Create the Global Finite Element Model

Define the meshes for the global finite element model.

A global finite element model (FEM) is typically composed of relatively coarse meshes to allow for a quick analysis of the model's key regions. When you define the global FEM, you can use automated modeling tools to define the mesh procedures and specifications for each part. You can then create the meshes in a single process.

In this example, a mesh of quadratic tetrahedral elements with a 10-mm mesh size is adequate for the global FEM.

  1. From the Compass, click Model Assembly Design.
  2. From the Automated FEM section of the action bar, click Automated FEM .

    Note: If a Confirmation dialog box displaying the message Product structure not up to date appears, click Yes to continue.

    The Automated FEM dialog box appears, indicating the available methods for generating a FEM representation.
  3. From the General Purpose section, click User Driven.
    The Automated FEM: User Driven dialog box appears and displays the structure of the model.
  4. Right-click the Procedure cell for any row containing a part, such as Hollow shaft A.1.
  5. From the context menu, click Apply Procedure > Tetrahedron Mesh.

    Tip: If the context menu does not show Tetrahedron Mesh, do the following:
    1. From the context menu, click Other Procedure.
    2. In the Preferred procedures section, under Parameters based procedures, click Tetrahedron Mesh.

      You can also select Submodel Tetrahedron Mesh so that it is available when you create the submodel FEM later in this example.

    The Inputs dialog box appears.
  6. Edit the inputs for the procedure.
    1. From the Selection mode options, select All geometries.
    1. Enter 10mm as the Mesh size.
    2. From the Element order options, select Linear.
    3. Enter 0.1mm as the Sag value.
    4. Select Create solid section.

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

    5. Click OK.
  7. Right-click the Tetrahedron Mesh procedure that you previously applied, and select Apply same procedure with inputs > To all.

    The app applies the tetrahedron mesh to all parts in the model, using the same input parameters that you defined for the first part.

  8. Click Run.
    The Finite Element Model dialog box appears, showing the progress as the app creates the FEM representations for all the parts. This process might take several minutes. When the process completes, the results become available in the Automated FEM: User Driven dialog box and the updateapp the model in the 3D area.
  9. Click Refresh to update the mesh, and then click Yes to refresh the session.

    The app shows the new finite element model names in the Procedure column, and the Report column shows the status of each mesh. All rows show a report with a green dot indicating no problems with the meshes. You can click the reports to see more details.

  10. From the tree, right-click the driveshaft assembly's new FEM representation, click Properties, and rename it Global FEM.

    Renaming objects makes it easier to identify them in the tree, especially when your simulation includes multiple objects of the same type.

    Tip: Press F3 to display the tree if it is not visible.

  11. Click OK.
    The 3D area displays the global model with all of its parts meshed. The app meshed each part individually and collected the meshes to create the global FEM.