Midmesh panel

Location: 2D page

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

Use the midmesh functionality in Altair HyperMesh 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.

midmesh_example

Figure 1: Midmesh Result Example

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

midmesh_models

Figure 2: Direct Midmesh Supported Parts

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.

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.

Nominal Run

Extract the base midmesh.

Cleanup Resulting Topology

Use the semi-automated midmesh edit edge and edit face 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 size 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.

midmesh_generation_workflow

Figure 3: Midmesh Workflow

Midmesh generation is possible on dirty geometry, but a cleaner output can be obtained by removing duplicate or overlapping 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 a smaller element size (for example, 2 or 4mm depending on model scale) in order to get a good sampling of the input geometry. The final rebuild mesh step takes care of remeshing to the desired size and quality. Using an element size smaller than the representative feature size will not necessarily give better results and will take significantly more run time.

Several options are available to control the resulting midmesh output.

Option

Action

ignore flat edges

Do not imprint flat edges from the input geometry to the midmesh.

midmesh_ignore_flat_edges_off

Figure 4: Option Disabled

midmesh_ignore_flat_edges_on

Figure 5: Option Enabled

flatten connections

Align/flatten the midmesh at ribs/connections.

midmesh_flatten_connections_off

Figure 6: Option Disabled

midmesh_flatten_connections_on

Figure 7: Option Enabled

suppress proximity edges factor

Remove 1D topology edges within the given factor of the output mesh size.

midmesh_suppress_proximity_edges_factor_off

Figure 8: Option Disabled

midmesh_suppress_proximity_edges_factor_on

Figure 9: Option Enabled

combine non- manifold edges factor

Join non-manifold edges within the given factor of the output mesh size.

midmesh_combine_nonmanifold_edges_factor_off

Figure 10: Option Disabled

midmesh_combine_nonmanifold_edges_factor_on

Figure 11: Option Enabled

defeature openings with width <

Remove small holes and openings less than the specified width.

midmesh_defeature_openings_with_width_off

Figure 12: Option Disabled

midmesh_defeature_openings_with_width_on

Figure 13: Option Enabled

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.

•	Use the Edit Edge tools to repair 1D topology edges.

Option

Action

create mid-edge

Create a new mid-edge, using the input geometry as a guide.

midmesh_create_mid_edge_off

Figure 14: Before

midmesh_create_mid_edge_on

Figure 15: After

split by two nodes

Create a new edge between two nodes.

midmesh_split_by_two_nodes_off

Figure 16: Before

midmesh_split_by_two_nodes_on

Figure 17: After

split by node-edge

Create a new edge between a node and an edge, using a shortest, tangential or mixed path.

midmesh_split_by_node_edge_off

Figure 18: Before

midmesh_split_by_node_edge_on

midmesh_split_by_node_edge_on2

Figure 19: After

delete edge

Delete an edge.

midmesh_delete_edge_off

Figure 20: Before

midmesh_delete_edge_on

Figure 21: After

t-edge align

Align/flatten a t-connection edge to a surface.

midmesh_tedge_align_off

Figure 22: Before

midmesh_tedge_align_on

Figure 23: After

by geom edge align

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

midmesh_by_geom_edge_align_off

Figure 24: Before

midmesh_by_geom_edge_align_on

Figure 25: After

•	Use the Edit Face tools 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.

midmesh_fill_face_off

Figure 26: Before

midmesh_fill_face_on

Figure 27: After

repair face

Attempt to fix topological problems (holes, intersections, slivers, overlaps) in the mesh and remesh the face.

midmesh_repair_face_off

Figure 28: Before

midmesh_repair_face_on

Figure 29: After

detect intersections

Detect intersecting element clusters and create element sets for further handling.

midmesh_detect_intersections_off

Figure 30: Before

midmesh_detect_intersections_on

Figure 31: After

align face

Align a selection of elements to an input geometry face, with optional offset and locking of boundary nodes.

midmesh_align_face_off

Figure 32: Before

midmesh_align_face_on

Figure 33: After

Midmesh generation is also supported from within Altair BatchMesher. This allows for generating midmesh representations via the standalone Altair BatchMesher, via the Part Browser, and interactively via the automesh panel and Mesh Controls browser.

midmish_batchmesher_rules