Mesh Connections

Mesh connections enable you to join the meshes of topologically disconnected surface bodies that may reside in different parts. They are an alternate option to connecting the geometry (for example, by using the DesignModeler application to repair small gaps). However, geometry tolerances are tighter than the tolerances used by mesh connections and often lead to problems in obtaining conformal mesh.

Scoping

With mesh connections, the connections are made at the mesh level and tolerance is based locally on mesh size. Connections are made edge-to-face or vertex-to-face; they connect edge(s) or vertices on face(s) to another face to pinch out the gap and create conformal mesh between the edge(s) and face(s).

Since mesh connections are a post mesh process–the mesh is pinched in a separate step after meshing is complete–the base mesh is stored to allow for quicker updates. That is, if you change a mesh connection or meshing control, only local re-meshing is required to clean up the neighboring mesh.


Note:  With ANSYS Workbench Release 16.0, post pinch behaviors are migrated into Mesh Connections. When you regenerate a mesh that was created using Pinch Behavior settings, the new mesh might report different results than the previous mesh.


Surface Bodies With No Shared Topology:

Same Surface Bodies With Edge-To-Edge Mesh Connection Established:

Treatment of Legacy Databases

Resuming a legacy database (prior to v16), the application moves Mesh Connection objects and the associated Connection Group folders that contain them to the new Model-level Mesh Edit parent folder.

Application

To apply mesh connections:

  1. Insert Mesh Connection objects automatically or manually.

    • Mesh connections can be automatically generated using the Detect Mesh Connections option available from the right-click context menu of the Mesh Connections or Mesh Connection Group folder. The Tolerance Value, pairing type, and other properties used for auto detection can be set in the Details view of the Mesh Connection Group folder under the Auto Detection category. Sheet thickness can also be used as a Tolerance Value.

      The automatic mesh connections feature is very helpful, but it can only detect edge-to-face connections. If you need to define edge-to-edge connections, you will need to define them manually. The feature can also find and create connections that you may not want. Always review the connections, or at least be aware that if problems arise, they may be due to automatically generated mesh connections.

    • For more control, or to control the engineering design, you may want to insert Mesh Connection objects manually.

      Highlight the Mesh Connection Group folder and select the Manual Mesh Connection option on the Mesh Edit toolbar, or right-click the object and select Insert > Manual Mesh Connection.

      The Manual Mesh Connection option is also available when the top-level Mesh Edit folder is selected. Selecting the option at this level adds a Mesh Connection Group object in addition to a Mesh Connection object.

      You can also select one or more Contact Regions or the Contacts folder, right-click, and select Create>Mesh Contact(s) or Connection(s). This option enables you to create Mesh Connection objects from Contact Regions. The application scopes the new Mesh Connection objects to the geometries of the Contact Region(s) and sets the tolerance to be equal to the trim tolerance of the contact region. The Mesh connections are added into a new Mesh Connection Group folder.

  2. In the Details view specify Master Geometry and Slave Geometry.

    • “Master” indicates the topology that will be captured after the operation is complete. In other words, it is the topology to which the slave topologies in the connection are projected.

    • “Slave” indicates the topology that will be pinched out during the operation. In other words, it is the topology that is projected and merged with the master.

    The master geometry can be one or more faces or edges. The slave geometry can only be one or more edges or vertices. When specifying faces, the annotation is displayed on both sides of the faces.


    Note:  Mesh connections support common imprints, which involve multiple slaves connected at the same location to a common master. See Common Imprints and Mesh Connections.


  3. In the Details view specify Tolerance. The Tolerance here has a similar meaning to the Tolerance Value global connection setting, and is represented as a transparent sphere. See Tolerances Used in Mesh Connections for details about Tolerance and how it relates to the Snap Tolerance described below.

  4. For edge-to-face mesh connections only, in the Details view specify Snap to Boundary and Snap Type. When Snap to Boundary is Yes (the default) and the distance from a slave edge to the closest mesh boundary of the master face is within the specified snap to boundary tolerance, nodes from the slave edge are projected onto the boundary of the master face. The joined edge will be on the master face along with other edges on the master face that fall within the defined pinch control tolerance. See Pinch Control for details.

    Snap Type appears only when the value of Snap to Boundary is Yes.

    • If Snap Type is set to Manual Tolerance (the default), a Snap Tolerance field appears where you may enter a numerical value greater than 0. By default, the Snap Tolerance is set equal to the pinch tolerance but it can be overridden here. See Tolerances Used in Mesh Connections for details about Snap Tolerance and how it relates to the Tolerance described above.

    • If Snap Type is set to Element Size Factor, a Master Element Size Factor field appears where you may enter a numerical value greater than 0. The value entered should be a factor of the local element size of the master topology.

  5. Highlight the Mesh Edit folder and choose Generate (right-click and choose from context menu). The surface bodies are displayed and show the mesh connections.

  6. If necessary, review the mesh connections:

    1. Select one or more Mesh Connection or Mesh Connection Group objects, right-click, and select Create Named Selections.

      A named selection is created for each mesh connection you selected. If you selected a mesh connection group, a named selection is created for each mesh connection within the group. Each named selection is automatically given the same name as the mesh connection from which you created it.

    2. Click a named selection to view the mesh for the mesh connection.

Tolerances Used in Mesh Connections

You can set two separate tolerances to define mesh connections. Setting appropriate tolerances is often critical to obtaining high quality mesh that adequately represents the geometry you want to capture.

The Tolerance value is used to find which bodies should be connected to which other bodies. Setting a larger Tolerance connects more bodies together, while setting it smaller may cause some connections to be missed. For this reason, you might want to set this to a larger value than needed. Setting a smaller value can avoid problems in automatic mesh connection creation, but can also result in other problems because the tolerance used in meshing is inherited from automatic mesh connection detection settings.

Using a Large Tolerance Value

For a large assembly for which you do not want to define mesh connections manually, automatic mesh connection detection provides many benefits. Setting a large Tolerance value to find connections yields more connections, which provides a higher level of comfort that the model is fully constrained. However, larger values can be problematic for the following reasons:

Using a Small Tolerance Value

When mesh connections are generated automatically, the Tolerance is used on the geometry edges and faces to determine which entities should be connected. However, the connections themselves are not generated until meshing occurs. Because the connections are performed on nodes and elements of the mesh rather than on the geometry, the tolerances do not translate exactly.

For example, in the case below, you would want to set a Tolerance that is slightly larger than the gap in the geometry. If the gap is defined as x and the tolerance is set to x, automatic mesh connection detection could find the connection, but the meshing process may result in mesh that is only partially connected.

Tips for Setting Tolerances

As detailed above, setting the correct tolerance can be very important, and in some cases may require some speculation and/or experimentation. The following tips may help:

Mesh Sizing and Mesh Connections

Mesh size has an effect on the quality and feature capture of a mesh connection as follows:

See Common Imprints and Mesh Connections.

Common Imprints and Mesh Connections

The tolerance for common imprints comes from the minimum element size in the footprint mesh, which is the horizontal plate in the example below. Common imprints are made if the gap between imprints is smaller than or equal to 5 percent of the element size in the connection region. For this reason, setting the mesh size appropriately is important to control whether the imprints will be common or not.

For example, in the case shown below, if you want a common imprint, the minimum element size (or element size if Size Function is Adaptive) should be >x.

In this case, you could scope local face mesh sizing on the horizontal plate to control the sizing.

Mesh Connections for Selected Bodies

You can select a geometric entity and lookup the mesh connection object in the tree outline. To find the relevant mesh connection object:

Mesh Connections Common to Selected Bodies

You can select a pair of geometric entities and lookup the shared Mesh Connection object in the tree outline. To find a relevant mesh connection object:

This option can be helpful for finding spurious mesh connections, in which case duplicates can be removed.

Displaying Multiple Views of Mesh Connections

Use the Body Views button on the Mesh Connections toolbar to display parts in separate auxiliary windows.

For closer inspection of mesh connections, you can use the Show Mesh option on the Graphics Options Toolbar along with Body Views and the Sync Views toggle button. When the Body Views button is engaged, any manipulation of the model in the Geometry window will also be reflected in both auxiliary windows. The Body Views toggle button enables you to display parts in separate windows and the Sync Views toggle button, when activated, causes any change in the Geometry window to also be reflected in the auxiliary windows.

Merging Mesh Connections

Mesh connections can be merged by selecting the desired objects, right-clicking, and selecting the Merge Selected Mesh Connections option. During the process, the application deletes the original objects and creates a new Mesh Connection object with a combined scoping.

Mesh Connections can only be merged under the following criteria:

When mesh connections are merged, the new mesh connections contain the merged set of entities as masters and slaves.


Note:  Be aware that the merge operation process can create undesired connections. This can create a connection that is not appropriate for mesh generation.


Diagnosing Failed Mesh Connections

The state of each mesh connection is displayed in the Tree Outline. For a description of the various states, see Understanding Mesh Connection and Contact Match States.

General Failures

In the event of a general mesh connection failure, the following approach is recommended:

  1. Select an ignored or failed mesh connection shown in the tree and look at Control Messages in the Details View.


    Note:  You can use the Filter to identify Mesh Connection objects that are State>Ignored. However, if a mesh connection is in an “error” state, it cannot be filtered in the tree.


  2. Click Yes, Click to Display to display related error messages.

  3. Right-click on the error messages:

    1. If a message provides “Problematic Geometry” information:

      1. Select the message, right-click, and select Show Problematic Geometry from the context menu.

        This action highlights the geometry in the Geometry window that is responsible for the message.


        Note:  Any error message that is related to a specific mesh connection will be associated with the slave geometry in the connection.


      2. Select the problematic bodies, right-click, and select Go To > Mesh Connections for Selected Bodies.

        This action highlights all mesh connections attached to the problematic geometry.

      3. Review the tolerances and mesh sizes associated with the highlighted connections.

    2. If a message provides “Go to Body” information:

      1. Select the message, right-click, and select Go to Body from the context menu.

        This action highlights the object in the Details view that is responsible for the message.

      2. Review the tolerances and mesh sizes associated with the highlighted body or bodies.

        This action highlights all mesh connections attached to the problematic geometry.

Mesh Connection Failure

If you receive an error or warning message about one or more mesh connections:

  1. Highlight and review the message.

  2. Right-click the message and select the option Go To Object. The corresponding Mesh Connection object that is at issue becomes active in the tree.

  3. Verify that all of the associated properties are properly defined.

  4. Right-click the message and select the option Show Problematic Geometry. The corresponding Master/Slave geometry that is at issue becomes highlighted in the Graphics window.

  5. Verify that the all of the associated geometries are properly defined.

Failures Due to Defeaturing from MultiZone Quad/Tri Meshing and/or Pinch Controls

Due to the patch independent nature of the MultiZone Quad/Tri mesh method, a connection may fail because the mesh is associated with some face of the body but not with the face that is involved in the connection. This type of mesh connection failure, which may also occur when pinch controls are defined, is the result of the part mesh being significantly defeatured prior to mesh connection generation. To avoid mesh connection failures when using MultiZone Quad/Tri and/or pinch controls, use one of the following approaches:

The software does not automatically extend the connection region because doing so may lose the engineering intent of the model.

For example, consider the two parts shown below.

If you are using the MultiZone Quad/Tri mesh method or pinch controls, the part mesh may look like the one shown below. Notice that one face has been defeatured out.

In this case:

Since you cannot always control which face is defeatured, the most robust and recommended approach is to include both faces in the mesh connection.

Points to Remember


Release 18.2 - © ANSYS, Inc. All rights reserved.