Learning Forum

[Samuele Luigetti]

Good morning everybody.

I have to do an harmonic response analysis and i have to apply in different places of the structure the same load (sinusoidal) but with a different phase angle. First of all, i see that i can set the magnitude of the load and the phase angle, but how i can set the frequency of the load? Moreover, to set different phase angle between the load,  for example 30 degress and more (so 30° load2 ,60° load 3,90° load 4 ecc) how i have to do? Thanks 

[Claudio Pedrazzi]

 

 

Hi Samuele

I am not sure that harmonic analysis can handle different phases in different nodes as excitation.  I always understood harmonic analysis as like to put the object on a shaker table and excite a set of constrained nodes with the same forcing function.   But maybe I’m wrong.

Concerning the frequency, you provide a range, not one single frequency, this is the whole idea of harmonic analysis: you sweep the frequency!.  If you refer to APDL, the command is HARFRQ.  Or do you use Workbench?

Hope this helps, 

Best regards

Claudio

 

 

[Samuele Luigetti]

Hello and thanks for the response. I'm using workbench. So are you saying that a single load that i insert has a single value of amplitude and phase angle but different frequencies?

[Claudio Pedrazzi]

I would express it differently. At least this is what I used to do with harmonic analysis.  I imagine putting my object on a shaking table (or I have a vibrating thing, like a motor, somewhere in the model).  I want to know how the system answers (amplitude and phase at each node) to the different frequencies.  But the best you can do is to read accurately the description in the very useful "structural analysis manual".  It is in the APDL section but for me it remains the best :-)

So please read the description in: Help > Mechanical APDL > Structural Analysis Guide > Harmonic Analysis > 4.1 Uses for Harmonic Analysis

 

I copy a part of it that in my opinion confirms my point of view: "Harmonic analysis is a technique used to determine the steady-state response of a linear structure to loads that vary sinusoidally (harmonically) with time. The idea is to calculate the structure's response at several frequencies and obtain a graph of some response quantity (usually displacements) versus frequency. "Peak" responses are then identified on the graph and stresses reviewed at those peak frequencies."

[Samuele Luigetti]

ok thank you so much, i appreciate it!

[Claudio Pedrazzi]

I hope someone from the community will respond further, in case my answer regarding the impossibility of two different excitations with different phases in a harmonic analysis is false.  

However theoretically (but I have never tried) it might be conceivable to perform two, three separate harmonic analyses, one for each excitation, and then do a superposition (linear combination) of them (available in Workbench).  

[peteroznewman]

Hello Claudio,

Harmonic Response supports loads at different nodes having different phases as Samuele saw in the load Details window where there is a field for Phase.

You clarified for Samuele that Harmonic Response is a sweep over a range of frequencies.

I will add that all loads have the same freqency during the sweep, while the amplitude and phase of each load can be set independently. But see the note in the image below.

Here is an example from the Ansys Help Structural Analysis Guide

[Samuele Luigetti]

Thank you Peter. So the set different phase angle between loads i need only to set different phase angles in the details window right?

[peteroznewman]

Correct

 

[Samuele Luigetti]

Hi Peter, can you help me to understand the frequency response plot?

For example what is the correlation with the frequency of the peak response and for example the mode shapes? Moreover, the peak corresponds to a resonance's situation for sure?

[peteroznewman]

Hello Samuele,

Here is a non-mathematical article. 

Here is a mathematical article.

After you have read those, can you answer your own question?  Let me know in your reply.

[Samuele Luigetti]

Ok thank you i understood something new. 

So if i have a peak on the frequency response at a certain frequency, like 300 Hz, since we can not set a single value of the frequency's load but a range, it means that if the excitation load have a frequency equal to 300 Hz, is there resonance in the structure? 

[peteroznewman]

A peak in the FRF is the definition of a resonance.

Say you have six modes at different frequencies. The mode shapes for those frequencies have nodes moving harmonically in different directions by different magnitudes and at different phases to the forcing phase of 0 degrees.

When you pick a node and a direction to plot the Frequency Response, you get a Magnitude and Phase plot where you can see the peaks and valleys.  Those peaks and valleys are a superposition of modes from Modal analysis. The amount of each mode is determined by the Participation Factor.

[Samuele Luigetti]

Good morning Peter. I have another problem, hope that you can help me. I've done a modal analysis of a rotating structure with different step of velocities and with solver type set to program controlled. This work without problem, but when i link this to an harmonic response, this fail and the following message appear: "MSUP harmonic do not support full damped or unsymmetric solver type of the upstream modal analysis". So i set the solver type of the modal on reduced damped and the harmonic response work, but with reduced damped i can not set on Campbell diagram and then i can't set more step of velocites. I don't know how to do.

thank you

[peteroznewman]

Set the Modal analysis to be Undamped.

Apply the damping in the Harmonic Response.

Read the Ansys Help > Mechanical APDL > Rotodynamics Guide which has instructions on Campbell diagram.

 

[Samuele Luigetti]

 I can not set the modal to be undamped cause i need to define more than 1 step of rotational velocity. If i set undamped there's not the option to set multiple step.

[peteroznewman]

Sorry, I am not an expert on Campbell diagrams or rotodynamics. Search YouTube for some videos and read the Ansys Help Rotodynamics Guide.

[Samuele Luigetti]

Already done, thanks anyway for the support