Contact analyses require a careful, logical approach. Divide the analysis into several steps if necessary, and apply the loading slowly making sure that the contact conditions are well established.

In general, it is best to use a separate step for each part of the analysis in Abaqus/Standard even if it is just to change boundary conditions to loads. You will almost certainly end up with more steps than anticipated, but the model should converge much more easily. Contact analyses are much more difficult to complete if you try to apply all the loads in one step.

In Abaqus/Standard achieve stable contact conditions between all components before applying the working loads to the structure. If necessary, apply temporary boundary conditions, which may be removed at a later stage. The final results should be unaffected, provided that the constraints produce no permanent deformation.

Do not apply boundary conditions to nodes on contact surfaces that constrain the node in the direction of contact in Abaqus/Standard. If there is friction, do not constrain these nodes in any degree of freedom: zero pivot messages may result.

Always try to use first-order elements for contact simulations in Abaqus/Standard.

Both Abaqus/Standard and Abaqus/Explicit provide two distinct algorithms for modeling contact: general contact and contact pairs.

General contact interactions allow you to define contact between many or all regions of a model; contact pair interactions describe contact between two surfaces or between a single surface and itself.

Surfaces used with the general contact algorithm can span multiple unattached bodies. More than two surface facets can share a common edge. In contrast, all surfaces used with the contact pair algorithm must be continuous and simply connected.

In Abaqus/Explicit single-sided surfaces on shell, membrane, or rigid elements must be defined so that the normal directions do not “flip” as the surface is traversed.

Abaqus/Explicit does not smooth rigid surfaces; they are faceted like the underlying elements. Coarse meshing of discrete rigid surfaces can produce noisy solutions with the contact pair algorithm. The general contact algorithm does include some numerical rounding of features.

Tie constraints are a useful means of mesh refinement in Abaqus.

Abaqus/Explicit adjusts the nodal coordinates without strain to remove any initial overclosures prior to the first step. If the adjustments are large with respect to the element dimensions, elements can become severely distorted.

In subsequent steps any nodal adjustments to remove initial overclosures in Abaqus/Explicit induce strains that can potentially cause severe mesh distortions.

When you are interested in results that are likely to contain high frequency oscillations, such as accelerations in an impact problem, request Abaqus/Explicit history output with a relatively high output rate and (if the output rate is less than every increment) apply an antialiasing filter; then, use a postprocessing filter if stronger filtering is desired.

The Abaqus Analysis User's Guide contains more detailed discussions of contact modeling in Abaqus. “Contact interaction analysis: overview,” Section 36.1.1 of the Abaqus Analysis User's Guide, is a good place to begin further reading on the subject.