Context:
You can obtain data from a bolt load by using the field and history output request editors in the Step module. In the Domain section of the editor, select Bolt load and choose the desired bolt load from the menu that appears. For more information, see Creating an output request.
If you are working with native or imported geometry, create a partition that indicates the desired location of the bolt load. For more information, see The Partition toolset.”
If you are working with a solid part instance, create a datum axis that indicates the desired orientation of the bolt axis. You can also create a datum coordinate system and use one of its axes to indicate the desired orientation of the bolt axis. (For more information, see Creating datum axes.)
From the main menu, select .
Abaqus/CAE displays the Create Load dialog box.
In the Create Load dialog box, do the following:
- From the Category list, select Mechanical.
- From the Types for Selected Step list, select Bolt Load, and click Continue.
Select the internal 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 internal 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.
-
If you are using orphan mesh elements, you must select element faces to specify the internal 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.
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).
If the bolt is modeled with wire part instances, Abaqus/CAE displays the bolt load editor when you have finished choosing the side. If the bolt is modeled with solid part instances, you are prompted to select a datum axis.
If the bolt is modeled with solid part instances, select a datum axis that indicates the desired direction of the bolt axis. You can also select one of the axes of a datum coordinate system.
Abaqus/CAE displays the bolt load editor.
Click the arrow next to the Method field and select the loading method of your choice from the list that appears.
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.
If desired, specify an amplitude. (See The Amplitude toolset,” for more information.)
If you are creating a bolt load on a solid part instance or if you are editing a bolt load on a solid part instance in the first analysis step, an Edit axis button appears at the bottom of the editor. Click Edit axis if you want to change your datum axis selection.
Click OK to create the load and to close the Create Bolt Load dialog box.
Arrows appear in the viewport that represent the bolt load that you just created. For more information, see Understanding symbols that represent prescribed conditions.