To display a contour plot of the model:

From the main menu bar, select PlotContours.

ABAQUS/CAE displays a contour plot of von Mises stress superimposed on the deformed shape of the model at the end of the last increment of the loading step, as indicated by the following text in the state block:

Step: Load, Apply load  
Increment     6: Step Time =   1.000

By default, all surfaces with no results (in this case, the pin) are displayed in white.

The deformation is exaggerated because of the default deformation scale factor that ABAQUS/CAE selects.

To remove the white surfaces from the display, do the following:

From the main menu bar, select ToolsDisplay GroupCreate.

The Create Display Group dialog box appears.

In the Item options list, select Surfaces. In the Selection Method options list, select All surfaces.

At the bottom of the Create Display Group dialog box, click Remove.

The white surfaces disappear from the view.

Click Dismiss to close the dialog box.

To reduce the deformation scale factor, do the following:

From the main menu bar, select OptionsContour.

From the Contour Plot Options dialog box that appears, click the Shape tab.

From the Deformation Scale Factor options, choose Uniform.

In the Value text field, type a value of 100, and click OK.

ABAQUS/CAE displays the contour plot with a deformation scale factor of 100, as shown in Figure C–57.

Figure C–57 Contour plot of von Mises stress with a reduced deformation scale factor.



Use the view manipulation tools to examine the deformed model. Note where the pin appears to be exerting the most pressure against the insides of the flanges. Also note how the two flanges have twisted away from each other.

By default, the contour plot displays the von Mises stresses in the model. You can view other variables by selecting ResultField Output.

The Field Output dialog box appears.

Click the Primary Variable tab of the Field Output dialog box, and select S11 from the list of Component options. Click Apply to see a contour plot of the stresses in the 1-direction.

From the Invariant option list, select Max. Principal, and click Apply to see the maximum principal stresses on the model.

Select any other variables of interest from the Field Output dialog box.

From the Invariant option list, select Mises and click Apply to display the von Mises stresses again.

To create the display group:

From the main menu bar, select ToolsDisplay GroupCreate.

The Create Display Group dialog box appears.

In the Item options list, select Part instances.

The right side of the dialog box displays all the part instances in the model.

Select the Hinge-hole-1 part instance.

At the bottom of the Create Display Group dialog box, click Replace.

The contour plot of the entire model is replaced by a plot of only the selected hinge piece, as shown in Figure C–58.

Figure C–58 Use display groups to view a contour plot of the von Mises stress in the hinge piece with the lubrication hole.



Use the view manipulation tools to view the hinge at different angles. You can now see results for surfaces on the hinge that were hidden by the solid hinge.

From the main menu bar, select ResultField Output and click the Primary Variable tab of the Field Output dialog box that appears.

From the top of the Primary Variable tabbed page, toggle on List only variables with results: and choose at surface nodes from the menu.

From the list of variables that appears, select CPRESS, and click Apply.

ABAQUS/CAE displays a contour plot of the contact pressures in the flange hole.