Harmonic analysis with ANSYS and damping ratio 1

[crisbunget]

Hi,

I am doing research in ultrasonic technology, and I have to conduct harmonic response analysis in ANSYS with displacement applied. I am hoping that someone did this and can give me some suggestions.

I need to apply harmonic displacement on a rod, on the surface of the lower end, and to find the response in a point in the upper end. I have a rod formed by two segments with different diameters, 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 between 17000-30000 Hz, and I found a longitudinal mode shape at 18525 Hz. 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).

Some questions:
• 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.

PS: Sorry for posting the question on two forums. I wasn't sure which one is closer to the subject.

 

[fetraining]

crisbunget,

I think the rteason for the apparent resonant frequency shift in the frequency response analysis is beacuse you are changing the boundary conditions in several of the loading caes.

If the longitudinal natural frequency of 18525 Hz is found from a free-free normal modes analysis, then you are applying no boundary conditions to the structure. When you are applying the enforced motion you are applying a boundary condition to the structure which will change it's natural frequencies. Imagine each node has to be constrained to move in your specified input direction. Any relative movement of the fixed face will be eliminated, preventing the rod end from having lateral displacemenst due to poissons ratio and any possible end 'belling' shapes. The flexural modes will also be higher as you are stiffening the structure with the constraints.

The single node input for enforced motion is not constraining relative motion of the other nodes, so this boundary condition is close to free-free.

The pressure does not apply any constraints to the free free structure.

If the base of the rod is actually the attachment point to the rest of the structure, then carry out the normal modes analysis with this constraint applied, keep the same for the pressure loading and use the same degrees of freedom at the base when applying the base motion (dispacement). All these analyses should then have the same natural frequencies.

There should not be a frequency shift due to damping at these levels. In fact most FE solvers ignore the correction term you mention due to damping. You won't shift the frequences even if you put in really high damping.

As to damping levels - there is no way to answer accuratly without testing. We all have our favorite recipes for rough approximations. Mine is 1 - 2% critical damping for small clean fully machined structures with no fabrication up to 5% for highly fabricated structures and up to 8% for composites. However it is safest to err on the low damping side - it will give the most conservative response. Most safety or mission critical applications will actually dictate the response to use.

Hope this helps,

regards Tony


Tony Abbey

http://www.fetraining.com

 

[crisbunget]

Hi Tony,

Thanks a lot for your explanations. I think that I am clear now about what I have to do in the simulations.

Cristina