Create Midmesh

Use the Midmesh: Automatic tool to automatically generate a mesh at the midplane location, directly from the input geometry (components, elements, solids or surfaces), without first creating a midsurface. This saves significant time over the traditional midsurface-based approach.

  1. From the Mesh ribbon, click the Midmesh > Automatic tool.


    Figure 1.
  2. Optional: On the guide bar, click to define midmesh options.
  3. Select geometry.
    Use the drop down menu on the guide bar selector to choose components, elements, solids, or surfaces as the source geometry type.
  4. Edit the extraction size value in the microdialog.
  5. Click Midmesh in either the microdialog or the guide bar.
The midmesh is extracted as FE geometry. HyperMesh organizes the midmesh elements in the Midmesh.# component (the name is based on the Destination component option).

Options for Creating Midmesh

Access the following options by clicking on the Midmesh: Automatic tool guide bar.

Edit criteria
Set the minimum size and target element size settings in the criteria file to control the resulting midmesh via the Criteria File Editor.
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 target size, though that is not recommended unless there are problems extracting at the target size.
Minimum size
Minimum element 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.

Mask input entities
Hide input midmeshed entities in the modeling window upon exiting the context.
Destination component
Select which component newly created midmeshes are placed in.
Ignore flat edges
Do not imprint flat edges from the input geometry onto the midmesh.


Figure 2. Option Off


Figure 3. Option On
Flatten connections
Aligns/flattens the midmesh at ribs/connections.


Figure 4. Option Off


Figure 5. Option On
Step offset mode
This option allows finer control of how stepped geometry (one side continuous surface, and opposite side steps) is captured. This option is valid only when flatten connections is enabled. Values can be:
Automatic – Steps of different thickness across a common base surface are automatically offset to a uniform distance from the base surface.
Middle everywhere – Each step will be placed in the middle everywhere.
Middle of thickest plate – All steps that share a common base are moved to the middle of the thickest step. This might place portions of the midmesh outside the solid.
Middle of thinnest plate – All steps that share a common base are moved to the middle of the thinnest step.


Figure 6.
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 7. Option Off


Figure 8. Option On
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 9. Option Off


Figure 10. Option On
Defeature ribs width factor
The minimum size factor for removing small ribs. Ribs closer than this factor times minimum size will be suppressed. Default is 0.9.
Defeature openings with width <
The maximum width for removal of small holes and openings.


Figure 11. Option Off


Figure 12. Option On