Surface-to-Surface Contact (Simcenter Nastran, Simcenter 3D Multiphysics, Abaqus, ANSYS)

Video: Create surface-to-surface contact and regions

Surface-to-Surface Contact lets you define contact between two surfaces.

These solvers and solution types support Surface-to-Surface Contact:

Solver	Supported Solution Types
Simcenter Nastran	SOL 101 Linear Statics (Global Constraints and Subcase Constraints)SOL 103 Real Eigenvalues and SOL 103 Response DynamicsSOL 105 Linear BucklingSOL 107 Direct Complex EigenvaluesSOL 110 Modal Complex EigenvaluesSOL 111 Modal Frequency ResponseSOL 112 Modal Transient ResponseSOL 200 Design OptimizationSOL 200 Topology OptimizationSOL 401 Multi-Step NonlinearSOL 402 Multi-Step Nonlinear KinematicsSOL 601,106 Advanced Nonlinear Statics and SOL 601,129 Advanced Nonlinear TransientSOL 701 Explicit Advanced Nonlinear Analysis
Multiphysics	Structural (Multi-Step Nonlinear)Thermal-Structural (Multi-Step Nonlinear)
ANSYS	Linear StaticsNonlinear StaticsThermalFor more information, see Structural Contact (ANSYS) and Thermal Contact (ANSYS).
Abaqus	Structural – General AnalysisDynamic ExplicitCoupled Thermal-StructuralNote: For Abaqus Thermal-Heat Transfer and Dynamic Coupled Thermal-Structural analyses, you can use the Surface-to-Surface Thermal Conductance command to model conductive heat transfer between proximate or contacting surfaces. For more information, see Surface-to-Surface Thermal Conductance (Abaqus).
LS-DYNA	General Impact

Defining the contacting surfaces

You can either specify the contacting surfaces manually, or you can have the software automatically determine which pairs of faces come in contact with each other.

• To manually specify source and target surfaces in the contact definition, you can select an existing Simulation Region or create a new one. For more information, see Working with reusable regions.

• To have the software automatically determine the contacting surfaces, you can use the Create Automatic Face Pairs dialog box to specify the criteria the software uses to search for surfaces. For more information, see Automatic face pairing

Additional contact parameters available for Nastran or Multiphysics analyses

If you are working with Nastran (SOL 101, SOL 103, SOL 111, SOL 112, and SOL 401) or Multiphysics as your solver, you can create a Contact Parameters – Linear Global modeling object to define additional parameters to control the contact algorithm. This modeling object corresponds to the Nastran BCTPARM bulk entry. You then use the Global Contact Parameters option on the Case Control page (for Simcenter Nastran) or Solution Control page (for Multiphysics) of the Solution dialog box to include the Contact Parameters modeling object in your solution.

For more information, see:

• Contact Parameters–Global Pair dialog box

• BCTPARM in the Simcenter Nastran Quick Reference Guide

• Contact for Linear Solutions in the Simcenter Nastran User's Guide

If you are working with a Simcenter Nastran multi-step nonlinear kinematics analysis (SOL 402), you can create a Contact Parameters – Multi-Step Nonlinear Kinematics Pair modeling object to define contact parameters such as penetration, gap, distance, offset, and so on. The options correspond to the parameters in the BCTPAR2 bulk entry.

Additional contact parameters available for Abaqus analyses

If you are working with Abaqus as your solver, the contact parameters depend on the type of analysis and whether you are defining the surfaces manually or automatically.

• Contact parameters****Structural analysesFor Abaqus Structural analyses, you can create a Contact Pair modeling object to define additional parameters to control the contact algorithm for each solution step. You then use the Contact Pair option in the Surface-to-Surface Contact dialog box to apply those parameters to the contact definition. A Contact Pair modeling object corresponds to the Abaqus CONTACT PAIR, CPSET keyword. For Structural analyses, you can also change the friction properties of contact pair interactions, and change the friction definition for each solution step. Use the Abaqus Change Friction Definition modeling object to define friction.Defining contact pairs (Abaqus Structural and Thermal analyses)CONTACT PAIR* in the *Abaqus Keywords GuideDefining contact interaction analysis: overview* in the Abaqus Analysis Guide*Dynamic Explicit analyses**For Abaqus Dynamic Explicit analyses, you can create a Contact Property modeling object to manage the properties, interactions, and behaviors of the Surface-to-Surface Contact. You then use the Contact Property option in the Surface-to-Surface Contact dialog box to apply those parameters to the contact definition, including defining an initial clearance for the first step of the solution. A Contact Property modeling object corresponds to the Abaqus *CONTACT PAIR keyword.The Contact Property modeling object can include the Surface Interaction modeling object to define a mechanical surface interaction model, cohesive behavior, and damage modeling. A Surface Interaction modeling object corresponds to the Abaqus *SURFACE INTERACTION keyword. The Surface Interaction modeling object, in turn, can include the Friction, Surface Behavior, Cohesive Behavior, Damage Initiation, and Damage Evolution modeling objects.Defining contact properties (Abaqus Dynamic Explicit analyses)CONTACT PAIR* in the *Abaqus Keywords GuideMechanical contact properties* in the Abaqus Analysis Guide

• Contact surface smoothingFor Abaqus Structural and Coupled Thermal-Structural analyses, when defining the surfaces manually, you can create a Surface Smoothing modeling object to specify the method to use to improve the contact stress and pressure accuracy for axisymmetric, or nearly axisymmetric, surfaces. Three smoothing techniques are available: circumferential, spherical, and toroidal. You use the Surface Smoothing option in the Surface-to-Surface Contact dialog box to apply the contact smoothing properties to the master/slave surface pair. A Surface Smoothing modeling object corresponds to the Abaqus SURFACE SMOOTHING parameter to the *CONTACT PAIR keyword.

Surface-to-Surface Contact compared to Surface Contact Mesh

When the solution is set to the Nastran solution type SOL 101, there are two commands for defining surface contact:

• Surface-to-Surface Contact, when a Simulation file is active.

• Surface Contact Mesh, a legacy command, when a FEM file is active.

You should use Surface-to-Surface Contact to define contact between two surfaces. Unlike Surface-to-Surface Contact, Surface Contact Mesh generates contact (or gap) elements between the two surfaces. See Surface Contact Mesh for more information.

Where do I find it?

Application	Pre/Post
Prerequisites	A Simulation file as the work part and displayed part Simcenter Nastran, Simcenter 3D Multiphysics, Abaqus, or ANSYS as the specified solver
Command Finder	Surface-to-Surface Contact

How do I

Define surface-to-surface contact

Define surface-to-surface gluing (Simcenter Nastran)

Define edge-to-surface gluing

Create an axisymmetric nonlinear contact

Learn more

Contact and glue overview (Simcenter Nastran, Simcenter 3D Multiphysics)

Defining parameters for contact conditions (Simcenter Nastran)

Defining parameters for glue conditions

Previewing contact and glue element locations (Simcenter Nastran)

Surface-to-surface gluing (Simcenter Nastran, Simcenter 3D Multiphysics)

Edge-to-Edge Contact (Simcenter Nastran, Simcenter 3D Multiphysics)

Internal edges for source and target regions

Edge-to-Surface Gluing (Simcenter Nastran)

Controlling the stiffness of edge-to-surface glue (Simcenter Nastran)

Edge-to-Edge Gluing (Simcenter Nastran, Simcenter 3D Multiphysics)

Advanced nonlinear contact for axisymmetric elements (Simcenter Nastran)

Automatic face pairing

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Surface-to-Surface Contact (Simcenter Nastran, Simcenter 3D Multiphysics, Abaqus, ANSYS), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });