To view the results of your analysis:

After you select Results in the Model Tree, ABAQUS/CAE enters the Visualization module, opens Deform.odb, and displays the undeformed shape of the model, as shown in Figure B–13.

Figure B–13 Undeformed shape plot of model (title block suppressed).



The title block indicates the following:

The job description.

The output database from which ABAQUS/CAE read the data.

The version of ABAQUS/Standard or ABAQUS/Explicit that was used to generate the output database.

The date the output database was generated.

The state block indicates the following:

The step name and the step description.

The increment within the step.

The step time.

When you are viewing a deformed plot, the deformed variable and the deformation scale factor.

By default, ABAQUS/CAE plots the last step and the last frame of your analysis. Buttons that allow you to control which analysis results are plotted are available in the prompt area.

From the main menu bar, select PlotDeformed Shape to view a deformed shape plot.

Click the auto-fit tool so that the entire plot is rescaled to fit in the viewport, as shown in Figure B–14.

Figure B–14 Deformed shape plot of model (title block suppressed).



From the main menu bar, select PlotContoursOn Deformed Shape to view a contour plot of the von Mises stress, as shown in Figure B–15.

Figure B–15 Contour plot of Mises stress (title block suppressed).



For a contour plot the default variable displayed depends on the analysis procedure; in this case, the default variable is the von Mises stress. From the main menu bar, select ResultField Output to examine the variables that are available for display.

ABAQUS/CAE displays the Field Output dialog box; click the Primary Variable tab to choose which variable to display and to select the invariant or component of interest. By default, the Mises invariant of the Stress components at integration points variable is selected.

Click Cancel to close the Field Output dialog box.