How to Perform a Mesh Convergence StudyHow to Perform a Mesh Convergence StudyIn 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. This process is partially automated for CAD-based, auto-meshed models and only for the static stress with linear material models analysis type. For more information regarding the process, search for “Mesh Study Wizard” within the In-Product Help or Online Wiki Help. This article discusses how to perform a mesh convergence study manually, and is applicable to all types of models. The following basic steps are required: - 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:
- Right-click the 2-D Mesh heading near the bottom of the Browser (tree view) and choose the Edit command to access the "2-D Mesh Generation" dialog box; then, modify the Mesh Density value or the Mesh Size value.
- For a solid mesh:
- Click the 3D Mesh Setting command to access the “Model Mesh Settings” dialog box. Move the Mesh Size slider bar to alter the mesh size or click the Options button dialog and specify the Size value. The size may be specified as a percent of automatic or an absolute size dimension. Or,
- Use surface mesh enhancement.
For a beam element model, use the Draw: Modify: Divide command to divide beams into shorter elements. | Figure 1: A precision contour display gives a visual indication of the effects of the finite element mesh on accuracy. |
|
To determine when results have converged satisfactorily and accurately, you can use the following means: - Display the von Mises 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 areas needing localized mesh refinement.
- The easiest method for localized mesh refinement is to remesh after defining 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.
When comparing one version of the model with another, inquire on the result values at the same location for each variant (for example, the midpoint of an arc or edge, or the center of a surface). |
| Figure 2: A diagram shows a plate model with a 4x4 mesh. |
|
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. |
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 Autodesk Simulation In-Product Help or Online Wiki Help.
Support – Terms of UseAUTODESK DOES NOT GUARANTEE THAT YOU WILL BE ABLE TO SUCCESSFULLY DOWNLOAD OR IMPLEMENT ANY SERVICE PACK OR WORKAROUND, OR ANY OF THE TIPS, TRICKS, EXAMPLES OR SUGGESTIONS OUTLINED IN ANY AUTODESK PRODUCT SUPPORT TECHNICAL DOCUMENTS. TECHNICAL DOCUMENTS, SERVICE PACKS AND WORKAROUNDS ARE SUBJECT TO CHANGE WITHOUT NOTICE TO YOU. AUTODESK PROVIDES TECHNICAL DOCUMENTS, SERVICE PACKS AND WORKAROUNDS "AS IS" WITHOUT WARRANTY OF ANY KIND, WHETHER EXPRESS OR IMPLIED, INCLUDING WARRANTIES OF MERCHANTABILITY AND FITNESS FOR A PARTICULAR PURPOSE. IN NO EVENT SHALL AUTODESK OR ITS SUPPLIERS BE LIABLE FOR ANY DAMAGES WHATSOEVER INCLUDING DIRECT, INDIRECT, INCIDENTAL, CONSEQUENTIAL, LOSS OF DATA, OR LOSS OF BUSINESS PROFITS OR SPECIAL DAMAGES, THAT MAY OCCUR AS A RESULT OF IMPLEMENTING ANY SERVICE PACK OR WORKAROUND, OR ANY SUGGESTION OUTLINED IN ANY AUTODESK PRODUCT SUPPORT TECHNICAL DOCUMENT, EVEN IF AUTODESK OR ITS SUPPLIERS HAVE BEEN ADVISED OF THE POSSIBILITY OF SUCH DAMAGES. | |
