details on this topic, and in particular, see Element Selection (p. 319) for a table of corresponding
structural and interface elements.- Define material. Use TB,GASKET to define the gasket joint material. You can use TB,GASKET to
define four types of data input: general parameters, transverse shear stiffness, compression (loading),
and tension (unloading).You specify the type using TBOPT. You then input the sets of data using
the TBDATA and TBPT commands, as applicable. You can also plot most of the gasket data types
using the TBPLOT command. See Material Definition (p. 320) in this chapter for more details on this
topic. - Mesh the model. Use the AMESH or VMESH commands to mesh the structural element types, and
use the IMESH command to mesh the gasket layer. Special restrictions apply to the IMESH command
in terms of matching the source and target. Also, the order in which you execute these commands
is critical. You can also mesh interface layers using the VDRAG command, and can generat e interface
elements directly using the EGEN command. Each of these commands involve special considerations
for interface elements. See Meshing Interface Elements (p. 327) in this chapter for more details on
this topic. - Solve.There are special solving considerations when you perform a gasket joint analysis. These are
primarily concerned with the gasket element stiffness loss, and the gasket element's use with contact
elements. See Solution Procedure and Result Output (p. 331) in this chapter for more details on this
topic. - Review Results.You can print or plot any of four gasket output items: stresses (also pressure), total
closure, total inelastic closure, and thermal closure, using the PRESOL,PRNSOL,PLESOL,PLNSOL,
or ESOL commands. You can also use these items with the *GET command in POST1. See Reviewing
the Results (p. 333) in this chapter for more details on this topic.
10.2. Finite Element Formulation
The primary deformation behavior of gasket joints is through-thickness deformation. It is therefore dif-
ficult to use solid continuum elements to effectively model gasket joints. The interface elements, which
are based on the relative deformation of the top and bottom surfaces, offer a direct means to quantify
through-thickness deformation of the gasket joints. Thus the pressure versus closure behavior can be
directly applied to characterize the gasket material.
The element formulation is based on a corotational procedure. Refer to Gasket Material in the Mechan-
ical APDL Theory Reference for further details.
10.2.1. Element Topologies
An interface element is composed of bottom and top surfaces. ANSYS provides several types of interface
elements for the analysis of the gasket joints.Figure 10.1: Element Topology of a 3-D 8-Node Interface
Element (p. 319) shows the geometry of a 3-D 8-node interface element available in ANSYS. An element
midplane is created by averaging the coordinates of node pairs from the bottom and top surfaces of
the elements. The numerical integration of interface elements is performed in the element midplane.
The Gauss integration scheme is used for the numerical integration.
Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential informationGasket Joints Simulation