Contact Controls for Contact Pairs in Abaqus/Explicit

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).

CONTACT PAIR, MECHANICAL CONSTRAINT=PENALTY,
 CPSET=contact_pair_set_name 
surface_1, surface_2
CONTACT CONTROLS, CPSET=contact_pair_set_name, SCALE PENALTY=factor

Interaction module: 
Create Contact Controls: Name: contact_controls_name, 
Abaqus/Explicit contact controls: Penalty stiffness scaling 
factor: factor

Interaction editor: Mechanical constraint formulation: Penalty contact method, Contact controls: contact_controls_name

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.

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.