Displaying a subset of the model

By default, Abaqus/CAE displays your entire model; however, you can choose to display a subset of your model called a display group. This subset can contain any combination of part instances, geometry (cells, faces, or edges), elements, nodes, and surfaces from the current model or output database. For the connecting lug model you will create a display group consisting of the elements at the bottom of the hole. Since a pressure load was applied to this region, an internal set is created by Abaqus that can be used for visualization purposes.

This task shows you how to:

Display a subset of the model

  1. In the Results Tree, double-click Display Groups.

    The Create Display Group dialog box opens.

  2. From the Item list, select Elements. From the Method list, select Internal sets.

    Once you have selected these items, the list on the right-hand side of the Create Display Group dialog box shows the available selections.

  3. Using this list, identify the set that contains the elements at the bottom of the hole. Toggle on Highlight items in viewport below the list so that the outlines of the elements in the selected set are highlighted in red.

  4. When the highlighted set corresponds to the group of elements at the bottom of the hole, click Replace to replace the current model display with this element set.

    Abaqus/CAE displays the specified subset of your model.

  5. Click Dismiss to close the Create Display Group dialog box.

Display the face identification labels and element numbers on the undeformed model shape

Context:

When creating an Abaqus model, you may want to determine the face labels for a solid element. For example, you may want to verify that the correct load ID was used when applying pressure loads or when defining surfaces for contact. In such situations you can use the Visualization module to display the mesh after you have run a datacheck analysis that creates an output database file.

  1. From the main menu bar, select OptionsCommon.

    The Common Plot Options dialog box appears.

  2. Set the render style to filled; all visible element edges will be displayed for convenience.

    1. Toggle on Filled under Render Style.
    2. Toggle on All edges under Visible Edges.

  3. Click the Labels tab, and toggle on Show element labels and Show face labels.

  4. Click Apply to apply the plot options.

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

    Abaqus/CAE displays the element and face identification labels in the current display group.

  6. Click Defaults in the Common Plot Options dialog box to restore the default plot settings and then click OK to close the dialog box.