Creating a mesh

You can create meshes throughout entire parts or part instances or just within selected regions. To create a mesh, select either MeshPart, MeshInstance, or MeshRegion from the main menu bar.

Related Topics
Understanding mesh generation
Verifying and improving meshes
Advanced meshing techniques
Using the prompt area during procedures
Using the Mesh module toolbox
Selecting objects within the viewport

  1. From the Object field in the context bar, select the part to mesh or select the assembly.

  2. From the main menu bar, select MeshPart, MeshInstance, or MeshRegion.

    Abaqus/CAE displays prompts in the prompt area to guide you through the procedure.

    Tip: You can also mesh parts, part instances, or regions using the and tools, located with the mesh tools in the Mesh module toolbox. (For more information, see Using the Mesh module toolbox.)

  3. If you are meshing the assembly, you must select the instances or regions to mesh. Click mouse button 2 to indicate that you have finished selecting. (For more information on selecting objects, see Selecting objects within the viewport.”)

    Select only those part instances or regions that are colored green, pink, or yellow, indicating they are meshable. To make orange regions meshable, you must either subdivide them using the partitioning tools, assign the bottom-up meshing technique, or assign tetrahedral-shaped elements to them. Regions that you have already assigned the bottom-up meshing technique are colored light tan; you must either mesh them using the bottom-up technique or assign another meshing technique. (For more information on creating bottom-up meshes, see Bottom-up meshing.) Parts colored white cannot be meshed, because they are associated with independent instances.

    Note:

    Part instances are colored according to their meshability only when the Mesh defaults color mapping is selected. Apply this color mapping if the colors in your viewport do not match those described in this step.

  4. Do one of the following:

    • From the prompt area, click Yes to generate the mesh on those regions that are meshable.

    • If the assembly includes a solid region that will be meshed with tetrahedral elements, Abaqus/CAE asks if you want to preview the triangular mesh on the exterior faces of the region.

      1. To preview the mesh, toggle on Preview boundary mesh from the prompt area and click Yes to create the boundary mesh.

        Abaqus/CAE generates the triangular boundary mesh on the mesh on those regions that are meshable.

      2. If some regions fail to mesh or if the boundary mesh is not acceptable, Abaqus/CAE provides a variety of tools that will help you generate a mesh in all regions and create an acceptable mesh. For more information, see What can I do with a boundary mesh?.

      3. If the boundary mesh is acceptable, click Yes from the prompt area to continue meshing the interior of the parts, instances, or regions.

        Abaqus/CAE generates the mesh on those regions that are meshable.