Here is a tutorial to implement a simple Modal Analysis of a Cantilever Cylinder
1. Open the ANSYS workbench
2. Drop and drag the "Modal" analysis system into the project schematic
3. Right click on "Engineering Data" and edit the material. There are predetermined properties found in the "Engineering Data Sources" (Right click on the description or press the books in the top right hand corner). For this tutorial, fused silica was created with these parameters:
In order to put in the parameters, just drag and drop from the toolbox. Also make sure the filter is turned off (that's the filter symbol next to the engineering data sources/books in the top right hand corner) this will allow a user to few all the parameters.
4. Return to the project, and open/edit the geometry. The cantilever that was used for this tutorial is a cylinder with a diameter of 2 mm with a length of 200 mm, shown in image 1.
5. Return to the project and open the Model tab. With that open, go to the subtab of "Geometry", named "Solid". Under Solid go to "Assignment" under "Material" to assign Fused Silica or whatever material you decide to choose.
6. Go to the "Mesh" tab. In this case the "Element Size" under the "Sizing" tab is 0.04 and the "Relevance Center" as "Fine". Right click on the mesh and press "Generate mesh".
7. Under the Modal tab, go to the Analysis Settings and change the "Max Modes to Find" for ANSYS to calculate. In this tutorial, the amount of modes that were used was 17.
8. Right Click the Modal and press on "Fixed Support". This will make the bar a cantilever bar, once the geometry is set to fix one face of the bar. Press on one of the faces and click on "apply" on the Geometry.
9. Right click on the solution and press "Solve". Let ANSYS run the modes through.
10. On the Solution tab, the "Tabular Data" is listed but the Total Deformation has not been listed. In order to do so, select all the frequency of the modes in the column and right click and press "Create Mode Shape Results".
11. Once loaded, the total deformation will have a lightning bolt next to each entry, right click and press "Solve" or "Evaluate All Results". This will make all the entries have a green check mark.
12. This will give the user the ability to animate each entry. This is down by clicking the play (sideways triangle button). ANSYS will run through the simulation for that mode that is selected, shown in image 2.
13. Using Mathematica (or another computational system) input the analytical solution for a Cantilever bar fixed to one end.
14. Compare only to the bar actually bending, not twisting or contracting. There are modes that are the same due to the symmetry of the bar. In image 3 the underlined frequencies compare to the analytical calculations (Mathematica) and the computational calculations (ANSYS).