ANSYS - Vibration Analysis of a Frame

Problem Specification

The problem considered here is the vibration analysis of the right-angle frame in example 11.17 on page 436 of Cook et al.

Go to Step 1: Start-up and preliminary set-up

Go to all ANSYS Learning Modules

Step 1: Start-up and preliminary set-up

Create a folder

Create a folder called dynamics at convenient location. We'll use this folder to store files created during the session.

Start ANSYS

Start > Programs > ANSYS Release 7.0 > ANSYS Interactive

Specify directory and job name

In the window ANSYS Interactive 7.0 Launcher that pops up, enter the location of the folder you just created as your Working directory by browsing to it (for example, C:\dynamics). Specify raf as your Initial jobname. The jobname is the prefix used for all files generated by the ANSYS run. Click on Run.

Set Preferences

Main Menu > Preferences

In the Preferences for GUI Filtering dialog box, click on the box next to Structural so that a tick mark appears in the box.

Recall that this is an optional step that customizes the graphical user interface so that only the menu option valid for the structural problems are made available.

Enter Parameters

For convenience, we'll create scalar parameters corresponding to v, I , p, and E.

Utility Menu > Parameters > Scalar Parameters

Enter the parameter values and click Accept after each.

E = 200e9
nu = 0.29
rho = 7860
I = (1e-4)/12

Close the Scalar Parameters window.

We can now enter these variable names instead of the corresponding values as we set up the problem in ANSYS. This is also helpful in carrying out parametric studies.

Go to Step 2: Specify Element Types and Constants

Go to all ANSYS Learning Modules

Step 2: Specify element type and constants

Specify Element Type

In the Preprocessor Menu, Select:

Element Type > Add/Edit/Delete > Add...

Pick Beam in the left field and 2D elastic 3 in the right field.

Click OK.

Close the Element Types dialog box and also the Element Type menu.

Specify the Constants

In the Preprocessor menu, Select*:*

Real Constants > Add/Edit/Delete > Add...

This brings up the Element Type for Real Constants dialog box with a list of the element types defined in the previous step. Click OK to select the BEAM3 element. Enter the following values:

AREA = h*h
IZZ = I
HEIGHT = h

Save your work by clicking on the Save_DB button in the ANSYS Toolbar.

Go to Step 3: Specify material properties

Go to all ANSYS Learning Modules

Step 3: Specify material properties

Enter the Define Material Model Behavior menu

Select Main Menu > Preprocessor > Material Props > Material Models

In the Define Material Model Behavior menu, double-click on Structural, Linear, Elastic, and Isotropic.

Specify Material properties

Enter E for Young's modulus EX, nu for Poisson's Ratio PRXY.

Click OK.

Double-click on Density under Structural.

Enter rho for DENS.

Click OK.

This completes the specification for Material Model #1. Close the Define Material Model Behavior menu.

Save your work

Click on the SAVE_DB button in the ANSYS Toolbar.

Go to Step 4: Specify geometry

Go to all ANSYS Learning Modules

Step 4: Specify geometry

Create Keypoints

Select in Preprocessor menu:

Modeling > Create > Keypoints > In Active CS

Enter:

Keypoint 1: X=0, Y=0
Keypoint 2: X=0, Y=3
Keypoint 3: X=2, Y=3

Click OK.

Create the Lines AB and BC

Select in Preprocessor menu:

Modeling > Create> Lines > Lines > In Active Coord

Select keypoint 1 followed by keypoint 2.

Click OK.

Select keypoint 2 followed by keypoint 3.

Click OK.

Save your work

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

Go to Step 5: Mesh geometry

Go to all ANSYS Learning Modules

Step 5: Mesh geometry

Generate the Mesh

To bring up the MeshTool, Select:

Main Menu > Preprocessor > MeshTool.

Click on Set under Element Attributes in the MeshTool.

This brings up the Meshing Attributes menu. You will see that the correct element type, material number and real constants are already selected since we have only one of each.

Close this menu by clicking OK.

Define Number of Elements for Each Line

We'll use 20 elements for AB and 20 elements for BC to be consistent with Cook et al.

Under Size Control and Lines, click Set.

Select line AB.

Click OK.

Enter 30 for NDIV.

Click Apply.

Select line BC.

Click OK.

Enter 20 for NDIV.

Click OK.

Creating the Mesh

In the MeshTool, click on Mesh. This brings up the pick menu. Click on Pick All.

The geometry has been meshed and the elements are plotted in the graphics window. Close the MeshTool.

Save your work

Once you have successfully created the mesh, click on SAVE_DB in the ANSYS Toolbar to save the database.

Go to Step 6: Specify boundary conditions

Go to all ANSYS Learning Modules

Step 6: Specify boundary conditions

Set Options

Select in Main Menu:

Solution > Analysis Type > New Analysis > Modal

Then select in Main Menu:

Solution > Analysis Type > Analysis Options

Enter 10 for No of modes to extract.

Click OK and then OK again to accept defaults for the Block Lanczos Method.

Apply Displacement Constraints

Select in Preprocessor:

Loads > Define Loads > Apply > Structural > Displacement > On Keypoints

Select keypoint at A. Select UX and UY, Enter 0 for Displacement value.

Click OK.

Select keypoint at C. Select UY, Enter 0 for Displacement value.

Click OK.

Specify Damping Ratio

Select in Preprocessor:

Loads > Load Step Opts > Time/Frequency > Damping

Enter 0.02 for Constant damping ratio.

Click OK.

Save your work

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

Go to Step 7: Solve!

Go to all ANSYS Learning Modules

Step 7: Solve!

Enter Solution Module

Select in Main Menu:

Solution > Solve > Current LS

Review the information in the /STAT Command window.

Close this window.

Click OK in Solve Current Load Step dialog box_._

ANSYS performs the solution and a yellow window should pop up saying "Solution is done!"

Save your work

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

Go to Step 8: Postprocess the results

Go to all ANSYS Learning Modules

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

Go to all ANSYS Learning Modules

Step 9: Validate the results

Not available yet.

Back to Problem Specification

Go to all ANSYS Learning Modules