Creating a Bearing Load

You can create a bearing load applied to a selected geometry. Bearing loads simulates contact loads applied to cylindrical parts.

Creating bearing loads is done in only one step and is much quicker than creating first a virtual part and then a load. Computation is also much less time-consuming, because bearing loads do not generate either costly contact beam elements or virtual mesh parts.

You have to select a cylindrical boundary of the part. Any type of revolution surface can be selected. In the bearing load definition, you have to specify the resulting contact force (direction and norm). The components of the force can be given either in the global or in a user axis system (similar to the distributed force).

Bearing loads are flexible: you can vary the angle sector on which the force is applied as well as the type of the profile distribution.

Before you begin: A structural analysis simulation containing a load set must be open.
Related Topics
Working with Excitations
Authorized Supports
Modifying the Axis System
Reviewing Specifications

  1. In the Loads toolbar, click Bearing Load .

    The Bearing Load dialog box appears.

  2. Optional: In the Name box, modify the name of the load.

  3. Select the cylindrical surfaces on which you want to apply a bearing load.

    Multi-selection must be used on different cylindrical surfaces and not on different elements belonging to a same cylindrical surface. Indeed, if you apply a 10N norm force vector on a multi-selection of three surfaces belonging to the same geometry, the norm of the global resultant force will be equal to 30N (and not 10N).

    To apply a 10N norm force vector on three different cylindrical surfaces, the following methods are equivalent:

    • Create three bearing loads (select one cylindrical surface for each bearing load) with a 10N norm force vector.
    • Create one bearing load (multi-select three cylindrical surfaces) with a 10N norm force vector.

  4. Optional: By default, the vector components are defined relative to the fixed global axis system (fixed global rectangular coordinate system). To choose a different axis system, select User in the Type list, and select a user axis system in the specification tree. See Modifying the Axis System.

    The name of the user axis system is displayed automatically in the Current axis box, and the components of the resultant force are defined relative to the specified rectangular axis system.Only the force vector component which is perpendicular to the revolution axis is taken into account because this component is a contact component.

  5. Optional: Select the Display locally check box to display the selected axis system locally on the geometry.

  6. Enter values for the X, Y and Z components of the resultant force vector to specify the three components for the direction of the resultant force.

    The norm is computed and displayed automatically. Upon modification of any of these four values, the resultant force vector components and magnitude are updated based on the last data entry. The resultant force vector remains constant independently of the geometry selection.

    You can define the resultant force vector direction using the compass. By applying the compass to any part geometry, you can align the compass directions with the implicit axis directions of that geometry: drag the compass by handling the red square and drop it on the appropriate surface. The normal direction to this surface defines the new direction. Then, click on the Compass Direction button to take this new direction into account. You can now invert the direction if desired, editing the values of the three components.

    Symbols appear on the selected support to reflect the force orientation.

  7. In the Angle box, enter an angle value.

    The angle value corresponds to the angle over which the forces can be distributed. When you enter an angle value, a highly precise preview automatically appears on the model. 0 is the default value, < 180 is useful to take into account some positive clearance, > 180 is useful to take into account some negative clearance.

  8. Choose the orientation type.

    • If you want that all the force vectors at the mesh nodes are normal to the surface in all points, select Radial. This is generally used for force contact.

    • If you want that all the force vectors at the mesh nodes are parallel to the resulting force vectors, select Parallel. This can useful in the case of specific loads.

  9. In the Profile list, select the profile type to define how the force intensity varies according to the angle.

    • Sinusoidal
    • Parabolic
    • Law: or F=f(Θ) requires that a formal law (Formal parameters) was defined in Knowledge Advisor (Fog). On the condition you previously activated the Show relations option in Tools > Options > Analysis and Simulation (General tab) command, you can see the Law feature in the specification tree. No sooner do you select this feature in the specification tree, that this formal parameter appears in the Law box (Bearing Load dialog box).

    Important: The profile defines the force repartition but it does not influence the force orientation. The force orientation is given by both the vector components and the distribution.

  10. Choose the distribution type to specify the force distribution.

    • Outward distribution (B pushes on A):

    • Inward distribution (A pushes on B):



  11. Click OK.

    The bearing load is created.