Context:
When an output database is selected,
Abaqus/CAE
lists for your selection all variables available at the current
step and frame of your
output database by default. An
asterisk to the left of the description indicates that the variable includes
complex number results.
When a model in the current model database is selected,
Abaqus/CAE
lists for your selection all loads, predefined fields, boundary conditions, and
interactions available in the current step of your model by default. All of
these selectable items are preceded by a letter in parentheses to distinguish
them by category: (L) for loads, (P)
for predefined fields, (B) for boundary conditions, and
(I) for interactions. Only the real part of a complex load
or predefined field is available for display.
Use the Primary Variable options in the Field
Output dialog box to choose the variable and, if applicable, the
invariant or component that you want. For information on individual output
variable identifiers, see
Output Variables.
Locate the options that control the primary field output variable.
From the main menu bar, select. Click the Primary
Variable tab in the dialog box that appears.
The Primary Variable options appear.
To see the complete descriptions of the variables listed, increase the
width of the dialog box by dragging one corner.
To control which variables appear in the Name and
Description list:
- Toggle List only variables with results to
display a list that is limited by the storage location of the variables.
Limiting the list helps you select variables by presenting, for example, only
integration point quantities.
When List only variables with results is on,
filter options become available in the pull-down menu.
- Click the List only variables with results
arrow to reveal the filter options.
- Click the text stating the location of the variables you want to
include in the Name and Description
list.
The text appears in the List only variables with
results box, and the Name and
Description list is refreshed to include only variables
having that location.
From the Name and
Description list, click the name of the analysis variable
that you want. An asterisk to the left of the description in the list indicates
that the variable includes complex number results.
The selected variable is highlighted. If applicable, the
Component and Invariant lists on the
bottom of the dialog box are refreshed to display available components or
invariants, respectively.
If items are listed in the Component or
Invariant list, click the component or invariant that you
want.
The selected component or invariant is highlighted.
Note:
For S and E field output, there are two invariants, Max.
Principal (abs) and Max. In-Plane Principal
(abs), which are available only in
the Visualization module.
Max. Principal (abs) is the largest principal value when
the absolute value of all principal values are compared. Max.
In-Plane Principal (abs) is the largest principal value when the
absolute value of all in-plane principal values are compared. The out-of-plane
principal value is not considered when the Max. In-Plane Principal
(abs) value is computed.
When active, a contour plot in the current viewport changes to show
values for the analysis variable you have specified. If active, the text in the
legend and state block changes to identify the variable associated with the
plot. For more information on the legend and state block, see
Customizing the legend,
and
Customizing the state block.
In addition,
Abaqus
refreshes all dialog boxes in which the current primary variable is identified.
Your changes are saved for the duration of the session.