INTER192
## INTER192 Element Description

## INTER192 Input Data

### INTER192 Input Summary

## INTER192 Output Data

## INTER192 Assumptions and Restrictions

**2-D 4-Node Gasket**

Compatible Products: – | – | – | Enterprise | Ent PP | Ent Solver | –

INTER192 is a 2-D four-node linear interface element used for 2-D structural assembly modeling. When used with 2-D linear structural elements (such as PLANE182), INTER192 simulates 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 four nodes having two degrees of freedom at each node: translations in the nodal x and y directions.

See Gasket Material and
INTER192 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.

The element geometry, node locations, connectivity, and the nodal coordinate system are shown in Figure 192.1: INTER192 Geometry. The element geometry is defined by 4 nodes, which form bottom and top lines of the element. The bottom line is defined by nodes I, J; and the top line is defined by nodes K, L. The element connectivity is defined as I, J, K, L. This element has 2 integration points. The Gauss integration scheme is used for the numerical integration.

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 is capable of both through-thickness and transverse shear deformations (KEYOPT(2) = 1). The inclusion of transverse shear stiffness is 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 through-thickness deformation only (KEYOPT(2) = 0) to avoid unnecessary in-plane interaction between the gasket and the mating parts.

The following table summarizes the element input. See the Element Input section in the *Element Reference* for a general description of element input.

**Nodes**I, J, K, L

**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)

**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(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 )

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 192.1: INTER192 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 192.2: INTER192 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 192.1: INTER192 Element Output Definitions**

Name | Definition | O | R |
---|---|---|---|

EL | Element number | - | Y |

NODES | Node connectivity - I, J, K, L | - | Y |

MAT | Material number | - | Y |

TEMP | Temperatures T(I), T(J), T(K), T(L) | - | 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 (, where is the transverse shear strain, and is the gasket thickness. | 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 |

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.