Learning Forum

[Deepesh]

I wanted to use Harmonic analysis but some of my friends suggested to use pre stress analysis like connecting harmonic tab with modal tab and performing further.

I tried both; Harmonic alone as well as Harmonic connected to Modal. Both gave me different results. 

Can anyone explain why the results are different and how the modal results are taken into account if connected to harmonic?

Thanks

[peteroznewman]

A Modal Solution cell linked to the Setup cell of a Harmonic Response creates a Linear model for Harmonic Response. The harmonic response solution has the ability to automatically cluster solution points around a peak response as shown below. This means the peak response can be accurately found.

---

Full Harmonic Response sits on its own and the solution does not automatically cluster points around the peak response. That means the true peak response can be underestimated because of that. You can manually rerun the analysis with a narrower frequency range to get a more accurate estimate of the peak. The graph shown below is from a different system than the graph shown above, it is just to illustrate coarse sampling around the peak.

---

Those two systems look like this in Workbench.

---

You can also use a Static Structural model to Pre-stress either a MSUP Harmonic Response or a Full Harmonic Response as shown below.

In either case, the Static Structural changes the stiffness matrix that is used by the Modal or Harmonic Response, usually raising the frequency, such as when a guitar string or a drum head is tensioned.

[Deepesh]

But then if I use pre stress harmonic response, I am unable to input 'Rotating force' as it can be only used in 'Full' Harmonic Analysis(mentioned in the help section of ANSYS). Some force has to be given in Harmonic response for it to work but I am mainly interested in rotating force and as you said pre stress analysis would give more accurate result. So, is there any way to club 'Rotating force' in ore stress harmonic response?

[peteroznewman]

This discussion did not mention "Rotating Force".

Rotordynamics, which includes Rotating Force, cannot be done in WB with Modal Superposition (MSUP) Harmonic Response. You must use Full Harmonic Response according to April Wang.

You can probably do a Static Structural Prestress in front of a Full Harmonic and still use a Rotating Force. Have not tried it myself.

Have you read the ANSYS Help section, Rotordynamic Analysis Guide? It is in the Mechanical APDL section.

Have you watched this video?