When I did dynamic relaxation analysis in gravity loading process, it took a long time to get a converged solution. Is there a way to make this analysis faster?

If the dynamic relaxation method is used for static loading analysis, the following methods can improve the solution speed:

a) Use a coarse mesh. In a gravity loading analysis, the plastic deformation is usually small and most of the deformation is elastic. It is not necessary to use a very fine mesh. If coarse mesh is used, a larger time step can be used in the explicit analysis. After the final geometry is obtained from the gravity loading, the mesh can be refined adaptively either prior or to or during the subsequent forming analysis.

b) Change the value of DRFCTR (the third parameter in *CONTROL_DYNAMIC_RELAXATION). While the default menu value for this parameter has been set at 0.999, it has been found that a slightly larger value can improve the speed. For a gravity loading analysis, DRFCTF=0.9999 is suggested.

c) In a gravity loading simulation, most of the deformation can be considered as elastic, and therefore it may be unnecessary to use many integration points in the thickness direction that may be required during the forming analysis. The value of NIP (the fourth parameter under the card of *SECTION_SHELL) is usually 3 or 5 for the forming analysis alone. NIP is often set at seven (7) or five (5) if subsequent springback analysis is needed. However, for gravity loading, NIP = 2 may be sufficient to capture the stress distribution in all directions because the deformation is generally elastic, Hence the stress distribution through the sheet thickness direction can be regarded to be linear.

d) If the deformation in this process is mostly elastic, then the elastic material model may be used. For example, MAT_ELASTIC, which is much faster than plastic material model, has been successfully used for gravity loading applications.

e) If dynamic relaxation method is used for springback analysis, coarsen the mesh before doing the analysis.