Define the Loads and Restraints

Define the force that attempts to move the driveshaft assembly, and define the restraints that anchor the assembly.

In this example, you define a rotational force on the sprocket to mimic the driveshaft assembly's operational conditions. You also place restraints on the support shaft, because this part does not move during normal operation of the driveshaft assembly.

  1. Ensure that the analysis context is set to Submodel Analysis.
  2. From the Boundary Conditions section of the action bar, click Submodel Displacement .

    This feature transfers the displacement degrees of freedom from the global model to the submodel along their shared boundaries, such that the submodel motion follows that of the global model.

  3. Select the cut faces at the ends of the hollow shaft and the supportive shaft.
    1. From the tree, expand the shaft parts.
    2. Select the submodel FEMs (that is, the second FEM in each part).
    3. Hide the meshes.

      Tip: To hide a mesh, you can right-click the FEM in the tree and then select Hide/Show .

    4. In the 3D area, select the cut faces of the shaft parts.



  4. For the Global Step, select Static Step.1.
  5. Click OK.
  6. Change the analysis context to Global Analysis.
  7. From the Loads section of the action bar, click Force .
  8. Select one of the valleys between the gear teeth on the sprocket, and enter -1000N in the global Z-direction.
    The app applies the force, as shown below. The force transfers from the sprocket teeth to the driveshaft as a pure rotational force.

  9. From the Boundary Conditions section of the action bar, click Fixed Displacement .
  10. In the 3D area, select the end of the support shaft that is furthest from the sprocket.
  11. Select the X, Y, and Z rotational and translation degrees of freedom, and click OK.
    The restraint is shown below.

  12. Change the analysis context to Submodel Analysis.
  13. Similarly, create a restraint on the end of the support shaft that is closest to the sprocket.

    The displacement restraints for the submodel use only one end of the shaft. The submodel displacement load supports the shaft at the boundary between the global model and the submodel.