SimCafe

Space shortcuts

Child pages
  • ANSYS - Vibration Analysis of a Frame - Step 6

Versions Compared

Old Version 2

changes.mady.by.user Disabled Account stap_tech-mailbox@cornell.edu

Saved on

compared with

New Version Current

changes.mady.by.user user-87699

Saved on

Key

  • This line was added.
  • This line was removed.
  • Formatting was changed.
Comment: Migrated to Confluence 5.3
Panel

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
Image Added

Then select in Main Menu:

Solution > Analysis Type > Analysis Options

Enter 10 for No of modes to extract.
Image Added

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

...

Image Added

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.

Image Added

Click OK.

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

Image Added

Click OK.

Image Added

Specify Damping Ratio

Select in Preprocessor:

Loads > Load Step Opts > Time/Frequency > Damping

Enter 0.02 for Constant damping ratio.
Image Added

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