Displacement applied in harmonic analysis with ANSYS; 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, and 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.

 

[cbrn]

Hi,
1-2: generally speaking, the fact is that by applying a DISPLACEMENT boundary condition to the entire surface you don't "respect" the eigenform you determined with the modal analysis. The equivalent model for eigenmodes' extraction would have been to make the surface rigid (or constrain it to "ground" with zero-displacement).
In even more general terms, be sure to keep coherent with all the boundary conditions when you switch from one analysis type to a subsequent one.

3- Difficult to tell... Do you have experimental data or semiempirical data for systems similar to yours? If you only account for internal damping, can you retrieve information about Rayleigh coefficients of intrinsic damping of your material? Can you obtain in some way the logarythmic decay from an harmonic response measured on the real system or a system strictly similar to yours? Bear in mind that internal damping in metals can be extremely low, thus generally negligible. For example, 1% damping is used for rigid steel interconnected structures, 2 to 5% is used in beam-structures connected by bolts (so that a lot of energy is dispersed in the bolted connections, due to friction). But for a single-body made of steel, I would personally use no damping at all.

4- Not necessarily, it depends. By adding damping you lower the responses at frequencies corresponding to the eigenvalues (note that the eigenfrequencies will shift) but extend the responses' frequency ranges. So you could fall into a situation where by aplifying the responses of two "near" eigenfrequencies you end up having a total response higher than what you would have obtained with no damping, though the single max responses to the two eigenfrequencies are now lower.

Hope this helps

Regards

 

[crisbunget]

Hi,

1-2: Thanks a lot for the suggestion. You were right. I did some modal simulations and constrained the surface in axial direction (which is the direction of the displacement applied in harmonic analysis). I obtained exactly the same frequencies. Although I understand intuitively why the boundary conditions are equivalent, I would like to know more. If it is possible for you to recommend me some material (books, internet, etc.) where I could read more about this, that will be great.

3: We don’t have yet experimental data. We are still in the research stage. Therefore I will probably use three usual values for constant damping ratio, between 0 and 1%. We then should have an idea about the possible displacements.

4: I understand. I actually read a similar answer that you gave to another member. You included there even some calculation.

Thank you,


Cristina

 

[cbrn]

Hi,

1-2: well, no refs to tell you, but a little more explanation. When you apply the same sinusoidal displacement to all nodes of a surface (i.e. you "excite all the surface in the same time"), all these nodes, at each time instant, will have the exact same displacement with regards to a fixed reference system ("ground"). In other terms, the relative displacement between them will be always null. This is exactly the definition of a "rigid" region (with respect to the direction of the constraint, of course). So, when you do the modal extraction, you want that the eigenmodes respect that condition: you don't want any eigenform where the surface "ondulates". The best way to ensure that, apart from building a constraint equation so that the surface behaves rigidly in the desired direction, is to replicate the "uniform displacement" for... a zero-value displacement. And you're done! ;-)
If it's possible to express the excitation in terms of force, then you won't have this problem. Which, in turn, is not necessarily a "problem": it may be that you really want a "rigid" behaviour of this surface (this, I don't know).

4- Ah, yes, I remember ;-) See also useful comments and "caveats" by GregLocock in various posts. Also other posters have written very useful things herein, but Greg is the name I remember well ;-)

Regards

 

[elogesh]

Hi,

Can you outline procedure used for harmonic analysis? Whether you have used modal superposition method or direct(physical method)?

I perceive this analysis as base excitation analysis. The base excitation nodes (Surface where the excitation is applied). The specification of excitation nodes adds additional constrains to the system.Increasing the constraints will stiffen the structure and correspondingly the natural frequency, which is obvious with fig.2

Regards,
Logesh.E