For general information about how to apply mesh controls and preview the mesh, see Apply Mesh Controls and Preview Mesh in the Mechanical User's Guide

All mesh methods available in the Workbench meshing application can be utilized in Explicit Dynamics systems.

A smooth uniform mesh should be sought in the regions of interest for the analysis. Elsewhere, coarsening of the mesh may help to reduce the overall size of the problem to be solved. Use the Explicit meshing preference (set by default) to auto-assign the default mesh controls that will provide a mesh well suited for Explicit Dynamics analyses. This preference automatically sets the Rigid Body Behavior mesh control to Full Mesh. The Full Mesh setting is only applicable to Explicit Dynamics analyses. Other physics preferences can be used if better consistency is desired between implicit and explicit models.

Consideration should be given to the number of elements in the model and the quality of the mesh to produce larger resulting time steps and therefore more efficient simulations. A coarse mesh can often be used to gain insight into the basic dynamics of a system while a finer mesh is required to investigate nonlinear material effects and failure. The Mesh Metric option allows you to view mesh metric information and thereby evaluate the mesh quality. A very useful mesh metric is the Characteristic Length: it is primarily used to determine the timestep for an element.

Swept/multi-zone meshes are preferred in Explicit Dynamics analyses so geometry slicing, combined with multibody part options in DesignModeler, are recommended to facilitate hexahedral meshing. Alternatively, use the patch independent tetrahedral meshing method to obtain more uniform element sizing and take advantage of automatic defeaturing.

Define the element size manually to produce more uniform element size distributions especially on surface bodies.

Midside nodes should be dropped from the mesh (set Element Order to Linear) for all elements types (solids, surface and line bodies). Error/warning messages are provided if unsupported (higher order) elements are present in the mesh.

Pyramid elements are not supported in Explicit Dynamics analyses. Any elements of this type are converted into two tetrahedral elements, and will warrant a warning in the message window of the Mechanical application.

An Explicit Dynamics model with fewer elements than the number of worker processes specified cannot be run in parallel.

For LS-DYNA, only the element types listed below are supported (partly due to LS-DYNA limitations). Any parts with a mesh containing unsupported elements will be excluded from the exported mesh. A warning is displayed specifying excluded parts.

When performing an implicit static structural or transient structural analysis to an Explicit Dynamics analysis, the same mesh is required for both the implicit and explicit analysis and only low order elements are allowed. If high order elements are used, the solve will be blocked and an error message will be issued.

Any bodies with the reference frame Particle need to have been meshed with the Particle Method.