Gasket results are structural results associated with Ansys interface elements. When used with Ansys structural elements, interface elements simulate an interface between two materials. The behavior at these interfaces is highly nonlinear.
To mesh a body using interface elements, use one of two ways:
Highlight the Body object in the tree and set Stiffness Behavior to Gasket. In this case, a Gasket Mesh Control will be added as a child of the gasket body in the model tree. You need to define the source face of the gasket in the Gasket Mesh Control to define the gasket material orientation.
Highlight the Body object in the tree and set the Stiffness Behavior to Flexible. In this case, you need to define a Gasket Mesh Control in the mesh folder.
The following gasket results are available in the Mechanical Application:
Normal Gasket Pressure - corresponding to Mechanical APDL command PLNSOL,GKS,X
Shear Gasket Pressure - corresponding to Mechanical APDL commands PLNSOL,GKS,XY and PLNSOL,GKS,XZ
Normal Gasket Total Closure - corresponding to Mechanical APDL command PLNSOL,GKD,X
Shear Gasket Total Closure - corresponding to Mechanical APDL commands PLNSOL,GKD,XY and PLNSOL,GKD,XZ
These results are only available in the solution coordinate system.
Warning: Mechanical only supports the above gasket results. Note that there is a Mechanical APDL key option (KEYOPT(8)=1) that enables you to produce gasket results for standard stresses and strains (S, EPEL, and EPTH) on the interface elements. Mechanical gasket results do not support this key option and produce results with values of only zero. However, if you have the keyopt enabled, you can use a Commands (APDL) object to independently produce these stress results using the /POST1 command.
In addition, when using KEYOPT(8)=1, all Elemental Coordinate Systems results will incorrectly display in the Global Coordinate System.
Review the individual element references for the Ansys interface elements for KEYOPT(8) element output quantities.