Meshing Process

Get a good surface mesh because it controls the quality of the solid mesh.

Meshing basics

1. Open the solid model.
2. On the Model Mesh Settings dialog box, select the appropriate option for the model in the Mesh type section.  Note that the mesh type will default automatically to Solid when importing CAD solid data and to Plate/shell when importing CAD surface data. It is also possible to define the mesh type on a per-part basis, overriding the global setting (see the General Tips section below).
   • Select Solid if the model will be analyzed using brick elements.
   • Select Midplane if the model is a 3D solid model but will be analyzed using plate or shell elements. The solid part collapses down to plate elements at the midplane.
   • Select Plate/shell if the model already consists of only surfaces and will be analyzed as plate or shell elements.
   • If the part is  a gasket element type (nonlinear stress analysis), click the part in the browser (tree view) set the element type to 3D Gasket.
3. Click Mesh model. (Or use Mesh Mesh Generate 3D Mesh.)
4. After the meshing process completes, click Yes to view the results of the mesh.

If the results are not acceptable, adjust the mesh size with one of these techniques:

• On the Mesh Mesh 3D Mesh Settings dialog box, move the Mesh size slider towards Coarse or Fine and click Mesh Model again to create a new mesh.
• If a finer mesh is required around closely spaced features, select the Mesh Refinement Points Automatic command.
• Move the slider to the appropriate position and press Generate. Black refinement points are added to the model. Move the slider and click Generate again to change the number of refinements. Click Done after the appropriate number of refinement points are created. Use Mesh Mesh Generate 3D Mesh to create a new mesh.

Meshing of a CAD model is a two or three step process when generating a solid mesh. First, the surface of the CAD model is meshed (Surface meshing Part n shown in the progress dialog). After all parts are surface meshed, the surface mesh is verified to ensure that each part is properly meshed, meaning that the mesh on each face matches the adjoining face, and thereby creating a watertight solid (Verifying surface mesh for Part n). Finally, the solid mesh is created to fill the volume of each part with solid elements (Solid meshing Part n). Depending on the option chosen under Mesh Mesh 3D Mesh Settings Options Model, the solid mesh can be delayed until the analysis is started or performed immediately after generating the surface mesh.

Note: In a multi-part assembly, the parts are meshed in order of smallest to largest volume of the bounding box (overall dimensions) of each part. They are not meshed in numerical order. So the Information section of the Meshing Progress dialog may indicate that it is Surface meshing part 101 while the progress indicates Part 5 of 314.

When loads or boundary conditions are existing in the model and the model is re-meshed, the following will occur:

• Surface based loads and surface based conditions will be maintained.
• Edge loads and edge boundary conditions will be maintained.
• Nodal loads and nodal boundary conditions must be re-applied to the model.

Important

After generating the mesh, you can change the attributes of the lines (part, surface, and layer) for specific requirements. For example, it may be advantageous to combine multiple surfaces into one surface number to make it easier to apply and modify a load. Be aware that some manual changes may be overwritten if the CAD part is remeshed and some are not. In particular:

• If the lines are changed to a different part number (not a CAD part), the modified lines will remain when the CAD part is remeshed.
• If the lines are changed to a different surface number within the same part, then:
  • if the lines are placed on a surface number that does not exist in the CAD part, the modified lines will remain when the CAD part is remeshed. Be careful that the modified lines do not create a problem with the CAD model. That is, it may be necessary to manually select and delete the modified lines.
  • if the lines are placed on a surface number that exists in the CAD part, the modified lines will be overwritten when the CAD part is remeshed.
• If the lines are changed to a different layer number within the same part, the modified lines will be overwritten when the CAD part is remeshed.

In addition to the steps presented above, different situations may require some extra steps. This section presents some of the more common advanced features of meshing CAD solid models (in no particular order).

General Tips

• In a multi-part assembly, all of the activated parts are meshed when the Generate Mesh command is used. This ensures that matching of meshes occurs between mating parts. If for some unusual reason you do not want to mesh the entire model and are not concerned with the matching of the mesh, then deactivate all of the parts that you do not want to mesh (select, right-click, and choose Deactivate). Any existing meshes on the deactivated parts will not be changed.
• In some cases, a node is required at a specific location. To do this, add a construction vertex (formerly known as a seed point). After generating an initial surface mesh, select a vertex ( Selection Select Vertices ) in the area of and at a known position relative to the desired construction vertex, right-click, and choose Add Construction Vertices. Enter the offset DX DY DZ from the selected vertex for the construction node. See also the page Construction Vertices -Seed Points.
• If working with an assembly of parts and you want a different type of mesh on different parts (for example, bricks and plate elements), right-click a part in the browser (or select a part and right-click in the display area) and select the CAD Mesh Options Part command. This will access a screen identical to the screen accessed by Mesh Mesh 3D Mesh Settings but these mesh settings will only be applied to the selected part or parts. Then choose the desired Mesh type.
  Note: When importing a CAD assembly with a mixture of solid and surface parts, the global mesh type will be set based on the most prevalent type of part—Solid for a majority of solid CAD parts and Plate/shell for a majority of surface CAD parts. The less prevalent mesh type will be defined on a per-part basis using part mesh settings as an override of the global settings.

Mesh size

• In addition to using the slider on the Model Mesh Settings screen to set the mesh size based on an arbitrary percentage, clicking the Options button and setting the Mesh size: Type to Absolute mesh size will allow the mesh size to be entered as an actual dimension.
• If working with an assembly of parts, different mesh sizes can be used for each part. Right-click a part in the browser (or select and right-click in the display area) and choose the CAD Mesh Options Part command. This will access a screen identical to the screen accessed by Mesh Mesh 3D Mesh Settings but these mesh settings will only be applied to the selected part or parts. If you have specified part mesh settings for some parts in a model and want to mesh the entire model with the model mesh settings, use Mesh Mesh All Parts Use Model Settings. If you have specified part mesh settings for some parts in a model and want to mesh one of them with the model mesh settings, right-click that part in the browser (or select and right-click in the display area) and choose the CAD Mesh Options Model command.
  Note: When a part is assigned to the Part mesh settings, the symbol in the tree-view changes from (Model Mesh Settings) to.

  When using the Use automatic geometry-based mesh size function (set under Mesh Mesh 3D Mesh Settings Options Model), the mesh size created when using Percent of automatic is different in each part (based on the part's physical size). Use the Part mesh settings to further control the mesh size of individual parts.

• In addition to the automatic refinement point capabilities described above, user specified refinement points can be created using one of these techniques. See also the page Refinement Points.
  • After creating an initial surface mesh, select vertices (Selection Select Vertices), right-click, and choose Add Refinement Points. Enter the refined mesh size and radius around the refinement point in which mesh is to be refined.
  • If the coordinates of the desired refinement point are known, the refinement points can be added before meshing the model by using Mesh Refinement Points Specify.
• Small elements around curved features can be created by adjusting the parameters in the Edge curve refinement section of the Options tab of the Mesh Mesh 3D Mesh Settings Options Surface dialog. (See the page Meshing Overview: Meshing CAD Solid Models: Model Mesh Settings: Surface for details.)

Contact and mesh matching between parts

• When meshing assemblies where the meshes on the mating parts must be matched up, (to transfer a load from one part to another), use approximately (if not exactly) the same mesh size for both parts. This will assure a good match between the meshes of these parts.
• Small gaps between parts, whether intentional or not, can behave unexpectedly. When unintentional, the gap may prevent the meshes from being matched between mating parts. (Keep in mind that all numbers are subjected to round off, so even a perfect CAD model may have a mathematical gap between parts.) Or perhaps a small intentional gap between parts is removed when the model is meshed; that is, the parts are stretched to mate the parts. How far to stretch the mesh is controlled by the mesh matching tolerance. See the page Meshing Overview: Meshing CAD Solid Models: Model Mesh Settings: Model.
• The mesh around the perimeter where two parts match may be smoother if the parts are split when the CAD solid model is opened into Autodesk Simulation. See the page Opening Models: Opening CAD Files: Surface Splitting.
• The type of contact between two mating parts can be set using the Contact entry at the bottom of the browser. Contact can be set for the entire model with this browser entry. Or contact between two parts, or even between individual surfaces can be set by selecting those items, right-click, and choosing Contact. The types of contact available depend on the analysis type. See also the page Creating Contact Pairs.
• If performing a Mechanical Event Simulation (MES) analysis with surface-to-surface contact, and if the parts are starting in contact but will slide or separate, you should not have the meshes matched on the surfaces that will be involved in contact if possible. This condition can lead to poor convergence (longer runtime). To prevent the meshes from matching, use the Prevent part matching option on the Model Mesh Settings dialog. (See the page Meshing Overview: Meshing CAD Solid Models: Model Mesh Settings: Model.) On the other hand, if the parts are initially in contact and the sliding motion is negligible, then the meshes can be matched; specify Point-to-point as the contact type in this situation.

Solid meshing

• If generating a solid mesh, there are numerous options for the type of solid mesh (hybrid of bricks, all tetrahedral, and so on.) From the Mesh Mesh 3D Mesh Settings dialog, click the Options button, and then click Solid to view the types of solid mesh on the General tab. See also the page Model Mesh Settings: Solid.

Thin parts

• If your part is thin (one element through the thickness), consider using the Midplane option to generate plate mesh instead of a brick mesh. (Plate elements treat bending more accurately than one brick element through the thickness.) Another option would be to use the Bricks and wedges (layered mesh of thin parts) option for a solid mesh. This option creates a solid mesh with a user number of brick elements through the thickness. See also the page Model Mesh Settings: Solid.

Fluid flow analysis and multiphysics analysis

• If performing a fluid analysis, keep in mind that the fluid volume needs to be meshed. If the CAD model is of the solid parts, you may be able to generate the fluid volume by using the Mesh: Fluid Generation command.
• Fluid models often require a finer mesh near the wall than at the center of the volume to capture the wall effects. Use the Tetrahedra and wedges (boundary layer) option to produce a thin layer of elements at the wall. See the paragraph Controlling Boundary Layer Meshes on the page Meshing Overview: Meshing CAD Solid Models: Model Mesh Settings: Solid.
• If the boundary layer mesh is not used, then the solid mesh type will default to All tetrahedra for new fluid models. This option results in the best results for fluid models. (Multiphysics analysis uses the All tetrahedra mesh type for all parts so that the faces match between the fluid parts and the solid parts.) See the paragraph Selecting a Mesh Type on the page Meshing Overview: Meshing CAD Solid Models: Model Mesh Settings: Solid. (The solid mesh type on existing models will not be changed to All tetrahedra if the model is remeshed.)

Gasket materials

• If one of the parts of the model is destined to be a gasket, then set the element type to 3D Gasket before creating the mesh. This will instruct the mesh engine to generate only one element through the thickness: one of the requirements of the gasket element. See also 3D Gasket Elements.

  When a part is assigned to the Gasket mesh settings, the symbol in the tree-view changes to a part mesh setting. The gasket setting is also accessible by selecting the part, right-clicking and choosing CAD Mesh Options Part Options Solid Gasket.