Getting Started with ABAQUS/Standard: Keywords Version  


2.7 Postprocessing with ABAQUS/Viewer

Graphical postprocessing is important because of the great volume of data created during a simulation. For any realistic model it is impractical for you to try to interpret results in the tabular form of the data file. ABAQUS/Viewer allows you to view the results graphically using a variety of methods, including deformed shape plots, contour plots, vector 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 viewer
at 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/Standard generated during the analysis of the problem.

To open the output database file:

  1. From the main menu bar, select FileOpen; or use the tool in the toolbar.

    The Open Database dialog box appears.

  2. From the list of available output database files, select frame.odb.

  3. Click OK.

    Tip:  You can also open the output database frame.odb by typing 

    abaqus viewer odb=frame
    at the operating system prompt.

    ABAQUS/Viewer opens the output database created by the job and displays the undeformed model shape, as shown in Figure 2–15.

    Figure 2–15 Undeformed model shape.

    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.

    The state block at the bottom of the viewport indicates the following:

    • Which step is being displayed.

    • The increment within the step.

    • The step time.

    The view orientation triad indicates the orientation of the model in the global coordinate system.

The Results Tree

You will use the Results Tree to query the components of the model. The Results Tree allows easy access to the history output contained in an output database file for the purpose of creating X–Y plots and also to groups of elements, nodes, and surfaces based on set names, material and section assignment, etc. for the purposes of verifying the model and also controlling the viewport display.

To query the model:

  1. In the left side of the main window, click the Results tab to switch to the Results Tree.

  2. All output database files that are open in a given postprocessing session are listed underneath the Output Databases container. Expand this container and then expand the container for the output database named frame.odb.

  3. Expand the Materials container and click the material named STEEL.

    All elements are highlighted in the viewport because only one material assignment was used in this analysis.

The Results Tree will be used more extensively in later examples to illustrate the X–Y plotting capability and manipulating the display using display groups.

Customizing an undeformed shape plot

You will now use the plot options to enable the display of node and element numbering. Plot options that are common to all plot types (undeformed, deformed, contour, symbol, and material orientation) are set in a single dialog box. The contour, symbol, and material orientation plot types have additional options, each specific to the given plot type.

To display node numbers:

  1. From the main menu bar, select OptionsCommon, or use the tool in the toolbox.

    The Common Plot Options dialog box appears.

  2. Click the Labels tab.

  3. Toggle on Show node labels.

  4. Click Apply.

    ABAQUS/Viewer applies the change and keeps the dialog box open.

The customized undeformed plot is shown in Figure 2–16.

Figure 2–16 Node number plot.

To display element numbers:

  1. In the Labels tabbed page of the Common Plot Options dialog box, toggle on Show element labels.

  2. Click OK.

    ABAQUS/Viewer applies the change and closes the dialog box.

The resulting plot is shown in Figure 2–17.

Figure 2–17 Node and element number plot.

To disable the display of node and element numbers, repeat the above procedure and, under Labels, 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. You will also superimpose 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 2–18.

Figure 2–18 Deformed model shape.

For small-displacement analyses the displacements are scaled automatically to ensure that they are clearly visible. The scale factor is displayed in the state block. In this case the displacements have been scaled by a factor of 42.83.

To change the deformation scale factor:

  1. From the main menu bar, select OptionsCommon, or use the tool in the toolbox.

  2. From the Common Plot Options dialog box, click the Basic tab if it is not already selected.

  3. From the Deformation Scale Factor area, toggle on Uniform and enter 10.0 in the Value field.

  4. Click Apply to redisplay the deformed shape.

    The state block displays the new scale factor.

To return to automatic scaling of the displacements, repeat the above procedure and, in the Deformation Scale Factor field, toggle on Auto-compute.

To superimpose the undeformed model shape on the deformed model shape:

  1. Click the tool in the toolbox to allow multiple plot states in the viewport, then click the tool or select PlotUndeformed Shape to add the undeformed shape plot to the existing deformed plot in the viewport.

    By default, ABAQUS/Viewer plots the deformed model shape in green and the (superimposed) undeformed model shape in a translucent white (appears gray).

  2. The plot options for the superimposed image are controlled separately from those of the primary image. From the main menu bar, select OptionsSuperimpose; or use the tool in the toolbox to suppress the translucency of the superimposed (i.e., undeformed) image.

  3. From the Superimpose Plot Options dialog box, click the Other tab.

  4. In the Other tabbed page, select the Translucency tab.

  5. Toggle off Apply translucency.

  6. Click OK to close the Superimpose Plot Options dialog box and apply the changes.

The plot is shown in Figure 2–19.

Figure 2–19 Undeformed and deformed model shapes.

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 and checked using ABAQUS/Viewer.

To display boundary conditions on the undeformed model:

  1. From the main menu bar, select PlotUndeformed Shape; or use the tool in the toolbox.

  2. From the main menu bar, select ViewODB Display Options.

  3. In the ODB Display Options dialog box, click the Entity Display tab.

  4. Toggle on Show boundary conditions.

  5. Click OK.

    ABAQUS/Viewer displays symbols to indicate the applied boundary conditions, as shown in Figure 2–20.

Figure 2–20 Applied boundary conditions on the overhead hoist.

Exiting ABAQUS/Viewer

From the main menu bar, select FileExit to exit ABAQUS/Viewer.