Create the Submodel Finite Element Model

Define the meshes for the submodel finite element model.

A submodel finite element model (FEM) is typically composed of relatively fine meshes to allow for an accurate analysis of the submodel region. When you define a submodel FEM, you can use automated modeling tools to define the mesh procedures and specifications for each part, and then create the meshes in a single process.

In this example, you use the same automated modeling tools that you used to create the global FEM to define the submodel FEM. Since you used a 10-mm mesh size for the global FEM, you use a 5-mm mesh size for the submodel FEM.

  1. From the tree, double-click EXAMPLE-Driveshaft-Subassembly A.
    The 3DEXPERIENCE platform returns to Model Assembly Design.
  2. From the Automated FEM section of the action bar, click Automated FEM .
    The Automated FEM dialog box appears, indicating the available methods for generating a FEM representation.
  3. From the General Purpose methods, click User Driven.
    The Automated FEM: User Driven dialog box appears and displays the structure of the model. The plane is hidden because it is an abstraction shape, not a geometry that you can mesh.
  4. Select the rows for both the hollow shaft and the support shaft.
  5. Right-click the Procedure cell for one of the selected rows.
  6. From the context menu, click Apply Procedure > Submodel Tetrahedron Mesh.

    You can apply a submodel procedure only to the parts that extend through the submodel boundaries. The submodel meshing procedure ensures continuity from the coarse mesh of the global FEM to the finer mesh of the submodel FEM. In this example, the hollow shaft and supportive shaft cross the plane that defines the submodel. Therefore, you must define a submodel procedure for both of these parts before meshing them.

  7. Edit inputs for the submodel procedure.
    1. Select the rows for both the hollow shaft and the support shaft, and right-click the Procedure cell for one of the selected rows.
    2. From the context menu, click Edit Inputs.
    3. For the Cutting surface, use the tree to expand Abstraction Plane > PartBody, and select Plane.1.
    4. Enter 5mm as the Mesh size.
    5. From the Element order options, select Linear.
    6. Enter 0.1mm as the Sag value.
    7. Select Create solid section.

      You must create a solid section before you can apply a material definition to the parts.

    8. Click OK.
  8. In the Automated FEM dialog box, select the rows for the remaining parts in the submodel (that is, the sprocket, bearing, distance washer, and bearing stopper).

    These parts all belong to the submodel exclusively. They do not cross the submodel boundaries.

    Important: Do not use the Submodel Tetrahedron Mesh procedure for these parts. The app uses the submodel procedure only for those parts that are cut by the submodel boundaries (the two shafts).

  9. Similar to the procedure you defined for the hollow shaft and the support shaft, apply a procedure to these parts using a tetrahedron mesh, a 5-mm mesh size, and a 0.1-mm sag to create the solid sections.

  10. Click Run.
    The Finite Element Model dialog box appears, showing the solver's progress as it creates the FEM representations for the parts.
  11. When the process completes, click Yes to refresh the session.
    The Automated FEM dialog box displays the results, and the app updates the 3D area to show only the submodel. For visual clarity, the image below shows the submodel without the meshes.

  12. You may ignore bad elements in these meshes.

    Bad elements indicate that a tetrahedron mesh element's shape is skewed or stretched. Addressing bad elements is not within the scope of this example.

  13. Right-click the new FEM representation in the tree, and rename it Submodel FEM.

The 3D area displays the submodel with all of its parts meshed. The app meshed each part individually and collected the meshes to create the submodel FEM.