2-D 6-Node
Gasket
INTER193 Element Description
INTER193 is a 2-D 6-node quadratic interface element used for 2-D structural assembly modeling. When used in conjunction with 2-D quadratic structural elements (such as PLANE183), INTER193 is used to simulate gasket joints. The element can be used either as a plane element (plane stress or plane strain) or as an axisymmetric element. It is defined by six nodes having two degrees of freedom at each node: translations in the nodal x and y directions.
See Gasket Material and INTER193 in the Mechanical APDL Theory Reference for more details about this element.
Also see Gasket Joints Simulation in the Structural Analysis Guide for more details on the gasket capability in ANSYS.
INTER193 Input Data
The element geometry, node locations, connectivity, and the nodal coordinate system are shown in Figure 193.1: INTER193 Geometry. The element geometry is defined by 6 nodes, which form bottom and top lines of the element. The bottom line is defined by nodes I, J, M; and the top line is defined by nodes K, L, O. The element connectivity is defined as I, J, K, L, M, O. This element has 2 integration points. Dropping mid side nodes M or O is not permitted.
Temperatures may be input as element body loads at the nodes. The node I temperature T(I), defaults to TUNIF. If all other temperatures are unspecified, they default to T(I). For any other input pattern, unspecified temperatures default to TUNIF.
Input the nodal forces, if any, per unit of depth for a plane analysis (except for KEYOPT(3) = 3) and on a full 360° basis for an axisymmetric analysis.
By default, the element adopts a full-integration scheme (KEYOPT(4) = 2), and is capable of both through-thickness and transverse shear deformations (KEYOPT(2) = 1). The full-integration scheme and the inclusion of transverse shear stiffness are generally required when the interfaces between the gasket and the mating parts are modeled as sliding contact. However, if the interfaces are modeled with a matching mesh method (that is, with coincident nodes), ANSYS, Inc. recommends using the reduced integration scheme (KEYOPT(4) = 0) and through-thickness deformation only (KEYOPT(2) = 0) to achieve better efficiency and to avoid unnecessary in-plane interaction between the gasket and the mating parts.
The next table summarizes the element input. See Element Input in the Element Reference for a general description of element input.
INTER193 Input Summary
- Nodes
I, J, K, L, M, , O
- Degrees of Freedom
UX, UY
- Real Constants
None, if KEYOPT(3) = 0, 1, or 2 THK - Plane stress with thickness, if KEYOPT(3) = 3 - Material Properties
TB command: Gasket material
MP command: BETD, ALPX (or CTEX or THSX), DMPR
- Body Loads
- Temperatures --
T(I), T(J), T(K), T(L), T(M), T(O)
- Special Features
Linear perturbation - KEYOPT(2)
Element deformation:
- 0 --
Through-thickness deformation only
- 1 --
Through-thickness and transverse shear deformation (default)
- KEYOPT(3)
Element behavior:
- 0 --
Plane stress
- 1 --
Axisymmetric
- 2 --
Plane strain (Z strain = 0.0)
- 3 --
Plane stress with thickness (THK) real constant input
- KEYOPT(4)
Element technology:
- 0 --
Uniform reduced integration
- 2 --
Full integration (default)
- KEYOPT(8)
Element component quantity output:
- 0 --
Gasket quantities are output (GKD, GKD, GKI, and GKTH) (default)
- 1 --
Standard stresses and strains are output (including S, EPEL, and EPTH )
INTER193 Output Data
The solution output associated with the element is in two forms:
Nodal items such as nodal displacements are included in the overall nodal solution.
Element items such as stresses and closures are element outputs as shown in Table 193.1: INTER193 Element Output Definitions.
The output directions for element items are parallel to the local element coordinate system based on the element midplane as illustrated in Figure 193.2: INTER193 Stress Output. See Gasket Material in the Mechanical APDL Theory Reference for details.
A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to review results.
The Element Output Definitions table uses the following notation:
A colon (:) in the Name column indicates that the item can be accessed by the Component Name method (ESOL). The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availability of the items in the results file.
In either the O or R columns, “Y” indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.
Table 193.1: INTER193 Element Output Definitions
| Name | Definition | O | R |
|---|---|---|---|
| EL | Element number | - | Y |
| NODES | Node connectivity - I, J, K, L, M, O | - | Y |
| MAT | Material number | - | Y |
| TEMP | Temperatures T(I), T(J), T(K), T(L), T(M), T(O) | - | Y |
| GKS:X, (XY) |
X - Normal stress (also gasket pressure) XY - Transverse shear stress | Y | Y |
| GKD:X, (XY) |
X - Total closure XY - Relative transverse shear deformation ( | Y | Y |
| GKDI:X, (XY) | Total inelastic closure | Y | Y |
| GKTH:X, (XY) | Thermal closure | Y | Y |
| S:X, Y, Z, XY | Stresses (SZ = 0.0 for plane stress elements) | - | 1 |
| S:INT | Stress intensity | - | 1 |
| S:EQV | Equivalent stress | - | 1 |
| EPEL:X, Y, Z, XY | Elastic strains | - | 1 |
| EPEL:EQV | Equivalent elastic strain | - | 1 |
| EPTH:X, Y, Z, XY | Thermal strains | - | 1 |
| EPTH:EQV | Equivalent thermal strain | - | 1 |
| SEND:ELASTIC | Strain energy densities | - | 1 |
INTER193 Assumptions and Restrictions
This element is not supported for initial stress.
Pressure as a type of surface load on element faces is not supported by this element.
This element is based on the local coordinate system; therefore, setting an element coordinate system attribute pointer (ESYS) is not supported.