Analyzing gaskets with Simcenter Nastran

In Simcenter Nastran, you can analyze gaskets in advanced nonlinear analyses (SOL 601, 106 and SOL 601, 129). Though most gaskets are flat, you can use Simcenter Nastran to analyze any type of gasket geometry. The following sections describe the special considerations for performing a gasket analysis in Pre/Post with the Simcenter Nastran solver.

Defining a mesh for a gasket model

In Simcenter Nastran, you model gaskets with solid, linear CHEXA or CPENTA elements. The mesh must contain only one layer of elements through the thickness of the gasket itself. In Pre/Post, to create a mesh of CHEXA8 elements, use either the 3D Swept Mesh or Element Extrude command. When you sweep the mesh, if the mesh on the source face contains any CTRIA3 elements, the software also creates CPENTA elements.

Connecting the gasket to the surrounding components

In Simcenter Nastran, you have the following choices for how to model the relationship between the gasket and the surrounding (mating) structural components:

• The gasket can share a common surface with the mating surface. However, in this case, the gasket cannot separate from its target during the analysis. When you mesh the components, the gasket and the mating surface must share common nodes. You can use the Mesh Mating Condition command to ensure that the surfaces share nodes.

• The top and bottom surfaces of the gasket can be separate from the surrounding components. This allows the gasket to separate from its target during the analysis without putting the gasket into tension. In this case, you must connect the gasket to its mating surfaces through an Advanced Nonlinear Contact simulation object.

• The nodes on the gasket mesh can be connected to the nodes on the surrounding components by tied contact or a glue connection. A solution with this type of connection is faster than a solution that uses Advanced Nonlinear Contact to define the connection, but this type of connection does allow the gasket to be put into tension.To define tied contact between the gasket and mating surfaces, first create a Contact Set Parameters modeling object and set the Contact Regions in Each Pair option to Tied. Then, in the Advanced Nonlinear Contact dialog box, select that modeling object from the Contact Set Parameters list.To create a glue connection between the gasket and mating surfaces, create a Surface-to-Surface Gluing simulation object.

Defining a gasket material

In Simcenter Nastran, you use a special gasket material (MATG bulk data entry) to assign a gasket's membrane and through-thickness properties. The MATG entry defines the compressive behavior for the gasket in the thickness direction.

In Pre/Post, you can use the Gasket option in the Type list in the Assign Material dialog box to create a MATG entry. Then, you can use the following options in the Gasket Material dialog box to define the following properties that are required for a MATG entry:

• Use the Membrane Material option to specify the isotropic material that defines the material behavior for the membrane (in-plane) direction. This corresponds to the IDMEM field in the MATG entry. In Simcenter Nastran, you must use a MATG entry together with an elastic isotropic material (MAT1 bulk data entry) to define the gasket's in-plane properties.

• Use the Yield Pressure (YPRESS) option to specify the initial yield pressure for the gasket. This value must match a point on the specified Loading Curve.

• Use the Tensile Modulus (EPL) option to define the tensile modulus (force per volume mN/mm3).

• Use the Transverse Shear Modulus (GPL) option to define the transverse shear modulus (force per unit area).

• Use the Loading Curve option to specify a field that defines the loading curve of the gasket (pressure vs. closure).

• Use the Unloading Curve options to specify fields that define one or more unloading curves for the gasket. You must specify at least one unloading curve. All unloading curves must have the same number of points as the elastic portion of the loading curve (up to the defined initial yield pressure). The first point must be defined at pressure 0.0 and the last point must coincide with a yield point on the loading curve.

Requesting gasket results output

In Simcenter Nastran, you use a GKRESULTS Case Control command to request gasket-specific output from an analysis. In Pre/Post, use the options on the Gasket Result page in the Structural Output Requests dialog box to request the output of gasket results. Gasket results include gasket pressure, gasket closure, plastic gasket closure, gasket yield stress, and gasket status.

Reviewing gasket results

Once you solve your model, you can view results such as the displacements, stresses, strains, and reaction forces, as well as gasket-specific results, such as gasket pressure, in the Post Processing Navigator.

Viewing Simcenter Nastran gasket status in Pre/Post post-processing

In the Post Processing Navigator, gasket status is an elemental, scalar result, in which each element is assigned an integer value between 0 and 6. These integer values correspond to the gasket status shown in the .f06 file as follows:

Pre/Post post-processing	Nastran .f06
0	Open
1	Not used
2	Closed
3	Not used
4	Sealed
5	Leaked
6	Crushed

In the following figure, the elements in orange have a gasket status of Leaked. The elements in blue have the status Open.

Additional reference material

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

• MATG in the Simcenter Nastran Quick Reference Guide

• GKRESULTS in the Simcenter Nastran Quick Reference Guide

• Gasket material model in the Simcenter Nastran Advanced Nonlinear Solution – Theory and Modeling Guide

Learn more

Gasket analysis

Analyzing gaskets with Abaqus

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 Simcenter Nastran, 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 } });