INTER205 Element Description

INTER205 is a 3D 8-node linear interface element. When used with 3D linear structural elements (SOLID185, SOLSH190, SOLID272, SOLID273, and SOLID285), INTER205 simulates an interface between two surfaces and the subsequent delamination process, where the separation is represented by an increasing displacement between nodes, within the interface element itself. The nodes are initially coincident.

The element is defined by eight nodes having three degrees of freedom at each node: translations in the nodal x, y, and z directions.

See Cohesive Zone Material (CZM) Model and INTER205 in the Mechanical APDL Theory Reference for more information about this element. Also see Cohesive Material Law in the Material Reference.

For more information about the interface failure/delamination capability, see Crack-Initiation and -Growth Simulation, Interface Delamination, and Fatigue Crack-Growth in the Fracture Analysis Guide.

Figure 205.1: INTER205 Geometry

INTER205 Input Data

The element geometry, node locations, connectivity, and the nodal coordinate system are shown in Figure 205.1: INTER205 Geometry. The element geometry is defined by 8 nodes, which form bottom and top surfaces of the element. The bottom surface is defined by nodes, I, J, K, L; and the top surface is defined by nodes, M, N, O, P.

INTER205 is used to simulate interfacial decohesion with the cohesive zone model along an interface defined by this element. At the outset of the simulation, nodes pairs I and M, J and N, K and O, and L and P are coincident, both with each other and with the corresponding nodes in the adjacent structural elements. The subsequent separation of the adjacent elements (usually defined contiguously as components) is represented by an increasing displacement between the nodes within this element.

INTER205 can also be used to simulate interfacial delamination of laminate composite and general crack-growth with VCCT. For more information, see VCCT-Based Crack-Growth Simulation in the Fracture Analysis Guide.

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.

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

INTER205 Output Data

The solution output associated with the element is in two forms:

The output directions for element items are parallel to the local element coordinate system based on the element midplane as illustrated in Figure 205.2: INTER205 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.

Figure 205.2: INTER205 Stress Output

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 (ETABLE, 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 letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

INTER205 Assumptions and Restrictions

INTER205 Product Restrictions

There are no product-specific restrictions on this element.