Self-contact in rubber/foam components: jounce bumper

The bumper analysis is a two-step process. In the first step the interference between the bumper's inner diameter and the mandrel is resolved. In the Abaqus/Standard analysis the automatic “shrink” fit method (see Common difficulties associated with contact modeling in Abaqus/Standard) is used: the calculated initial penetration is allowed at the beginning of the step and scaled linearly to zero at the end of the step. In the Abaqus/Explicit analysis the interference resolution step is performed in one of two ways. In the first approach the mandrel is positioned so that no contact or overclosure exists between the bumper and the mandrel at the outset of the analysis. The rigid surface representing the mandrel is then moved in the radial direction to simulate the compression of the bumper due to the interference fit. In the second approach the shrink fit solution from Abaqus/Standard is imported into Abaqus/Explicit. A comparison of the Mises stresses predicted by Abaqus/Standard and Abaqus/Explicit at the end of the interference step shows that the results are very similar (see Figure 3 and Figure 4).

In the second step the bottom surface compresses the bumper 42.0 mm (1.7 in) as a result of the application of displacement boundary conditions to the reference node of the surface. Figure 5, Figure 6, and Figure 7 show the final deformed shape of the bumper; the high compressibility of the material is apparent, as well as the folding of the surface onto itself. Although a general knowledge of where the folding would occur was used in the definition of the self-contacting surfaces, it is not necessary to know exactly where the kinks in the surface will form.

The final deformed shapes predicted by Abaqus/Standard and Abaqus/Explicit for the CAX3 element mesh are the same (see Figure 5 and Figure 6, respectively). A similar shape is predicted by Abaqus/Explicit when CAX4R elements are used (see Figure 7). However, the solution obtained with CAX4R elements in Abaqus/Explicit reveals that local buckling occurs in the upper-left folding radius. This makes a similar analysis using CAX4R elements in Abaqus/Standard very difficult. The local buckling is not captured in the CAX3 analysis due to the stiffer nature of these elements.

The load versus displacement curves of the bottom surface are shown in Figure 8. The results obtained with CAX3 elements in Abaqus/Standard and with CAX3 and CAX4R elements in Abaqus/Explicit are very similar. The energy absorption capacity of the bumper is seen through these curves.