A common question in FEA is what mesh size is required to get accurate results. When working with a CAD model, the Mesh Study Wizard can be used to answer that question. The Mesh Study Wizard automates the task of meshing the model at different mesh sizes, performing the analysis, and querying the results.
Set up the model
Before performing the mesh study, you must first perform the following steps:
- Open the CAD model in Autodesk Simulation.
- Set the analysis type to Static Stress with Linear Material Models.
- Set any special meshing options such as the type of mesh (solid, midplane, plate/shell), refinement points, mesh matching tolerance, and so on.
- Add surface, edge or part loads and constraints to the model. Nodal loads applied to the CAD parts will not be retained during the study.
- Optionally, mesh the model.
- Define the Element Definitions.
- Define the Material properties.
- Define the Analysis Parameters.
- Optionally, do a Check Model or perform the analysis.
- Although the model does not need to be meshed before hand, we recommend to do so to reveal any problems with the model and setup.
- If adding refinement points, consider using a Divide factor type instead of a Mesh size type. This way, the mesh around the refinement will always be a factor smaller than the overall mesh size instead of being the same size in all iterations. (See Refinement Points for details.)
- Although it is not necessary to do a Check Model or perform the analysis, it is recommended to do so to uncover any problems with the model and setup.
Set up the Mesh Study
Click Analysis 
Analysis Mesh Study Wizard and press Next to begin the setup.
If a model is already opened and an applicable design scenario is loaded:
The currently loaded design scenario will be used as the basis of the mesh study. Skip to the procedure under the Steps common to all mesh studies heading.
If no model is currently open:
For a blank Autodesk Simulation session, the Mesh Study Wizard will display additional screens where you specify the model and design scenario to use.
Select a model: Press the browse button and navigate to the location of the model. The model must have at least one design scenario with a Static Stress with Linear Material Models analysis type. Press the Open button to load the model. Press the Next button to proceed.
Select a design scenario: Select the design scenario which will be used for the mesh study. Only design scenarios with the Static Stress with Linear Material Models analysis type will be available. Press the Next button to proceed. The remainder of the procedure is given under the Steps common to all mesh studies heading.
Steps common to all mesh studies:
Mesh size: This step is used to set what size meshes to use for the study.
- Specify the type of mesh size control that you want to use in the Type drop-down box. The Percent of automatic and Absolute mesh size options are available. (Refer to the page Model Mesh Settings: Surface for information on these options.)
- Specify the limits of the mesh size in the Start size and End size fields.
- Specify how many analyses will be performed in the Total iterations field. The difference between the start and end mesh sizes will be divided into equal segments using the total iterations value. For example, two iterations would perform the analysis at the start and end size, three iterations would perform one additional analysis with a mesh size half way in between, and so on.
Press the Next button to proceed.
Define the results: This step is used to set what result is recorded for each analysis, and loosely where the result occurs. When the design study finishes, a graph of the mesh size versus the result will be displayed.
- Two types of results are available in the Location drop-down box: Element Node and Node. Element Node results are element-based results in which the result is given at every node in every element; consequently, each node will have multiple results when shared by multiple elements. This type of result includes stress and strain results. Node results are nodal-based results in which the result is given only at the nodes. This type of result includes displacement and reaction forces.
- Select the basic result type that you want to be recorded in the Output Calculation drop-down box. The available options will depend on the selection in the Location drop-down box. Further manipulation of the basic result type can be performed by using the next two drop-downs. For example, to get von Mises stress, or maximum principal stress, the basic result type to select in the Output Calculation would be Stress Tensor.
- Select the operation which will be performed on the results type in the Unary Operator drop-down box. This operation will take a vector value (such as a stress tensor) and result in a single scalar value (either by extracting one component of the vector value, or by performing a calculation that results in a scalar value). Therefore, if a scalar result is selected in the Output Calculation, no option will be available in the Unary Operator. If the strain tensor or stress tensor is selected, the operators available will result in the individual tensors, von Mises, Tresca or principal values. If a node result is selected, the operators available will results in one of the X, Y or Z components or the magnitude.
- Specify which value from the entire model will be recorded in the Aggregator drop-down box. The mesh study will record one single result from the entire model for each analysis. For example, choose the maximum result or the sum of all results.
Run the mesh study
Press the Finish button on the wizard to proceed. The wizard will show the progress of generating the new design scenario, meshing, performing the analysis, and so on. Each step of the process does all of the iterations before starting the next step. That is, all of the new design scenarios are created first (progress bar proceeds from 0 to 100%), then all of the new design scenarios are meshed (progress bar proceeds from 0 to 100%), then all of the new design scenarios are analyzed (progress bar proceeds from 0 to 100%), and so on.
View the results
When the mesh study completes, a graph of the result versus the mesh size will be shown. Right-click in the graph window to perform various graphing functions, such as customizing the layout, saving the graph to an image, and so on. (The graph behaves the same as the graphs in the Results environment, so if you are familiar with customizing and exporting those graphs, the mesh study graphs will be the same.)
Also, the results of each analysis are saved in the model as new design scenarios. Open the model in Autodesk Simulation and load in the appropriate design scenario to review the input and results.
Display the results graph
Once a mesh study has been performed, the graph of the results can be displayed as follows:
- Use My Computer to show the contents of the folder containing the model.
- Use another My Computer window to show the contents of the Autodesk Simulation installation folder (such as C:\Program Files\Autodesk\Autodesk Simulation followed by the version number of the software).
- Drag the file modelname.msw from the first window and drop it onto the program MeshStudyViewer.exe in the second window.