ANSYS - Vibration Anaylsis of a Frame - Step 6

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 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!