You can obtain linearized stresses along a line through your model. Abaqus/CAE separates the stress results along the line into constant membrane and linear bending
stresses and displays the results in the form of an X–Y plot.
From the main menu bar, select ToolsQuery or click the
tool in the Query toolset.
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 ToolsQuery or click the
tool in the Query toolset 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/CAEalways 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.
Select Use Maximum Stress Value to use the maximum
available value at a point.
By default, Abaqus/CAE will use the average of multiple values available at a point.
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.