Contact Controls for Contact Pairs in Abaqus/Explicit

Scaling Default Penalty Stiffnesses

If you use the penalty method to enforce contact constraints in a contact pair (see Contact Constraint Enforcement Methods in Abaqus/Explicit), Abaqus/Explicit resists penetrations between surfaces by applying a “spring” stiffness to penetrating nodes. The “spring” stiffness that relates the contact force to the penetration distance is chosen automatically by Abaqus/Explicit, such that the effect on the time increment is minimal yet the allowed penetration is not significant in most analyses. Significant penetrations may develop in an analysis if any of the following factors are present:

Displacement-controlled loading
Materials at the contact interface that are purely elastic or stiffen with deformation
Deformable elements (especially membrane and surface elements) that have relatively little mass of their own and are constrained via methods other than boundary conditions (for example, connectors) involved in contact
Rigid bodies that have relatively little mass or rotary inertia of their own and are constrained via methods other than boundary conditions (for example, connectors) involved in contact

See The Hertz contact problem for an example in which the first two of these factors combine such that the contact penetrations with the default penalty stiffness are significant.

You can specify a scale factor by which to modify penalty stiffnesses for specified contact pairs. This scaling may affect the automatic time incrementation. Use of a large scale factor is likely to increase the computational time required for an analysis because of the reduction in the time increment that is necessary to maintain numerical stability (see Contact Constraint Enforcement Methods in Abaqus/Explicit for further discussion).

Adjusting the Finite-Sliding Contact Tracking Algorithm

In a finite-sliding contact pair, searches are conducted continually throughout an analysis to track the relative motion between the two contacting surfaces. The contact tracking algorithm consists of an expensive, periodic global search and a less expensive, regular local search; the search algorithms are discussed in detail in Contact Tracking Algorithms. You can use contact controls to adjust the frequency and cost of these searches.

Specifying More Frequent Global Contact Searches

By default for two-surface contact pairs, Abaqus/Explicit performs a more thorough search of the main faces near each secondary node every one hundred increments, which is sufficient for most analyses. However, there are some valid contact situations where a global search needs to be used more or less often during the step. Figure 1 illustrates a situation that might require more frequent global tracking. The main surface is a valid surface, but it contains a hole. The secondary node shown identifies the shaded element facet as the closest main surface facet during an increment. The local contact search looks at this main surface facet and its neighbors.

If the secondary node displaces across the hole in relatively few increments, the potential contact between the secondary node and the main surface facets across the hole will not be detected because the local contact search will still be checking the shaded facet. This same situation can occur when a secondary node moves rapidly across a deep valley in the main surface. The solution to this problem is to conduct global contact searches more frequently. You can specify the number of increments between global searches, n, for a given contact pair, if a value other than the default of 100 is desired.

Using a More Conservative Local Contact Search

The default local contact search used by Abaqus/Explicit uses techniques that allow it to use a minimum amount of computational time. If the local contact search has difficulty enforcing the appropriate contact conditions, a more conservative local contact search may resolve the problem. The contact search specified has no effect on contact pairs using self-contact.

Tracking Contact with Highly Warped Surfaces

Calculating the correct contact conditions along a surface that is highly warped is very difficult, especially when the relative velocity of the contacting surfaces is very large. By default, Abaqus/Explicit monitors the orientation of every deformable main surface formed by element faces every 20 increments to check that the surface is not highly warped; rigid faceted surfaces are checked for large warping only at the beginning of a step. If a surface becomes highly warped, a warning message is issued in the status (.sta) file (see Contact Diagnostics in an Abaqus/Explicit Analysis), and a more accurate algorithm is used to calculate each secondary node's nearest point on the warped main surface. The alternate algorithm provides a more accurate solution but uses slightly more computational time.

Redefining the Criteria for a Highly Warped Surface

By default, Abaqus/Explicit considers a surface to be highly warped when the angle between surface normals at the nodes of a facet varies by more than 20°. The maximum variation of the surface normal over a facet is called the out-of-plane warping angle. You can change the default value of the out-of-plane warping angle cutoff from step to step for any contact pair in the model.

Modifying How Frequently Abaqus/Explicit Checks for Warped Surfaces

You can specify the frequency, in increments, at which Abaqus/Explicit checks for warped surfaces for any contact pair in the model. The frequency can be changed from step to step. Checking for warped surfaces more frequently (the default is every 20 increments) will cause a slight increase in computational time for the analysis.