You can select the variable to display for contour plots, model probing, view cuts based on an isosurface, and for which to obtain results along a model path; this variable is called the primary field output variable. Abaqus/CAE also uses the primary field output variable to form display groups, to apply color coding based on results, and for display of loads, predefined fields, or interactions from a model in the current model database.
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,” Section 4.2 of the Abaqus Analysis User's Guide.
To select the primary field output variable:
Locate the options that control the primary field output variable.
From the main menu bar, select Result
Field Output. Click the Primary Variable tab in the dialog box that appears.
The Primary Variable options appear.
Tip: You can also access these options by clicking the Field Output button in any dialog box in which it appears.
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.
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,” Section 56.1, and “Customizing the state block,” Section 56.3. 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.
