Automatically generate a mesh at the midplane location, directly from the input geometry (components, elements, solids or surfaces), without first creating a midsurface.

The midmesh functionality in HyperMesh saves significant time over the traditional midsurface-based approach.

Figure 1. Midmesh Result Example

The resulting output consists of 2D shell elements created with the user-provided target size, as well as 1D elements defining the topology of the mesh (vertices/edges/faces). Midmesh generation is also multithreaded to take advantage of multi-core environments.

Direct Midmesh Supported Parts

Direct midmesh is supported for a large majority of parts including cast, machined, injection molded and extruded as shown in Figure 2.

Figure 2. Direct Midmesh Supported Parts

Midmesh Generation Workflow

There are several steps involved in generating a good quality midmesh. Following the workflow shown in Figure 3 helps guarantee the best result with minimal manual effort.
Base Extraction
Extract the base midmesh.
Cleanup Resulting Topology
Use the semi-automated midmesh editing tools to correct the 1D topology and fix any bad/missing faces. The goal is to prepare the model for final remeshing.
Rebuild Mesh
Remesh to the final flow and quality using the rebuild mesh functionality, and correct any remaining mesh quality issues.
Apply Thickness
Map the thickness from the original solid to the midmesh via the Map Thickness tool.

Figure 3. Midmesh Workflow

Create Midmesh

Midmesh generation is possible on dirty geometry, but a cleaner output can be obtained by removing duplicate or overlappinng surfaces, stitching free edges, removing logos and other small features that are not of interest, and merging any solids that should be topologically connected.

It is recommended to use the target element size as the extraction size. It is important to have a properly defined criteria file, specifically the target and minimum sizes, as these are used during the midmesh extraction. The final rebuild mesh step takes care of remeshing to the desired flow and quality. Using an extraction size smaller than the representative feature size will not necessarily give better results and will take significantly more run time.

  1. From the 2D page, click the Midmesh panel.
  2. Select the create subpanel.
  3. Set the minimum size and target element size settings in the criteria file to control the resulting midmesh output by clicking edit criteria.
    Option Action
    Extraction size

    The midmesh extraction element size. By default, this is taken as the target element size from the criteria file. This can be set smaller than the targetsize, though that is not recommended unless there are problems extracting at the target size.

    Minimum size Minimum size allowed in the finalized mesh. This in combination with the ‘suppress proximity edges factor’ and 'combine non-manifold edges factor’ can ensure that the output mesh is ready for rebuild with the same criteria. Can only be modified in the Criteria File Editor.
  4. Define options accordingly to control the resulting midmesh output.
    Option Action
    destination comp Select which component newly created midmeshes are placed in.
    ignore flat edges Do not imprint flat edges from the input geometry to the midmesh.

    Figure 4. Option Disabled

    Figure 5. Option Enabled
    flatten connections Align/flatten the midmesh at ribs/connections.

    Figure 6. Option Disabled

    Figure 7. Option Enabled
    suppress proximity edges factor

    The minimum size factor for removing edges within proximity. Edges closer than this factor times minimum size will be suppressed.

    Figure 8. Option Disabled

    Figure 9. Option Enabled
    combine non-manifold edges factor

    The minimum size factor for joining non-manifold edges. Non-manifold edges closer than this factor times minimum size will be combined.

    Figure 10. Option Disabled

    Figure 11. Option Enabled
    defeature openings with width <

    The maximum width for removal of small holes and openings.

    Figure 12. Option Disabled

    Figure 13. Option Enabled
  5. Click create.

Edit Midmesh

Once the midmesh is generated, there may be problem areas that need to be corrected.

The 1D topology is important for the rebuild mesh operation, and care must be taken to prepare it accordingly. In addition, making sure the faces do not have intersected, overlapped, or missing elements, and that they have proper alignment, is also essential. Specialized midmesh edit tools streamline the process of repairing the 1D topology edges, and correcting issues with the midmesh faces.
  • Select the edit edge subpanel access tools which can be used to repair 1D topology edges.
    Option Action
    create mid-edge Create a new mid-edge, optionally using the input geometry as a guide.

    Figure 14. Before

    Figure 15. After
    split by two nodes Create a new edge between two nodes.

    Figure 16. Before

    Figure 17. After
    split by node-edge Create a new edge between a node and an edge, using a shortest, tangential or mixed path.
    Figure 18. Shortest Path
    Figure 19. Tangential Path
    Figure 20. Mixed Path
    delete edge Delete an edge.

    Figure 21. Before

    Figure 22. After
    t-edge align Align/flatten a t-connection edge to a surface.

    Figure 23. Before

    Figure 24. After
    by geom edge align

    Align mesh edges to input geometry lines and smooth the mesh.

    Figure 25. Before Align

    Figure 26. After Align
  • Select the edit face subpanel to access tools which can be used to correct issues with midmesh faces.
    Option Action
    fill face Create a mesh within a closed 1D topology loop, attempting to keep tangency. Optionally, the 1D loop can be deleted, keeping only free and non-manifold edges.

    Figure 27. Before

    Figure 28. After
    repair face Attempt to fix topological problems (holes/gaps/cracks, intersections, slivers, overlaps) in the mesh and remesh the face.

    Figure 29. Before

    Figure 30. After
    detect intersections/gaps Detect intersecting element clusters and holes/gaps/cracks, and create element sets for further handling.

    Figure 31. Before

    Figure 32. After
    align face

    Align a selection of elements to an input geometry surface.

    Figure 33. Before

    Figure 34. After

BatchMesher Midmesh Generation Rules

Midmesh generation is also supported from within BatchMesher.

This functionality allows for generating midmesh representations via the standalone BatchMesher, via the Part Browser, and interactively via the Automesh panel and Mesh Controls Browser.

Figure 35.