Accessing the
Model meshing options:
Mesh
Mesh 3D Mesh Settings Options. Then, click the
Model icon. The
Model icon is present regardless of which radio button is selected in the
Mesh type section of the
Model Mesh Settings dialog. There is a single tab (General) within the
Model
settings.
Model Settings (General tab)
Model Meshing options section:
Automatically refine surface mesh: [Available only when using the legacy mesh engine (Mesh Mesh Use VCAD disabled).] If this check box on the
General tab is activated, an initial surface mesh is created on the model when the model is meshed. Next, refinement points are added depending on the geometry. Finally, the mesh is regenerated with the refinement points active.
Use automatic geometry-based mesh size function: [Available only when using the VCAD mesh engine (Mesh Mesh Use VCAD enabled).] This single option governs multiple aspects of the surface mesh that normally would require you to set up multiple inputs. In general, it automatically refines the mesh in the areas of curved surfaces and adjusts the mesh size based on the volume of each part. The particular effects are summarized in the following table:
| Activated | Not Activated |
|---|---|
| When the mesh size is set based on Percent of automatic (i.e., using the slider), a different mesh size is used for each part. The mesh size is based on the size of the individual part, the number of curves, bounding box dimensions of the part, average length of curves, and so on. | The mesh size is the same in each part, and is based on the size of the entire model. |
| Curved surfaces are meshed more finely depending on the curvature of the surface. A limit is used to control the angle between the element edge segments or the planar element faces that represent the curved surface. | Curved surfaces are meshed based on the user-entered mesh size and refinements. |
| The mesh size is anisotropic on curved surfaces, meaning that the ratio of the element's length divided by the element's width is not forced to be near 1. For example, take a mesh size of 1-inch. The mesh in a fillet of 0.5-inch radius and 20-inches long may have elements roughly 0.25-inch by 1-inch. | The mesh size is isotropic. The element's length divided by the width is near 1. |
| The refinement settings on the
Options tab of the
Model Mesh Settings Surface dialog are disabled. You cannot set the values.
|
The refinement settings on are available to change. |
| In general, the default mesh size is larger. | In general, the default mesh size is smaller. |
Perform solid meshing at time of analysis (Available when using either mesh engine.) If this check box is activated and the Solid radio button is selected in the Mesh type section of the Model Mesh Settings dialog, the model will not be solid meshed until the analysis is performed. This is convenient for large models that may take a significant amount of time for a solid mesh to be generated. With this option, the solid meshing time is combined with the analysis time instead of the surface meshing time.
If the Perform solid meshing at time of analysis check box is not activated, a model will be solid meshed immediately after the surface mesh is created. Deactivating the option is convenient when you plan on scheduling one or more models to run at a future time (using the scheduling options of the Solver Manager). Scheduled simulations are executed from a command window, not the user interface. In this case, solid meshing is not performed automatically at run time. So, if you do not deactivate this option, then you will have to check the model or manually execute solid mesh generation prior to the scheduled solution time.
Number of threads/cores for solid meshing: Sets the number of threads/cores on your machine that you want to use when meshing your solid model. The default value is Automatic/All.
Multi-cores are used when verifying the surface mesh and for solid meshing, while other mesh operations use a single core. Each part is meshed by one core, not split among multiple cores. Therefore, if the number of cores exceeds the number of parts, not all of the cores are used. For example, if your computer has eight cores and your model has five parts, the solid meshing process uses five cores (not all eight). Conversely, if the number of parts exceeds the number of cores, all cores are used, but all parts cannot be solid meshed concurrently.
Solid mesh retries upon failure section
This section control surface mesh retries that occur when solid meshing fails for a part. Even when surface meshing is completely successful, solid meshing can sometimes fail. When the subsequent solid meshing operation is performed and fails, the process will be retried from the surface meshing phase. The following two settings apply:
Number of retries: Set the maximum number of retry attempts that is permitted. The defaults is 6.
Retry reduction factor: The mesh size for each successive surface meshing attempt is reduced by this factor. The default is 0.75, so the mesh for each retry is 75% of the prior mesh size.