To define bolt loads:

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 Chapter 44, “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,” Section 40.7.)

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.

In the viewport, use the mouse to select the internal surface that indicates the location of the bolt load. You can use a combination of drag select, [Shift]+Click, [Ctrl]+Click, and the angle method to select more than one face or edge. For more information, see “Selecting objects within the current viewport,” Section 6.2.

Tip:  If you are unable to select the desired faces or edges, you can change the selection behavior by clicking the selection options tool in the prompt area. For more information, see “Using the selection options,” Section 6.3.

When you have finished selecting, click mouse button 2. For detailed information on selecting surfaces on wire part instances, see “Specifying a particular side or end of a region,” Section 48.2.5.)

If the bolt is modeled with wire part instances, ABAQUS/CAE displays the bolt load editor when you have finished selecting the cross-section surface. 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 Chapter 38, “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,” Section 16.5.