Creating Sweep 3D Meshes

You can mesh a solid part by generating hexahedron elements (HE8 and HE20) and wedge elements (WE6 and WE15) from surface meshes.

The sweep 3D mesher uses a surface mesh as the starting point to mesh a volume. If no surface mesh exists, an internal one is created as part of the sweep mesh. When possible, neighboring lateral and source meshes are captured to create a compatible mesh. The resulting 3D mesh might include linear hexahedron, parabolic hexahedron, linear pentahedron, or parabolic pentahedron elements.

In most cases source and target face selections are made automatically. Automatic selections are based on the shape of the volume to be meshed, the availability of existing meshed faces (as a potential source side), the complexity of the features on the sides, and other factors.

Before you begin: A finite element model representation must exist.
See Also
Finite Element Model Representations
Updating Meshes
  1. From the Mesh section of the action bar, click Sweep 3D Mesh .
    The Sweep 3D Mesh dialog box appears.
  2. Optional: Enter a Name for the sweep 3D mesh.
  3. Select the geometric support.
    The support is highlighted.
  4. To manually select the source and target sides, toggle on Manual Source/Target selection and select the desired faces from the geometry.

    In most cases, preliminary source and target sides are selected and displayed automatically upon completion of Step 2. If automatic selections were made, they are provided as the initial source and target selections.

    If your desired source or target selection includes Extracted or Joined faces, you must select them from the model view; you cannot select them from the tree.

    A toolbox appears, allowing you to choose a selection method for adding faces.

    • Select to select faces manually. This is the default method.
    • Select to select faces and to propagate face selection to nearby faces. A propagation toolbox appears to complete your selection.
    By Angle
    Enter a value for the Angle. Adjacent faces that join the selected face at less than the entered angle are added to the selection. Propagation continues through successive sets of adjacent faces until an angle exceeds the entered value.
    By Curvature
    Enter a value for the Curvature. Adjacent faces are added to the selection as long as the faces are joined along a tangent and the curvature radius of the adjacent faces is greater than the specified value.
    By Tangency
    Adjacent faces are added to the selection as long as the faces are joined along a tangent. Propagation continues as long as the connected faces are all joined along tangent lines.

    Tip: The Angle and Curvature options include a context menu that allows you to measure the values by selecting an edge or a face, respectively. Edge selections must be edges of the first selected face, and face selections must be joined to the first face to obtain valid measurements.

    Click Propagate to complete face selection and to close the propagation tool.

  5. Select the element order, Linear or Quadratic .
  6. Specify the Size, or click Initialize from geometry to set the values based on the size of the support selected in Step 2.

    The size value is an approximation of the mesh element size that will be used.

  7. Use the Distribution parameters to change the distribution of layers through the swept mesh.

    Set the Number of layers to specify the number of mesh layers through the swept volume. Alternatively, you can specify the Layer size to create the sweep mesh using the appropriate number of layers of that thickness.

    Note: Additional distribution parameters are available when you click Edit all parameters. For more information on distribution options, see the mesh section in Mesh Parameters.

  8. Optional: Click Edit all parameters to edit advanced parameters or to load parameters from a saved mesh rule.

    See Editing or Loading Sweep Mesh Parameters.

    For more information about meshing rules, see Creating and Modifying Meshing Rules.

  9. To capture nodes and edges of elements from the neighboring meshes to obtain a compatible mesh:
    1. Select Automatic mesh capture.

      Use Apply on to select meshes to be captured. By default all meshes in the model are checked.

    2. Select the meshes to be captured either in the 3D area or in the tree.

      Tip: To select all meshes at once, right-click the Apply on field, and pick Select all.

    3. In the Tolerance box, enter a maximum distance to capture nodes and edges of elements of the selected mesh parts.
    4. Click Check to run an interference check on the captured meshes.
    5. Click Preview to visualize the mesh.

      If there is an existing mesh, you must confirm creation of the preview since the existing mesh must be removed to create the preview.

    The edge nodes of the captured mesh and the sweep rule mesh are shared; they are not duplicated. The mesh capture is performed dynamically on all constraints (free edges, internal edges,...) and after all constraint modifications.

    Note: To also capture face nodes and ensure no duplication at shared mesh faces, use Face Capture. For more information, see Mesh Compatibility with Captured Elements and Faces.

  10. Optional: Click Edit Guides to specify edge guides for the swept mesh.
    1. To include edges in the guide computation, click .
    2. To exclude edges from the guide computation, click .

    Guides specify the path from a node on the source to a node on the target.

  11. Click one of the following:
    • OK to save the parameters that you defined, to create the mesh, and to close the dialog box. To generate and visualize the mesh, you must update it.
    • Mesh to save the parameters you defined and to create, update, and generate the mesh.

      The PLM Update progress bar appears. The mesh dialog box remains open to allow further edits.

    • Cancel to cancel the modifications and to close the dialog box.
    If you click OK or Mesh, the mesh specification is created and appears in the tree.