Graphical postprocessing is important because of the great volume of data created during a simulation. ABAQUS/Viewer allows you to view the results graphically using a variety of methods, including deformed shape plots, contour plots, symbol plots, animations, and X–Y plots. All of these methods are discussed in this guide. For more information on any of the postprocessing features discussed in this guide, consult the sections on the Visualization module in the ABAQUS/CAE User's Manual. For this example you will use ABAQUS/Viewer to do some basic model checks and to display the deformed shape of the frame.
Start ABAQUS/Viewer by typing
abaqus viewerat the operating system prompt. The ABAQUS/Viewer window appears.
Reading the output database file
To begin this exercise, open the output database file that ABAQUS/Explicit generated during the analysis of the problem.
To open the output database file:
From the main menu bar, select File
Open; or use the 
tool in the toolbar.
The Open Database dialog box appears.
From the list of available output database files, select frame_xpl.odb.
Click OK.
Tip: You can also open the output database frame_xpl.odb by typing
abaqus viewer odb=frame_xplat the operating system prompt.
ABAQUS/Viewer displays a fast plot of the model. A fast plot is a basic representation of your undeformed model shape and is an indication that you have opened the desired file.
Important: The fast plot does not display results and cannot be customized; for example, to display element and node numbers. You must display the undeformed model shape to customize the appearance of the model.
The title block at the bottom of the viewport indicates the following:
The description of the model (from the first line of the *HEADING option in the input file).
The name of the output database (from the name of the analysis job).
The product name (ABAQUS/Standard or ABAQUS/Explicit) and version used to generate the output database.
The date the output database was last modified.
Which step is being displayed.
The increment within the step.
The step time.
Displaying and customizing an undeformed shape plot
You will now display the undeformed model shape and use the plot options to enable the display of node and element numbering in the plot.
From the main menu bar, select PlotUndeformed Shape; or use the 
tool in the toolbox. ABAQUS/Viewer displays the undeformed model shape, as shown in Figure 2–13.
To display node numbers:
From the main menu bar, select OptionsUndeformed Shape.
The Undeformed Shape Plot Options dialog box appears.
Click the Labels tab.
Toggle on Show node labels.
Click Apply.
ABAQUS/Viewer applies the change and keeps the dialog box open.
To display element numbers:
In the Undeformed Shape Plot Options dialog box, toggle on Show element labels.
Click OK.
ABAQUS/Viewer applies the change and closes the dialog box.
To suppress the display of node and element numbers in the undeformed shape plot, repeat the above procedure and toggle off Show node labels and Show element labels.
Displaying and customizing a deformed shape plot
You will now display the deformed model shape and use the plot options to change the deformation scale factor and overlay the undeformed model shape on the deformed model shape.
From the main menu bar, select PlotDeformed Shape; or use the 
tool in the toolbox. ABAQUS/Viewer displays the deformed model shape, as shown in Figure 2–16.
The scale factor for the deformed plot is displayed in the state block. By default, the displaced shape is not scaled. For this analysis, change the deformation scale factor so that the displaced shape is evident.
To change the deformation scale factor:
From the main menu bar, select OptionsDeformed Shape.
In the Deformed Shape Plot Options dialog box, click the Basic tab if it is not already selected.
From the Deformation Scale Factor area, toggle on Uniform and enter 40.0 in the Value field.
Click Apply to redisplay the deformed shape.
The plot title displays the new scale factor.
To overlay the undeformed model shape on the deformed model shape:
In the Deformed Shape Plot Options dialog box, toggle on Superimpose undeformed plot.
Click OK.
By default, ABAQUS/Viewer plots the undeformed model shape in green and the deformed model shape in white. Change the line style of the undeformed model shape to more clearly distinguish the two plots.
To change the undeformed model shape's line style:
From the main menu bar, select OptionsUndeformed Shape.
The Undeformed Shape Plot Options dialog box appears.
Click the Color & Style tab.
In the Edge Attributes area, choose the dotted line style.
Click OK.
To return the undeformed plot's line style to solid, repeat the above procedure and select the solid line style. Alternatively, to return all the undeformed plot options to their default values, you can click Defaults in the Undeformed Shape Plot Options dialog box.
Checking history data with ABAQUS/Viewer
By default, both the model data and history data are written to the output database file during the datacheck phase. Thus, you can use ABAQUS/Viewer to check that the input data are correct before running the simulation. You have already learned how to draw plots of the model and to display the node and element numbers. These are useful tools for checking that ABAQUS is using the correct mesh.
The boundary conditions applied to the overhead hoist model can also be displayed using ABAQUS/Viewer.
To display boundary conditions on the undeformed model:
From the main menu bar, select PlotUndeformed Shape; or use the tool in the toolbox.
From the main menu bar, select ViewODB Display Options.
In the ODB Display Options dialog box, click the Entity Display tab.
Toggle on Show boundary conditions.
Click OK.
Exiting ABAQUS/Viewer
From the main menu bar, select FileExit to exit ABAQUS/Viewer.
