• Specifications
• MeshGeneration
• Discussion

Below is the information from prior workflows:

QUADRILATERAL MESHING

Model components: rigid bodies, shell (i.e. bone: femur, tibia, patella)

IA-FEMesh + rounded STL:

Software: IA-FEMesh, Version 1.0

Method: Quadrilateral Surface Meshing

Input: rounded STL triangulated surface geometry (i.e. no sharp edges in STL surface geometry)

Example Files:

OpenKnee, Gen. 1 model, femoral geometry (w/o holes): femur.stl,

IA-FEMesh block: femur_IA-FEMesh_Block.vtk

NOTES: block edges should be tangential to and circumscribed about surface geometry

LIMITATION: not able to control projection of block edge elements nodes to geometric edges!

1. Run IA-FEMesh.
2. Load surface geometry:
   • Surface tab: select "Load" from drop-down menu (e.g. femur.stl).
3. Change surface geometry opacity:
   • Click on name of loaded surface geometry in Object Manager.
   • e.g. set Opacity to 0.5 (out of 1.0 = opaque).
4. Create a basic block:
   • Block(s) tab: select "Create" from drop-down menu.
   • Select "Create block from surface bounds".
   • Click "Apply".
5. Move basic block nodes to project to desire locations on surface:
   • Block(s) tab: select "Build/Edit" from drop-down menu.
   • Click hand button.
   • Iteratively refine node positions:
     • Rotate view (left mouse button outside of block geometry).
     • Move node in planes perpendicular to view.
     • Rotate view orthogonal to first view.
     • Move node to final desired location.
     • Click "Cancel" to finish.
6. Partition block to refine block geometry to match surface geometry:
   • Block(s) tab: select "Build/Edit" from drop-down menu.
   • Iteratively partition block and edit/move newly created nodes:
     • Click "Split" button.
     • Select an edge perpendicular to desired block partitioning dimension (turns green when selected).
     • Click "Apply".
     • Iteratively move nodes (as in prior step).
   • Click "Cancel" to finish.
7. Save block IF desired:
   • Block(s) tab: select "Save" from drop-down menu.
   • Select desired "Building Block" in drop-down menu.
   • Click "Apply".
   • Name "File name" as desired.
   • Click "Save".
8. Assign Mesh Seeds:
   • Mesh tab: select "Assign/Edit Mesh Seeds" from drop-down menu.
   • Select "Element Length" from drop-down menu.
   • Click "Apply".
   • Iteratively refine seed sizes:
     • Select a block edge in the 3D view to refine seeding for a particular partition of the block (vectors showing partition dimension will appear, i.e. Rx (red), Ry (green), Rz (blue)).
     • Make desired partition dimension seeding either smaller or larger to decrease or increase the seed size respectively.
     • Click "Cancel" to finish.
9. Create mesh:
   • Mesh tab: select "Create" from drop-down menu.
   • Select "Surface Mesh", select "quad" (square).
   • Specify "Node" and "Element" Label names.
   • Click "Apply".
10. Inspect mesh quality:
    • Quality tab: select "Evaluate/Display Mesh Quality" from drop-down menu.
    • Select Metric from drop-down menu: e.g. "Jacobian"
    • Click "Cancel" to finish.
11. Iteratively smooth mesh IF needed:
    • Quality tab: select "Mesh Improvement" from drop-down menu.
    • Set "Smoothing Iterations": e.g. 5.
    • Click "Apply".
12. Export mesh:
    • Mesh tab: select "Export ABAQUS File" from drop-down menu.
    • Select desired "Mesh" in drop-down menu.
    • Click "Apply".
    • Name "File name" as desired.
    • Click "Save".

Example file results:

IA-FEMesh quad surface mesh: femur_IA-FEMesh_SurfMesh.vtk

HEXAHEDRAL MESHING

Model components: deformable bodies, volumetric (i.e. cartilage, ligaments, menisci)

IA-FEMesh + rounded STL:

Follow the corresponding procedure from the Quadrilateral Meshing section above, besides the following step:

1. Create mesh:
   • Mesh tab: select "Create" from drop-down menu.
   • Select "Volumetric Mesh", select "hex" (cube).
   • Specify "Node" and "Element" Label names.
   • Click "Apply".

Salome Sub-Meshing + Hex-topology IGES:

Software: Salome 7.5.1

Method: Hexahedral Sub-Meshing (NOTE: tried Salome HEXABLOCK meshing, but face elements were twisted due to edge curvature)

Input: IGES parametric surface/volume geometry with hexahedral topology (i.e. 8 nodes, 12 edges, 6 faces)

Example Files:

OpenKnee, Gen. 1 model, lateral tibia cartilage geometry: lat_tibial_cartilage.igs,

Salome meshing script: lat_tibial_cartilage_Salome_HEX.py

1. Run Salome.
2. Activate "New" Geometry Module.
3. Load IGES file:

   • File -> Import -> IGES (e.g. lat_tibial_cartilage.igs)

   • If warned to "take units in account", select "Yes".
4. If geometry is not visible in OCC 3D scene viewer:
   • click 'Global Panning" button in OCC viewer.
5. If 3D view manipulation shortcut + mouse button control is not working:
   • click "Rotation" button in OCC viewer and rotate view a little, then shorcut + mouse will work.
6. To volumetrically render the geometry, select:

   • View -> Display Mode -> Shading With Edges

7. Check geometry information:

   • Measures -> What is

   • Need to REPAIR the geometry IF:
     1. faces are not watertight
     2. it is NOT a solid.
     3. it does NOT have: 8 vertices, 12 edges, 6 wires, 6 faces.
8. IF geometry REPAIR is needed:
   1. IF edges of faces are not watertight, SEW the geometry:

      • Repair -> Sewing

      • Select shape: loaded geometry (e.g. lat_tibial_cartilage_1)
      • Iteratively reduce the tolerance (from 1e-7) one order of magnitude at a time until geometry is valid:
        • Check "What is" geometry until the result has: 6 wires, 6 faces, 1 shell.
        • e.g. 1e-5 works with example geometry (lat_tibial_cartilage_1)
      • OUTPUT GEOMETRY NAME: Sewing_#
   2. IF geometry is NOT SOLID:

      • New Entity -> Build -> Solid

      • Select sewing: Sewing_#
      • Check "What is" geometry: 6 wires, 6 faces, 1 shell, 1 solid.
      • OUTPUT GEOMETRY NAME: Solid_1
   3. IF geometry has MORE THAN 8 vertices OR 6 edges:

      • Repair -> Remove Extra Edges

      • Select: Solid_1
      • Check "What is" geometry: 8 vertices, 12 edges, 6 wires, 6 faces, 1 shell, 1 solid.

      • OUTPUT GEOMETRY NAME: NoExtraEdges_1

9. Explode edges from solid geometry:

   • New Entity -> Explode

   • Select Sub-shape Types: Edge
10. Activate the Mesh module.
11. Create a new mesh:

    • Mesh -> Create Mesh

    • Geometry: NoExtraEdges_1

    • Mesh type: Hexahedral
    • 3D tab:
      • Algorithm: Hexahedron (i,j,k)
    • 2D tab:
      • Algorithm: Quadrangle (Mapping)
      • Hypothesis:
        • Transition: Standard
12. Create 3 sub-meshes for each set of 4 matching hex-mesh block dimension edges:

    • Mesh -> Create Sub-mesh

    • Name: SubMesh_<dim> (e.g. SubMesh_z -or- SubMesh_3)

    • Mesh: Mesh_1
    • Geometry: interactively select 4 corresponding edges in Geometry hierarchy window
      • use Shift or Ctrl to select multiple edges at once

      • e.g. for SubMesh_z, select: Edge_1, Edge_2, Edge_9, Edge_10

      • e.g. for SubMesh_x, select: Edge_3, Edge_4, Edge_11, Edge_12

      • e.g. for SubMesh_y, select: Edge_5, Edge_6, Edge_7, Edge_8

    • 1D tab:
      • Algorithm: Wire Discretisation
      • Hypothesis: Nb. Segments

        • Name: Nb. Segments_<dim> (e.g. Nb. Segments_z)

        • Number of Segments: <desired #> (e.g. z = 3, x = 50, y = 50)

        • Type of distribution: Equidistant distribution
        • NOTE: create new Hypothesis for each block dimension: x,y,z
13. Calculate mesh:

    • Mesh -> Compute

14. Export mesh:
    • Select mesh name in Geometry hierarchy window.

    • File -> Export -> UNV file.

    • Name "File name" as desired.
    • Click "Save".

Example file results:

Salome hex mesh: lat_tibial_cartilage_Salome_HEX.unv

Salome + STL:

Output

• Finite element mesh of tissue of interest; in human readable format, e.g., Abaqus input (INP) file, XML file, or as open format binary files, e.g., MED file, including
  • node definitions (numbering and coordinates)
  • element definitions (numbering, element-specific node numbers and connectivity)
  • node set definitions (set name(s) and relevant node numbers)
  • element set definitions (set name(s) and relevant element numbers)
  • face definitions (numbering, face-specific node numbers and connectivity)
  • surface set definitions (set name(s) and relevant face numbers)