Adding Local Mesh Specifications

Local specifications control the size and number of elements in specific regions of a mesh.

Note: Not all local specifications are available for each type of mesh.

For a video overview that explains the benefits of defining local mesh specifications and shows one process for defining them, see Create a Local Mesh Specification in 3DEXPERIENCE.

This task shows you how to:

Before you begin: Create an Octree triangle, Octree tetrahedron, tetrahedron, tetrahedron filler, surface triangle, or surface quad mesh, as appropriate for the specific local specification you are adding.
See Also
Creating Octree Triangle Meshes
Creating Octree Tetrahedron Meshes
Creating and Editing Surface Meshes
Creating and Editing Tetrahedron Meshes
Creating Tetrahedron Filler Meshes

Add Boundary Layers

You can generate regular layers of elements at the boundary of a solid for tetrahedron and tetrahedron filler meshes.

This local specification is not available for Octree tetrahedron meshes.

Note: The use of both local and global boundary layers is not recommended. If you do specify both, local boundary layer specifications should not be in close proximity to any inlets and outlets (excluded faces) in the global boundary layer specification to avoid conflicts in generating the mesh layers.

  1. Click Boundary layers .
    The Boundary Layers dialog box and the Select toolbox appear.
  2. Select the supports.

    You can select one or more geometry supports or select groups from the tree.

    The Select toolbox allows you to choose a selection method for adding geometry supports.

    • Click to select entities manually. This is the default method.
    • Click to select faces and to propagate face selection to nearby faces.

  3. In the Offset box, enter a (positive) value for the total thickness of all the boundary layers.
  4. Toggle off Only tet elements to generate boundary layers using primarily prismatic elements.

    Some pyramids and tetrahedrons might be used to mesh sharp corners and narrow sections.

  5. In the Type box, choose one of the following distributions:

    • Uniform to distribute elements uniformly.
    • Arithmetic to distribute elements using an arithmetic progression.
    • Geometric to distribute elements using a geometric progression.

  6. In the Number of layers box, enter a value for the number of layers you want to create.
  7. If you selected Arithmetic or Geometric for the type, enter a Size ratio to impose a ratio between the thickness of the last and first layers in the distribution.
  8. If you selected Arithmetic or Geometric, you can distribute elements symmetrically by selecting Symmetric.
  9. Click OK.
    A boundary layer specification appears in the tree under a Mesh Specifications set for the active mesh.

Exclude from Boundary Layers

You can exclude supports from the generation of global boundary layers for tetrahedron meshes. This allows you to specify global boundary layers while still excluding inlets and outlets for fluid flow.

This local specification is not available for Octree tetrahedron or tetrahedron filler meshes.

Before you begin: Enable global boundary layers, and select Add boundary layers.
  1. Click Exclude from boundary layers .
    The Excluded Boundary Layer dialog box and the Select toolbox appear.
  2. Select the supports.

    You can select one or more geometry supports or select groups from the tree.

    The Select toolbox allows you to choose a selection method for adding geometry supports.

    • Click to select entities manually. This is the default method.
    • Click to select faces and to propagate face selection to nearby faces.

  3. Click OK.
    An excluded boundary layer specification appears in the tree under a Mesh Specifications set for the active mesh.

The image below is a pipe cross section with the end (on the left) excluded from boundary layer creation; the pipe walls include three boundary layers.

Add a Local Mesh Size

You can specify the element size to use in specific model regions.

Local mesh size specification is not available for surface quad meshes.

  1. Click Local mesh size .
    The Local Mesh Size dialog box and the Select toolbox appear.
  2. Select the supports.

    You can select several geometry supports to apply the local size to all supports simultaneously. You can apply several local mesh size specifications to the system in sequence. A separate object will be created for each specification in the tree.

    The Select toolbox allows you to choose a selection method for adding supports.

    • Click to select entities manually. This is the default method.
    • Click to select edges and to propagate edge selection by angle, by tangency, by picking a path direction (arrow), or along a contour (following a free edge of the mesh).
    • Click to select faces and to propagate face selection to nearby faces.

  3. Enter a Size value.

    Tip: You can use the context menu to measure a distance and enter that value.

    The smallest element size that can be used to generate a mesh is 0.1 mm. To avoid geometrical problems in the mesher, the smallest size of an element is set to 100 times the geometrical model tolerance. This tolerance is set to 0.001 mm regardless of the dimension of the part and cannot be modified. Therefore, the global mesh size must be larger than 0.1 mm.

  4. Enter a local Absolute sag value.
  5. Select Add boundary layers.
  6. Click OK.
    A local mesh size specification appears in the tree under a Mesh Specifications set for the active mesh.

Add a Local Edge Distribution

You can specify the number of nodes to distribute on an edge.

  1. Click Edge Distribution .
    The Edge Distribution dialog box and the Select toolbox appear.
  2. Select edges or faces as supports.

    If you select faces, the node distribution is applied to the boundary edges.

    The Select toolbox allows you to choose a selection method for adding supports.

    • Click to select entities manually. This is the default method.
    • Click to select edges and to propagate edge selection by angle, by tangency, by picking a path direction (arrow), or along a contour (following a free edge of the mesh).
    • Click to select faces and to propagate face selection to nearby faces.

  3. Choose the distribution type:
    • Select Number of edges and enter the number of mesh edges to distribute over each selected edge.
    • Select Size and enter the desired mesh edge size. The actual mesh edge size will be an approximation calculated by fitting the desired size on each support.
  4. Click OK.
    An edge distribution specification is created in the tree under a Mesh Specifications set for the active mesh.
    Notes:
    • If you apply multiple distributions to the same edge, the smallest distribution is used.
    • If you apply an edge distribution and a local mesh size on the same edge, the edge distribution takes precedence.
    • Edge distributions determine element sizes only near the selected edges; they cannot be used to control the mesh size inside large faces.

Impose Points Locally

You can specify geometry points where you want mesh nodes to appear.

  1. Click Imposed Points .
    The Imposed Points dialog box appears.
  2. Select the points to be preserved as mesh nodes.
  3. Click OK.
    An imposed point specification is created in a Mesh Specifications set for the active mesh.

Preserve Local Boundaries

You can specify vertices, edges, and faces to preserve as boundaries within the mesh.

This local specification is available for Octree triangle, Octree tetrahedron, and tetrahedron meshes.

  1. Click Preserved Boundaries .
    The Preserved Boundaries dialog box and the Select toolbox appear.
  2. Select vertices, edges, or faces as supports.

    The Select toolbox allows you to choose a selection method for adding supports.

    • Click to select entities manually. This is the default method.
    • Click to select edges and to propagate edge selection by angle, by tangency, by picking a path direction (arrow), or along a contour (following a free edge of the mesh).
    • Click to select faces and to propagate face selection to nearby faces.

  3. Click OK.
    A preserved boundary specification is created in the tree under a Topology Specifications set for the active mesh.

Project Curves

You can project external curves and use the result of this projection to constrain the mesh topology.

  1. Click Project Curves .
    The Project Curves dialog box appears.
  2. Select the curves that you want to constrain.
  3. In the Tolerance box, enter a maximum distance to project external curves.

    If the distance between an external curve and the mesh is greater than the tolerance value, the curve is not projected.

  4. Click OK.
    A Topology Specifications set containing an Imposed Curve local specification appears in the tree under the mesh.

Project Weld Curves

You can project external curves and use the result of this projection to create compatible seam welds between shell features.

  1. Click Project Weld Curve .
    The Project Weld Curve dialog box appears.
  2. Select the curves that you want to constrain.

    Tip: Click to select all previously defined line fastener connections involved with the shell part being meshed.

  3. In the Tolerance box, enter a maximum distance to project external curves.

    If the distance between an external curve and the mesh is greater than the tolerance value, the curve is not projected.

  4. Specify the Number of layers, and enter the desired height for each layer.

    Multiple layers are supported for welding of separate features and for Self welding of a single feature. However, the mesh for Self welding is optimized only for a single layer.

  5. Select Self welding to allow welding of one geometric feature to itself.

    Self welding supports connecting seams of sheet metal designs where the folded part needs to be welded to itself.

  6. Click OK.
    A Topology Specifications set containing an Imposed Weld Curve local specification appears in the tree under the mesh.

Imposed Points

You can project external points and use the result of this projection to impose constraints on the mesh topology.

  1. Click Imposed Points .
    The Imposed Points dialog box appears.
  2. Select the points that you want to constrain.
  3. In the Tolerance box, enter a maximum distance to project external points.

    If the distance between an external point and the mesh is greater than the tolerance value, the point is not projected.

  4. Click OK.
    A Topology Specifications set containing an Imposed Points local specification appears in the tree under the mesh.

Fillets

You can define layer parameters for fillets.

  1. Click Fillet .
    The Fillet dialog box appears.
  2. Select the faces that you want to constrain.
  3. In the Number of layers list, select the number of layers you want to use to mesh the fillets.
  4. Specify the Max. aspect ratioof the fillet mesh.
  5. Optional: Select Layers condensation in narrow regions to reduce the number of layers to improve the mesh quality.
  6. Click OK.
    A Mesh Specifications set containing a Fillet local specification appears in the tree under the mesh.