-
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 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.
-
If you selected the Interior Surface method, do the
following:
-
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,
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.
-
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.
-
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.
-
If you selected the Bolt Shank Surface method, do the
following:
-
Select the bolt shank face to partition. You can only select a
cylindrical face.
-
In the prompt area, enter the cut position value to define the
partition location.
-
Click Done.
Abaqus/CAE creates an interior surface by partitioning the selected face and 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.)
-
By default, the surface normal of the pre-tension section is fixed during
analysis. Toggle on Varying normal for pre-tension section
to write the
FOLLOWER=YES
for pre-tension section at part level. If you selected the Pre-tension
section at part level option, it indicates that the normal is
updated when performing a large-displacement analysis.
-
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.
-
Select Specify.
-
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.
-
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 the instances from
the same part.
-
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.
|