Postprocessing the dynamic analysis results

For the static linear perturbation analysis done in Abaqus/Standard you examined the deformed shape as well as stress, displacement, and reaction force output. For the Abaqus/Explicit analysis you can similarly examine the deformed shape and generate field data reports. Because this is a dynamic analysis, you should also examine the transient response resulting from the loading. You will do this by animating the time history of the deformed model shape and plotting the displacement history of the bottom center node in the truss.

This task shows you how to:

Context:

Plot the deformed shape of the model. For large-displacement analyses (the default formulation in Abaqus/Explicit) the displaced shape scale factor has a default value of 1. Change the Deformation Scale Factor to 20 so that you can more easily see the deformation of the truss.

Create a time-history animation of the deformed model shape

  1. From the main menu bar, select AnimateTime History; or use the tool in the toolbox.

    The time history animation begins in a continuous loop at its fastest speed. Abaqus/CAE displays the movie player controls in the right side of the context bar (immediately above the viewport).

  2. From the main menu bar, select OptionsAnimation; or use the animation options tool in the toolbox (located directly underneath the tool).

    The Animation Options dialog box appears.

  3. Change the Mode to Play Once, and slow the animation down by moving the Frame Rate slider.

  4. You can use the animation controls to start, pause, and step through the animation. From left to right of Figure 1, these controls perform the following functions: play/pause, first, previous, next, and last.

    Figure 1. Postprocessing animation controls.

Create an X–Y plot of the vertical displacement for a node

Context:

The truss responds dynamically to the load. You can confirm this by plotting the vertical displacement history of the node set Center.

You can create X–Y curves from either history or field data stored in the output database (.odb) file. X–Y curves can also be read from an external file or they can be typed into the Visualization module interactively. Once curves have been created, their data can be further manipulated and plotted to the screen in graphical form. In this example you will create and plot the curve using history data.

  1. In the Results Tree, expand the History Output container underneath the output database named expFrame.odb.

  2. From the list of available history output, double-click Spatial displacement: U2 at Node x in NSET CENTER.

    Abaqus/CAE plots the vertical displacement at the center node along the bottom of the truss, as shown in Figure 2.

    Figure 2. Vertical displacement at the midspan of the truss.

    Note: The chart legend has been suppressed and the axis labels modified in this figure. Many X–Y plot options are directly accessible by double-clicking the appropriate regions of the viewport. To enable direct object actions, however, you must first click in the prompt area to cancel the current procedure (if necessary). To suppress the legend, double-click it in the viewport to open the Chart Legend Options dialog box. In the Contents tabbed page of this dialog box, toggle off Show legend. To modify the axis labels, double-click either axis to open the Axis Options dialog box, and edit the axis titles as indicated in Figure 2.

Exiting Abaqus/CAE

Save your model database file; then select FileExit from the main menu bar to exit Abaqus/CAE.