ANSYS - Vibration Anaylsis of a Frame - 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