Transferring rigid elements

The verification problems outlined in this section test the transfer of rigid elements between Abaqus/Explicit and Abaqus/Standard. Contact definitions specified in the original analysis are not imported; they have to be specified again in the import analysis.

These verification problems consist of a deformable block and a rigid surface, as shown in Figure 1. The analysis consists of four steps. The first step is performed in Abaqus/Explicit. In this step the block is moved until contact is established between the block and the rigid surface.

Figure 1. Sequence of loading for the testing of rigid elements.

The results at the end of the Abaqus/Explicit analysis are then imported into Abaqus/Standard with the material state imported and the reference configuration not updated. The contact conditions are redefined since they are not imported. In the second step contact between the block and the rigid surface is resolved. In the third step the block is made to slide on the rigid surface. A coefficient of friction of 0.1 is defined at the contact interface.

The results at the end of the third step of the analysis are then imported into Abaqus/Explicit with the material state imported and the reference configuration not updated. In this step another rigid surface is defined along the top surface of the block. In the course of the Abaqus/Explicit import analysis, the block is compressed between the two rigid surfaces. The sequence of loading is shown in Figure 1.

The verification problems outlined in this section test the transfer of rigid elements and contact definitions from one Abaqus/Standard analysis to another. The contact definitions and the contact state from the first analysis are transferred to the import analysis. Therefore, the contact definitions do not need to be redefined in the import analysis.

The finite element model consists of a block of deformable material initially located a small distance above a rigid surface. The rigid surface is defined using one of the rigid element types listed. The first step of the first analysis is a static step, in which the deformable block is moved down toward the rigid surface so that contact is established. During the second step of this analysis the block is moved parallel to the rigid surface. The coefficient of friction between the contacting surfaces is 0.1.

The results from the end of the first step of this analysis are then imported into another Abaqus/Standard static analysis with the material state imported and the reference configuration not updated. During this import analysis the block is moved parallel to the rigid surface in exactly the same manner as in the second step of the first analysis. The results at the end of this import analysis should be identical to the results at the end of the first analysis.

The results for only the deformable block are then transferred from the end of the second analysis into a third Abaqus/Standard analysis by specifying only the element set that contains the deformable block on the data line of the import option. The material state is imported, and the reference configuration is updated. A new rigid surface is then defined along the top surface of the deformable block; new contact definitions for the interaction between the rigid surface and the top surface of the block are also specified. The bottom of the block is held fixed and the block is compressed by moving the newly defined rigid surface downward.