3.13.10 Transferring hourglass forces

Products: Abaqus/Standard Abaqus/Explicit

Elements tested

C3D8R CPE4R CPS4R C3D10M CPE6M CPS6M

Problem description

The problem outlined in this section consists of a cantilever beam, as shown in Figure 3.13.10–1. This problem performs two tests. It tests the use of the direct-integration implicit dynamic procedure in the first step of Abaqus/Standard and the transfer of hourglass forces between Abaqus/Standard and Abaqus/Explicit. The following material definition is used for this model:

Young's modulus = 200 × 10⁹

Poisson's ratio = 0.3

Density = 1000.

Figure 3.13.10–1 Model used for the bending test.

The analysis consists of four steps:

The first step is performed in Abaqus/Standard using the direct-integration implicit dynamic procedure. In this step the beam is loaded by applying a displacement boundary condition at the tip of the beam, as shown in Figure 3.13.10–1.
The results at the end of the first step are then imported into Abaqus/Explicit with the material state imported and the reference configuration not updated. In this step the displacements applied to the tip of the beam at the end of the first step are held fixed.
The third step is also performed in Abaqus/Explicit. In this step the beam is displaced in the same direction as before by imposing an additional displacement boundary condition at its tip.
The results at the end of the third step of the analysis are then imported into Abaqus/Standard with the material state imported and the reference configuration not updated. In this step displacement boundary conditions identical to those specified at the end of Step 1 are imposed at the tip of the cantilever beam. This step is performed using the direct-integration implicit dynamic procedure.

Verification tests of the enhanced hourglass control method are also included.

Step 2 of the analysis is also performed in Abaqus/Standard by continuing the analysis from the end of the first step. This allows for the comparison of the results between Abaqus/Explicit and Abaqus/Standard.

Results and discussion

Figure 3.13.10–2 shows the time history of the stress component, at the integration point of element 1 (CPE4R elements are used in this test). It can be seen that the stress state in Step 2 obtained from the Abaqus/Explicit analysis is nearly the same as that obtained from the Abaqus/Standard analysis. In all cases results similar to the ones shown in Figure 3.13.10–2 are obtained.