There are fundamental differences in the mechanical contact algorithms in Abaqus/Standard and Abaqus/Explicit. These differences are reflected in how contact conditions are defined. The main differences are the following:

• Abaqus/Standard uses a strict master-slave weighting when enforcing contact constraints (see “Defining contact pairs in Abaqus/Standard,” Section 31.3.1 of the Abaqus Analysis User's Manual); the nodes of the slave surface are constrained not to penetrate into the master surface. The nodes of the master surface can, in principle, penetrate into the slave surface. Abaqus/Explicit includes this formulation but typically uses a balanced master-slave weighting by default (see “Contact formulation for general contact in Abaqus/Explicit,” Section 33.2.1 of the Abaqus Analysis User's Manual, and “Contact formulations for contact pairs in Abaqus/Explicit,” Section 33.2.2 of the Abaqus Analysis User's Manual).

• Abaqus/Standard and Abaqus/Explicit both provide a finite-sliding contact formulation (see “Contact formulations in Abaqus/Standard,” Section 33.1.1 of the Abaqus Analysis User's Manual, and “Contact formulations for contact pairs in Abaqus/Explicit,” Section 33.2.2 of the Abaqus Analysis User's Manual). However, the two-dimensional finite-sliding contact formulation in Abaqus/Standard requires that the master surfaces be smooth; whereas in Abaqus/Explicit the master surfaces are faceted, except for analytical rigid surfaces, which can be smoothed.

• Abaqus/Standard and Abaqus/Explicit both provide a small-sliding contact formulation (see “Contact formulations in Abaqus/Standard,” Section 33.1.1 of the Abaqus Analysis User's Manual, and “Contact formulations for contact pairs in Abaqus/Explicit,” Section 33.2.2 of the Abaqus Analysis User's Manual). However, the small-sliding contact formulation in Abaqus/Standard transfers the load to the master nodes according to the current position of the slave node. Abaqus/Explicit always transfers the load through the anchor point.

• Many benefits of the Abaqus/Explicit general contact algorithm are not available in Abaqus/Standard.

As a result of these differences, contact definitions specified in an Abaqus/Standard analysis cannot be imported into an Abaqus/Explicit analysis and vice versa (see “Transferring results between Abaqus/Explicit and Abaqus/Standard,” Section 9.2.2 of the Abaqus Analysis User's Manual).