9 Replies Latest reply on Aug 14, 2014 10:02 PM by Magnum So

    how to choose the mesh density for a model?

    Magnum So

      Hi, here is a really good discussion environment but more discussion make more questions indeed! 


      Now I am confused about mesh size and made the following simulation example to analyze:

      a beam model dimension : 100mmx100mmx500mm

      Force applied at the end :  5000N

      Study : static study

      Fixture : one end of beam


      Simulation result:

      Default mesh density = 17mm    Max. stress = 15MPa

      Fine mesh density = 8.5mm   Max. stress = 18.6MPa


      So, I increase the beam length to 2000mm

      Default mesh density =27mm   Max. stress = 57.0MPa

      Fine mesh density = 13.5mm   Max.stress = 68.4MPa


      This make me think about one question: Should I use the fine mesh density(8.5mm) for the 2000mm beam simulation?

      If I apply 8.5mm mesh density, the max.stress will be  78.0MPa


      So, in solidworks simulation, how to choose the mesh size for your model? Should I consider the model volume? 

        • Re: how to choose the mesh density for a model?
          Shaun Densberger

          Before I answer your question, I want to point out a flaw with your test procedure. While the model you're using is very basic, it won't allow you to study how the mesh size relates to the size of the geometry you're studying. That's because this model (a cantilever beam) has singular results at the constraints. This means that as you progressively refine the mesh so that the elements are smaller and smaller, the maximum stress will continue to increase to infinity. You'd be better off using a model that doesn't have this issue, such as a 1/8th symmetry tensile test specimen or plate with a hole.


          Now, to answer your question there is no hard rules of thumb for the size of the elements relative to the geometry because there are too many different factors that come into play. Research into this area has shown trends for extremely basic geometries and boundary conditions, but this can't be applied to all geometry. What element size is best for your model depends on what results you need to capture at what locations in the model and how the "true" results field (i.e. stress, strain, displacement, etc.) will look in that area. Since we don't know what the solution field looks like, we can't determine the best mesh.


          You also want to keep in mind that you only want to refine the mesh in areas that need refinement, as a global refinement is very expensive from a computational standpoint. Typically you'll need a higher density of elements to capture a results field that has a steep gradient associated with it (such as an area of stress concentration), but you don't (and won't) want the same high density mesh in areas that either have a smooth gradient or that you're not really concerned with accurate results.


          Finally, progressively refining the mesh not only helps to hone in on an efficient mesh, but also allows you to check and confirm that your analysis converges. Convergence is one of the most important parts of an analysis that gets overlooked most of the time. If you were to just apply a very fine mesh from the start, it would not only be very expensive computationally, but you wouldn't know how much uncertainty there is in the results you've obtained. The only way to find with out would be to either refine the mesh even more, or degrade the mesh; in either case, you're essentially back to where you are now (albeit more computationally demanding).