CONTAC12 Element Description

CONTAC12 represents two surfaces which may maintain or break physical contact and may slide relative to each other. The element is capable of supporting only compression in the direction normal to the surfaces and shear (Coulomb friction) in the tangential direction. The element has two degrees of freedom at each node: translations in the nodal x and y directions.

The element may be initially preloaded in the normal direction or it may be given a gap specification. A specified stiffness acts in the normal and tangential directions when the gap is closed and not sliding.

Figure 12.1: CONTAC12 Geometry

CONTAC12 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 12.1: CONTAC12 Geometry. The element is defined by two nodes, an angle to define the interface, two stiffnesses (KN and KS), an initial displacement interference or gap (INTF), and an initial element status (START). An element coordinate system (s-n) is defined on the interface. The angle θ (THETA) is input (or calculated) in degrees and is measured from the global X axis to the element s-axis. The orientation of the interface may be defined (KEYOPT(2)) by THETA or by the node locations.

The normal stiffness, KN, should be based upon the stiffness of the surfaces in contact. See Performing a Node-to-Node Contact Analysis in the Contact Technology Guide for guidelines on choosing a value for KN. In some cases (such as initial interference analyses, nonconvergence, or over penetration), it may be useful to change the KN value between load steps or in a restart in order to obtain an accurate, converged solution. The sticking stiffness, KS, represents the stiffness in the tangential direction when elastic Coulomb friction is selected (µ > 0.0 and KEYOPT(1) = 0). The coefficient of friction µ is input as material property MU and is evaluated at the average of the two node temperatures. Stiffnesses may also be computed from the maximum expected force divided by the maximum allowable surface displacement. KS defaults to KN. Stiffnesses should be on a full 360° basis for an axisymmetric analysis.

The initial displacement interference, Δ, defines the displacement interference (if positive) or the gap size (if negative). The value may be input as a real constant (INTF) or automatically calculated from the input node locations if KEYOPT(4) = 1. Stiffness is associated with a zero or positive interference. The initial element status (START) is used to define the "previous" condition of the interface to be used at the start of the first substep. This input is used to override the condition implied by the interference specification and is useful in anticipating the final interface configuration and in reducing the number of iterations required for convergence.

The force deflection relationships for the interface element can be separated into the normal and tangential (sliding) directions as shown in Figure 12.2: CONTAC12 Force-Deflection Relationship. The element condition at the beginning of the first substep is determined from the START parameter. If the interface is open, no stiffness is associated with this element for this substep. If the interface is closed and sticking, KN is used in the gap resistance and KS is used in the sliding resistance. If the interface is closed but sliding, KN is used in the gap resistance and the limit friction force µFN is used for the sliding resistance.

In the normal direction, when the normal force (FN) is negative, the interface remains in contact and responds as a linear spring. As the normal force becomes positive, contact is broken and no force is transmitted.

KEYOPT(3) can be used to specify a "weak spring" across an open interface, which is useful for preventing rigid body motion that could occur in a static analysis. The weak spring stiffness is computed by multiplying the normal stiffness KN by a reduction factor. The default reduction factor of 1E-6 can be overridden with real constant REDFACT.

In the tangential direction, for FN < 0 and the absolute value of the tangential force (FS) less than (µ|FN|), the interface sticks and responds as a linear spring in the tangential direction. For FN < 0 and FS = µ|FN|, sliding occurs.

If KEYOPT(1) = 1, rigid Coulomb friction is selected, KS is not used, and the elastic sticking capability is removed. This option is useful for displacement controlled problems or for certain dynamic problems where sliding dominates. With this option, no tangential resistance is assumed for the first substep.

The only material property used is the interface coefficient of friction MU. A zero value should be used for frictionless surfaces. Temperatures may be input at the element nodes (for material property evaluation only). The node I temperature T(I) defaults to TUNIF. The node J temperature defaults to T(I). The circular gap option (KEYOPT(2)) is useful where the final contact point (and thus the orientation angle) is not known, such as with concentric cylinders. With this option the angular orientation THETA is initially set to 0.0 and then internally calculated from the relative displacements of the nodes at the end of the substep for use in the next substep. The user specified THETA (if any) is ignored. A negative interference (gap) and a zero coefficient of friction is used with this option.

For analyses involving friction, using NROPT,UNSYM is useful (and, in fact, sometimes required) for problems where the normal and tangential (sliding) motions are strongly coupled, such as in a wedge insertion problem.

A summary of the element input is given in "CONTAC12 Input Summary". A general description of element input is given in Element Input.

CONTAC12 Output Data

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

Several items are illustrated in Figure 12.2: CONTAC12 Force-Deflection Relationship.

The value of USEP is determined from the normal displacement (u_n) (in the element x-direction) between the interface nodes at the end of this substep. That is: USEP = (u_n) _J - (u_n) _I - Δ. This value is used in determining the normal force, FN. For an axisymmetric analysis, the element forces are expressed on a full 360° basis. The value represented by UT is the total translational displacement. The maximum value printed for the sliding force, FS, is µ|FN|. STAT describes the status of the element at the end of this substep. If STAT = 1, the gap is closed and no sliding occurs. If STAT = 3, the gap is open. A value of STAT = +2 indicates the node J slides positive relative to node I as shown in Figure 4.12-1. STAT = -2 indicates a negative slide. For a frictionless surface (µ = 0.0), the element status is either STAT = ±2 or 3. The value of THETA is either the input orientation angle (if KEYOPT(2) = 0), or the calculated angle (if KEYOPT(2) = 1). A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

Figure 12.2: CONTAC12 Force-Deflection Relationship

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.

Table 12.3: CONTAC12 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) of the Basic Analysis Guide and The Item and Sequence Number Table of this manual for more information. The following notation is used in Table 12.3: CONTAC12 Item and Sequence Numbers:

CONTAC12 Assumptions and Restrictions

CONTAC12 Product Restrictions

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

Ansys Professional  —