The user subroutine VUINTER used in this example models a mechanically compliant, thermally conductive contact interface material with uniform thickness. The interface material is assumed to be bonded to each of two contacting surfaces. The interface material exhibits elastic-plastic behavior with linear hardening in the normal contact direction and purely elastic resistance to relative sliding. Membrane straining of the interface does not affect the stress transmitted to the surfaces. The interface material is thermally conductive; and the conductance remains constant, independent of the gap or pressure at the interface.

With this interface model all slave nodes within a specified initial gap distance relative to the master surface remain bonded throughout the analysis. The other slave nodes are not bonded (they never have contact forces or heat fluxes applied). The initial gap distance (see the gapInit variable in the example user subroutine) accounts for surface thicknesses (equal to zero in these examples) as well as the value of the PAD THICKNESS parameter specified on the *SURFACE INTERACTION option. It is assumed that the initial strain of the interface is zero. ABAQUS/Explicit will not make strain-free adjustments to resolve initial overclosures or gaps for contact pairs that use the VUINTER user subroutine.

The PAD THICKNESS parameter is not required to specify an interface thickness; it is used here for convenience so that the interface thickness will be used when calculating the penetration or gap for each node (the variable rdisp(1,...)). Alternatively, the user could model an interface thickness within the user subroutine without the use of the PAD THICKNESS parameter by constructing a state variable that contains an offset value for each node. This offset can be a function of the initial penetration and the interface thickness at the node (for example, set the offset equal to the negative of the initial penetration). The actual penetration would then be the sum of the value given in rdisp(1,...) and the stored nodal offset value. Since strain-free adjustments are not made to the nodes, this procedure allows a convenient way to eliminate any spurious initial contact forces resulting from inaccurate nodal coordinates, removing the requirement to position the surface nodes accurately when constructing a model.

Strain increments in the normal direction are calculated within the user subroutine as the change in contact penetration divided by a specified interface thickness. This thickness is a property of the interface model. For consistency, this thickness should be set to the same value as the PAD THICKNESS parameter in these examples. Strain increment components corresponding to transverse shearing of the interface are likewise computed as the appropriate sliding increment component divided by the specified interface thickness.

Heat fluxes are calculated by multiplying the thermal conductivity of the interface material by the nodal area and temperature difference between the slave node and master contact point and dividing by the initial interface thickness. Effects such as heat generation due to friction are not taken into account.

A complete list of properties specified for this interface model, in the order in which the values are specified on the second data line of the *SURFACE INTERACTION option, is as follows:

Three user-defined state variables are employed in this example. The first simply indicates whether the initialization to determine which nodes are bonded has been completed. The second is used to mark which nodes are bonded. The third keeps track of the current yield stress at each slave node.

Two simple configurations are used to test this user subroutine in both two and three dimensions. In the first configuration each of two identical elastic bodies is modeled with a row of four elements: CPS4R or C3D8R elements in the purely mechanical analyses; CPS4RT or C3D8RT elements in the thermal-mechanical analyses. The second configuration is the same as the first configuration, but one row of elements is replaced by a fixed analytical rigid surface. The bodies are initially parallel and are separated by the thickness of the interface (i.e., zero gap after accounting for the thickness). Half the nodes lie along the contact interface and are bonded.

In the purely mechanical analyses in which both bodies are modeled with elements, boundary conditions are applied to the nonbonded nodes on one of the bodies. Three separate loading conditions are applied to the other body to generate the following stress states in the interface: uniform normal stress without yielding, uniform shear stress, and nonuniform normal stress causing significant yielding at one end of the interface.

In the thermal-mechanical analyses in which both bodies are modeled with elements, the nonbonded nodes on both bodies are held fixed. An initial temperature of 100 degrees is given to one body; an initial temperature of 0 degrees is given to the other body. The temperature differential causes heat to flow between the bodies, resulting in a uniform temperature of 50 degrees in both bodies.

In the thermal-mechanical analyses containing an analytical rigid surface, boundary conditions are applied to the nonbonded nodes of the deformable body to generate a uniform normal stress without yielding. The reference node of the rigid body is held fixed. An initial temperature of 100 degrees is given to the rigid body; an initial temperature of 0 degrees is given to the deformable body. The heat capacitance of the rigid body is defined to match that of the deformable body so that the temperature differential between the bodies will result in a uniform temperature of 50 degrees in both bodies at the end of the analyses.