p. 27).) 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 Selecting
Surface Interaction Models (p. 50) 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
(open and not near 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.

     Note

     The program will warn you when there is an abrupt change in status (for example, from far-field
     to closed) during a contact analysis. This may indicate that the substep increment is too large,
     or possibly (but not likely) that the pinball value (PINB) is too small.

See Positive and Negative Real Constants for more information on this real constant.

3.8.10. 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.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               49
Chapter 3: Surface-to-Surface Contact

Figure 3.22: Auto Spurious Prevention

                                                  Location where
                                                  spurious contact
                Contact normal                    most likely occurs




     Target normal




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.

3.8.11. Selecting Surface Interaction Models
3.8.11.1. Background
The surface-to-surface contact elements support normal unilateral contact models as well as other mechan-
ical surface interaction models.

3.8.11.2. Using KEYOPT(12)
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.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
50                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                              3.8.11. Selecting Surface Interaction Models

 •   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 all types of bonded contact (KEYOPT(12) = 2, 3, 4, 5, and 6), separation of contact can be modeled using
the debonding feature. For more information, see Chapter 12, Debonding (p. 131).

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 Using PINB (p. 49) 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 the real constants mentioned above.

     Note

     For bonded contact definitions (KYEOPT(12) = 5 or 6), if the contact is not in a “just touching”
     position, you may find that no zero modes appear for free vibration. To avoid this issue, use the
     MPC approach instead of other contact algorithms.

3.8.11.3. Using FKOP
The FKOP real constant can be used in two different ways, depending on the surface interaction model used.
For no separation or bonded contact (KEYOPT(12) = 2 through 6), FKOP is the stiffness factor applied when
contact opens. For standard or rough contact (KEYOPT(12) = 0 or 1), FKOP represents a contact damping
coefficient.

When modeling either no-separation or bonded contact, you may need to set a value for FKOP to apply a
stiffness factor 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 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 standard contact (KEYOPT(12) = 0) or rough contact (KEYOPT(12) = 1), you can use FKOP to define a
contact damping coefficient. This option is primarily used to damp relative motions between the contact

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                  51
Chapter 3: Surface-to-Surface Contact

and target surfaces for open contact. It provides certain resistance to reduce the risk of rigid body motion.
The damping force is calculated by

Fd = ∫ FKOP ⋅ Vrel dA c

where Vrel is the slip rate and Ac is the area domain of the contact surface. The units of the damping coefficient
are FORCE/(AREA*VELOCITY). For the contact force-based model, the units are FORCE/VELOCITY. To specify
the contact damping coefficient, enter a negative number for FKOP. Positive input will be ignored.

3.8.11.4. Bonded Contact for Shell-Shell Assemblies
The bonded contact options (KEYOPT(12) = 5 or 6) can be used with the MPC approach (KEYOPT(2) = 2) to
model various types of assemblies (see Chapter 9, Multipoint Constraints and Assemblies (p. 99)). When this
method is used to model shell-shell assemblies, there may be cases where the MPC approach causes the
model to be overconstrained. To alleviate this problem, you can use a penalty-based method for shell-shell
assemblies. Using the penalty-based method constrains rotational DOFs in addition to translational DOFs.
This capability is available for contact elements CONTA173, CONTA174, and CONTA175 in conjunction with
TARGE170.

To use this method, first set KEYOPT(2) = 0 or 1 (augmented Lagrangian or penalty function) and KEYOPT(12)
= 5 or 6 (bonded always or bonded initial contact) in the contact elements. Setting KEYOPT(5) = 2 (shell-
shell constraint) for the target elements will cause this penalty-based method to be used.

The penalty stiffness used for rotational DOFs is equal to (contact stiffness used for translational DOFs) *
(contact length). The contact stiffness for translational DOFs is input by real constant FKN, or defaults to an
internal value. The contact length is always calculated internally and it is printed in the output file. The figure
below shows the difference in using a conventional penalty-based shell-shell assembly and this method.

Figure 3.23: Penalty-Based Shell-Shell Assembly




     Note

     In the case of a penalty-based shell-shell assembly, spurious rotational energy exists if there are
     gaps or penetrations between the contact and target surfaces. This can affect the accuracy of the
     solution. In this case it is recommended that you use a shell-solid constraint type by setting
     KEYOPT(5) = 3, 4, or 5 on the target element, which requires use of the MPC algorithm (KEYOPT(2)
     = 2 on the contact element).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
52                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                          3.8.12. Modeling Contact with Superelements

3.8.12. Modeling Contact with Superelements
3.8.12.1. Background
The surface-to-surface contact elements can model a rigid body (or one linear elastic body) contacting an-
other 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 ele-
ments before they were assembled into superelements.

3.8.12.2. 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.

     Note

     KEYOPT(3) has different meanings in the node-to surface contact element, CONTA175, and in the
     line-to-line contact element, CONTA176. KEYOPT(3) is not used for the line-to-surface contact
     element, CONTA177.

     For 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 KEYOPT(3) (p. 70).

     For CONTA176, KEYOPT(3) specifies the type of beam-to-beam contact. See Performing a 3-D
     Beam-to-Beam Contact Analysis (p. 75).




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               53
Chapter 3: Surface-to-Surface Contact

3.8.13. Accounting for Thickness Effect
3.8.13.1. Background
You can account for the thickness of shells (2-D and 3-D) and beams (2-D) using KEYOPT(11). (This does not
apply to 3-D beam-to-beam contact.) 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 automat-
ically 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.

3.8.13.2. 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 Steps in a Contact Analysis (p. 11).

     Note

     Only use KEYOPT(11) = 1 to account for thickness when you have shell or beam elements with
     nodes located at the middle surface.

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, SHELL208, SHELL209, SHELL281, or ELBOW290, changes in thickness
during deformation are also taken into account.

Note that KEYOPT(11) is not used with the line-to-line contact element (CONTA176). For the line-to-surface
contact element (CONTA177) KEYOPT(11) is only used for shell elements on the target side.

     Note

     For shell and beam contact, the penetration and gap distances are always measured from the
     midsurface of the shell or beam element. Any defined offset of the shell or beam element is ignored
     by the contact elements.


3.8.14. Using Time Step Control and Impact Constraints
3.8.14.1. 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.

Impact constraints are used in a transient dynamic analysis to satisfy the momentum and energy balance
at the contact and target interface. See Chapter 10, Dynamic Contact and Impact Modeling (p. 117) for more
information.

3.8.14.2. Using KEYOPT(7)
Use KEYOPT(7) = 0, 1, 2, or 3 to control time stepping, where KEYOPT(7) = 0 provides no control (the default),
and KEYOPT(7) = 3 provides the most control.

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
54                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                              3.9. Controlling the Motion of the Rigid Target Surface

 •   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.

Use KEYOPT(7) = 4 to activate impact constraints.

 •   KEYOPT(7) = 4: Use impact constraints for standard or rough contact (KEYOPT(12) = 0 or 1) in a transient
     dynamic analysis with automatic adjustment of the time increment.

3.8.15. 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
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.

3.9. Controlling the Motion of the Rigid Target Surface
Rigid target surfaces are defined in their original configuration, and the motion of the entire surface is then
defined by the motion 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.
 •   When modelling surface-based constraints or a rigid body.

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. You can also define a follower element (FOLLW201) on the pilot node; the element-specified
external forces and moments will follow the motion of the pilot node.

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.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               55
Chapter 3: Surface-to-Surface 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.

Keep in mind the following restrictions on the target surface when using a pilot node:

 •   Each target surface can have only one pilot node.
 •   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 a node on the contact element. The location of the pilot node becomes im-
     portant 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. Generally,
     you should not apply external constraint equations (CE) or node coupling (CP) to the pilot node.
 •   ANSYS ignores all boundary conditions on all nodes other than the pilot node when KEYOPT(2) = 0
     (default) for the target elements.
 •   When KEYOPT(2) = 0 (default), only the pilot node can connect to other elements.
 •   By setting KEYOPT(2) = 1 for the target elements, you can apply boundary conditions on any rigid target
     nodes rather than only on the pilot node. In this case, it is your responsibility to make sure the rigid
     target surface is not under-constrained or over-constrained. It is still recommended that you apply all
     boundary conditions on the pilot node, even when KEYOPT(2) = 1.

     Note

     For flexible-to-flexible contact, no special boundary conditions treatment is performed, and KEY-
     OPT(2) = 0 should be used.


3.10. Applying Necessary Boundary Conditions to the Deformable Ele-
ments
You can now apply any necessary boundary conditions as you would for any ANSYS analysis. For more in-
formation on applying boundary conditions, see the appropriate analysis descriptions in the Structural Ana-
lysis Guide.

3.11. Applying Fluid Pressure-Penetration Loads
Pressure-penetration loads can simulate surrounding fluid or air penetrating into the contact interface, based
on the contact status. You can apply pressure-penetration loads to flexible-to-flexible or rigid-to-flexible
contact pairs. 2-D and 3-D surface-to-surface contact elements (CONTA171, CONTA172, CONTA173, CONTA174)
support pressure-penetration loading.

Fluid pressure can penetrate into the contact interface from one or multiple locations. The fluid pressure-
penetration load has a path dependent nature. The penetrating path can propagate and vary, and it will be
determined iteratively. At the beginning of each iteration, ANSYS first detects starting points which are ex-
posed to the fluid pressure. Among the starting points, ANSYS then finds fluid penetrating points where the
contact status is open or lost, or where the contact pressure is smaller than the user defined pressure-pen-


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
56                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                 3.11.1. Applying Fluid Penetration Pressure

etration criterion. When a contact detection point has a contact condition of “penetrating,” it is subjected
to the fluid pressure, and its nearest neighboring nodes are considered to be the starting points which are
exposed to the fluid pressure as well.

The fluid pressure will not be applied to an area having a contact status of open unless the edges/ends of
the area belong to the starting points.

Figure 3.24: Path Dependent Fluid Penetration Loading

                      Fluid pressure is applied




                          Starting Point




The fluid pressure starts to penetrate into the interface between contact and target surfaces from the pen-
etrating points. The fluid penetration can be cut off when contact between the surfaces is reestablished or
when contact pressure is larger than the fluid penetration criterion.

To model fluid penetration loads, you need to specify the following quantities:

 •   fluid pressure
 •   fluid penetration starting points
 •   fluid penetration criterion
 •   fluid penetration acting time

An example analysis showing how to apply fluid penetrating loading is presented in Appendix A (p. 135).

3.11.1. Applying Fluid Penetration Pressure
The fluid pressure must be applied to contact and target elements using the SFE command:
 SFE,ELEM,1,PRES,,VAL1,VAL2,VAL3,VAL4

The pressure is applied only on the corner nodes of the contact and target elements. The pressure on the
midside nodes of CONTA172, CONTA174, TARGE169, and TARGE170 will be averaged using the pressures of
two adjacent corner nodes. VAL3 and VAL4 are not used for 2-D contact and target elements.

Pressure value VALi, which is applied to the ith node (where i = 1, 2, 3, 4 indicates node I, J, K, L, respectively)
of the contact or target element, can be a constant numerical value or a table name. If it is constant, the
magnitude of pressure will be step-applied or ramped based on the KBC command setting. To specify a
table, enclose the table name in percent signs (for example, %tabname%). Use the *DIM command to define
the table. Only one table can be specified, and it must be specified in the VAL1 position; tables specified
in the VAL2, VAL3, and VAL4 positions will be ignored.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                  57
Chapter 3: Surface-to-Surface Contact

The fluid pressure-penetration load will be automatically applied to the penetrating points on contact and
target surfaces based on the contact status.

By default (KEYOPT(14) = 0 on the contact element), the fluid pressure-penetration load varies during iterations
based on the current contact status. In certain cases, the default can cause an unstable convergence pattern
since the contact status and the resulting applied fluid penetration load keep changing during iterations.

When KEYOPT(14) = 1, the fluid pressure-penetration load will be applied to the contact and target elements
at the beginning of each substep and will remain constant over that substep even if the contact status keeps
changing during iterations. Small increments are often needed to obtain accurate results.

Keep the following points in mind when defining fluid penetration loads:

 •   For flexible-to-flexible contact with a symmetric contact pair definition (including a self-contact pair),
     you should apply the fluid pressure only to the contact elements.
 •   For flexible-to-flexible contact with an asymmetric contact pair definition, you should generally apply
     fluid pressure on both contact and target elements which are currently or will potentially be exposed
     to the surrounding fluid. ANSYS will ignore fluid penetration loads applied to a target surface if there
     are no fluid penetration loads applied to the associated contact surface within the contact pair. When
     the fluid pressures are applied to both contact and target elements, ANSYS will have to identify the
     penetration paths for both the contact surface and the target surface. The iterative process of determ-
     ining the penetration path on the target surface is very time-consuming, particularly for 3-D contact
     models. Therefore, we strongly recommend that you use a symmetric contact pair definition since it
     does not require the specification of fluid penetration pressure on the target surface.
 •   For rigid-to-flexible contact, you should apply the fluid pressure only to the contact elements. ANSYS
     will automatically apply equivalent forces to the rigid target surface to balance out the applied pressure
     on the contact surface. Fluid pressure applied to the rigid target surface will be ignored.
 •   For situations in which multiple contact pairs are defined on the same surface, contact elements may
     overlap each other. In this case, be careful to apply the fluid penetration pressure only once in areas
     where contact elements overlap.
 •   The fluid penetration pressure can only be applied to the contact and target elements using the SFE
     command. Other pressure load commands (SF, SFL, SFA) can not be used. In addition, you should not
     apply the pressure on the underlying elements.
 •   ANSYS ignores any fluid penetration pressures applied to MPC based contact pairs.
 •   The effects of pressure load stiffness are automatically included. If an unsymmetric matrix is needed to
     achieve convergence for pressure load stiffness effects, issue the NROPT,UNSYM command.

3.11.2. Specifying Fluid Penetration Starting Points
When a fluid pressure-penetration load is applied, the fluid pressure penetrates to the surface from defined
starting points. There can be one or multiple starting points. ANSYS will automatically find the default
starting points by selecting free end points of 2-D contact/target surfaces or nodes of free open edges on
3-D contact/target surfaces ("free" meaning that the element is not fully surrounded by adjacent elements;
see figure below).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
58                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                    3.11.3. Specifying a Pressure-Penetration Criterion

Figure 3.25: Free End Points (2-D) and Free Open Edges (3-D)

          Free End Points
                                                                       Contact Surface



         Contact Surface



                                                                                                                  Free Open Edge
                                                                                                                     
            Target Surface




                                                                       Target Surface
          Free End Points

  2D contact: Free End Point                               3D contact: Free Open Edge



The starting points are initially exposed to the fluid and are potentially subjected to the penetration pressure.
There are no default starting points if the contact or target surface is continuous with a closed loop. The
default starting points can be overwritten using the SFE command. You can specify starting points, specify
penetrating points, and remove the default starting points with the SFE command and STAi values, as
described below. Be sure to set LKEY = 2 on the SFE command in order to specify the STAi settings. The
command format is:
 SFE,ELEM,2,PRES,,STA1,STA2,STA3,STA4


STAi =       ANSYS determines whether the ith node is a starting point based on the contact status.The ith
0 (de-       node can be a default starting point if the node is a 2-D free point or is on a 3-D free edge.
fault)
STAi =       The ith node is the starting point which is initially exposed to the fluid. It can be a penetrating
1            point if the initial contact status is "open." The node may no-longer be the starting point when
             the contact status changes during the deformation process.
STAi =       The ith node is a penetrating point.The node is always subjected to the fluid pressure in spite of
2            any contact status change.
STAi =       The ith node will not be a default starting point even though it belongs to a 2-D free point or a
-1           3-D free edge node.


     Note

     If only STA1 is specified and the other STAi values are blank, STA2, STA3, and STA4 will default
     to STA1.


3.11.3. Specifying a Pressure-Penetration Criterion
You can specify a pressure-penetration criterion using the contact element real constant PPCN. When the
contact pressure is less than the criterion, the starting point turns into the penetrating point; that is, fluid
pressure starts to penetrate. Thus, a higher criterion value will allow the fluid to penetrate more easily. When

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               59
Chapter 3: Surface-to-Surface Contact

the contact pressure is greater than the criterion, the penetrating point returns back to the starting point;
that is, fluid penetration is cut off. By default, the penetration criterion (PPCN) is zero. In this case the fluid
penetration occurs only when the contact is open, and the cutoff of fluid penetration occurs only when the
contact is reestablished.

You can input PPCN as a constant value or as a table of values. The tabular input can be a function of contact
point current location (global X , Y, Z), contact pressure, time, or temperature. To input a table name, you
must enclose the name in % symbols (for example, %tabnam%). Use the *DIM command to define the table.

3.11.4. Specifying a Fluid Penetration Acting Time
When the fluid pressure penetration occurs, the fluid pressure is applied normal to the contact/target surfaces.
As with conventional pressure loading, the current amount of fluid pressure at a given substep will depend
on whether the pressure is input as a constant value or a table of values, and whether the pressure is ramp-
or step-applied (KBC command). If the total amount of fluid pressure is applied instantaneously, convergence
difficulties may arise due to large changes in stresses near the contact interface. This is also true when the
fluid penetration pressure is removed instantaneously, as when the fluid penetration is cut off. To help sta-
bilize the solution, ANSYS offers an option to ramp the fluid pressure linearly over a time period, during one
or several substeps.

To implement this ramping option, specify the fluid penetration acting time using the contact element real
constant FPAT. Input a positive number to define the fraction of the time increment of the load step; input
a negative number to define the absolute acting time. The default penetration acting time is 0.01 times the
time increment of the current load step.

At each penetrating point, if the time increment of the current substep is less than the fluid penetration
acting time (FPAT > (tn - tn-1)), the fluid pressure is ramped up linearly from the actual applied pressure of
the previous substep to the full current amount of the fluid pressure over the penetration acting time period;
otherwise (FPAT ≤ (tn - tn-1)), the full amount of current fluid pressure will be applied. (See figures below.)
At the pressure-penetration cutoff points, if the time increment of the current substep is less than the fluid
penetration acting time, the fluid pressure is ramped down linearly from the applied pressure of the previous
substep to a zero magnitude over the penetration acting time period; otherwise, the fluid pressure will be
immediately removed.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
60                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                   3.11.4. Specifying a Fluid Penetration Acting Time

Figure 3.26: Fluid Penetration Acting Time (FPAT) Greater Than Substep

Pressure


                                         (tn-1)                                         FPAT




                                                                                                                                 Current Applied Pressure
                                                                                                                                 (input via SFE,,,PRES)

                                                                                                                                 Actual Applied Pressure
                                                                                                                                 (reported as output item FPR



                                                                                                                                 Time

                                           tn-1                               tn

    Acual applied pressure is ramped to the full current applied pressure
    when FPAT>(tn-tn-1)




                   Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                               of ANSYS, Inc. and its subsidiaries and affiliates.                                                61
Chapter 3: Surface-to-Surface Contact

Figure 3.27: Fluid Penetration Acting Time (FPAT) Less Than Substep

Pressure




                                                             FPAT



                                                                                                                                   Current Applied Pressure
                                                                                                                                   (input via SFE,,,PRES)

                                                                                                                                   Actual Applied Pressure
                                                                                                                                   (reported as output item FPRS)




                                                                                                                                         Time
                                                  tn-1                                 tn

      Acual applied pressure is ramped to the full current applied pressure
      when FPAT<(tn-tn-1)



3.11.5. Redefining or Modifying the Pressure-Penetration Loads
You can redefine or modify fluid pressure-penetration loads and fluid penetration starting points between
load steps using the SFE command.

You can also modify the pressure-penetration criterion (real constant PPCN) and acting time (real constant
FPAT) using the RMODIF command.

To remove a fluid pressure-penetration load, use one of the following methods:

 •   Delete the pressure load using the SFEDELE command.
 •   Apply zero pressure using the SFE command.
 •   Deactivate the contact elements using the EKILL command.

Because these methods remove the fluid penetration pressure immediately, convergence difficulties may
occur. To avoid this problem you can add an extra load step which applies a small fluid pressure (for example,
VALi = 1e-8) via the SFE command instead of removing the pressure.

3.11.6. Postprocessing Fluid Pressure-Penetration Loads
You can list and display the actual fluid penetration pressure applied on contact and target elements using
FPRS as a contact result item on the PLNSOL, PLESOL, PRNSOL, and PRESOL commands. For example:
 PLESOL,CONT,FPRS
 PLNSOL,CONT,FPRS


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
62                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                         3.12. Defining Solution and Load Step Options

You can also list and display the fluid penetration pressure applied on target elements by using the ETABLE
command.

3.12. 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 Com-
mand 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

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)


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               63
Chapter 3: Surface-to-Surface Contact

     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 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.


      Note

      By default, displacement (U) and rotation (ROT) convergence checking are not active. Issue the
      CNVTOL,U or CNVTOL,ROT command to add displacement or rotation convergence checking, if
      necessary.


3.13. 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 unex-
     pected gap (or no contact) or overestimated penetration, abort the analysis and then check your geo-
     metric 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.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
64                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                               3.14.2. Reviewing Results in POST1

      NLDIAG,CONT can also be used to monitor contact information. When turned on, this feature will track
      the same contact information available through NLHIST for all defined contact pairs according to the
      specified writing frequency (each iteration, substep, or load step). The resulting output is stored in a
      text file called Jobname.cnd.
 •    Always check your results carefully using standard engineering guidelines.

See Solve the Analysis in the Structural Analysis Guide.

If you are restarting a contact analysis, follow the normal restart procedures as discussed in Restarting an
Analysis in the 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.

      Note

      Singleframe restart does not support surface-to-surface, node-to-surface, line-to-line, or line-to-
      surface contact. Use multiframe restart if your model contains any of the following contact ele-
      ments: CONTA171, CONTA172, CONTA173, CONTA174, CONTA175, CONTA176, CONTA177.


3.14. 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 Element 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.

3.14.1. Points to Remember
See Points to Remember in the Structural Analysis Guide.

3.14.2. Reviewing Results in POST1
The steps for reviewing results in POST1 are the same as those for a typical nonlinear analysis (see Reviewing
Results in POST1 in the Structural Analysis Guide) with the following exceptions:

For step 4, the following shows the various CONT options for the PLNSOL and PLESOL commands. 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
below.

     CONT     STAT[1]               Contact status[2]:

                                          3-closed and sticking
                                          2-closed and sliding

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                       65
Chapter 3: Surface-to-Surface Contact

                                              1-open but near contact (near-field)
                                              0-open and not near contact (far-field)
      “          PENE                   Contact penetration
      “          PRES[3]                Contact pressure
      “          SFRIC[3]               Contact friction stress
      “          STOT[3]                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
      “          FPRS                   Fluid penetration pressure (surface-to-surface contact only)

 1.       Status notation is for all contact elements except CONTAC12 and CONTAC52. If you are using these
          elements, check the output listing in the corresponding element documentation.
 2.       For MPC-based contact definitions, the value of STAT can be negative. This indicates that one or more
          contact constraints were intentionally removed to prevent over-constraint. STAT = -3 is used for MPC
          bonded contact; STAT = -2 is used for MPC no-separation contact. Negative values are valid for CON-
          TA171, CONTA172, CONTA173, CONTA174, CONTA175, CONTA176, and CONTA177.
 3.       For the contact force-based model, used for CONTA175 with KEYOPT(3) = 0, CONTA176, and CONTA177,
          PRES, SFRIC, and STOT are the contact normal force, contact friction force, and total contact force, re-
          spectively.

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.

       Note

       The contact results are only reported at the corner nodes of contact elements. Therefore, for
       higher order contact elements, mid-side node contact can occur without pressure being reported.
       In this case, the element’s contact status and contact pressure reported via ETABLE may give
       more precise information.

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

                            Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
66                                                      of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                          3.14.3. Reviewing Results in POST26

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.

3.14.3. Reviewing Results in POST26
The steps for reviewing results in POST26 are the same as those for a typical nonlinear analysis See Reviewing
Results in POST26 in the Structural Analysis Guide.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                      67
     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
68                               of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 4: Node-to-Surface Contact
You can use the 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.

The following node-to-surface contact topics are available:
 4.1.The Node-to-Surface Contact Element
 4.2. Performing a Node-to-Surface Contact Analysis
 4.3. Using CONTA175 for Multiphysics Contact

4.1. The Node-to-Surface Contact Element
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 4.1: Node-to-Surface Contact Elements (p. 69).

Figure 4.1: Node-to-Surface Contact Elements

                                                                                                                           I
Y (or Axial)                                                                                                                    CONTA175
                                                                                             Y
                            I CONTA175

                               target normal                                                                      target normal



               2-D associated target                                                                     3-D associated target
               surface (TARGE169)                                                                        surface (TARGE170)
                                                      X                                                                                    X
                                                 (or Radial)
                                                                                z

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.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                     69
Chapter 4: Node-to-Surface Contact

 •   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.


4.2. Performing a Node-to-Surface Contact Analysis
CONTA175 follows the contact pair concept used by surface-to-surface elements CONTA171 through CON-
TA174. 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 a 20-node brick (SOLID95), 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       in the ANSYS Standard Toolbar, or via the
menu path Main Menu> Preprocessor> Modeling> Create> Contact Pair. See Chapter 2, GUI Aids for
Contact Analyses (p. 7) 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 PRESOL,CONT or PRETAB commands.

4.2.1. CONTA175 KEYOPTS
CONTA175 uses most of the same KEYOPTS that are used by the surface-to-surface contact elements CON-
TA171 through CONTA174. KEYOPT(3) and KEYOPT(4) are used but have different meanings when used with
CONTA175. See Element KEYOPTS (p. 28) for a listing of the remaining KEYOPTS.

4.2.1.1. 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 de-


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
70                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                           4.3. Using CONTA175 for Multiphysics Contact

termine 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
force-based model, but FORCE/LENGTH3 for the traction-based model. PRES is the contact normal force in
the force-based model, but contact pressure in the traction-based model.

4.2.1.2. 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 diffi-
culties 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 de-
flection (NLGEOM,ON).

4.2.2. 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 Real Constants (p. 25).

4.3. Using CONTA175 for 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 real
constants TCC, ECC, 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.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               71
     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
72                               of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 5: 3-D Beam-to-Beam Contact
Contact between beams undergoing large displacements can be encountered in many practical applications.
Some examples are hydrogen sensors, water supply lines, nuclear power plant piping, cable wires and coils,
woven fabrics, and tennis racquet strings. You can model 2-D beam-to-beam contact by using 2-D surface-
to-surface contact elements, CONTA171 and CONTA172. (See Chapter 3, Surface-to-Surface Contact (p. 11)
for details on how to use these elements.) You can model 3-D beam-to-beam contact by using the 3-D line-
to-line contact element, CONTA176.

The following beam-to-beam contact topics are available:
 5.1.The 3-D Line-to-Line Contact Element
 5.2. Modeling Beam-to-Beam Contact
 5.3. Performing a 3-D Beam-to-Beam Contact Analysis

5.1. The 3-D Line-to-Line Contact Element
3-D line-to-line contact is represented in the ANSYS program by following the positions of lines on the
contact surface, modeled by CONTA176 elements, relative to lines on the target surface, modeled by TARGE170
elements. Line-to-line contact in three dimensions is depicted in the figure below.

Figure 5.1: Line-to-Line Contact Elements

                                                                         CONTA176
           Y
                                                                     J
                    X                         K
     Z
                I


3-D associated target
line segments (TARGE170)

The CONTA176 element type:

 •   Has two nodes or three nodes.
 •   Is paired with a target surface defined by TARGE170 elements.
 •   Uses the same real constant set as used for the surface-to-surface contact elements. See Real Con-
     stants (p. 25) for more information.
 •   Supports 3-D rigid-flexible and flexible-flexible contact.
 •   Supports 3-D beams and pipes with or without midside nodes.
 •   Can be generated by the ESURF command, similar to the surface-to-surface contact elements.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                               73
Chapter 5: 3-D Beam-to-Beam Contact


5.2. Modeling Beam-to-Beam Contact
There are three different scenarios for 3-D beam-to-beam contact:

 •   Internal contact, where one beam slides inside another hollow beam (Figure 5.2: Internal Contact (One
     Beam Sliding Inside Another) (p. 74)).
 •   External contact, where two beams are roughly parallel and contact each other along their outer surfaces
     (Figure 5.3: External Contact (Two Beams Roughly Parallel) (p. 74)).
 •   External contact, where contact between the exterior surfaces of two beams is pointwise (Figure 5.4: Ex-
     ternal Contact (Two Beams Cross Each Other) (p. 75)).

Figure 5.2: Internal Contact (One Beam Sliding Inside Another)



                        TARGE170                                                                                         rt


             n
                                                           rc


                 d




                                                   CONTA176

Figure 5.3: External Contact (Two Beams Roughly Parallel)

     CONTA176
                                n

                                                         rc




                            d




                                                                     rt



                                                          TARGE170




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
74                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                               5.3. Performing a 3-D Beam-to-Beam Contact Analysis

Figure 5.4: External Contact (Two Beams Cross Each Other)

                                                n


      CONTA176


                 rc



                                   d


                                                         rt




                      TARGE170

For all three scenarios shown above, use 3-D line segments (straight line or parabola) to define the target
surface (TARGE170). You can attach the contact elements and target elements to 3-D beams or pipes, which
can be first or second order elements. Both flexible-flexible and rigid-flexible contact between two beams
can be considered.

When modeling internal contact, the inner beam (or pipe) should usually be considered the contact surface
and the outer beam (or pipe) should be the target surface. The inner beam can be considered as the target
surface only when the inner beam is much stiffer than the outer beam. When modeling external contact,
the target surface should be associated with the stiffer beam or with the beam having the coarser mesh.

5.3. Performing a 3-D Beam-to-Beam Contact Analysis
Contact element CONTA176 follows the contact pair concept used by the surface-to-surface elements
(CONTA171 through CONTA174). You must pair CONTA176 with 3-D target line segments (TARGE170) to
model 3-D beam-to-beam contact. See Identifying Contact Pairs (p. 12) for more information. CONTA176
uses most of the same element KEYOPTs and real constants as the surface-to-surface contact elements. Any
differences are described in the next section.

The basic steps for performing a 3-D beam-to-beam contact analysis are the same as those used for a typical
surface-to-surface analysis using CONTA171 through CONTA174. See Steps in a Contact Analysis (p. 11) for
details.

Use the ESURF command to generate CONTA176 elements between corresponding contact pairs. (In the
GUI, pick Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surf to Surf.) This
procedure is similar to that used for the surface-to-surface contact elements. If the underlying elements of
target element TARGE170 are part of shell edges, use ESURF,,,LINE to generate 3-D line or parabola target
segments.

When using the line segments to form the target surface or using line-to-line contact elements to form the
contact surface, the nodes must be entered in a sequence that defines a continuous line, as shown in the
figure below.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               75
Chapter 5: 3-D Beam-to-Beam Contact

Figure 5.5: Continuous Line Segments




The line can be made up of linear or parabolic segments, depending on whether the attached beam is made
up of first order or second order elements. If the nodal ordering of the underlying beam elements is not
consistent, you must either change them by reversing the node number order of the selected elements
(ESURF,,REVERSE command) or make a consistent element ordering (ENORM command).

You can list the CONTA176 results using the PRESOL,CONT or PRETAB commands. Since CONTA176 is a 3-
D line element, you can also use the PLLS command to display element table items.

5.3.1. KEYOPTs and Real Constants
CONTA176 uses most of the same KEYOPTs that are used by the surface-to-surface contact elements, CON-
TA171 through CONTA174. KEYOPT(3) and KEYOPT(4) differ from the other contact elements, and KEYOPT(11)
is not used by CONTA176. See Element KEYOPTS (p. 28) for a listing of the remaining KEYOPTs.

CONTA176 uses the same real constants used by the surface-to-surface contact elements (CONTA171 through
CONTA174), except for the units of FKN and FKT. See a listing of the real constants in Real Constants (p. 25).

5.3.1.1. Real Constants R1, R2
For beam-to-beam contact, an important assumption is that of constant circular beam cross section. The
contact radius is assumed to be the same for all CONTA176 elements in the contact pair. Likewise, the target
radius is assumed to be the same for all TARGE170 elements in the contact pair. You supply the target and
contact radii through real constants R1 and R2, respectively.

For a general beam cross section, you can use an equivalent circular beam in the contact definition (see
figure below). Use these guideline to define the equivalent circular cross section:

 •   Determine the smallest cross section along the beam axis.
 •   Determine the largest circle embedded in that cross section.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
76                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                5.3.1. KEYOPTs and Real Constants

Figure 5.6: Equivalent Circular Cross Section


     
                                                                        Actual beam




                                                             Contact surface


Use the first real constant, R1, to define the radius on the target side (target radius rt). Use the second real
constant, R2, to define the radius on the contact side (contact radius rc).

The contact radius R2 is always a positive number. The target radius R1 can be entered as either a negative
or positive value. Use a negative value when modeling internal contact (a beam or pipe sliding within an-
other beam or pipe), with the input value equal to the inner radius of the outer beam. Use a positive value
when modeling external contact between the exterior surfaces of two cylindrical beams.

For beam-to-beam contact, the thickness effect is accounted for through the contact and target radii.
Therefore, KEYOPT(11) (which is used for the surface-to-surface contact elements to include or exclude
thickness effects) is not used for CONTA176.

5.3.1.2. KEYOPT(3)
For CONTA176, KEYOPT(3) determines the type of beam-to-beam contact as follows:

 •       Use KEYOPT(3) = 0 to model external contact between parallel beams or internal contact between beams
         (a beam inside a hollow beam or a pipe inside a pipe). For this case, the sign of the target radius, R1,
         will determine whether you are modeling parallel beams (R1 > 0) or a beam inside a beam (R1 < 0).
 •       Use KEYOPT(3) = 1 to model beams that cross. The target radius must be a positive value.

5.3.1.3. Real Constants FKN and FKT
CONTA176 uses the contact force-based model. The units of real constants FKN and FKT have a factor of
AREA with respect to those used in the surface-to-surface contact elements. For instance, contact stiffness
FKN has units of FORCE/LENGTH in the force-based model, but FORCE/LENGTH3 in the surface-to-surface
contact elements. PRES is the contact normal force in the force based model, but contact pressure in CON-
TA171 to CONTA174.

5.3.1.4. Real Constant TOLS
For CONTA176, the contact normal is uniquely defined and is perpendicular to both the contact and the
target surfaces (two contacting beams). 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 be completely out of
contact, resulting in convergence difficulties from oscillations.




                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                     of ANSYS, Inc. and its subsidiaries and affiliates.                                      77
Chapter 5: 3-D Beam-to-Beam Contact

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 de-
flection (NLGEOM,ON).

5.3.1.5. KEYOPT(4)
You can use CONTA176 with the multipoint constraint (MPC) approach (KEYOPT(2) = 2) to define surface-
based constraints. The KEYOPT(4) setting will determine the type of surface-based constraint. Set KEYOPT(4)
= 1 for a force-distributed constraint, or set KEYOPT(4) = 0 for a rigid surface constraint. See Surface-based
Constraints for more information.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
78                                                of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 6: Line-to-Surface Contact
You can use the 3-D line-to-surface contact element, CONTA177, to model flexible-flexible or rigid-flexible
contact between a 3-D beam and a surface or between a shell edge and a surface.

The following line-to-surface contact topics are available:
 6.1.The 3-D Line-to-Surface Contact Element
 6.2. Performing a 3-D Line-to-Surface Contact Analysis

6.1. The 3-D Line-to-Surface Contact Element
3-D line-to-surface contact is represented in the ANSYS program by following the positions of lines on the
contact surface, modeled by CONTA177 elements, relative to 3-D surface segments on the target surface,
modeled by TARGE170 elements. Line-to-surface contact in three dimensions is depicted in the figure below.

Figure 6.1: Line-to-Surface Contact Elements

               Y

                                              CONTA177
                       X
         Z                                   J
                       K
I


                                                                                       I       K J
                                                                      CONTA177                                                 Edge of
                                                                                                                               shell elements

                                                  3-D target surface
                                                    (TARGE170)

The CONTA177 element type:

    •   Has two nodes or three nodes.
    •   Is paired with a target surface defined by TARGE170 elements.
    •   Uses the same real constant set as used for the surface-to-surface contact elements. See Real Con-
        stants (p. 25) for more information.
    •   Supports 3-D rigid-flexible and flexible-flexible contact.
    •   Supports 3-D beams and shell edges with or without midside nodes.
    •   Can be generated by the ESURF command (similar to the surface-to-surface contact elements) in many
        cases. See Performing a 3-D Line-to-Surface Contact Analysis (p. 80) for details.



                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                       of ANSYS, Inc. and its subsidiaries and affiliates.                                      79
Chapter 6: Line-to-Surface Contact


6.2. Performing a 3-D Line-to-Surface Contact Analysis
Contact element CONTA177 follows the contact pair concept used by the surface-to-surface elements
(CONTA171 through CONTA174). You must pair CONTA177 with 3-D target surface segments (TARGE170)
to model 3-D beam-to-surface or 3-D shell edge-to-surface contact. See Identifying Contact Pairs (p. 12) for
more information. CONTA177 uses most of the same element KEYOPTs and real constants as the surface-to-
surface contact elements. Any differences are described in the next section.

The basic steps for performing a 3-D line-to-surface contact analysis are the same as those used for a typical
surface-to-surface analysis using CONTA171 through CONTA174. See Steps in a Contact Analysis (p. 11) for
details.

When the underlying elements are beams or edges of shell elements you can use the ESURF command to
create CONTA177 elements. (In the GUI, pick Main Menu> Preprocessor> Modeling> Create> Elements>
Surf/Contact> Surf to Surf.) This procedure is similar to that used for the surface-to-surface contact elements.

When using line-to-surface contact elements to form the contact surface, the nodes must be entered in a
sequence that defines a continuous line, as shown in the figure below.

Figure 6.2: Continuous Line Segments




The line can be made up of linear or parabolic segments, depending on whether the attached beam or shell
edge is made up of first order or second order elements. If the nodal ordering of the underlying beam ele-
ments is not consistent, you must either change them by reversing the node number order of the selected
elements (ESURF,,REVERSE command) or make a consistent element ordering (ENORM command).

You can list the CONTA177 results using the PRESOL,CONT or PRETAB commands. Since CONTA177 is a 3-
D line element, you can also use the PLLS command to display element table items.

6.2.1. KEYOPTs and Real Constants
CONTA177 uses most of the same KEYOPTs that are used by the surface-to-surface contact elements, CON-
TA171 through CONTA174. KEYOPT(4) differs from the other contact elements. KEYOPT(3) and KEYOPT(8)
are not used by CONTA177. See Element KEYOPTS (p. 28) for a listing of the remaining KEYOPTs.

CONTA177 uses the same real constants used by the surface-to-surface contact elements (CONTA171 through
CONTA174), except for the units of FKN and FKT. See Real Constants (p. 25) for a complete list.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
80                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                             6.2.1. KEYOPTs and Real Constants

6.2.1.1. Real Constants FKN and FKT
CONTA177 uses the contact force-based model. (Since this is the only model used for this element, KEYOPT(3)
is not used.) The units of real constants FKN and FKT have a factor of AREA with respect to those used in
the surface-to-surface contact elements. For instance, contact stiffness FKN has units of FORCE/LENGTH in
the force-based model, but FORCE/LENGTH3 in the surface-to-surface contact elements. PRES is the contact
normal force in the force based model, but contact pressure in CONTA171 to CONTA174.

6.2.1.2. Accounting for Thickness Effect (CNOF and KEYOPT(11))
For line-to-surface contact, the thickness effect of underlying beam elements (on the contact side) is accounted
for through the contact offset real constant, CNOF. The thickness effect of underlying shell elements (on the
target side) is accounted for by setting KEYOPT(11).

For the case of a beam contacting a solid, input half of the beam thickness for CNOF; KEYOPT(11) is ignored.
For the case of a beam contacting a shell surface, input half of the beam thickness for CNOF and set KEY-
OPT(11) = 1 to include the shell thickness effect. CNOF remains constant for the entire contact pair during
the solution. For more information on using CNOF, see Adjusting Initial Contact Conditions (p. 41). For more
information on using KEYOPT(11), see Using KEYOPT(11) (p. 54).

6.2.1.3. Real Constant TOLS
For CONTA177, the contact normal is uniquely defined and is perpendicular to the target surfaces. 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 be completely out of contact, resulting in convergence diffi-
culties 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 de-
flection (NLGEOM,ON).

6.2.1.4. KEYOPT(4)
You can use CONTA177 with the multipoint constraint (MPC) approach (KEYOPT(2) = 2) to define surface-
based constraints. The KEYOPT(4) setting will determine the type of surface-based constraint. Set KEYOPT(4)
= 1 for a force-distributed constraint, or set KEYOPT(4) = 0 for a rigid surface constraint. See Surface-based
Constraints for more information.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                      81
     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
82                               of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 7: Multiphysics Contact
Multiphysics applications (involving two or more fields) often require the inclusion of contact interaction
between two or more surfaces or between a surface and its surroundings. These contact interactions can
be modeled by using the thermal, electric, and magnetic capabiities of the surface-to-surface and node-to-
surface contact elements (CONTA171, CONTA172, CONTA173, CONTA174, and CONTA175) .

The following multiphysics contact topics are available:
 7.1. Modeling Thermal Contact
 7.2. Modeling Electric Contact
 7.3. Modeling Magnetic Contact

7.1. 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 (thermal DOF only), ANSYS ignores heat generation due to friction.


7.1.1. 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.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                               83
Chapter 7: Multiphysics Contact

7.1.2. 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 asso-
ciated 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.

7.1.3. 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. For a general target surface, the temperature varies along the surface
(see figure below). In this case, the temperature at the intersection between the target surface and the
normal from the contact detection point represents the target temperature. For a rigid target, the temper-
ature on the pilot node represents the entire rigid target surface temperature, if the pilot node exists.

Figure 7.1: Target Temperature



                         Target


       Target temperature
       at the intersection
                                                                         Far-field
                                                                         contact

                        Contact


7.1.4. Modeling Conduction
To take into account the conductive heat transfer between contact and target surfaces, you need to specify
the thermal contact conductance coefficient which is real constant TCC.

7.1.4.1. 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) for
     force-based node-to-surface contact, or units of HEAT/(TIME * TEMPERATURE * AREA) for the traction-
     based model.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
84                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                            7.1.6. Modeling Radiation

     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 dis-
continuity 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).

7.1.4.2. 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 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.

7.1.5. Modeling Convection
To model convective heat transfer, you must specify the heat convection coefficient CONV using the SFE
command. This surface load must be applied to the contact elements. CONV can be a constant value (only
uniform is allowed) or a function of temperature, time, or location as specified through tabular input. For
free surface convection, you must also 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

7.1.6. Modeling Radiation
7.1.6.1. Background
To model radiative heat transfer, you need to specify one of the following:

 •    Emissivity value EMIS, specified through the material property definition.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                            85
Chapter 7: Multiphysics Contact

 •   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).

7.1.6.2. 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 free-
     surface 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 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).

7.1.7. Modeling Heat Generation Due to Friction
7.1.7.1. 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.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
86                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                     7.2. Modeling Electric Contact

7.1.7.2. 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

         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.

7.1.8. 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.

7.2. 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 structur-
al/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.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                          87
Chapter 7: Multiphysics Contact

 •    Electric charge across the contacting interface.

7.2.1. Modeling Surface Interaction
7.2.1.1. 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.

7.2.1.2. 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.


7.2.2. 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.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
88                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                  7.3. Modeling Magnetic Contact

      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.

7.3. 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 dis-
cussions in the appropriate chapter of the Low-Frequency Electromagnetic Analysis Guide. For information on
the use of the AZ degree of freedom, see Specifying Element Types and Options. For more information on
the use of the MAG DOF, see Build 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 Doing an Example 2-D
Static Magnetic Contact Analysis (Command Method).



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                       89
Chapter 7: Multiphysics Contact

7.3.1. 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 per-
meability 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.

7.3.2. 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.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
90                                                of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 8: Node-to-Node Contact
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 is
negligible. In addition, the deflections (rotations) of the two surfaces must remain small.

The following node-to-node contact topics are available:
 8.1. Node-to-Node Contact Elements
 8.2. Performing a Node-to-Node Contact Analysis

8.1. Node-to-Node Contact Elements
The most commonly used node-to-node elements are shown in the following figure.

Figure 8.1: Node-to-Node Contact Elements

                     J                                         J                                      J




        I
                                                                       I
                            I
     CONTAC12                      CONTA178                                       CONTAC52
     (2D)                          (2D and 3D)                                    (3D)

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 fol-
lowing 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)



                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                     of ANSYS, Inc. and its subsidiaries and affiliates.                               91
Chapter 8: Node-to-Node Contact


      Note

      CONTA178 supports only elastic Coulomb friction behavior. For rigid Coulomb friction models,
      use CONTAC12 and CONTAC52


8.2. Performing a Node-to-Node Contact Analysis
The procedure for performing a node-to-node contact analysis is similar to that described for the node-to-
surface contact elements in Chapter 4, Node-to-Surface Contact (p. 69). 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.

8.2.1. 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.

8.2.2. 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
 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.

8.2.2.1. 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.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
92                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                               8.2.3. Defining the Contact Normal

8.2.2.2. 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 8.2: Contact Between Two Concentric Pipes




8.2.2.3. 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 or-
dering 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
     NSLE
     EPLOT

8.2.3. 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.

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                       93
Chapter 8: Node-to-Node Contact

 •   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 8.3: 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.

         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.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
94                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                        8.2.6. Applying Necessary Boundary Conditions

8.2.4. 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 CON-
TAC52. 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.

8.2.5. 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 “semi-
automatic” 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.

8.2.6. Applying Necessary Boundary Conditions
You can now apply necessary boundary conditions as you would do for any ANSYS analysis. For more inform-
ation on applying boundary conditions, see the appropriate analysis description in the Structural Analysis
Guide.

When using the Lagrange multiplier method, be careful not to overconstrain the model. The model is over-
constrained 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:




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               95
Chapter 8: Node-to-Node Contact

Figure 8.4: 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.

8.2.7. 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.

        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.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
96                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                        8.2.9. Reviewing the Results

        Command(s): NROPT,FULL,,ON
        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 re-
     defining 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.


8.2.8. Solving the Problem
You can now solve the analysis the same as you would for any linear or nonlinear analysis. See Solve the
Analysis in the Structural Analysis Guide.

8.2.9. 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 Reviewing
Results in POST26 in the Structural Analysis Guide.

For general information on post processing, refer to the Basic Analysis Guide.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                            97
     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
98                               of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 9: Multipoint Constraints and Assemblies
You can use the internal multipoint constraint (MPC) approach (KEYOPT(2) = 2), in conjunction with certain
bonded and no separation contact definitions (KEYOPT(12) = 4, 5, or 6), to define various contact assemblies
and kinematic constraints. This capability is available for contact elements CONTA171, CONTA172, CONTA173,
CONTA174, CONTA175, CONTA176, and CONTA177. By this method, the program builds MPC equations in-
ternally 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 surface constraint - the contact nodes are constrained to the rigid body motion defined by the
     pilot node (similar to the CERIG command)
 •   Force-distributed constraint - 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 surface constraint or force-distributed constraint 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, reducing 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 iterations are needed to solve the system of equations. For large deformation
     problems, the MPC equations are updated during each iteration, overcoming the small strain restriction
     in conventional constraint equations.
 •   Both translational and rotational degrees of freedom can be constrained.
 •   Generation of internal MPC is simple because it uses 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 you use higher order elements or
     axisymmetric elements. In addition to forces, displacements can be applied on the pilot node for this
     type of MPC.

The following MPC topics are available:
 9.1. Modeling Solid-Solid and Shell-Shell Assemblies
 9.2. Modeling a Shell-Solid Assembly
 9.3. Surface-Based Constraints
 9.4. Modeling Rigid Bodies
 9.5. Overconstraint Detection and Elimination
 9.6. Restrictions and Recommendations for Internal MPC


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               99
Chapter 9: Multipoint Constraints and Assemblies

Before using the internal MPC feature, be sure to review the last topic listed above on restrictions and re-
commendations.

9.1. 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) = 4, 5, or      No separation (see note below), bonded always, or
6                          bonded initial
KEYOPT(4) = 1 or 2         Nodal detection for CONTA171, CONTA172, CON-
                           TA173, CONTA174
KEYOPT(4) = 0 or 1         Contact normal direction for CONTA175


      Note

      When used with the MPC approach, the no separation option (KEYOPT(12) = 4) is only valid for
      modeling solid-solid assemblies that represent a slider line or slider plane.

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). Com-
paring it to the CEINTF command, the contact surface acts as "region A nodes," and the target surface acts
as "region B elements."

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 overconstraint, 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 Nonlinear Options in the 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) and no separation option (KEYOPT(12) = 4), any contact
node that lies inside the pinball region (PINB) can be the constrained node in the MPC definition if an inter-
section 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 KEYOPT(12) is set to the bonded always or no separation option, PINB defaults to
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 Using PINB (p. 49) 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.

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
100                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                 9.1. Modeling Solid-Solid and Shell-Shell Assemblies

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 Adjusting Initial
Contact Conditions (p. 41) for more information on using KEYOPT(5), CNOF, and ICONT.

You can use KEYOPT(4) on the target element (TARGE169 or TARGE170) to control individual degrees of
freedom for the constraint. For example, if you are using TARGE170 elements with 3-D contact elements,
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 the 3-D case, you can also use KEYOPT(5) of the target element (TARGE170) to explicitly define the type
of constraint. 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 as-
sembly. The constraint types available through KEYOPT(5) are as follows:

     KEYOPT(5) = 0 - Auto constraint type detection (default)
     KEYOPT(5) = 1 - Solid-solid constraint (no rotational DOFs are constrained)
     KEYOPT(5) = 2 - Shell-shell constraint (both translational and rotational DOFs are constrained, but they
     are decoupled)

For a shell-shell assembly, you can also use the shell-solid constraint types (KEYOPT(5) = 3, 4, and 5). See
Modeling a Shell-Solid Assembly (p. 102) for more information on the shell-solid constraint types.

Keep these important points in mind when determining the type of constraint to use for the assembly:

 •    For the 3-D case, if you specify KEYOPT(4), only the degrees of freedom that are common to both the
      KEYOPT(4) degree-of-freedom set and the KEYOPT(5) degree-of-freedom set will be considered in the
      constraint equations.
 •    When the no separation option (KEYOPT(12) = 4 on the contact element) is used with the MPC approach
      to model solid-solid assemblies, only the KEYOPT(5) = 0 and 1 options (auto detection or solid-solid
      constraint) described above are valid. If the auto detection option is set and the program finds a shell-
      shell or shell-solid constraint in this situation, the solution will terminate.
 •    If overconstraint occurs in bonded shell-shell assemblies when using the MPC algorithm, you can switch
      to the penalty method or the augmented Lagrangian method. See Bonded Contact for Shell-Shell Assem-
      blies (p. 52) for more information.
 •    The shell-shell constraint type (KEYOPT(5)=2) constrains the rotational and translational degrees of
      freedom from both sides. However, the rotational and translational degrees of freedom are decoupled.
      This option can model situations where one shell edge lines up well with another shell surface. This
      provides a valid answer which is closer to a matching mesh solution.

      If a certain amount of gap or penetration exists in the assembly interface, the shell-shell constraint option
      causes artificial constraints to be added, which can result in an a inaccurate solution. In this case, it is
      recommended that you use a shell-solid constraint type by setting KEYOPT(5) = 3, 4, or 5 on the target
      element. One drawback of using the shell-solid constraint type is that the initial gap or penetration will
      remain during the solution (similar to setting KEYOPT(9) = 1 on the contact element).




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               101
Chapter 9: Multipoint Constraints and Assemblies


9.2. 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 9.1: Example of Shell-
Solid Assembly (p. 102)). 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 9.1: Example of Shell-Solid Assembly




                                              Constraint interface
                                                                                     Shell elements




                                                                                                            Solid elements




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, CON-
                         TA173, CONTA174
KEYOPT(4) = 0 or 1       Contact normal direction for CONTA175

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.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
102                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                        9.2. Modeling a Shell-Solid Assembly

In most cases, ANSYS will automatically constrain both translational and rotational degrees of freedom for
a shell-solid assembly (see Figure 9.2: Shell-Solid Assembly (Original Mesh) (p. 103)). 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 (default)
   KEYOPT(5) = 1 - Solid-solid constraint; no rotational DOFs are constrained (see Figure 9.3: Shell-Solid Assembly
   with Solid-Solid Constraint Option (p. 104))
   KEYOPT(5) = 2 - Shell-shell constraint; both translational and rotational DOFs are constrained (see Fig-
   ure 9.4: Shell-Solid Assembly with Shell-Shell Constraint Option (p. 104))
   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 9.5: Shell-Solid Assembly with
   Shell-Solid Constraint Option (p. 105))
   KEYOPT(5) = 4 - Shell-solid constraint, all directions. This option acts the same as KEYOPT(5) = 3 if an in-
   tersection 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. (See Figure 9.6: Shell-
   Solid Constraint - No Intersection (use KEYOPT(5) = 4 or 5) (p. 106) later in this section.)
   KEYOPT(5) = 5 - Shell-solid constraint, anywhere inside the pinball region. Constraint equations are always
   built as long as contact node(s) and target segments are inside the pinball region, regardless of whether
   an intersection exists between the contact normal and the target surface. (See Figure 9.6: Shell-Solid
   Constraint - No Intersection (use KEYOPT(5) = 4 or 5) (p. 106) later in this section.)

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 9.2: Shell-Solid Assembly (Original Mesh)


      Shell elements
      (thickness J)



                                                                                 Contact elements
                                                                                  (pre-existing)

Solid elements




Target elements
  TARGE170
(on top of solid)




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                    103
Chapter 9: Multipoint Constraints and Assemblies

Figure 9.3: Shell-Solid Assembly with Solid-Solid Constraint Option



             New Virtual
            shell elements
             SHELL181
          (can be created with
           SHSD command)

                                                                                                                   New Contact
                                                                                                                    elements
                                                                                                                   CONTA175




      MPC equations
  (translation DOF only)
Virtual shell - solid surface
                                                                                                            Shell thickness




Figure 9.4: Shell-Solid Assembly with Shell-Shell Constraint Option



              New Virtual
             shell elements
          (can be created with
           SHSD command)




        MPC equations
 (translation + rotation DOF)
 for shell edge - virtual shell
                                                                                                        FTOLN
                                                                                                 (influence distance)




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
104                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                         9.2. Modeling a Shell-Solid Assembly

Figure 9.5: Shell-Solid Assembly with Shell-Solid Constraint Option




      MPC equations for
   shell edge solid surface
                                                                                                         FTOLN
                                                                                                  (influence distance)


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 rel-
atively 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 Using PINB (p. 49) 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 rep-
resent 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.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                    105
Chapter 9: Multipoint Constraints and Assemblies

When choosing a constraint type (KEYOPT(5) = 1, 2, 3, 4, or 5 on TARGE170), you should consider the following
points. 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-shell constraint approach (KEYOPT(5) = 2) decouples
constraints of translational DOFs and rotational DOFs. It may not carry moments correctly when the shell
nodes do not lie exactly on the solid surface. The shell-solid constraint (KEYOPT(5) = 3, 4, or 5) 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 is parallel to the normal of the solid
surface.

The KEYOPT(5) = 4 option (shell-solid constraint, all directions) can be used for the case when the shell node
does not overlap or intersect the contact surface (see figure below). However, if any intersection is detected
from the contact normal to the target surface, this option may not be the best choice because it only builds
very localized constraints between the shell node and the target segment which is intersected. The same is
always true for KEYOPT(5) = 3.

The KEYOPT(5) = 5 option (shell-solid constraint, anywhere inside pinball) is the recommended shell-solid
constraint because constraint equations are always built between a shell node and all target segments which
are inside the pinball region, regardless of the contact normal and contact intersection. Thus, the pinball
size is important since a larger pinball will result in a larger constraint set. This option is useful when you
wish to completely constrain one contact side to another. The stresses are more evenly distributed at the
shell-solid interface for this option than they would be for other shell-solid constraint types.

Figure 9.6: Shell-Solid Constraint - No Intersection (use KEYOPT(5) = 4 or 5)

                                                                                 Shell elements


                                                                                            Pinball region

                                 Target normal


               Contact normal
                                                                                     Shell node


                                                                                 Solid elements

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
shell-solid constraint type (KEYOPT(5) = 3, 4, or 5), 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.

9.3. 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:




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
106                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                   9.3. Surface-Based Constraints

•   Rigid surface constraint - In this type of constraint, the contact nodes are constrained to the rigid body
    motion defined by the pilot node (see Figure 9.7: Rigid Surface Constraint (p. 107)), similar to a constraint
    defined by the CERIG command.
•   Force-distributed constraint - 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 9.8: Force-
    Distributed Constraint (p. 108)), similar to a constraint defined by the RBE3 command.

Figure 9.7: Rigid Surface Constraint

    Imposed displacement at Pilot node                                 Constraint surface
    (UX, UY)                                                           remains rigid




                 Contact elements




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                         107
Chapter 9: Multipoint Constraints and Assemblies

Figure 9.8: Force-Distributed Constraint

 Imposed displacement at Pilot node                    Deformed constraint surface
 (UX, UY)




                Contact elements

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 constraint.
 •    To model rigid bodies. Example: rigid body definition in multi-body dynamics.
 •    To model rigid end conditions. Example: using a rigid surface constraint to model a rigid end plate or
      rigid plane section of 3-D solid elements.
 •    To model interactions with other joints. Example: two flexible parts linked by a hinge. This can be
      modeled by two force-distributed constraint definitions whose pilot nodes are connected by a revolute
      joint element.
 •    To define transitions between solid and structure elements. Example: a beam element connected to a
      solid element face.

9.3.1. 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
and the contact nodes. You can define a follower element (FOLLW201) on the pilot node so that the element-
specified external forces and moments on the follower element will follow the motion of the pilot node.

For a force-distributed constraint, use the following contact element key options:

Force-distributed Constraint KEYOPT Settings
KEYOPT(2) = 2            MPC based approach
KEYOPT(12) = 5 or 6      Bonded always or bonded initial



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
108                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                           9.3.3. Degrees of Freedom of Surface-Based Constraints

KEYOPT(4) = 1            Indicates a force-distributed constraint for CONTA171,
                         CONTA172, CONTA173, CONTA174, CONTA175,
                         CONTA176, and CONTA177

For a rigid surface constraint, use the following contact element key options:

Rigid Surface Constraint KEYOPT Settings
KEYOPT(2) = 2            MPC based approach
KEYOPT(12) = 5 or 6      Bonded always or bonded initial
KEYOPT(4) = 2            Indicates a rigid surface constraint for CONTA171,
                         CONTA172, CONTA173, and CONTA174
KEYOPT(4) = 0            Indicates a rigid surface constraint for CONTA175 ,
                         CONTA176, and CONTA177

The following key options are ignored for surface-based constraints: KEYOPT(8), KEYOPT(5), KEYOPT(7),
KEYOPT(10).

With the exception of PINB, none of the standard contact real constants are used for surface-based constraints
using internal MPC.

9.3.2. Defining Influence Range (PINB)
By default, all the contact nodes are included in the surface-based constraints. You can select a subset of
nodes from these contact nodes by defining a radius of influence range, PINB. The nodes that lie within the
spherical range (radius = PINB) centered about the pilot node are selected for the definition of the surface-
based constraints.

9.3.3. Degrees of Freedom of Surface-Based Constraints
KEYOPT(1) > 0 is ignored for a force-distributed constraint since only structural degree-of-freedom constraints
are included. However, for a rigid surface constraint, you can use KEYOPT(1) to include other field degrees
of freedom (in addition to the structural DOFs) in the constraint sets.

The pilot node has both translational and rotational degrees of freedom. The active degrees of freedom at
the pilot node depend on the defined type of target elements. Use TARGE169 for 2-D surface-based constraints
that contain UX, UY, and ROTZ degrees of freedom. Use TARGE170 for 3-D surface-based constraints that
contain UX, UY, UZ, and ROTX, ROTY, ROTZ degrees of freedom. Generally, you should always set KEYOPT(2)=1
for the target element to indicate that boundary conditions for rigid target nodes will be user-specified.
Otherwise, ANSYS may apply internal constraints on the pilot node.

The degrees of freedom of the surface-based constraints can also be controlled 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.

The basic formulation for the rigid surface constraint is similar to the MPC184 rigid beam and rigid link ele-
ments. However, this constraint type offers additional flexibility when you fully or partially constrain the
degrees of freedom. For examples, the following are possible configurations:

 •   All six degrees of freedom are selected, which is equivalent to the MPC184 rigid beam.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               109
Chapter 9: Multipoint Constraints and Assemblies

 •    One rotational degree of freedom is excluded, which is equivalent to the MPC184 revolute joint.
 •    Only three translational degrees of freedom are selected, which is equivalent to the MPC184 spherical
      joint or MPC184 rigid link.

9.3.4. Specifying a Local Coordinate System
You can specify the surface-based constraint in a local coordinate system. For the rigid surface constraint,
rotate the contact nodes into a local coordinate system. For the force-distributed constraint, rotate the pilot
node into a local coordinate system.

When KEYOPT(12) = 5 is set on the contact elements, the coordinate system does not rotate and it keeps
its initial configuration. When the rotation is finite and KEYOPT(12) = 6 is set on the contact elements, the
coordinate system in which the constrained degrees of freedom are specified will be co-rotated according
to the rotation of the pilot node. The degrees of freedom of the surface-based constraints will be assigned
with the co-rotated system. This is true even for the constrained degrees of freedom specified in the global
coordinate system.

      Note

      If all degrees of freedom are included in the constraint equations, there will be no difference
      between the KEYOPT(12) = 5 and KEYOPT(12) = 6 settings.

Figure 9.9: Slider Link (p. 110) shows an example of a slider link modeled with contact. A local cylindrical co-
ordinate system is defined at a contact node such that the x-direction is coincident with the line connecting
the contact node and pilot node. KEYOPT(4) = 10 is set for the target element type to specify that only the
y degree of freedom is constrained and other degrees of freedom are free. The coordinate system at the
contact node will be co-rotated according to the rotation of the pilot node.

Figure 9.9: Slider Link




                        Contact node
                                                                                                  Rigid body



                                     x

                                                           y


Pilot node

                                                                                                                    Apply rotation


In another example, a cylindrical ring is clamped at one end and loaded by a torque at the other end (Fig-
ure 9.10: Free Radial Expansion Under Torque Load (p. 111)). A rigid surface constraint is used with all the contact


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
110                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                     9.3.7. Modeling a Beam-Solid Assembly

nodes rotated into a cylindrical coordinate system. If the x-direction constraint is free (KEYOPT(4) = 110), the
ring is allowed to expand in the radial direction.

Figure 9.10: Free Radial Expansion Under Torque Load




9.3.5. Additional Guidelines for a Force-Distributed Constraint
 •   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 MPC equations are rewritten so that the degrees of freedom
     of the pilot node are no longer dependent DOF.
 •   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.

9.3.6. Additional Guidelines for A Rigid Surface Constraint
 •   The pilot node is an independent (retained) node in the constraint equation. The contact nodes are the
     dependent (removed) nodes. Use with great caution when you apply any displacement constraints,
     coupling (CP command), or constraint equations (CE command) on the contact nodes since redundant
     constraints are likely to occur.
 •   KEYOPT(4) of TARGE169 and TARGE170 controls the DOF set (the number of DOF) of the contact (de-
     pendent) nodes used in the internally-generated MPCs.
 •   The number of internally-generated MPCs is equal to the number of contact nodes times the number
     of DOF.
 •   The contact surface does not require underlying elements.

9.3.7. 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. The rigid surface constraint is generally
well-suited for the solid beam to solid surface case (see Figure 9.11: Beam-Solid Assembly Defined by Rigid
Surface Constraint (p. 112)), and the force-distributed constraint is well-suited for the flexible beam (such as
a thin wall beam) to solid/shell surface case (see Figure 9.12: Beam-Solid Assembly Defined by Force-distributed
Constraint (p. 112)).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                 111
Chapter 9: Multipoint Constraints and Assemblies

Figure 9.11: Beam-Solid Assembly Defined by Rigid Surface Constraint


                           Solid elements


                   Pilot node



      Beam elements


              Contact elements




Figure 9.12: Beam-Solid Assembly Defined by Force-distributed Constraint



                                       Shell elements

              Pilot node




      Beam elements




                                            Contact elements




9.4. Modeling Rigid Bodies
Rigid bodies are widely used for numerical simulation of multibody dynamic applications. The definition of
a rigid body in ANSYS is similar to the definition of a rigid surface constraint, except that all the elements
are defined by target elements. The motion of the rigid body is governed by the degrees of freedom at a

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
112                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                          9.5. Overconstraint Detection and Elimination

pilot node which allows accurate representation of the geometry, mass, and rotary inertia of the rigid body.
Each rigid body is only associated with one pilot node. The pilot node can be one of the nodes on a target
element or a node at any arbitrary location. It can be connected to point mass, follower (FOLLW201), and
deformable elements. For transient analysis you should locate the pilot node at the gravity center of the rigid
body if the center of mass is known or can be approximated. You can add a point mass element, MASS21,
to the gravity center. See Modeling Rigid Bodies in a Multibody Analysis in the Multibody Analysis Guide for
more details.

9.4.1. Modeling Contact between Rigid Bodies
You can model contact between two rigid bodies by specifying a contact pair consisting of a contact surface
on one rigid body and a target surface on another rigid body. These contact and target elements should
overlap the existing contact elements defined for the rigid bodies. Use either the augmented Lagrange al-
gorithm or penalty algorithm (KEYOPT(2) on the contact elements) to avoid overconstraint between rigid
body constraints and contact constraints.

You cannot use the multipoint constraint (MPC) algorithm (KEYOPT(2) = 2) with bonded or no-separation
contact behavior (KEYOPT(12)) to connect two rigid bodies; doing so would cause the model to be overcon-
strained. Instead, add a third rigid body which connects the first two rigid bodies at their pilot nodes.

MPC bonded contact between a flexible body and a rigid body is allowed. For this case, the contact surface
of the MPC bonded contact pair must belong to the flexible body. Otherwise, the MPC bonded constraints
and rigid body constraints would be redundant.

It is possible to model two rigid bodies that are connected or overlapping through shared rigid body nodes
or pilot nodes. To prevent overconstraint, ANSYS internally merges the two rigid bodies into one rigid body
and treats the second pilot node as a regular rigid body node.

9.5. Overconstraint Detection and Elimination
When a degree of freedom is subjected to multiple constraints, overconstraint occurs. Overconstraint can
be caused by the combination of the following constraints within the model:

 •   User-specified constraints, including displacement constraints, constraint equations (CE command), and
     coupling (CP command)
 •   Lagrange multiplier-based contact definitions
 •   MPC-based contact definitions
 •   Constraints introduced through joint elements

Overconstraint may result in convergence difficulties or inaccurate solutions. In order to prevent this problem,
ANSYS tries to detect and eliminate overconstraints automatically. You can verify the eliminated constraints
during postprocessing.

ANSYS issues warning messages outlining the cause of the potential overconstraints in the beginning of a
contact analysis. You can use the CNCHECK,DETAIL command to identify the overconstraints indicated by
the messages. You should then manually remove as many unnecessary constraints as possible.

Some overconstraints occur only during the solution due to new deformed configurations or due to changes
in contact status. ANSYS will automatically eliminate a limited set of overconstraints detected during solution;
appropriate messages are issued when this occurs. For MPC-based contact pairs, the contact statuses (contact
result item STAT) are set to negative values if one or more contact constraints are removed. STAT is set to



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               113
Chapter 9: Multipoint Constraints and Assemblies

-3 for bonded contact; STAT is set to -2 for no-separation contact. Be aware that, due to complexities, certain
overconstraints may not be easily detected.

The way the program removes the overconstraint is not unique. The order of the redundant constraints will
influence how they are removed (the first encountered is kept, the next is removed). You should always
verify the modified model carefully. You can list and display the contact status using STAT as a contact result
item for the PLESOL and PRESOL commands; for example:
 PLESOL,CONT,STAT


9.6. Restrictions and Recommendations for Internal MPC
The following restrictions and guidelines apply when using the internal MPC approach.

 •    To prevent overconstraint, displacement boundary conditions and other constraint equations or coupling
      equations (ideally) should not be applied on the contact nodes for solid-solid, shell-shell, and shell-solid
      assemblies, or for the rigid surface constraint type.
 •    Sparse, PCG, and AMG solvers are recommended to solve models with constraint equations.
 •    The MPC-based algorithm must be used 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
      large and dense submatrices for the global stiffness matrix. This may significantly increase the peak
      memory required during element stiffness assembly. Consider reducing the number of contact nodes
      if real memory or virtual memory is limited.
 •    The force-distributed constraint creates internal constraint equations such that the motion of the pilot
      node is the average of the contact nodes. For the rotations, a least-squares approach is used to define
      the "average rotation" at the pilot node from the translations of the contact nodes. If the contact nodes
      are colinear, then one of the rotations on the pilot node that is parallel to the colinear direction can
      not be determined in terms of the translations of the contact nodes. Therefore, the associated moment
      component on the pilot node in that direction can not be transmitted. When this case occurs, a warning
      message is issued.
 •    The internal MPC option will only support element birth and death if all the MPC-based contact and
      target elements are active in the first load step. The birth or death option can be set only after the first
      load step.
 •    The contact related postprocessing items (ETABLE items, PRESOL,CONT, etc.) are not supported for the
      internal MPC option.
 •    MPC contact only generates internal constraint equations. It does not calculate element internal force
      and stiffness matrices. Therefore, during postprocessing the option ITEM = CONT is not valid on the
      PRNLD, NFORCE, and FSUM commands.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
114                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                        9.6. Restrictions and Recommendations for Internal MPC

•   You can use the CELIST command to list the internally-generated constraint equations associated with
    MPC contact . You can also use CELIST to convert the internal constraint equations to external constraint
    equation. (See CELIST for details.)
•   MPC contact generates constraint equations that can include constant terms. These terms are included
    on the right hand side of the system equation. Thus, they are scaled by the LVSCALE command when
    it is used in a mode superposition analysis.




                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                of ANSYS, Inc. and its subsidiaries and affiliates.                               115
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
116                               of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 10: Dynamic Contact and Impact Modeling
Performing contact analysis in a transient dynamic procedure is always challenging due to the presence of
contact chattering (frequent change in contact status). One of the reasons for contact chattering is that the
contact constraints enforce constraints on nodal displacements (penetration) but do not impose any con-
straints on nodal velocities. Since nodal velocities and nodal accelerations are dependent on nodal displace-
ments (see Section 17.2 Transient Analysis in the Theory Reference for the Mechanical APDL and Mechanical
Applications), any constraints on nodal displacements make the nodal velocities and nodal accelerations in-
consistent. This introduces numerical errors in the transient dynamic solution in subsequent time increments
and, if left untreated, leads to numerical instability (non-convergence or incorrect solution).

Numerical damping is usually added to the time integration scheme to suppress such numerical errors.
However, addition of numerical damping does not work in several cases. For example, in problems with
multiple or repeated impacts there is constant growth of numerical error in the solution, and the analysis
eventually fails to converge in spite of large numerical damping. In other situations the analysis may converge
with addition of numerical damping, but the system response may be underdamped or overdamped depend-
ing on the growth of numerical error.

A more appropriate solution to the contact chattering problem is to treat nodal displacement and nodal
velocities consistently. One such solution is provided by Energy and Momentum Conserving Contact (p. 117).

10.1. Energy and Momentum Conserving Contact
In transient dynamic analysis with contact, if the contact and target surfaces impact each other with nonzero
relative velocities, it is important to satisfy momentum and energy balance for the contact/target interface.
This helps to more accurately predict the duration of impact and the rebound velocities after separation. In
ANSYS this can be achieved by using impact constraints with any of the 2D or 3D contact elements: CONTA171,
CONTA172, CONTA173, CONTA174, CONTA175, CONTA176, CONTA177, and CONTA178.

Impact constraints include constraints on penetration and relative velocity (see Energy and Momentum
Conserving Contact in the Theory Reference for the Mechanical APDL and Mechanical Applications). To activate
the impact constraints the following contact options must be defined for a contact element:

 •   Contact algorithm must be one of the following:
     –   Augmented Lagrangian (KEYOPT(2) = 0)
     –   Penalty function (KEYOPT(2) = 1)
     –   Lagrange multiplier on contact normal and penalty on tangent (KEYOPT(2) = 3)
     –   Pure Lagrange multiplier on contact normal and tangent (KEYOPT(2) = 4)

 •   Standard or rough contact (KEYOPT(12) = 0 or 1)
 •   Impact constraints (KEYOPT(7) = 4)

The impact constraints can be used with both frictionless and frictional contact.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               117
Chapter 10: Dynamic Contact and Impact Modeling

10.1.1. Energy Conservation
The impact constraints are active only on the contact/target interface, so energy conservation is enforced
only for contact elements. The underlying finite elements defining the interior of impacting bodies do not
satisfy energy conservation. To ensure energy conservation, the following conditions must be satisfied for
contact elements:

 •    Relative velocity constraint should be satisfied exactly.

 •    No numerical damping should be used.

 •    No friction should be specified.

Energy conservation is relatively easy to satisfy for rigid impact (when both contact and target surfaces are
rigid) as compared to flexible impact (when the target surface is rigid and the contact surface is flexible, or
both surfaces are flexible). This is because the underlying finite elements for flexible bodies excite higher
frequencies, which can make the time integration scheme unstable unless some numerical damping is used.
For rigid bodies undergoing only translation motion and impact, numerical damping is generally not needed;
however, when rigid bodies are undergoing large rotations, a small amount of numerical damping is necessary
to keep the time integration scheme from becoming unstable.

10.1.2. Automatic Time Stepping
An automatic time stepping scheme is provided to adjust the time increment size. This can be activated by
SOLCONTROL,ON,ON at the procedure level when AUTOTS,ON is set. This scheme starts adjusting size of
the time increments before impact such that there is minimum penetration in the substep where contact
is first detected. This is important because the contact algorithm will enforce the relative velocity constraints
to only prevent further penetration.

If the automatic time stepping scheme is not used, there may be some uncontrolled penetration of the
surfaces depending on the size of the time increment for the substep where contact is first detected before
the relative velocity constraint prevents further penetration.

When using fixed time increment, fixed number of substeps, or automatic time stepping (AUTOTS,ON)
without SOLCONTROL,ON,ON, you should make sure that the penetrations remain sufficiently small.

10.1.3. Penetration and Relative Velocity
When using the impact constraints, the penetration value depends on two factors:

 •    Size of the time increment where contact is first detected

 •    Accuracy of relative velocity constraint

The “initial” penetration value depends on the size of the time increment, as explained above. There is no
contact force associated with this value. The remaining penetration value comes from the enforcement of
relative velocity constraint using the contact algorithm. The value of this penetration depends on the choice
of contact algorithm, contact normal stiffness (FKN), and/or allowable penetration (FTOLN). The contact
normal force is directly related to this penetration value.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
118                                                of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 11: Spot Welds
The traditional way of modeling spot welds involves matching the meshes of different parts at the spot weld
connection points, which introduces meshing difficulties and often requires parts to be meshed manually.
In addition, this approach does not take into account the effects of the spot weld radius, and it underestimates
the strength of the spot weld connection when the radius of the spot weld is the same or lesser order of
magnitude than the mesh size.

The ANSYS spot weld feature, based on the internal multipoint constraint (MPC) approach, offers a robust
alternative to the traditional method. This feature allows you to easily model thin sheet components that
are connected with spot welds, rivets, or fasteners. The spot weld can be located anywhere between the
parts that are to be connected, independent of the mesh and the node locations. The figure below shows
an example of the spot weld configuration. Each spot weld set connects two or more surfaces.

Figure 11.1: Example Spot Weld Configuration




                                  Node 3                                Surface 3




       Spot weld radius




                                   Node 2                            Surface 2




Basic Spot Weld Set



                                       Node 1                           Surface 1




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               119
Chapter 11: Spot Welds

There are several advantages to using this mesh independent spot weld capability:

 •    Parts can be meshed independently.
 •    A basic spot weld set can be easily defined by specifying two surfaces to be connected and a single
      node called the spot weld node near the surfaces. The spot weld node determines the location of the
      spot weld.
 •    This approach takes into account effects of the spot weld radius input by the user. ANSYS will create
      multipoint constraint equations (MPCs) internally through two contact pair definitions, one on each
      spot weld surface. The internal constraint equations (force-distributed constraints) couple the motion
      of the surface nodes to the motion of the spot weld node in an average sense.
 •    The spot weld can be rigid (default) or deformable. To specify a deformable spot weld, you simply define
      a deformable beam element type prior to creating the spot weld.

The following spot weld topics are available:
 11.1. Defining a Spot Weld Set
 11.2. Listing and Deleting Spot Welds

11.1. Defining a Spot Weld Set
The general procedure for defining a spot weld set consists of the following steps:

 1.    Define the basic spot weld set (SWGEN command)
 2.    Define any additional surfaces for the existing spot weld set (SWADD command)

In addition, ANSYS supplies the SWLIST and SWDEL commands for listing and deleting spot weld sets.

11.1.1. Creating a Basic Spot Weld Set with SWGEN
Use the SWGEN command to define a basic spot weld set (in the GUI, pick Main Menu> Preprocessor>
Modeling> Create> Element > SpotWeld> Create New Set). The required arguments are:

 •    Name of the spot weld set
 •    Spot weld radius
 •    Spot weld surfaces
 •    First spot weld node

You can optionally specify the following:

 •    Second spot weld node
 •    Spot weld projection direction
 •    Search radius
 •    Contact and target element types

All of these inputs are discussed in detail below.

Spot Weld Set Name (Ecomp):
   Use the Ecomp argument to assign a name to a new basic spot weld set. The spot weld set is a com-
   ponent composed of new beam, target, and contact elements. The name entered for the Ecomp argu-
   ment will be used to list, delete, output, or add new surfaces to the spot weld set.



                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
120                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                  11.1.1. Creating a Basic Spot Weld Set with SWGEN

Spot Weld Surfaces (NCM1, NCM2):
   Each basic spot weld set contains two surfaces, surface 1 and surface 2, to be connected together. Use
   arguments NCM1 and NCM2 to specify these surfaces. You can input the name of a predefined node
   component or a meshed area number. If no nodal component names matching NCM1 and NCM2 are
   found, they are assumed to be meshed area numbers.
Spot Weld Nodes (SND1, SND2):
   You must specify the first spot weld node, SND1. The location of each spot weld depends on SND1. If
   you specify the second spot weld node (SND2), it is used to determine the spot weld projection direction.
   The second node will be generated automatically if it is not specified. You should locate SND1 and SND2
   (referred to as node 1 and node 2 in figures that follow) as close to the corresponding surfaces as possible.
   They can be nodes on the corresponding surfaces or independent nodes in space. If they are not on the
   corresponding surfaces, node 1 will be moved to surface 1 and node 2 will be moved to surface 2.

   ANSYS will determine the actual location for the spot weld nodes by first projecting node 1 onto surface
   1 along the spot weld projection direction. Next, ANSYS projects node 2 to surface 2 along the spot
   weld projection direction. The spot weld nodes are moved to the surfaces in the beginning of the ana-
   lysis.
Spot Weld Projection Direction:
   By default, the projection direction is a surface normal vector from node 1 to surface 1 (see figure below).
   If you specify node 2 (SND2), the projection direction is in line with the two spot weld nodes. If node 2
   is not specified, you can still explicitly define the projection direction with the DIRX, DIRY, and DIRZ
   arguments.

   Figure 11.2: Default Projection Direction for Node 1


                                   Original position of
                                   Node 1



       Node 1                Surface 1
       after projection



   Once the actual location of node 1 has been determined, ANSYS will project node 2 to surface 2 along
   the spot weld projection direction that was used for node 1. The figure below shows the projection
   locations of nodes 1 and 2 given a default projection normal to surface 1.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               121
Chapter 11: Spot Welds

      Figure 11.3: Default Projection Direction for Nodes 1 and 2




                   Node 2                         Surface 2




                     Node 1
                                                    Surface 1



      Original position of
      Node 1

      The figure below shows spot weld node 1 projected as specified by the user (either through the input
      of DIRX, DIRY, and DIRZ, or by the specification of a second spot weld node).

      Figure 11.4: User-specified Projection Direction, Node 1


                                        Original position of
                                        Node 1



         Node 1                 Surface 1
         after projection



      The figure below is another example showing the projection location of spot weld nodes 1 and 2 given
      a user-specified projection direction.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
122                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                  11.1.1. Creating a Basic Spot Weld Set with SWGEN

   Figure 11.5: User-specified Projection Direction, Nodes 1 and 2




                Node 2                         Surface 2


                                                                     User-defined
                                                                     projection
                                                                     direction




                   Node 1                        Surface 1



   Original position of
   Node 1

Spot Weld Radius (SWRD):
   Each spot weld is assumed to have a circular projection onto the spot weld surfaces. The projection is
   defined by the required spot weld radius argument SWRD. For each spot weld surface ANSYS will build
   6 force-distributed constraint equations through a contact pair. The spot weld radius determines the
   influence range of the constraint equations. Each spot weld node couples with a group of nodes on the
   corresponding surface within the radius. (See Figure 11.7: Nodes Included in Constraint Equations (p. 125)
   later in this section.)
Search Radius (SHRD):
   ANSYS will create a contact pair for each spot weld surface. The contact pair contains one contact element
   defined by the spot weld node, and target elements overlaid fully or partially on the corresponding spot
   weld surface. Only the surface nodes that fall within a sphere of radius, called the search radius, with its
   center at the original position of the corresponding spot weld node are used to form target elements
   (see figure below). The search radius must be larger than the spot weld radius. If the search radius argu-
   ment (SHRD) is not defined, ANSYS uses a default search radius that is four times the spot weld radius.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               123
Chapter 11: Spot Welds

      Figure 11.6: Search Radius for Spot Weld

              Search radius
            Spot weld radius                                                            Original position of
                                                                                        node 1


      TARGE170 elements
      within search radius



                                                                                              CONTAC175
                                                                  Surface 1                   (spot weld node 1)

Target and Contact Element Types (ITTY, ICTY):
    By default, the program automatically creates the target and contact element types required for the
    spot weld. However, you may use the ITTY and ICTY arguments to specify the target and contact
    element types, respectively. You must also set certain key options if you specify the element types to
    be used. See The Components of a Spot Weld (p. 124) for more information.

11.1.2. The Components of a Spot Weld
Each new spot weld set created by the SWGEN command consists of a beam element and two node-to-
surface MPC contact pairs (see Modeling a Shell-Solid Assembly (p. 102) for more information). Each node-to-
surface pair will generate 6 constraint equations. You can choose either a rigid MPC184 element (the default)
or a deformable BEAM188 element to link the spot weld surfaces. Below are detailed explanations of how
these items are generated:

 1.    Contact Pairs: Two node-to-surface contact pairs are created for each new spot weld set. One pair is
       for spot weld surface 1 and the other is for surface 2. Each contact pair has only one contact element,
       CONTA175, which is defined by the associated spot weld node. The target elements (TARGE170) are
       formed by a group of surface nodes lying within the region of the search radius. ANSYS will create an
       independent real constant ID for each contact pair, and proper contact and target element type IDs.

       If you prefer, you can specify the contact or target element type IDs to be used. To specify a contact
       element type, use the ICTY argument on SWGEN and set the following contact element options for
       that element type: KEYOPT(2) = 2 (MPC approach), KEYOPT(12) = 5 (bonded always). To specify a target
       element type, use the ITTY argument on SWGEN and set the target element option KEYOPT(5) = 4
       (shell-solid constraint) for that element type.
 2.    Force-distributed constraint equations: For each contact pair, ANSYS will internally form force-dis-
       tributed constraint equations that distribute the internal forces of the spot weld node (that is, the
       contact node) to the surface nodes (that is, the target nodes) lying within the region of the spot weld
       radius. This includes all elements that fall entirely or partially within the radius (see the figure below).
       In other words, it couples the motion of certain surface nodes to the motion of the spot weld node
       (in an average sense). There are six constraint equations generated for each spot weld surface (that
       is, each contact pair).




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
124                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                  11.1.2.The Components of a Spot Weld

     Figure 11.7: Nodes Included in Constraint Equations

                  Spot weld radius                                                          CONTAC175

     Nodes to be constrained




      TARGE170 elements




                                                                   Surface 1

3.   Beam element: A beam element is created to connect spot weld surface 1 and surface 2. The two
     beam end-nodes are the spot weld nodes, node 1 and node 2 (see Figure below). The spot weld set
     can be rigid or deformable. By default ANSYS will create a rigid beam element (MPC184 with KEY-
     OPT(1)=1) to represent a rigid spot weld. However, if the currently defined element type is BEAM188
     with a solid circular cross-section, ANSYS assumes the spot weld set is deformable and a BEAM188
     element is created. In this case, you must input the material properties with the MP command and
     define the geometry of the beam section using the SECTYPE and SECDATA commands (see the example
     listing below). Generally, BEAM188 is capable of handling a short beam situation.

     Figure 11.8: Beam Element Created for Spot Weld




       Node 2                  Surface 2
                                                          Beam element
                                                          (MPC184 or
                                                          BEAM188)




         Node 1
                                 Surface 1




The following example input shows typical commands used to define a spot weld with a deformable BEAM188
element having a circular cross section.
MP,EX,3,200000000000. ! spot weld material properties
MP,NUXY,3,0.3


                   Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                               of ANSYS, Inc. and its subsidiaries and affiliates.                                125
Chapter 11: Spot Welds

 SECTYPE,3,beam,csolid ! define a circular solid beam section
 SECDATA,2.75e-002     ! beam circular radius
 ET,3,188              ! element type for a deformable spot weld
 TYPE,3
 MAT,3
 SECNUM,3
 *SET,NODE1,9000       ! define parameter for node number
 N,NODE1,0.1,0.5,10.2 ! define spot weld node
 SWGEN,SWELD1,2.75e-2,2,3,NODE1 ! Spot weld name = SWELD1
                                ! Radius = 2.75e-2
                                ! Spot weld surfaces = areas 2 and 3


      Note

      All limitations that are documented for the MPC184 link/beam element in the Element Reference
      also apply when the element is used in a rigid spot weld definition. Please read the MPC184-
      Link/Beam description carefully, especially the assumptions and restrictions.


11.1.3. Adding Surfaces to a Basic Set
Once a basic spot weld set has been created, additional surfaces can be added to the existing spot weld
set. Use the SWADD command to define the additional surfaces (in the GUI, pick Main Menu> Preprocessor>
Modeling> Create> Element > SpotWeld> Add More Surfaces). Each added surface (input as NCM1 through
NCM9) can be specified by an existing nodal component name or by a meshed area number.

In the example command below, four surfaces are added to an existing spot weld set named SWELD1. The
four surfaces include area number 3, area number 4, nodal component FAC5, and nodal component FAC6.
The search radius is 0.8.
 SWADD,SWELD1,0.8,3,4,FAC5,FAC6          ! Adds 4 surfaces to spot weld SWELD1.

For each new surface, ANSYS will create a new spot weld node, a new contact pair, and a new beam element
(see figure below). The location of the new node is determined by projection of one of the closest existing
spot weld nodes onto the newly added surface along the spot weld projection direction. The new node-to-
surface contact pair contains the new spot weld node as a single contact node in the pair, and surface nodes
within the range of the search radius (SHRD) specified on the SWADD command. The search radius defaults
to 4 times the spot weld radius (SWRD) defined for the basic spot weld set. Each new contact pair will create
6 force-distributed constraint equations internally. A new beam is created to link the new surface to the
closest existing surface through the spot weld nodes.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
126                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                        11.1.3. Adding Surfaces to a Basic Set

Figure 11.9: Surfaces Added to Basic Spot Weld Set

                                                           More surfaces




                          Node 4                                Surface 4



                                                                              Beam 3




                              Node 3                                Surface 3




                                                                              Beam 2
      Spot weld radius




                                Node 2                            Surface 2
Basic spot weld

                                                                              Beam 1




                                    Node 1                           Surface 1



            Original position of
            Node 1

After all spot weld nodes are created, the nodes of the beam elements may be reordered to link every two
adjacent spot weld nodes (see Figure below). The ordering is important for the output, which is calculated
for each beam in a spot weld set.

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                      127
Chapter 11: Spot Welds

Figure 11.10: Node Reordering for Beam Elements

                                                              Reordered surfaces




                          Node 3
                                                            Surface 3



                                                                             Beam 3




                              Node 4                             Surface 4 (inserted
                                                                 between 2 and 3)



                                                                              Beam 2




                                Node 2                              Surface 2
Basic spot weld
                                                                              Beam 1




                                    Node 1                          Surface 1




Assuming the basic spot weld set is named SWELD, below is an example of commands that could have
produced the above figure.
 SWADD,SWELD, ,3 ! Add Area 3 to spot weld set SWELD
 SWADD,SWELD, ,4 ! Add Area 4 (between surfaces 2 and 3) to SWELD




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
128                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                       11.2. Listing and Deleting Spot Welds

Initially, when spot weld surface 3 was added, a beam was created between surfaces 2 and 3. When surface
4 was added between surfaces 2 and 3, the beam that went between surfaces 2 and 3 was redefined to go
between surfaces 2 and 4, and a new beam was created to link surfaces 4 and 3.

You can add more surfaces by repeating the SWADD command. However, the maximum number of allowable
surfaces for each spot weld set (including the two surfaces used for the basic set) is 11.

11.2. Listing and Deleting Spot Welds
Use the SWLIST command to list the spot weld sets for a specific spot weld or for all spot weld sets (in the
GUI, pick Main Menu> Preprocessor> Modeling> Create> Element > SpotWeld> List). To ensure that all
defined spotwelds are listed, issue CMSEL,ALL (to select all components) before issuing the SWLIST command.
The listing will include nodes, beams, and contact pair information. If the SWLIST command is issued in
POST1 (in the GUI, pick Main Menu> General Postproc> List Results> SpotWeld Solution), the beam
forces and moments, are also output in the beam local coordinate system. The output includes axial force,
shear forces, torque, and bending moments. For a deformed spot weld set, axial stress and bending stress
are also reported.

Use the SWDEL command to delete a specified spot weld set or all spot weld sets. In the GUI, pick Main
Menu> Preprocessor> Modeling> Create> Element > SpotWeld> Delete.




                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                of ANSYS, Inc. and its subsidiaries and affiliates.                                     129
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
130                               of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 12: Debonding
The debonding capability in ANSYS refers specifically to separation of bonded contact. It can be used to
simulate interface delamination where the interface is modeled using bonded contact with the augmented
Lagrangian method or the pure penalty method. A cohesive zone material must be used to define the
traction separation behavior of the interface. The following contact elements support debonding: CONTA171,
CONTA172, CONTA173, CONTA174, CONTA175, CONTA176, and CONTA177.

An alternative method of modeling interface delamination is to use interface elements with a cohesive zone
material (see "Interface Delamination and Failure Simulation"). However, debonding with contact elements
has the following advantages over delamination with the interface elements:
 •   Parts forming the interface can be meshed independently.
 •   Existing models with contact definitions can be easily modified for debonding.
 •   Standard contact and debonding can be simulated with the same contact definitions.
 •   Debonding can be used for various applications; for example, delamination, spot weld failure, and stitch
     failure.

12.1. Including Debonding in a Contact Analysis
Debonding can be defined in any model that includes surface-to-surface (CONTA171 through CONTA174),
node-to-surface (CONTA175), line-to-line (CONTA176), or line-to-surface (CONTA177) contact. For a detailed
discussion on how to set up a contact analysis, see Chapter 3, Surface-to-Surface Contact (p. 11).

To activate debonding for a contact pair, the following contact options must be defined for the contact
element:

 •   Augmented Lagrangian method or pure penalty method (KEYOPT(2) = 0 or 1)
 •   Bonded contact (KEYOPT(12) = 2, 3, 4, 5, or 6)

In addition, you must specify a cohesive zone material model with bilinear behavior for the contact elements.
Two ways to specify the material data are available:

 •   Bilinear material behavior with tractions and separation distances (TB,CZM command with TBOPT =
     CBDD)
 •   Bilinear material behavior with tractions and critical fracture energies (TB,CZM command with TBOPT
     = CBDE)

This material model is discussed in more detail in the following section.

Once you have defined the required input parameters, you can solve the analysis the same as you would
for any nonlinear analysis (see Solving the Problem (p. 64)). After debonding is completed, the surface inter-
action is governed by standard contact constraints for normal and tangential directions. Frictional contact
is used if friction is specified for contact elements.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               131
Chapter 12: Debonding

12.1.1. Cohesive Zone Materials Used for Debonding
A cohesive zone material model is needed to model debonding in a contact analysis. This material is defined
using the data table method (TB and TBDATA commands). Temperature dependent data is also allowed
(TBTEMP command). On the TB command, use Lab = CZM to denote a cohesive zone material, and use
TBOPT = CBDD or CBDE to indicate the specific material data you will provide. The two data definitions are
described below. For more information on this material, see Cohesive Zone Material Model in the Theory
Reference for the Mechanical APDL and Mechanical Applications.

12.1.1.1. Bilinear Material Behavior with Tractions and Separation Distances (TBOPT
= CBDD)
This is a linear elastic material behavior with linear softening characterized by maximum traction and max-
imum separation. To define this material, use the TB,CZM command with TBOPT = CBDD. Specify the ma-
terial constants as data items C1 through C6 on the TBDATA command:

 Constant           Symbol                                           Meaning
      C1               σmax             maximum normal contact stress
      C2                 c              contact gap at the completion of debonding
                        un

      C3               τmax             maximum equivalent tangential contact stress
      C4                                tangential slip at the completion of debond-
                        uc
                         t
                                        ing
      C5                 η              artificial damping coefficient
      C6                 β              flag for tangential slip under compressive
                                        normal contact stress

Sample command input for this material is shown below.
 TB,CZM,1,2,,CBDD
                   c
                  un             uc
                                  t
 TBDATA,1, max,        , max,         , ,


12.1.1.2. Bilinear Material Behavior with Tractions and Critical Fracture Energies (TBOPT
= CBDE)
This is a linear elastic material behavior with linear softening characterized by maximum traction and critical
energy release rate. To define this material, use the TB,CZM command with TBOPT = CBDE. Specify the
material constants as data items C1, through C6 on the TBDATA command:

 Constant           Symbol                                           Meaning
      C1               σmax             maximum normal contact stress
      C2                Gcn             critical fracture energy for normal separation
      C3               τmax             maximum equivalent tangential contact stress
      C4                Gct             critical fracture energy for tangential slip
      C5                 η              artificial damping coefficient
      C6                 β              flag for tangential slip under compressive
                                        normal contact stress


                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
132                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   12.1.4. Postprocessing

Sample command input for this material is shown below.
 TB,CZM,1,2,,CBDE
 TBDATA,1, max,Gcn, max,Gct, ,


12.1.2. Debonding Modes
Debonding involves separation of surfaces forming an interface. The direction of separation determines the
debonding mode. ANSYS detects the debonding mode based on material data that you input for normal
and tangential directions:

 •   Mode I debonding involves separation normal to the interface. It is activated by inputting data items
     C1, C2, and C5 on the TBDATA command.
 •   Mode II debonding involves slip tangent to the interface. It is activated by inputting data items C3,
     C4, and C5 on the TBDATA command.
 •   Mixed mode debonding involves both normal separation and tangential slip. It is activated by inputting
     data items C1, C2, C3, C4, and C5, and C6 on the TBDATA command.

12.1.3. Other Considerations for Debonding
Artificial Damping

Debonding is generally accompanied by convergence difficulties in the Newton-Raphson solution. Artificial
damping can be used to stabilize the numerical solution. It is activated by specifying the damping coefficient
η (input on TBDATA command as C5 using TB,CZM). The damping coefficient has units of time and should
be smaller than the minimum time step size so that the maximum traction and maximum separation (or
critical fracture energy) values are not exceeded in debonding calculations.

Tangential Slip under Normal Compression

ANSYS provides an option to control tangential slip under compressive normal contact stress for mixed
mode debonding. By default, no tangential slip is allowed for this case, but it can be activated by setting
the flag β to 1 (input on TBDATA command as C6 using TB,CZM).

Pinball Radius and Mesh Density

When using a fine mesh for underlying elements of bonded surfaces, you may need to increase pinball radius
(PINB) for contact elements so that it is greater than the maximum separation value in the normal direction
(contact gap when normal contact stress goes to zero). The default value for PINB is based on the depth of
the underlying element. If PINB is smaller than the maximum separation value, debonding calculations will
be bypassed when the contact gap exceeds PINB.

12.1.4. Postprocessing
All applicable output quantities for contact elements are also available for debonding: normal contact stress
(PRES), tangential contact stress (TAUR, TAUS, SFRIC), contact gap (GAP), tangential slip (TASR, TASS, SLIDE),
etc. In addition, the following debonding specific output quantities are available as NMISC data: debonding
time history (DTSTART), debonding parameter (DPARAM), and critical fracture energy (DENERI, DENERII).

For more information on how to review results in a contact analysis, see Reviewing the Results (p. 65) in
Chapter 3, Surface-to-Surface Contact (p. 11).




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                                 133
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
134                               of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix A. Example 2-D Contact Analysis with Fluid
Pressure-Penetration Loading
This example represents a planar seal compression with applied fluid pressure-penetration loading at the
contact interface. It demonstrates the application of the fluid pressure loads and the propagation of the
fluid penetration path from one starting point into the contact interface.

A.1. Problem Description
The model represents a half symmetry planar hyperelastic seal. Figure A.1: Diagram of Planar Seal Model (p. 135)
shows a diagram of the model, and Figure A.2: Meshed Planar Seal Model (p. 136) shows the meshed half
symmetry model.

Figure A.1: Diagram of Planar Seal Model

                                      0.865 inches
                                         applied
                                      displacement




                        1/2 symmetry




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               135
Appendix A. Example 2-D Contact Analysis with Fluid Pressure-Penetration Loading

Figure A.2: Meshed Planar Seal Model




The seal is compressed by a displacement-controlled load in the first load step. Fluid pressure is applied to
all contact elements in the second load step (see Figure A.3: Fluid Pressure Loading on Planar Seal (p. 136)) so
that the fluid opens and penetrates into the contact interface that was previously closed by compression.

The fluid pressure is applied using the SFE command with the load key set to 1 (LKEY = 1 on SFE). Using
SFE with the load key set to 2 (LKEY = 2 on SFE), all default starting points are suppressed (STA1 = -1) and
two elements are chosen as starting locations initially exposed to the fluid (STA1 = 1). (See Specifying Fluid
Penetration Starting Points (p. 58) for more information on the STA values.) From this location the fluid
penetrates gradually by opening the bottom part of the contact surface, while the top part of the contact
surface completely closes.

Figure A.3: Fluid Pressure Loading on Planar Seal




At the end of the first load step (compression load step) most of the contact is closed as shown in the above
figure. Plots of contact fluid pressure at an intermediate substep of load step 2 and at the end of load step
2 are shown in Figure A.4: Intermediate Fluid Pressure Distribution (p. 137) and Figure A.5: Final Fluid Pressure
Distribution (p. 137).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
136                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                            A.1. Problem Description

Figure A.4: Intermediate Fluid Pressure Distribution




Figure A.5: Final Fluid Pressure Distribution




Three contact elements at the bottom of the seal are used for time history postprocessing, representing
each region that undergoes fluid penetration. Time history results for fluid contact pressure and gap are
printed and plotted to show the path of fluid penetration along the bottom contact elements. The fluid
pressure history is shown in Figure A.6: Time History of Fluid Pressure for Three Contact Elements (p. 138).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                           137
Appendix A. Example 2-D Contact Analysis with Fluid Pressure-Penetration Loading

Figure A.6: Time History of Fluid Pressure for Three Contact Elements




A.2. Input File
 /title,Seal compression with fluid pressure-penetration loading
 /com =====================================================================
 /com   OBJECTIVE:
 /com   The objective of this test is to verify the path of fluid
 /com   penetration pressure with rigid-flex contact
 /com   and CONTA171 default keyoptions.
 /com
 /com   DESCRIPTION:
 /com   The model represents a planar seal that is compressed. Fluid
 /com   pressure is applied to all contact elements so that the fluid
 /com   penetrates and opens the contact that used to be closed by
 /com   compression.
 /com
 /com   The fluid pressure is applied after the compression, and one
 /com   starting point is chosen to be initially in fluid (STA=1 on SFE).
 /com   From this location the fluid penetrates gradually at the bottom
 /com   surface.
 /com
 /com   TEST SPECIFICATIONS:
 /com   SOLID ELEMENTS: PLANE182 - PLANE STRESS
 /com   TARGET ELEMENT: TARGE169
 /com   CONTACT ELEMENT: CONTA171, K(14)=0, K(2)=0, K(4)=0
 /com   MATERIAL MODEL: HYPERELASTIC
 /com
 /com
 /com   RESULTS:
 /com   At the end of load step 1 there are 3 regions where contact is
 /com   closed at the bottom surface. One element from each of these
 /com   regions is chosen, and the time history results for fluid
 /com   contact pressure and gap are printed and plotted to show the
 /com   path of fluid penetration along the bottom contact elements.
 /com   Notice that at the time when the contact opens
 /com   (gap is not zero), the FPRS is nonzero.
 /com =====================================================================

 /prep7



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
138                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    A.2. Input File

et,1,182    ! PLANE182 with plane stress option

tb,HYPER,1,1,2,MOON
tbtemp,0
tbdata,,80,20,0,,,

/com   **** Build the model ****

k,1
k,2,0.333,0
k,3,0.867,0.867
k,4,1.1,0.867
k,5,1.1,1
k,6,0.8,1
k,7,0.267,0.133
k,8,0,0.133
l,1,2
*repeat,7,1,1
l,8,1
lfillt,1,2,0.20
lfillt,2,3,0.15
lfillt,5,6,0.20
lfillt,6,7,0.15
lfillt,7,8,0.05
lfillt,8,1,0.05
al,all
k,98,-1.0,0
k,99,1.1,0
lstr,99,98
k,100,-1.0,1.0
k,101,1.1,1.0
lstr,100,101

lcomb,8,13
lcomb,8,14

esize,0.02    ! Set element attributes and meshing parameters
type,1
mat,1
smrtsize,5

amesh,all    ! Mesh the model
allsel


lsel,s,,,4    ! BCs to model half symmetry
nsll,s,1
d,all,ux,0
allsel

/com   **** Contact pair creation ****

et,2,169
et,3,171
keyopt,3,10,2
mp,mu,2,0.2 ! Friction

r,2

/com   **** Top and bottom rigid targets ****

type,2
real,2
mat,2
lesize,15,,,1
lesize,16,,,1
lmesh,15,16

/com   **** Contact on the planar seal ****

lsel,s,line,,1,12
lsel,u,line,,4


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                         139
Appendix A. Example 2-D Contact Analysis with Fluid Pressure-Penetration Loading

 nsll,s,1
 type,3
 esurf

 allsel,all
 finish

 /solu
 allsel

 esel,s,ename,,169
 nsle
 nsel,r,loc,y,1
 d,all,uy,-0.865 ! Move top rigid target

 nlgeom,on
 time,1
 nsubst,25,2000,5
 outres,all,all
 allsel
 nropt,unsym ! Unsymmetric due to friction
 solve

 esel,s,ename,,171 ! Select only contact elements
 sfe,all,1,PRES, ,150 ! Apply fluid pressure of 150 to all contact elements
 sfe,all,2,pres,,-1 ! Suppress default starting points (STA1 = -1)

 nsel,s,loc,x ! Select a location for starting points
 esln
 esel,r,ename,,171 ! Reselect only the contact elements
 sfe,all,2,pres,,1 ! Specify the above location to be initially in fluid (STA1 = 1]

 allsel

 nsubst,100,1000,10
 solve
 finish

 /com   **** Post1 postprocessing ****

 /post1
 /show
 set,2,last
 finish

 /com   **** Post26 time history postprocessing ****

 /post26
 timerange,1,2

 esol,2,523,138 ,cont,fprs,CONTFPRS1
 esol,3,523,138 ,cont,gap,CONTGAP1
 /com *****************************************************************************
 /com History of contact gap and fluid pressure for an element in the
 /com region that opens first
 /com *****************************************************************************
 prvar,2,3
 esol,4,578,53 ,cont,fprs,CONTFPRS2
 esol,5,578,53 ,cont,gap,CONTGAP2
 /com ****************************************************************************
 /com History of contact gap and fluid pressure for an element in the
 /com region that opens later
 /com *****************************************************************************
 prvar,4,5
 esol,6,517,6,cont,fprs,CONTFPRS3
 esol,7,517,6,cont,gap,CONTGAP3
 /com ****************************************************************************
 /com History of contact gap and fluid pressure for contact element
 /com that opens last
 /com *****************************************************************************
 prvar,6,7



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
140                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                 A.2. Input File

/title,Time history of fluid pressure for three contact elements
/axlab,y,Fluid pressure
plvar,2,4,6

finish




                   Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                               of ANSYS, Inc. and its subsidiaries and affiliates.                                         141
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
142                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                 line-to-surface, 79
Index                                                                            localized contact zone, 20
                                                                                 magnetic contact, 89
                                                                                 moving contact nodes, 47
B                                                                                node ordering in node-to-node analysis, 93
beam-to-beam contact, 73
                                                                                 node-to-node, 2, 4, 91
                                                                                 node-to-surface, 2, 4, 69
C                                                                                node-to-surface KEYOPTS, 70
contact analysis, 1                                                              node-to-surface real constants, 71
  asymmetric vs. symmetric contact, 14                                           normals, 7, 20, 23, 93
  beam-to-beam, 2, 73                                                            open far-field contact status, 48
  birth and death option, 55                                                     open near-field contact status, 48
  boundary conditions for node-to-node contact, 95                               overall steps, 11
  boundary conditions for surface-to-surface contact,                            overconstrained contact problem, 95
  56                                                                             penalty stiffness, 23
  chattering controls, 30                                                        penetration, 30
  choosing surfaces, 13                                                          piezoelectric elements, 87
  conduction, 84                                                                 pinball region, 48
  contact algorithm, 30, 95                                                      point-to-point, 4
  contact direction, 20                                                          point-to-surface, 4
  contact location detection, 39                                                 radiation, 85
  Contact Manager, 7, 11                                                         results, 65
  contact pairs, 9, 12                                                           rigid-to-flexible, 1, 11, 55
  contact status, 48, 83                                                         self contact, 14, 49
  contact stiffness, 30–31                                                       shells, 54
  contact surface elements, 3                                                    sliding contact status, 48
  Contact Wizard, 8                                                              slippage, 39
  convection, 85                                                                 solution options for node-to-node contact, 96
  debonding, 131                                                                 solution options for surface-to-surface contact, 63
  deformable contact surface, 21                                                 solving, 64
  direct generation to create rigid target elements, 16                          spurious contact, 49
  electric contact, 87                                                           Stefan-Boltzmann constant, 85
  electrostatic elements, 87                                                     sticking contact status, 48
  emissivity, 85                                                                 summary of contact capabilities, 2
  explicit dynamics, 1                                                           superelements, 53
  flexible-to-flexible, 1, 11                                                    surface interaction for electric contact, 88
  fluid pressure-penetration loads for surface-to-sur-                           surface interaction models, 50
  face contact, 56                                                               surface-to-surface, 2–3, 11, 22
  free surface convection, 84                                                    surface-to-surface KEYOPTS, 28
  free surface radiation, 84                                                     surface-to-surface material properties, 23
  free thermal surface, 84                                                       surface-to-surface real constants, 23–24
  friction model, 35                                                             symmetric/unsymmetric solver, 35
  gap, 95                                                                        target element shapes, 16
  Gauss integration points, 39                                                   target surface definition, 15
  generating node-to-node contact elements, 92                                   target surface element types and real constants, 15
  generating surface-to-surface contact elements, 23                             target surface modeling and meshing tips, 20
  heat flux, 84, 87                                                              target surface nodal number ordering, 20
  heat generation due to electric current, 88                                    target surface pilot node, 15, 55
  heat generation due to friction, 86                                            target surface primitives, 15
  initial contact conditions, 41                                                 temperature required, 84
  initial interference, 95                                                       thermal contact, 83
  internal MPC, 99                                                               thickness effect, 54
  line-to-line, 4

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               143
Index

    time step control, 54
    using meshing tools to create rigid target elements,
    17

D
debonding, 131
delamination
  in a contact analysis, 131

F
fluid pressure-penetration loads, 56

I
internal MPC, 99

L
line-to-surface contact, 79

M
magnetic analysis
  contact, 89
multipoint constraint, 99

P
penalty stiffness
   in contact analysis, 23
pilot node
   in contact analysis, 15, 55

S
spot welds, 119




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
144                                                 of ANSYS, Inc. and its subsidiaries and affiliates.

				
DOCUMENT INFO
Categories:
Tags:
Stats:
views:16
posted:8/22/2012
language:English
pages:152
Subrahmanian KR Subrahmanian KR
About Civil Engineer