ANSYS - harmonic response analysis and damping ratio 2

[crisbunget]

Hi,

I am doing research in ultrasonic technology, and I have to conduct harmonic response analysis in ANSYS with displacement applied. I need to apply harmonic displacement on a rod on one end, and to find the response in a point in the other end. The rod has two segments with different diameters, and it is constrained at the middle, where the step in diameter is. The excitation on the lower surface should be applied as displacement in the axial direction (10×10E-6 m).

I did the modal analysis and I found one mode shape in the range I was interested in. I continued with the harmonic response analysis, in order to calculate the amplitude response (displacement) for the node in the center of the upper end surface. These are some observations:

• When a displacement is applied on the whole lower end surface, the response frequency is very far to the natural frequency, although the damping coefficient used is 0.1% (constant). If the surface where the excitation is applied is reduced, the response frequency decreases. If the displacement is applied just in one node in the center of the surface, then the frequency response is very close to the natural frequency.
• If a pressure is applied on the whole surface, then the frequency response is very close to the natural frequency. The amplitude response is similar with the response when the displacement in a node is applied. The pressure applied here is chosen in such a way that the displacement on the lower end for damping of 0.1% will be the same as the one imposed in the previous case (10×10E-6 m).

I have some questions and I am hoping that someone did this and can give me some suggestions.

• Why the frequency response for displacement applied on the whole surface is so much different that the natural frequency? If the damping ratio is small, the difference in frequencies should be insignificant.
• Why the displacement and the pressure applied give different results in terms of frequency? Shouldn't they be similar?
• Could you recommend some values for the damping ratio that can be used in the simulations?
• If there would be another mode shape in the range, but with lower amplitude, will the increase in damping result in attenuation up to losing that mode shape, and having just the dominant (larger) one?

Please find attached a document with details and results.

Thank you.

 

[meshparts]

Hello crisbunget,

the problem with the difference in response frequency in relation to the longitudinal eigenvalue is, that the longitudinal eigenvalue is computed with different boundary conditions than the freq. response.

To solve this problem you should apply forces instead of displacements, if possible (I don't know how the excitation looks like in reality)

If not possible, then compute the eigenvalues with the same displacement boundary conditions on the bottom surface as during the frequency response (e.g hole surface or just one node).

The second question should be clear now. Different boundary conditions gives you different results, since the system is stiffer with applied displacement than with applied pressure.

Damping for steel is very low. Unless you have friction on the middle of the rod, I would go with 0.1% of critical damping.

Regards
Alex

 

[crisbunget]

Hi mihaiupb (Alex),

I would like first to thank you for having the patience to go through my post.

You are right, applying a displacement changes the boundary conditions. I will try to see what I obtain in modal analysis when I apply the same conditions. Thanks a lot for the advice.

The excitation comes from a transducer which is connected tightly with the rod and vibrates in axial direction. I would have preferred to apply force or pressure, since it is much easier to understand physically, but the manufacturer of the transducer recommended using displacement.

One more question about damping. If I would want to consider the friction, should I go up to 1%?

Thank you,

Cristina

 

[meshparts]

Hello Cristina,

Replacing frinction with vsicous damping is not so easy.

Since friction is nonlinear an viscous is linear, the amount of equivalent viscous damping is inversely proportional to the amplitude and frequency of the nonlinear vibration.

Do you have any measurements of the freq. response (even from similar systems) from the manufacturer? Then it will be very easy to get the amount of damping using the half-power bandwidth method (3 dB method).

Regards
Alex

 

[Transient1]

My two cents, are depending on the cost and if you have the available equipment, build a prototype as soon as possible. Early correlation between a physical device and a model, will make future design work much easier and more accurate. Damping is a difficult quantity to determine (and in some cases is just pure math and not reality) and in the end the computational model must match reality.

 

[crisbunget]

Hi,

I don't have measurements from the manufacturer, but thanks for the advice. We will build the system and we will measure the real values for the amplitudes and also the damping.

I think that I am clear what to do in the simulations.

Thanks everybody for the help given. It was really valuable.

Cristina