Step 8

Problem Specification
1. Start-up and preliminary set-up
2. Specify element type and constants
3. Specify material properties
4. Specify geometry
5. Mesh geometry
6. Specify boundary conditions
7. Solve!
8. Postprocess the results
9. Validate the results

Step 8: Postprocess the results

Enter Postprocessing module to analyze solution

Main Menu > General Postproc

Select Results Summary.

This shows you the cyclic frequencies of the ten modes. Compare with the values in the book.

View Mode Shape for Mode 2

Read Results > By Set Numbers

Enter 2 for NSET.
Click OK.

Plot Results > Deformed Shape

Select Def+undeformed.
Click OK.

This plots the mode shape for mode 2. Similarly, look at the other mode shape and compare them with figure 11.17-2 in the book.

Find Mode Numbers

Table 11.17-1 gives amplitude values for selected d.o.f. for three nodes.

To find the node numbers corresponding to the ones in the book, turn on node numbering.

Utility Menu > PlotCtrls > Numbering

Turn on Node Numbers.
Click OK.

If you need to refresh the screen: Utility Menu > Plot > Multi-plots

By comparing the node numbers, we find:

Determine the Displacement Amplitude

To determine the displacement amplitude at node 17 for mode 3,

General Post Proc > Read Results > By Set Number

Enter 3 for NSET.
General Post Proc > List Results > Nodal Solution

Select UCOMP.
From the list, the displacement amplitude, denoted as USUM, is 23.9e-3. The corresponding value in table 11.17-1 is 23.8e-3. Similarly, you can determine the other entries in the table. Note that the rotational d.o.f. to use for the second row in the table is ROTZ.

Save your work

Click on SAVE_DB in the ANSYS Toolbar to save the database.

Go to Step 9: Validate the results