Creating and editing bolt loads

You can create bolt loads to model tightening forces or length adjustments in bolts or fasteners.

See Also
Creating and modifying prescribed conditions
Understanding symbols that represent prescribed conditions
In Other Guides
Prescribed Assembly Loads
  1. From the main menu, select LoadCreate.

    Abaqus/CAE displays the Create Load dialog box.

  2. In the Create Load dialog box, do the following:
    1. From the Category list, select Mechanical.
    2. From the Types for Selected Step list, select Bolt Load, and click Continue.
  3. Select the method to specify the surface that defines the bolt cross-section.
    • Select Interior Surface to use a previously created interior surface.
    • Select Bolt Shank Surface to create an interior surface by partitioning the bolt shank surface.
  4. If you selected the Interior Surface method, do the following:
    1. Select the interior surface or wire segment that indicates the location of the bolt load.

      • If you are working with native or imported geometry, use the mouse to select the interior surface or wire segment in the viewport. You can use a combination of drag select, ShiftClick, CtrlClick, and the angle method to select more than one face or edge. For more information, see Selecting objects within the current viewport.

        Tip: If you are unable to select the desired faces or edges, you can use the Selection toolbar to change the selection behavior. For more information, see Using the selection options.

      • If you are using orphan mesh elements, you must select element faces to specify the interior surface. You can use display groups to remove selected elements from the viewport to reveal the element faces of the cross-section surface. For more information, see Using display groups to display subsets of your model.

      When you have finished selecting, click mouse button 2.

    2. Choose the side on which the surface is defined using the techniques described in Specifying a particular side or end of a region. The side you select determines which elements are adjusted to produce the desired tightening load or length adjustment (see Prescribed Assembly Loads for details).
    Abaqus/CAE displays the bolt load editor.
  5. If you selected the Bolt Shank Surface method, do the following:
    1. Select the bolt shank face to partition. You can only select a cylindrical face.
    2. In the prompt area, enter the cut position value to define the partition location.
    3. Click Done.
    Abaqus/CAE creates an interior surface by partitioning the selected face and displays the bolt load editor.
  6. Click the arrow next to the Method field and select the loading method of your choice from the list that appears.
  7. In the Magnitude field, enter the force magnitude (for the Apply force method) or the change in length (for the Adjust length method).

    Note:

    The Fix at current length method becomes available if you edit the load in a step that follows the step in which you create the load. If, while editing the load, you change the method to Fix at current length, the Magnitude field becomes unavailable.

  8. If desired, specify an amplitude. (See The Amplitude toolset for more information.)
  9. By default, the surface normal of the surface that defines the bolt cross-section is used as the bolt axis. If desired, you can define a different bolt axis direction.
    1. Select Specify.
    2. Select a datum axis.

      • To create a datum axis, click and select two points in the viewport that define the axis. If desired, select Make Independent from the prompt area to create the datum as an independent feature.
      • Click , and select a datum axis that is aligned with the bolt centerline.

  10. The pre-tension section is written at the assembly level. Toggle on Pre-tension section at part level to write the pre-tension section at the part level (applicable only for dependent part instances). If you selected the Pre-tension section at part level option, the bolt load is defined for all of the instances from the same part.
  11. Click OK to create the load and to exit the editor.

    Arrows appear in the viewport that represent the bolt load that you just created. For more information, see Understanding symbols that represent prescribed conditions.