A question that frequently arises in a finite element analysis is, "How fine should the element mesh be in order to obtain reasonably good results?" Unfortunately, no one can give you a definitive answer to this question. You must resolve this issue for yourself. Some of the techniques you might use to resolve this question include:
Compare the results of a preliminary analysis with independently derived experimental or known accurate analytical results. Refine the mesh in regions where the discrepancy between known and calculated results is too great. (For all area meshes and for volume meshes composed of tetrahedra, you can refine the mesh locally with the NREFINE, EREFINE, KREFINE, LREFINE, and AREFINE commands.)
Perform an initial analysis using what seems to you to be a "reasonable" mesh. Reanalyze the problem using twice as many elements in critical regions, and compare the two solutions. If the two meshes give nearly the same results, then the mesh is probably adequate. If the two meshes yield substantially different results, then further mesh refinement might be required. You should keep refining your mesh until you obtain nearly identical results for succeeding meshes.
If mesh-refinement testing reveals that only a portion of your model requires a finer mesh, you can use submodeling to "zoom in" on critical regions.
Mesh density is extremely important. If your mesh is too coarse, your results can contain serious errors. If your mesh is too fine, you will waste computer resources, experience excessively long run times, and your model may be too large to run on your computer system. To avoid such problems, always address the issue of mesh density before you begin your model generation.