Locate the stress linearization options.
From the main menu bar, select
or click the
tool in the
Query toolbar.
The Query dialog box appears.
Select Stress linearization.
The Stress Linearization dialog box appears.
In the Stress line name field, provide a name for
the stress line. This name will be used as a prefix for the linearized results.
To save the X–Y data that will be
generated, toggle on Save XY data. The data will be
available for the duration of your
Abaqus/CAE
session.
To save the endpoints and interval points as a path, toggle on
Save stress line to path. The points of the stress line
will be saved for the duration of your
Abaqus/CAE
session as a point list path with the same name as the stress line.
Select the endpoints for the stress line by selecting nodes or points
in space or by selecting a saved path.
- Manual
-
This is the default method. You can select nodes directly from the
viewport or type in node labels or points in space.
- To select nodes directly
from the viewport:
-
Click
to the right of the Start and
End fields, and click on the desired nodes in the
viewport.
The node labels, including the part instance name, will appear in the
text field for the Start and End
points of the stress line.
- To type in
node labels or points in space:
-
-
In the Start text field, enter a part
instance name and node label or the coordinates of a point in space. The part
instance name and node label must be of the form
Instance.Node;
specify coordinate values as X-, Y-,
and Z-coordinates separated by spaces or commas.
If you do not know the part instance names in the model, use the
previous method to select a node directly from the viewport. Alternatively, you
can select
or click the
tool in the
Query toolbar
and choose the Probe values method to determine the
instance name and node label (for more information, see
Understanding probing).
-
Repeat the preceding step to complete the End
text field.
- From a path
-
Toggle on From a path, and select a path name
from the list that appears; you cannot use an edge list path to define the
endpoints of a stress line. (For more information on paths, see
Viewing results along a path.”)
Abaqus/CAE
uses the endpoints of the saved path as the endpoints of the stress line. The
points are defined in the same manner as they were originally defined in the
path—a node list path provides node points on the model, and a point list path
or circular list path provides the coordinates of points in space.
Regardless of the method you use to select the endpoints,
Abaqus
highlights the stress line in the viewport and labels the start and end. If you
selected node points or a node list path to define the endpoints of the stress
line, the labels in the viewport indicate the node numbers.
Note:
If you chose to save the stress line as a path in Step 5,
Abaqus/CAE
always saves a point list path—even if you
selected nodes, node labels, or a node list path to define the stress line.
Choose the model shape for which to obtain the stress results. The
default is to obtain the results for the deformed model shape. Toggle on
Undeformed to obtain results for the undeformed model
shape.
Specify the number of intervals into which the stress line should be
divided. Type a positive integer greater than 0 into the Number of
intervals on stress line text field. If you do not enter a number,
Abaqus
will use a default number of intervals.
By default,
Abaqus/CAE
writes the linearized stress values (including all available components of
stress and the computed linearized stress invariants) to a file called
linearStress.rpt. If you do not wish to write this report,
you can toggle off Write to file in the
Report area of the dialog box.
You can specify a new name for the report file by entering the name
in the File name field or clicking
and choosing from the list of existing files that appears.
If you write the report to an existing file, the new data will be
appended to the file by default; if you wish to overwrite the file, toggle off
Append to file.
Click the Computations tab.
Select the stress components to be linearized by toggling on each
membrane and bending component.
Select the bending components to use for calculating invariants.
For axisymmetric models enter an approximate value for the in-plane
radius of curvature of the midplane of your model at the location of the stress
line. The default value is Infinite, which implies a
lack of curvature. To specify a radius of curvature, click
Specify and enter a number in the text field.
For axisymmetric models enter an approximate value for the
out-of-plane radius of curvature of the midplane of your model at the location
of the stress line. The default value is Compute, which
allows
Abaqus
to calculate the radius based on the axisymmetric shape and the position of the
selected stress line. To specify a radius of curvature, click
Specify and enter a number in the text field.
For nonaxisymmetric models select whether
Abaqus
should use curvature correction. If curvature correction is selected, specify a
local coordinate system or use the default (global) coordinate system; if you
use a local coordinate system for curvature correction, you can also use that
local coordinate system to evaluate stress line orientation.
Click OK.
An X–Y plot similar to the one shown in
Figure 1
appears in the viewport.
Figure 1. Stress linearization results.