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. Decide whether you want the meshes to match where adjacent parts meet (conformal mesh). The option, Create matched mesh between parts, is activated by default. A matched mesh is the easiest and most direct way to bond adjacent parts. Matching meshes are also required for surface contact in linear analyses solved using the native SimMech processor. However, there are some situations where generating an unmatched (non-conformal) mesh may be advantageous. For example:
   • For MES or nonlinear static analyses with general surface-to-surface contact, the best performance and results are obtained when the meshes do not match between parts (non-conformal mesh). In nonlinear solutions contact is detected between a node on one part and an element face on the adjacent part. When the nodes are matched, the contact solution can oscillate between the element faces around each node, making convergence difficult.
   • For large or complex assemblies, or assemblies in which the part size varies drastically, successfully matching the meshes of all of the parts can be problematic. The mesh can fail for some parts, or the surface mesh may be distorted near part intersections.
   Note: For linear analyses solved using the native SimMech processor, parts with unmatched meshes can be bonded by enabling one of the Smart Bonding options (found within the General Contact Settings dialog. Neither smart bonding nor matched meshes are required for bonded contact when using the Autodesk Nastran solver. In addition, the Nastran solver does not require matched meshes for linear surface contact. Finally, the Nastran solver can also bond parts that are separated by a gap (using the Offset Weld type of contact).
4. Click Generate Mesh (or use the Mesh Mesh Generate 3D Mesh ribbon command).
5. 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 Generate Mesh again to create a new mesh.
• If a finer mesh is required around particular critical areas of the geometry, apply Mesh Refinement to selected points, edges, or surfaces.
  • Use Mesh Mesh Generate 3D Mesh 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 refinement points. Each time you automatically generate refinement points, the previously created ones are replaced by those dictated by the new coarse/fine slider position.
  • Click Done after the appropriate number of refinement points are created.
  • Use Mesh Mesh Generate 3D Mesh to create a new mesh.

Solid Meshing of a CAD model is a three step process:

1. First, the surface of the CAD model is meshed (Surface meshing Part n shown in the progress dialog).
2. After all parts are surface meshed, the surface mesh is verified to ensure that each part is properly meshed. The mesh on each face is checked to confirm that it matches the adjoining faces, and thereby the mesh encloses a watertight solid (Verifying surface mesh for Part n).
3. Finally, the solid mesh is created to fill the volume of each part with solid elements (Solid meshing Part n).

   Depending on the state of the option, Perform solid meshing at time of analysis, the solid mesh can be delayed until the analysis is started or performed immediately after generating the surface mesh. This option is found under Mesh Mesh 3D Mesh Settings Options Model. It is enabled by default, postponing solid meshing until the first time you click Run Simulation or until a Check Model operation is performed.

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 window may indicate that the program is Surface meshing part 27 while the progress indicates Part 5 of 34, for example.

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

• Surface based loads and surface based conditions are maintained.
• Edge loads and edge boundary conditions are maintained.
• Nodal loads and nodal boundary conditions are discarded and you must re-apply them 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 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 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 are overwritten when the CAD part is remeshed.
• If the lines are changed to a different layer number within the same part, the modified lines are overwritten when the CAD part is remeshed.

In addition to the steps presented above, different situations may require some extra steps. The following 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, when enabled, occurs between mating parts. If, for some unusual reason, you do not want to mesh the entire model, and you are not concerned with mesh matching, 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 the desired construction vertex (and at a known position relative to the desired construction vertex). Right-click and choose Add Construction Vertices. Enter the construction vertex offset (DX, DY, and/or DZ) relative to the selected vertex. Also, see the Construction Vertices - Seed Points page.
• If you are working with an assembly of parts, and you want a different type of mesh on different parts (for example, bricks and plate elements), do the following:
  1. Right-click a part in the browser (or select a part and right-click in the display area) and select CAD Mesh Options Part from the context menu. This command accesses a dialog identical to the dialog accessed using Mesh Mesh 3D Mesh Settings , but these mesh settings are applied only to the selected part or parts.
  2. Choose the desired Mesh type and specify the desired meshing options.
  3. Click Save.
  4. Repeat steps 1 through 3 for any other parts that you want to deviate from the global mesh settings.
  5. Click Mesh Mesh Generate 3D Mesh.
  Note: When importing a CAD assembly with a mixture of solid and surface parts, the global mesh type is 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 is defined automatically on a per-part basis using part mesh settings as an override of the global settings.

Mesh size

• There is an alternative to using the slider on the Model Mesh Settings screen to set the mesh size based on a percentage of the default size. Click the Options button and set the Type parameter (under Mesh size) to Absolute mesh size. Then, enter the mesh size as an actual dimension in the Size field.
• If working with an assembly of parts, different mesh sizes can be used for each part:
  1. 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 command accesses a dialog identical to the dialog accessed using Mesh Mesh 3D Mesh Settings , but these mesh settings will only be applied to the selected part or parts.
  2. Specify the desired Mesh size and any other meshing options you want to differ from the global settings.
  3. Click Save.
  4. Repeat steps 1 through 3 for any other parts that you want to deviate from the global mesh settings.
  5. Click Mesh Mesh Generate 3D Mesh.

  If you have specified part-based mesh settings overrides and later decide that you want to mesh the entire model using the global model mesh settings, click Mesh Mesh All Parts Use Model Settings.

  If you have specified part mesh settings for some parts in a model and decide that you want to mesh one of them with the global model mesh settings, do the following: Right-click that part in the browser (or select and right-click in the display area) and choose CAD Mesh Options Model from the context menu.

  Note: When a part is assigned Part mesh settings, the symbol in the browser changes from (Model Mesh Settings) to (Part mesh settings).

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

• If the coordinates of a desired refinement point are known, the refinement point can be added before meshing the model for the first time by using Mesh Refinement Points Specify. You can also specify edge and surface refinements before meshing the model for the first time. See the Mesh Refinement page for more information.

  Of course, you can also generate an initial mesh; select vertices, edges, or surfaces; apply refinement; and regenerate the mesh.

• 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 Model Mesh Settings: Surface page for details.)

Contact and mesh matching between parts

• When the meshes on the mating parts must be matched, use approximately (if not exactly) the same mesh size for adjacent parts. This helps to assure a good match between the meshes of these parts and reduces the likelihood of bad elements at or near mating regions.
• 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 error, 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 Mesh Matching page.
• The mesh around the perimeter where two parts meet may be smoother if Virtual imprinting is enabled, which it is by default for matched meshes. See the Virtual imprinting section on the Mesh Matching page for more information. Additionally, you can split the part surfaces at intersections when the CAD solid model is opened into Simulation Mechanical. See the Surface Splitting page. This second method is preferred when an applied load or constraint needs to be applied only to the exposed portion of a surface (not the surface that extends beneath an adjacent part.
• 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 surface pairs can be set by selecting those items, right-clicking, and choosing Contact. The types of contact available depend on the analysis type. Also, see the Contact Pairs page.
• 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 between the adjacent surfaces. Mesh-matched general surface contact pairs often lead to poor convergence (longer runtime). To prevent the meshes from matching, deactivate the Create matched mesh between parts option in the Model Mesh Settings dialog. (See the Mesh Matching page.) 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

• There are several options for the type of solid mesh to generate (hybrid of bricks and tetrahedra, all tetrahedral, bricks and wedges, and gasket.) 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. Also, see the Model Mesh Settings: Solid page.

Thin parts

• If your part is thin (one element through the thickness), consider using the Midplane option to generate plate elements 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-specified number of brick elements through the thickness. See the Model Mesh Settings: Solid page.

Models to be exported to another FEA program for Fluid flow analysis

• If you plan on exporting your mesh to another FEA application for fluid flow analysis, keep in mind that the fluid volume needs to be meshed. If the CAD model consists only of the solid parts (such as a valve body or pump housing), you will have to derive the fluid parts that fill the interior or surround the exterior of the existing CAD assembly. You can use the CREATE Fluid Volume command within SimStudio Tools to create the fluid part.
• An All tetrahedra mesh is preferred over a hybrid Bricks and tetrahedra mesh for fluid flow analysis models. This mesh type tends to have a more uniform density of nodes throughout the fluid domain.

Gasket materials

• For nonlinear analyses, if one of the parts of the model is a gasket, then set the element type to 3D Gasket before creating the mesh. This option instructs the mesh engine to generate only one element through the thickness, which is one of the requirements of the gasket element. See also 3D Gasket Elements.

  When a part is assigned the 3D Gasket element type, part-based mesh settings are also applied. Accordingly, the symbol in the browser changes to the part-based mesh settings symbol ().

• Though the 3D Gasket element type is not available for linear analyses, the same effect can be achieved manually using the following method:
  1. Right-click the CAD Mesh Options heading for the part to be meshed as a gasket and choose Part from the context menu.
  2. In the Part Mesh Settings dialog, ensure that the Solid mesh type is selected and click Options.
  3. Click the Solid icon along the left edge of the dialog.
  4. Activate the Bricks and wedges (layered mesh of thin parts) option.
  5. Go to the Layered Mesh tab of the dialog.
  6. In the Extrusion control list, set Layers to 1.
  7. Click OK and then Save to accept the settings and exit the Part Mesh Settings dialog.

  This method also works for nonlinear analyses, but setting the Element Type to 3D Gasket is more convenient.