The verification problems outlined in this section test the addition and the removal of elements in a sequential import analysis. The problems also test the application of initial stresses and velocities on imported elements that can be applied only under certain conditions (see “Transferring results between ABAQUS/Explicit and ABAQUS/Standard,” Section 7.7.2 of the ABAQUS Analysis User's Manual).

The finite element model in these verification problems consists of two elements that are not connected to each other, as shown in Figure 3.12.5–1. The following material models are used in the verification problems: *ELASTIC, *PLASTIC, *HYPERELASTIC, and *HYPERFOAM.

Each analysis, for a given combination of an element type and material model, consists of four steps, with the first step being an ABAQUS/Explicit analysis. In this step the two elements, 1 and 11, are loaded in tension for all material models except for *HYPERFOAM, where the elements are loaded in compression.

The second step is an import analysis, with the results being imported into ABAQUS/Standard. In this case the results of element 1 only are imported with UPDATE=YES and STATE=NO on the *IMPORT option. Since the material state is not imported, initial stresses can be prescribed for the imported element. In addition, a new element, 111, is defined in the import analysis and subjected to loading in tension (compression when the *HYPERFOAM material model is used).

The third step is another import analysis, with the results now being imported into ABAQUS/Explicit from the previous ABAQUS/Standard analysis. The UPDATE and STATE parameters are both set equal to YES on the *IMPORT option. The results for element 111 are imported into the ABAQUS/Explicit analysis, while the results for element 1 are not imported. Initial velocities are prescribed at the nodes of the imported element using the *INITIAL CONDITIONS, TYPE=VELOCITY option. A new element, 201, is defined in this import analysis and subjected to a tensile load (compressive load when the *HYPERFOAM material model is used).

The results of element 201 at the end of the third step are then imported into ABAQUS/Standard, with UPDATE=YES and STATE=NO on the *IMPORT option. A new element, 211, is defined in this step. When UPDATE=YES and STATE=NO, the nodal definitions and the element connectivities of the imported nodes and elements can be redefined. This feature is tested in the fourth step by modifying the connectivity of element 201 and redefining nodes 203 and 204.

The verification problems outlined in this section test the addition and the removal of elements in a sequential import analysis. The problems also test the application of initial stresses and velocities on imported elements that can be applied only under certain conditions (see “Transferring results between ABAQUS/Explicit and ABAQUS/Standard,” Section 7.7.2 of the ABAQUS Analysis User's Manual).

The finite element model in these verification problems consists of two elements that are not connected to each other, as shown in Figure 3.12.5–1. The following material models are used in the verification problems: *HYPERELASTIC and *HYPERFOAM.

Each analysis, for a given combination of an element type and material model, consists of four steps. In the first step the two elements, 1 and 11, are loaded in tension for the *HYPERELASTIC model, while for *HYPERFOAM the elements are loaded in compression.

The second step is an import analysis, with the results being imported into another ABAQUS/Standard *STATIC analysis. In this case the results for element 1 only are imported with UPDATE=YES and STATE=NO on the *IMPORT option. Since the material state is not imported, initial stresses can be prescribed for the imported element. In addition, a new element, 111, is defined in the import analysis and subjected to loading in tension (compression when the *HYPERFOAM material model is used).

The third step is another import analysis, with the results now being imported from the second analysis into an ABAQUS/Standard *DYNAMIC analysis. The UPDATE and STATE parameters are both set equal to YES on the *IMPORT option. The results for element 111 are imported into the current analysis, while the results for element 1 are not imported. Initial velocities are prescribed at the nodes of the imported element using the *INITIAL CONDITIONS, TYPE=VELOCITY option. A new element, 201, is defined in this import analysis and subjected to a tensile load (a compressive load when the *HYPERFOAM material model is used) using the *DYNAMIC option.

The results for element 201 at the end of the third step are then imported into ABAQUS/Standard, with UPDATE=YES and STATE=NO on the *IMPORT option. A new element, 211, is defined in this step. When UPDATE=YES and STATE=NO, the nodal definitions and the element connectivities for the imported nodes and elements can be redefined. This feature is tested in the fourth step by modifying the connectivity of element 201 and redefining nodes 203 and 204.

The addition and removal of S4R elements with enhanced hourglass control is also tested.