Use this interface ... with one of these structural elements:
element:For elements with
these characterist-
ics:
2-D, quadratic INTER193 PLANE183
3-D, quadratic INTER194 SOLID96,SOLID186,SOLID187
SOLID65,SOLID185,SOLSH190,SOLID272,SOLID272,
SOLID2853-D, linear INTER195Proper element type is chosen based on the stress states of interest and structural element types used.
Element selection is done by the element type command,ET, for example,
ET,1,195defines element type 1 as element INTER195.
10.3.2. Applications
In general, linear and quadratic elements are chosen for the following reasons:
- Fewer nodes produce a smaller model that runs faster with less computer resources.
- Quadratic elements are necessary if stress gradients are present in surrounding bodies.
- If elements are to follow a curved boundary closely, quadratic elements are ideal because their edges
are arcs. - With a free mesh (tetrahedral elements) the mid-node (quadratic) is required for an accurat e solution.
When a surrounding structure can be considered as a 2-D structure, for example, plane stress / strain
/ axisymmetric, 2-D elements are the ideal choice. A good example of the use of 2-D element INTER192
or INTER193 is the gasket between the "flanged" ends of pipe line. In this case the gasket properties
do not vary significantly with geometric location.
For a 3-D structure such as an internal combustion engine, 3-D element INTER194 or INTER195 is a good
choice for simulating the gasket between the cylinder head and block. In this case there is no "nice"
geometry because the gasket must fill in between two complicated surfaces, in between cylinders, and
around other holes and passages. Also the gasket properties can vary in different zones. For example
in a cylinder head, there is usually a much stiffer zone immediately around the cylinder to contain
combustion pressure (called the "fire ring"). The remainder of the gasket is much softer.
10.4. Material Definition
10.4.1. Material Characteristics
The TB command option GASKET allows gasket joints to be simulated with the ANSYS interface elements,
in which there is only one element through the thickness, and the through thickness deformation is
decoupled from the in plane deformation. The gasket material is usually under compression. The mater-
ial under compression is highly nonlinear. The gasket material also exhibits quite complicated unloading
behavior when compression is released. The GASKET option allows you to directly input data for the
experimentally measured complex pressure closure curve for the material model (compression curve),
and also for several unloading pressure closure curves. When no unloading curves are defined, the
material behavior follows the compression curve while it is unloaded.
Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential informationGasket Joints Simulation