You can display a plot of your model showing the deformed shape during each frame of the analysis. When you request a deformed shape plot of data from a force-displacement analysis, ABAQUS plots the nodal displacements by default; but you can display any nodal vector field output variable that is available on the output database. You can also use the plot options to customize the appearance of a deformed plot.
Most procedures in ABAQUS/Standard or ABAQUS/Explicit write displacement to the output database by default and also select displacement for the nodal vector quantity to use as the default deformed variable. When ABAQUS reads the output database, it uses the default deformed variable to determine the shape of a deformed plot. In the elastomeric block example the user requested output of the displacements (U) for every node in the model after every 10 increments, and displacement was selected as the default deformed variable.
(Some procedures—for example, heat transfer—do not write nodal vector quantities to the output database by default and do not select a variable as the default deformed variable. Therefore, ABAQUS cannot display a deformed plot, since in such cases the output database does not contain any variables that can be used to compute a deformed shape.)
To display a deformed shape plot:
From the main menu bar, select Plot
Deformed Shape.
Tip:
You can also plot the deformed model using the 
tool in the Visualization module toolbox.
ABAQUS displays the deformed model in the same increment and step that it last displayed the undeformed model. The state block indicates the default deformed variable being plotted (U) and the deformation scale factor (1.000e+00). ABAQUS selects a default deformation scale factor of 1.00 for large-displacement analyses. If the deformation is small (for example, for a perturbation analysis), ABAQUS increases the scale factor. Conversely, if the deformation is large, ABAQUS decreases the scale factor to fit the viewport optimally.
The buttons in the prompt area allow you to move between frames of the analysis, but you can also move directly to a selected step and increment using the following technique:
From the main menu bar, select ResultStep/Frame.
ABAQUS displays the Step/Frame dialog box.
Select Step 1, Increment 0, and click Apply.
The Step/Frame dialog box also displays the step time associated with an increment. Use the Step/Frame dialog box to display the deformed model approximately halfway through the second step.
Use a combination of the buttons in the prompt area and the Step/Frame dialog box to view the deformed plot in different frames and in different steps.
Display the deformed model after the last increment of the third step (Step 3 and Step Time = 10.00), as shown in Figure D–5.
Click Cancel to close the Step/Frame dialog box.
You can use the deformed plot options to customize the appearance of your deformed plot.
To customize a deformed shape plot:
From the main menu bar, select OptionsDeformed Shape.
ABAQUS displays the Deformed Shape Plot Options dialog box.
Click the Basic tab if it is not already selected, and toggle on Superimpose undeformed plot.
Click the Labels tab, and toggle on Show node symbols.
Click OK to apply your changes and to close the Deformed Plot Options dialog box.
ABAQUS displays the customized deformed plot overlaid with the undeformed plot.
To turn off the fill color and the element numbering of the undeformed plot, select OptionsUndeformed Shape from the main menu bar.
ABAQUS displays the Undeformed Shape Plot Options dialog box.
Note: The button at the far right of the prompt area displays the options dialog box for the current plot mode—Deformed Shape Plot Options in this example. You must use the main menu bar to display the undeformed plot options.
From the buttons at the bottom of the Undeformed Shape Plot Options dialog box, click Defaults. Click OK to apply the default undeformed plot options and to close the Undeformed Shape Plot Options dialog box.
ABAQUS displays the customized deformed plot, as shown in Figure D–6.
