Meshing Tips

  • When you mesh a study, the software meshes all unsuppressed solids, shells, and beams:
    • Uses Solid mesh for bulky objects.
    • Uses Shell elements for thin objects like sheet metals.
    • Uses Beam or Truss elements for extruded or revolved objects with constant cross-sections.
    • For assemblies, check component interference. To detect interference in an assembly, click Tools > Evaluate > Interference Detection . Interference is allowed only when using shrink fit. The Treat coincidence as interference and Include multibody part interferences options allow you to detect touching areas. Theses are the only areas affected by the global and component contact settings.
    • Option Mesh all solid bodies with solid mesh (Default Options > Mesh) allows you to mesh all solid, sheet metal, and weldment bodies with a solid mesh. Meshing all solid bodies with solid elements saves you time in preparing the model for meshing (particularly useful for novice simulation users), but can increase the overall solution time.

      At a study level, you can override the mesh assignments enforced by the option Mesh all solid bodies with solid mesh. In a simulation study tree, right-click the top Parts folder, and select Treat all sheet metals as shells, or Treat all weldments as beams.

  • Check for interferences between bodies when using a compatible mesh with the curvature-based mesher. If you specify a bonded contact condition between bodies, they should be touching. If interferences are detected, meshing stops, and you can access the Interference Detection PropertyManager to view the interfering parts. Make sure to resolve all interferences before you mesh again.
  • If meshing fails, use the Failure Diagnostics tool to locate the cause of mesh failure. Try the proposed options to solve the problem. You can also try different element size, define mesh control, or activate Enable automatic looping for solids.
  • The SOLIDWORKS Simplify utility lets you suppress features that meet a specified simplification factor. In the Simulation study tree, right-click Mesh and select Simplify Model for Meshing . This displays the Simplify utility.
    Simplification of geometry can alter stress results significantly.
  • The SOLIDWORKS Geometry Analysis utility identifies small features of a part's geometry that might fail to mesh. You can remove these insignificant geometry features, or use a mesh tolerance value slightly higher than their size. The mesher merges these nodes whose distance is smaller than this tolerance value.
  • It is good practice to check mesh options before meshing. For example, Automatic transition can result in generating an unnecessarily large number of elements for models with many small features. The high-quality mesh is recommended for most cases. Automatic looping can help solve meshing problems automatically, but you can adjust its settings for a particular model. The Blended Curvature-based and Curvature-based meshers automatically use smaller element sizes in regions with high curvature.
  • To improve results in important areas, use mesh control to specify a smaller element size. When meshing an assembly with a wide range of component sizes, default meshing results in a relatively coarse mesh for small components. Component mesh control offers an easy way to give more importance to the selected small components. Use this option to identify important small components.
  • The curvature-based mesher supports multi-threaded surface and volume meshing for assembly and multi-body part documents. The standard mesher supports only multi-threaded volume meshing.
    For static studies, you can use the h-adaptive method to refine the mesh automatically.
  • After meshing, use the Mesh Quality Diagnostics PropertyManager to identify poor quality mesh elements based on a defined criterion.

Checking for Small Features that Fail to Mesh

Before meshing, you can check a part’s geometry for small features that might fail to mesh such as short edges, narrow faces, small faces, sharp corners. The SOLIDWORKS Geometry Analysis utility identifies these features.

To run Geometry Analysis for a part:

  1. Click Geometry Analysis Tool_Geometry_Analysis_Utilities.gif (Tools toolbar) or Tools > Geometry Analysis.

    Geometry Analysis identifies these entities: sliver faces, small faces, short edges, knife (sharp) edges and vertices, discontinuous edges and faces.

    For more information about these entities, see SOLIDWORKS Online Help: Geometry Analysis Options.
  2. You can specify values of control parameters to identify these geometric entities. For example, you can specify the maximum length for short edges. As a general rule, the length value for all three Insignificant geometry parameters (short edges, small faces, sliver faces) should be the same.
    The Geometry Analysis function automatically detects all insignificant geometry features classified by type. Review the detected features and try to resolve the underlying modeling issues.
  3. For example, measure the shortest significant edge on your model. For some models, the shortest significant edge is the plate's thickness, a chamfer, or a hole diameter. Divide this length value by two. Enter this new value as the control parameter for Edge Length, All Edge lengths and Face Width values.
    For sharp angles, the default 5 deg value is fine for most cases.
  4. If you cannot remove some small features from the geometry, use a tolerance value for meshing slightly higher than their size.
    If the distance between two nodes is smaller than this tolerance value, the mesher merges these nodes and meshing is successful.