Transferring results from multiple previous analyses

The verification problems presented in this section test the transfer of results of selected element sets from two Abaqus/Standard analyses to an Abaqus/Explicit analysis.

The first Abaqus/Standard analysis consists of a quarter circular plate in the X–Y plane modeled with elastic-plastic S4R shell elements. The circular edge is clamped, and symmetry boundary conditions are specified along the cut edges. Uniform pressure loading is applied on the top of the plate. In Step 1 an Abaqus/Standard analysis runs to compute the static response.

The second Abaqus/Standard analysis consists of a partially rigid rotating shaft modeled with elastic C3D8R solid elements. One of the solid elements is deformable, and the rest are rigid bodies whose reference nodes all lie on the longitudinal axis of the shaft. Different rotations about the axis of the shaft are specified on the reference nodes of the rigid body. In Step 1 an Abaqus/Standard analysis runs to compute the static response.

In Step 2 the model and results of the two Abaqus/Standard analyses are imported into an Abaqus/Explicit analysis. The solid element model is imported once, and the shell element model is imported four times: first at the original location and then relocated with rotations of 90°, 180°, and −90° about the z-axis. The result is a model for the whole circular plate formed by the four quarter circles. The Abaqus/Explicit import analysis is performed with the same loading on the circular plate as in the previous static Abaqus/Standard analysis, and the rigid solid elements are given additional rotations. The clamped and symmetry boundary conditions are maintained for the circular plate model.

The verification problems presented in this section test the transfer of results of selected element sets from two Abaqus/Explicit analyses to another Abaqus/Explicit analysis.

The first Abaqus/Explicit analysis consists of a quarter circular plate X–Y plane modeled with elastic-plastic S4R shell elements. The circular edge is clamped, and symmetry boundary conditions are specified along the cut edges. Uniform pressure loading is applied on the top of the plate. In Step 1 an Abaqus/Explicit analysis runs to compute the steady-state response.

The second Abaqus/Explicit analysis consists of a partially rigid rotating shaft modeled with elastic C3D8R solid elements. One of the solid elements is deformable, and the rest are rigid bodies whose reference nodes all lie on the longitudinal axis of the shaft. Different rotations about the axis of the shaft are specified on the reference nodes of the rigid body. In Step 1 an Abaqus/Explicit analysis runs to compute the steady-state response.

In Step 2 the model and results of the two Abaqus/Explicit analyses are imported into an Abaqus/Explicit analysis. The solid element model is imported once, and the shell element model is imported four times: first at the original location and then relocated with rotations of 90°, 180°, and −90° about the z-axis. The result is a model for the whole circular plate formed by the four quarter circles. The Abaqus/Explicit import analysis runs with the same loading on the circular plate as in the previous steady-state Abaqus/Explicit analysis, and the rigid solid elements are given additional rotations. The clamped and symmetry boundary conditions are maintained for the circular plate model.

The verification problem tests the transfer of results with nodal temperature and field variables from four Abaqus/Standard analyses to an Abaqus/Explicit analysis.

The first and second Abaqus/Standard analysis models each consist of a rectangular column modeled with C3D8R solid elements. The column is fixed at one end and subject to compression at the other end. In the first analysis the column is modeled with an elastic material with constant properties. In the second analysis the elastic properties are dependent on the temperature and two field variables. In Step 1 the static response is computed for both analyses for given values of the compression and the temperature and field variables.

The third and fourth Abaqus/Standard analysis models each consist of a rectangular plate modeled with S4R shell elements. In the third analysis the plate is modeled with an elastic material with properties that are dependent on the temperature and two field variables, and seven temperature points per shell node are specified. In the fourth analysis the elastic properties are dependent on three field variables, and five temperature points per shell node are specified. In Step 1 the static response is computed for both analyses for given values of the compression and the temperature and field variables.

In Step 2 the model and results of the four Abaqus/Standard analyses are imported into an Abaqus/Explicit analysis and each model is repositioned using translation and rotation. In addition, a new rectangular column modeled with C3D8R solid elements is added to the import analysis. The new column is fixed at one end and subject to compression at the other end. It is modeled with elastic properties that are dependent on the temperature and one field variable.

In the Abaqus/Explicit import analysis, the same end conditions and temperature and field variables values used in Step 1 are applied to the imported models. The initial response of the imported models is compared with the Step 1 results of the corresponding previous analyses.

The verification problem tests the transfer of results with nodal temperature and field variables from four Abaqus/Explicit analyses to an Abaqus/Explicit analysis.

The first and second Abaqus/Explicit analysis models each consist of a rectangular column modeled with C3D8R solid elements. The column is fixed at one end and subject to compression at the other end. In the first analysis, the column is modeled with an elastic material with constant properties. In the second analysis, the elastic properties are dependent on the temperature and two field variables. In Step 1 the dynamic response is computed for both analyses for given values of the compression and the temperature and field variables.

The third and fourth Abaqus/Explicit analysis models each consist of a rectangular plate modeled with S4R shell elements. In the third analysis, the plate is modeled with an elastic material with properties that are dependent on the temperature and two field variables, and seven temperature points per shell node are specified. In the fourth analysis, the elastic properties are dependent on three field variables, and five temperature points per shell node are specified. In Step 1 the dynamic response is computed for both analyses for given values of the compression and the temperature and field variables.

In Step 2 the model and results of the four Abaqus/Explicit analyses are imported into an Abaqus/Explicit analysis, and each model is repositioned using translation and rotation. In addition, a new rectangular column modeled with C3D8R solid elements is added to the import analysis. The new column is fixed at one end and subject to compression at the other end. It is modeled with elastic properties that are dependent on the temperature and one field variable.

In the Abaqus/Explicit import analysis, the same end conditions and temperature and field variables values as used in Step 1 are applied to the imported models. The initial response of the imported models is compared with the Step 1 results of the corresponding previous analyses.