Analyzing gaskets with Abaqus

In Abaqus, you use gasket elements to model gaskets and other types of seals between structural components. The following sections describe the special considerations for performing a gasket analysis in Pre/Post with the Abaqus solver.

Defining a Gasket Section physical property table

In Abaqus, you use a *GASKET SECTION keyword to define the properties of gasket elements. In Pre/Post, you create a gasket section physical property table (Gasket Section or Line Gasket Section, depending on the type of gasket element). The gasket section physical table defines all the necessary properties for the *GASKET SECTION keyword. You can define a gasket section physical property table either before or after you create the gasket elements.

In a gasket section dialog box, the Type list controls how the gasket's behavior is defined.

• If you select Material, you can define the gasket's behavior using a material model. When you click Choose Material, you can use the Assign Material dialog box to specify an isotropic, orthotropic, or anisotropic material. For more information, see Defining the gasket behavior using a material model in the Abaqus Analysis User's Manual.

• If you select Behavior, you can define the gasket's behavior using a gasket behavior model. When you click Choose Material, you can use the Gasket Behavior Material dialog box to directly define the gasket behavior. In the Gasket Behavior Material dialog box, you use:The Gasket Elasticity options to specify elastic properties for the membrane and transverse shear behaviors of a gasket. These options correspond to the *GASKET ELASTICITY keyword in Abaqus.The Gasket Thickness Behavior options to define the behavior in the thickness direction for a gasket.For more information, see Defining the gasket behavior directly using a gasket behavior model in the Abaqus Analysis User's Manual.

Creating a mesh for a gasket analysis

In Abaqus, gasket elements are small-strain, small-displacement elements, though you can use them in large-displacement analyses. For Abaqus analyses, you can model gaskets as either a single layer of gasket elements or as multiple layers of gasket elements in the gasket thickness direction. In Pre/Post, you can create the following types of Abaqus gasket elements:

Abaqus Element	Description
GK3D4L	4-noded, three-dimensional line gasket element
GK3D4LN	4-noded, three-dimensional line gasket element with thickness-direction behavior only
GK3D6	6-noded, three-dimensional gasket element
GK3D6N	6-noded, three-dimensional gasket element with thickness-direction behavior only
GK3D8	8-noded, three-dimensional gasket element
GK3D8N	8-noded, three-dimensional gasket element with thickness-direction behavior only

How you create the gasket elements depends upon the element's type:

• To create GK3D4L and GK3D4LN type elements, use the 2D Mesh command. Then, use the Element Formulation option in the Mesh Associated Data dialog box to specify the element type: standard (GK3D4L) or thickness behavior only (GK3D4LN). You can also define the gasket behavior directly using the Line Gasket Section Physical Property Table.

• To create GK3D8 or GK3D8N type elements, use the 3D Swept Mesh command.You can also define the gasket behavior directly using the Gasket Section Physical Property Table.

• To create GK3D6 or GK3D6N type elements, first use the 2D Mesh command to create a mesh of either linear or parabolic triangular elements. Then, use the 3D Swept Mesh command to generate the GK3D6 or GK3D6N elements.

Note:

When you generate the gasket elements, ensure that their destination mesh collector is associated with the appropriate Gasket Section orLine Gasket Section physical property table.

For more information on modeling gaskets in Abaqus and on gasket-specific elements, see Gasket elements in the Abaqus Analysis User's Manual.

Connecting gasket elements to the surrounding components

In Abaqus, 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:

• If you are working with GK3D8 or GK3D6 elements, 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.

• If you are working with any type of Abaqus gasket element, you can create a Surface-to-Surface Contact, Automatic Coupling, or Manual Coupling simulation object to establish contact between the gasket elements and the elements on the surrounding components.

For more information on connecting gasket components, see Assembling gaskets to other components in a model in the Abaqus Analysis User's Manual.

Learn more

Gasket analysis

Analyzing gaskets with Simcenter Nastran

Analyzing gaskets with ANSYS

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 Abaqus, 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 } });