INTER202 Element Description

INTER202 is a 2D 4-node linear interface element used for 2D structural assembly modeling. When used with 2D linear structural elements (such as PLANE182), INTER202 simulates the interface surfaces and the subsequent delamination process, where the separation is represented by an increasing displacement between nodes, within the interface element itself, that are initially coincident. The element can be used as either 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 Cohesive Zone Material (CZM) Model and INTER202 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 Interface Delamination and Failure Simulation.

Figure 202.1: INTER202 Geometry

INTER202 Input Data

The element geometry, node locations, connectivity, and the nodal coordinate system are shown in Figure 202.1: INTER202 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.

INTER202 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 I,L and J,K 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.

INTER202 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.

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.

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

INTER202 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 202.2: INTER202 Stress Output. See Cohesive Zone Model 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 202.2: INTER202 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.

INTER202 Assumptions and Restrictions

INTER202 Product Restrictions

There are no product-specific restrictions for this element.