How to Perform a Mesh Convergence Study

In finite element modeling, a finer mesh typically results in a more accurate solution. However, as a mesh is made finer, the computation time increases. How can you get a mesh that satisfactorily balances accuracy and computing resources? One way is to perform a mesh convergence study as follows:

• Create a mesh using the fewest, reasonable number of elements and analyze the model.
• Recreate the mesh with a denser element distribution, re-analyze it and compare the results to those of the previous mesh.
• Keep increasing the mesh density and re-analyzing the model until the results converge satisfactorily.

This type of mesh convergence study can enable you to obtain an accurate solution with a mesh that is sufficiently dense and not overly demanding of computing resources.

To modify the density of a finite element mesh, you can use a number of features including the following:

• For a hand-generated mesh:
• Return to the unmeshed wireframe geometry and modify the number of divisions; or
• Use surface mesh enhancement.
• For a two-dimensional automatically generated mesh:
• Return to the unmeshed wireframe geometry and use the "FEA Mesh:Two-Dimensional Mesh Generation:Generate Mesh..." command sequence in Superdraw to access the "Two-Dimensional Mesh Generation" dialog; then, modify the "Mesh Density" value or the "Mesh Size" value.
• For a solid mesh:
• In the CAD Solid Model environment, on the "Create Mesh" dialog, move the slider bar to specify the mesh size or access the "Detailed Mesh Creation Options" dialog and specify the "Size" value; or
• Use surface mesh enhancement.
• For a beam element model, use the "Construct:Divide" command sequence in Superdraw to break beams into smaller elements.

To determine when results have converged satisfactorily and accurately, you can use the following means: Display precision contours (see Figure 1), which show a graphical representation of the stepped changes in results from one element to the next. This contour can be used to determine the effect of the mesh on accuracy and as guidance for the locations needing localized mesh refinement. The easiest method for localized mesh refinement is to remesh using refinement points, which are available for both 2-D and solid meshes. See How to Enhance a Surface Mesh by Using Refinement Points for models originating in CAD. Refinement points can be used to improve the precision and overall quality of the mesh as well as the accuracy at a key area of interest. Display unsmoothed result contours to see the stepped changes in the results between adjacent elements. Display residual forces in the model and check the reactions at supports to make sure they balance or otherwise meet expectations based on engineering judgment. Inquire on the result values at the same location (e.g., the center).

Figure 1: A precision contour display gives a visual indication of the effects of the finite element mesh on accuracy.

As an illustration, consider the following example: As shown in Figure 2, a stainless steel plate (4" x 4" x 0.1") with fixed boundary conditions on all sides is subjected to a uniform pressure load of 100 psi normal to the element faces. A mesh convergence study is performed using an n x n mesh where n = 2, 4, 8, 16 and 32 plate elements.
	Figure 2: A diagram shows a plate model with a 4 x 4 mesh.

As shown in Figure 3, the displacement results converged as the mesh density increased. The displacement magnitudes are as follows: n Displacement 2 0.01299 4 0.01163 8 0.01230 16 0.01254 32 0.01261
	Figure 3: A plot of maximum displacement versus n shows the changes in displacement results for the different mesh densities.

As shown in Figure 4, the stress results at the center of the plate model converged upon a solution (~22 ksi) as the mesh density increased. The maximum von Mises stresses are as follows: n Stress 2 14344 4 22867 8 22240 16 22047 32 21994
	Figure 4: A plot of maximum von Mises stress versus n shows the changes in stress results for the different mesh densities.

Although this example shows displacement and stress results, the same general method can be used to perform a mesh convergence study for other types of results.

For more information about meshing and mesh convergence studies, see the ALGOR User's Guide.