Analyzing gaskets with ANSYS

In ANSYS, the overall process for performing a gasket joint analysis is the same as the process for performing any ANSYS nonlinear statics analysis. The following sections describe the special considerations for performing a gasket analysis in Pre/Post with the ANSYS solver.

Creating a mesh on a gasket model

In ANSYS, you model gaskets using interface elements. Pre/Post supports the INTER195 gasket element. You can use the 3D Swept Mesh command to create INTER195 elements. To mesh the structural components on either side of the gasket, you should use SOLID185 elements.

Connecting gasket elements to the surrounding components

In ANSYS, the faces of the elements on the top and bottom of the gasket must be in contact with the element faces on the surrounding components. There are two different ways to ensure that contact occurs:

• The gasket and the mating surfaces can share common nodes. In Pre/Post, you can use the Mesh Mating Condition command to ensure that the surfaces share nodes when you mesh the components. This is the preferred method for establishing contact between a gasket and the surrounding components.

• You can create a Surface-to-Surface Contact simulation object or a CE type of Manual Coupling simulation object to establish contact between the interface elements and the elements on the surrounding components.

Defining a gasket material

In ANSYS, you use a gasket material (TB command with the GASKET option) to assign a gasket's transverse and through-thickness properties. In Pre/Post, you first select the Gasket option in the Type list in the Assign Material dialog box. Then, you use the following options in the Gasket Material dialog box to define the following general parameters for a TB, GASKET command

• Use the Initial Gap option to specify the initial gap for the gasket. A value of 0 indicates that there is no initial gap.

• Use the Stable Stiffness option to specify the stable stiffness for the gasket. A value of 0 indicates that there is no stable stiffness.

• Use the Maximum Tension Stress option to specify the maximum tension stress value allowed when the gasket material is in tension. A value of 0 indicates that there is no tension stress in the gasket material.

• Use the Loading Curve option to specify a field that defines the loading (compression) curve of the gasket material.

• Use the Unloading Curve options to specify fields that define the unloading behavior of the gasket material. If you define more than one unloading curve, ANSYS requires that the starting point of each unloading curve be on the compression curve. This ensures that the unloading behavior is correctly simulated.

Reviewing gasket results

Once you solve your model, you can view results such as the displacements, stresses, strains, and reaction forces in the Post Processing Navigator. Currently, you cannot use the Post Processing Navigator to view gasket joint-specific results, such as gasket pressure and closure.

Additional reference material

For more information on modeling and analyzing gaskets with ANSYS, see:

• Performing a Gasket Joint Analysis in the ANSYS Structural Analysis Reference Guide

• Generating an Interface Mesh for Gasket Simulations in the ANSYS Modeling and Meshing Guide

Learn more

Gasket analysis

Analyzing gaskets with Simcenter Nastran

Analyzing gaskets with Abaqus

Analyzing gaskets with Simcenter Samcef

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Analyzing gaskets with 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 } });