There are many parameters you can check to ensure the simulation has achieved the desired output. Most of them are indicators that something went wrong rather than that something is working as it should. Start with the stability of the time step, the energy errors, and unexpected erosion. These should be examined and the reasons behind any unexpected results should be investigated. Using the animations to determine the eroding areas can show a number of issues either with the mesh, the setup, or the geometry. Missed contact is also something to watch out for in the animations, especially because the Explicit solver does not have a specific contact tool like the Implicit simulation. Such problems can be addressed by increasing the mesh density or examining the overlap of the parts. It is also useful to examine parts of the model using a section plane. This might give insight to some problems which are not obvious at first glance.

It is important for these quasi-static simulations that the velocity values in the model are in the range of 1 to 10 m/s. If they are too low, it means that the Explicit solver might not be modeling the activity correctly because it is out of range of its normal velocity modes. If they are too high, this means that higher stresses and strains may have been introduced due to inertial and shock effects. Evaluating the velocity also gives indication of how close the simulation is to the real, experimental expectations. Ideally, the solver should simulate the velocities that are desired for the actual mechanism at work. This is not always possible but it is the target to aim for. Increasing the end time while keeping the same displacement values, for example, will decrease the velocities in the simulation but will also increase the run time required.

The solution output includes files that also hold information, though more technical and not as easy to understand as the details in the graphical interface. One example is the .prt file which gives extensive information about the setup and the solve, including which operations took more CPU time, the energy and momentum balance, and errors. After careful examination of the results, you can start working on model improvements. Optimization may include: stabilization (damping), modifying the mesh to give more consistent results, modifying displacement boundary conditions, adding or removing constraints, and so on. The Explicit solver has extensive capabilities for postprocessing, allowing you to get the information you need for making necessary adjustments.