Discussion Forum

Hi

the Q factor is related to the damping, but by default COMSOL does not add any damping (though sometimes the solver algorithm behaves as if there is some "numerical" artificial and non physical damping). In your experiment I assume you are in air at about 20°C and a pressure of 1atm. If so the main damping source is the motion of air (if its a Si beam there is hardly any "material" damping in such a perfect crystal, perhaps a little in the oxide, but that is normally very thin), a simple way is to try this: see blog www.comsol.eu/blogs/natural-frequencies-immersed-beams/

To do it more precisely you need the acoustic module as the vibration is dissipated as an acoustic wave in air, furthermore as you are in the small scale regime here, this is rather thermo-acoustics, as over the 0.1-0.2 mm of the interaction region you have for a small beam the air heat conduction is such that the temperature T of the air is governed by the conduction from the beam and we are no longer in an adiabatic hypothesis. This is why COMSOL is so essential and unique to simulations of the MEMS and the nano-world, here the physics couple very differently from our ordinary macroscopic world, and the older FEM tools, that work fully segregated, fully ignore this (their resellers too !)

Another way is to add run only a structural analysis, to some damping as a variable and have COMSOL to optimize it to the Q value you measure. But read carefully the damping theory pages, as depending on the solver you use all damping proposed do not apply .

--
Good luck
Ivar

Dear Ivar,

Thank you so much for your comment. I think that I need to be a bit more specific though.

My experiment is not just at 1 atm and room temperature, I measure at high vacuum e-11 bar and at cryogene temperatures: 40 mK. Therefore I find high Q-values, i.e. for the first resonance mode (f = 3000 Hz) I found a Q value of 30000.

In my experiment I am AC driving the cantilever at resonance (thus 3000 Hz) using a piezo element. My first question is, how can I implement this driving into Comsol? Then I want to do analysis, i.e. I want to know the displacement of my magnet (in units um) as a function of time. If that works, I also want to know whether I can simulate the time varying magnet field the magnet is producing, that would be very nice if I can do that as well.

Having this information, I assume that this changes the whole story right? What methods in Comsol would you recommend for right implementation of the problem? I am quite new to Comsol (learned it last week), and I couldn't figure out yet which physics and studies I should use to do this simulation.

Hi

Indeed that changes the issue ;)
if there is no air there is no fluid damping indeed, at least not significant at your level, but if your micro-cantilever is very small perhaps you have the shot noise of the remaining molecules hitting it as background noise ? I'm not sure the molecular flow physics can give you something there, I haven't used that one enough to tell, but others out here might have an idea and suggestions

Anyhow at those temperatures the material properties of Si and particularly any crystalline damping (perhaps also in any thin layer) could be different, I'm not sure, mK is not my domain, I stop at most at LHe ;)

The thing is that for any frequency domain analysis you need a representative damping, and that is mostly a very difficult parameter to define. Or you try to inversely identify the damping by using measurement data to optimize the simulation value to fit a series of measurement values.

Now if you drive it with a PZT element is this also on the cantilever ? then your PZT layer would probably also influence the damping. Then support of the "fixed" part must also really be "fixed" and "solid" else you get losses there a Q of 30k means really small losses. Even the electronic drive circuit by its internal impedance will effect the damping somewhat (can also be added if you know the equivalent RC circuit of your electronics and cables.

The driving of the cantilever can be implemented either by the PZT layer or if you know how by a varying boundary load but you need to then model correctly the PZT elements and the attachment of your device, then once you have the oscillation amplitude you might try out a ACDC model for the B field of your oscillating magnet, but still, can you measure your magnet at that size or just assume it's "perfect" ? how many Weiss domains do you have across ? check that your are still in a reasonable linear continuous material conditions. In all cases, my suggestions: start simple a physics at the time then couple the next one etc.

--
Good luck
Ivar

Hi,

Thank again for your advice, it is really cool that you help so many scientists here with their simulations!

I attached some pictures which shows you some details of the actual set-up. The cantilever is attached to a cantilever holder (number 3 in picture), and the holder is attached to a piezo element. As you can see, the system is build such that we have very little dissipation, that's why we can achieve Q-values of 30k.

I also attached an electron microscopy picture of the magnet, assuming that I have a perfect sphere is a good enough approximation.

I measured the driving force of the piezo, so I could as you suggest implement this first using a time-varying boundary load.

Now a silly question since I'm not an expert on the field of damping, but can't I just omit everything and just tell Comsol that I have a Q-value of 30k? If I then tell Comsol with what force I am driving, then I hoped that Comsol could tell me what the position (displacement in um) is of my magnet at any time. during the oscillations. Or is this naive and completely wrong?

Hi

Thanks for the nice photos, you seem to have an interesting subject there, and far from obvious to set up and tune I believe :)

To come back to your fundamental question about damping in structural in COMSOL, it's a confusing issue for many, and I'm not sure I'll manage to iron it out here.
But first you can get some insights by reading (at least the introduction) to these articles I have found on the web (there are plenty more out there):
engweb.swan.ac.uk/~adhikaris/fulltext/conference/ftc27.pdf
alexandria.tue.nl/repository/books/612399.pdf

COMSOL uses the Rayleigh damping factors (Alpha and Beta) as default, turn on the equations to see how these variables enters the equations, and this depends on the type of damping and type of solver you choose, if the equation field is "blank" that damping does NOT apply !

Q factor or isotropic loss factor via Eta=1/(2*Q) is only a viscous factor acting on C (the velocity multiplier in the ODE) and works only for eigenfrequency analysis and for frequency domain analysis but NOT for time dependent solving.
For the latter you need to define the Alpha and Beta of the Rayleigh factors (these are always applicable for all dynamic studies), which acts respectively on the mass M and the stiffness K multipliers of the ODE. The Alpha and Beta contributes differently and opposite w.t.h. their frequency dependence (check the doc of COMSOL Structural)

For your case where you have one frequency, its rather easy, you can balance alpha and beta such that you get an equivalent "flat" Q factor for your single f0 frequency and so long you stay around that frequency you should be representative.
Previously (older versions of COMSOL) there were a simple Matlab code given in the doc to estimate rapidly reasonable alpha & beta for a given frequency span and Q value equivalents.

What I would suggest is that you look at the figure "Figure 2-12: An example of Rayleigh damping" page 114 of my COMSOL 5.2 Structural doc, and you select f1, f2 around your 3kHz f0 (in a lin or log way depending on your usual approach) and adapt alpha and beta to get a flat damping value between f1 and f2.
But be aware, with your high Q factor the time resolution settings of your solver will be critical, you might need to go down to 1E-6 or even below to ensure reasonable stable response.

Now the damping comes from many sources, in your case I would also suggest to try also to understand the sensitivity of your model to the "stiffness" of attachment of your cantilever to the PZT excitatory (replace it by a representative 3D spring mass damper), and on the other side the effect of any "skin" oxide you might have on your cantilever material, even a few to ten nm of oxide on the surfaces could well be a major contributor, as your beam is only a fraction of a micron across and the oxide is on the external skin hence sees maximum stress changes. For the oxide I see an issue to know what kind of material data damping one could use (I do certainly not have any values to propose :( but COMSOL can allow you to get the order of magnitude of sensitivity of the effect of a skin layer.

--
Have fun COMSOLing
Ivar

Dear Ivar,

Thank you once again, also for the comment on the oxide layer, I haven't thought about that yet. I think I will give a look at that after I have build in the basic damping.

I managed to implement the driving and I get displacements which are realistic (order micro meters). I also see resonance. To build a realistic model however, I am now convinced that I indeed need to include the physics of damping. I studied the articles you sent me. Rayleigh damping is used to model proportional/modal damping. However, I assume that I'm in the weak damping regime (eigenmodes are approximately equal to the undamped eigenmodes). This vision is also supported by experiment, since the eigenfrequencies I found are all within 10% of the eigenfrequencies computed with Comsol. Still, I think that I cannot just ignore damping, driving at resonance would probably mean that without damping the displacement of my cantilever would be "infinite" if I exclude damping.

So if I follow your advise, I will ignore Q since I do my studies in the time dependent module. There, I will find and tune alpha and beta such that we have a flat damping between f1 and f2.

Now some questions:

1. If I'm correct, the values of alpha and beta in my case are very small, aren't they? This will help me with finding the good combination.

2. Following your procedure, how do I know when I have achieved a damping level which is equivalent to Q = 30k? Somehow this is important for me because I also want to study a specific higher mode, which has a Q value of only 500 (measured in experiment).

3. Once I have managed to implement the damping, should I redo the eigenfrequency analysis? I suppose that it would be interesting to see whether indeed the eigenfrequencies are pretty similar or different.

4. Some practical question, where can I find your example of Rayleigh damping, on internet or is this manual somehow build into Comsol?

Thank you very much for helping out, your advise already helped me a lot. I will write your name at the acknowledgement paragraph within my master thesis, that's the least what I can do :-)

Hi

If you do frequency domain scans you may use the Q factor (isotropic loss factor)) or rather eta=1/2Q, but else in all generality you must adapt alpha and beta around your resonant frequency such that you get an equivalent and quasi constant Q factor as desired for your frequency and its immediate vicinity.

So either you study your two modes separately, or you adapt alpha and beta such that you have both Q factors correct for the two frequencies, I expect this to be possible as you have two variables and two frequencies. Unfortunately I haven't found back those few Matlab lines of code COMSOL proposed in the old docs to adjust alpha and beta depending on two Q values for two frequencies. But its a simple optimisation of the formula you find in the doc.

What is also possible, as you probably have only a few modes is to do an damped eigenfrequency modal reduction and i.e. run a time series based on a modal time reduction, with corresponding damping. This is a bit more work to set up, particularly the damping, but allows for fast time response calculations as you model only includes a few modes, however I find this approach far less documented and easy to implement in COMSOL, even if it has been for the last 50+ years the traditional engineering way to handle time series analysis of complex models, and is still widely used via the Craig Bampton modal reduction method in space engineering.

The Rayleigh damping is a general approach, nothing COMSOL specific, you find a lot by a few Google searches, but I would suggest that you start with the COMSOL doc and the references therein

--
Good luck
Ivar

Dear Ivar,

Thank you for your advice once again. I’ve read the literature about Rayleigh damping and I studied the Structural Mechanics Module. After several studies, I still did not achieved one proper simulation. I tried the following:

(i) Eigen frequency study: I did the study and found my resonance frequencies, which are within 10% of the measured resonance frequencies. So this works so far.

(ii) Time domain analysis: I implemented a time varying point load (#) located at the top of my spherical magnet. The boundary on the other side was kept fixed. I also implemented Rayleigh damping (##). I looked at the z-displacement of the same point and I saw resonance occurring, see attached graph. Unfortunately, the z-displacement decreases at some point and increases later again, a ‘beat pattern’ becomes visible. This could indicate that I’m not driving at resonance, but close to resonance. Though, if you look at the beat pattern, it becomes clear that if this explanation is valid, I’m 200 Hz off resonance… Next to this problem, I also don’t know when I am in steady state. This wouldn’t be a problem to sort out if these calculations wouldn’t cost my computer hours to calculate.

(iii) Frequency domain analysis: I was inspired by Comsol’s example hpc.mtech.edu/comsol/pdf/Structural_Mechanics_Module/StructuralMechanicsModelLibraryManual.pdf, page 3. Using this method, I will get the steady state displacements right away. As a toy model, I played with this for a simple cantilever without a magnet and different dimensions. This worked perfectly, I got a nice displacement vs frequency plot. Unfortunately, when I applied the same strategy to my real model, I got the error ‘Failed to find a solution for the initial parameter. The relative residual (0.55) is greater than the relative tolerance. Returned solution is not converged.’

For the latter study, I used the same Rayleigh damping, and this time a load of 0.1 N/m (corresponds to a point force used earlier, spread over the cantilever’s surface).

Do you have any suggestions what is going wrong here? I’ve also included my Comsol file without the results, perhaps you can spot some classic mistakes I’m making. Perhaps I must indeed not set alpha to 0 but set alpha and beta such that I will get the flat Q.
The point is, that I want to study a specific higher mode and I just want to know how the displacement of the magnet is, that’s all, but it turns out to be a tough simulation…
I hope you can help me a bit further with this problem! Thank you very much in advance :-)

(#) load: F=F0*sin(omega*t), where F0 = (k*x)/Q
Omega: 2*pi*resonance frequency mode 1 (3174.5 Hz, found in eigenfrequency study)
k: stiffness cantilever (7e-5 N/m)
x: expected displacement cantilever at resonance mode 1, here x = 4 um
Q: quality factor, here Q = 30000

(##) damping: set alpha = 0 (this is done frequently in literature), then beta = 1/(omega * Q). Inserting omega and Q gives beta = 1.77e-9 s

As per my experience the Q factor is related to the damping and COMSOL does not add any damping.
It is looking that in your experiment you are in air at about 20°C and a pressure of 1atm.
And If the main damping source is the motion of air, is a simple way to try this.

www.7pcb.co.uk/

Thanks Stefa,

No, you totally miss the point here, I'm in a high vacuum and at very low temperatures (25 mK), I know how to include damping (mostly internal friction) thanks to Ivar (Q is 30k, very little losses). I would like to know the cantilever's tip displacement while driving it in a certain mode with a certain input energy. So far my studies fail, although I am able now to analytically approximate the displacement.

Dear Ivar,

You never replied to this message, I am still very interested in a simulation of this problem
I hope you find some time to anwser!

Best,

Rembrandt

Hi

it's not that much the time to reply that is missing, it's the time to be sure I have understood, done my "toy models" checked it out... And I have my dozen "internal" clients to serve first (and a family too :)

So a few advices, because your model is delicate due to the high Q value, or very low damping:

1) time domain: these simulations are always delicate as you have the transients at start that need time to damp out, and by that time a too large time stepping will induce other side effects, highest risk integration errors. There you need to play carefully with the time stepping, and normally any transients will damp out after 3 tau =< very loooong time for you.

2) Try to avoid point loads in 3D or 2D, basically loads should apply to Boundaries, the way COMSOL defines them, one dimension below your highest space dimension. Point load generate singularities and instabilities in your matrix inversions, hence in your results. A point load (except in 1D) can always be improved by some spreading function to cover the required dimensions.

3) frequency domain, for me your best choice: here you have the issue of you high Q that imposes a low frequency stepping, passing the resonance might be difficult, or even impossible, the stepping should ideally be made smaller and smaller around the frequency you get by the eigenfrequency study. Another way, when one cannot manage, is to approach the resonance from both sides, once with increasing frequency and once with decreasing frequencies, and then fit a smoothing function to estimate the peak height. It's not ideal, but if no other way works it's the best approach.

4) Note that with damping your eigenfrequencies become complex, be sure you follow both or plot the Bode plots to have phase and amplitudes, as COMSOL by default plots only the real part of any results, even if it is complex. Furthermore, I agree using alpha = 0 is not the best approach, try to balance alpha and beta to get the corresponding Q value to be flat around your frequency, that is easy for you with only one frequency.

Once this is running, you still have to ask yourself what is happening with your vibrating magnet, does it see some conducting material in it's magnetic vicinity, does it interact, i.e. via induced Eddy currents ? but that is for next addition of new physics ;)

--
Good luck
Ivar

Dear Ivar,

It has been a while since the last time we had contact. I continued to do some exciting experiments in the lab and now I'm writing my results down, we will soon publish an article about this topic.

In order to understand the data better it is still interesting to know the displacement of the magnetic tip for several higher eigenmodes. I started to do some COMSOL simulations again, see the picture for the 1st mode.

By tuning the damping parameters (or actually only beta and setting alpha to 0) and the driving frequency I managed to reproduce the spectrum we measure around the first mode. However, with these settings I wasn't able to find Lorentzian peeks around other modes, do you know what is going on here? I do however when I disable any damping at all, but I suspect that I actually see Dirac Delta spikes here...

p.s., because I did measurements in the vincity of a Cu plate, the induced Eddy currents coupled to my magnet, that's why we don't measure a Q factor of 30k, but 'only' 500.

Hi Rembrandt

Good to hear you are progressing, and that the models fit (somewhat).
If I understand your image, you are fitting a Laurentzian function model onto your COMSOL model data.

What I see is that you have a good frequency fit, as both measured and modeled curves are rather symmetric, but their amplitude differs slightly, so you will have (and this is very common for this type of function fits) a far larger amplitude variation between measured (true) modeled by COMSOL and modeled by your fit onto the COMSOL data.
The least square fit averages out the surfaces under the integrals, so if your integration or fitting width (in the frequency domain) is too wide the errors on the base will influence and most probably cut off the top. You should try to plot the max value as function of the bandwidth width you fit over. Then most probably you will notice that the amplitude is rather stable for a narrow width and will decrease or oscillate more as you widen out. Just the contrary for the frequency variable (by the way you need to have a good (lateral) frequency fit to not measure a coupling of both.

So for me this covers the main issues for the one peak and amplitude of the Lorentzian fit (I noticed you have a detailed frequency resolution, and I assume COMSOL calculated all steps so little risk of under-sampling/under-discretization there).

Now why is the COMSOL model not giving you the absolute peak value as you measure it (5700 versus 4000 nm as I interpret it). This can come from the choice of alpha and beta, here you can also add an ODE equation to your physics, define your alpha and beta and optimize them with COMSOL during the solving process (it takes some extra iterations and time though). But then I would recommend that you do it for a region around ONLY one peak, as the optima alpha and beta fitted most probably will vary from peak to peak. If this is still not enough to get to your absolute value then the damping model is not good enough, you have other (non-linear) effects going on the in the true physics, and you need to add some other physics (but like that I have none to propose, or perhaps some bidirectional thermoelasticity, for these small samples its possible ;).

Finally, you say that with this alpha=0 and beta value your multiple peak does not really fit well your measurements, but in frequency or in amplitude or both? The amplitude of the COMSOL model is highly dependent on your damping model, and to some extend to the input load/impulse and how that excitation is propagating through your model, so for the amplitude you are stuck to tweak alpha and beta, or add some other dissipation physics. for the frequency peaks, these depend essentially on the stiffness and the mass, hence stiffness distribution via the material stiffness tensor field properties and model discretization, and the mass depends on the material density field and the geometrical model discretization. But with added damping the frequency also shifts slightly and if you have a damping depending on the frequency value, then this would also influence the peak locations. If you check the doc you will see that alpha relates to the mass matric while Beta multiplies the stiffness matrix. Rayleigh damping is not really physical neither, but its mathematically well behaved for FEM modeling, hence its well used. For frequency sweeps, you can also use the loss Damping (check the doc) and Viscous damping.

By the way, with damping the COMSOL eigenfrequency and frequency sweep results become complex, but the plots of COMSOL are only the real part!
You have checked that you use both real and imaginary and/or amplitude and phase contributions ?

Finally for these small elastic structures, the deformations are often of non-linear geometry type, have you turned this feature on ? It makes the solver slow down, often one need to tweak the solver settings and used Constant Newton, as non-linear method under the Fully coupled solver node, in this case.

So I cannot give you any direct answers, but I hope that my thoughts can give you some clues or arguments to continue.

--
Have fun COMSOLing
Ivar

Thanks for your advise once again!

I have found the heigher mode by adjusting Rayleigh parameter beta (still keeping alpha 0) such that I have a Q-factor at this mode of approx. 500 (as measured in real experiment).

See the results in attachement - this time showing the amplitude and phases and a better fit procedure. Everything looks very fine. However, there must be something COMPLETELY WRONG in the simulation:

The displacement of the tip is of the order picometer. This is way too small (by a factor 200), ie the changing magnetic field we measure at this mode should be explained by the rotational motion the magnet makes, see attachement (the little sphere on the beam is the ferromagnet I am reffering to).

I did the simulation in Comsol as follows - perhaps the way I build the simulation is complety wrong:

1. build cantilever geometry, put a fixed constraint on the side where there is no magnet.
2. find eigenmodes (These DO correspond with real experiment within 10%)
3. minimize #mesh elements such that the solution to find the eigenmodes do not change significantly.

4. frequency domain study at first mode (3000 Hz). Add a boundary load at the tip edge (order 1 Pa). Add Rayleigh damping: when alpha = 0 than beta = 1/(Q*omega_resonance_mode_n). Tune driving load such that the Lorentzian curve peeks around 4000 nm (it is known from experiment that we have this tip displacement at the first mode when driving the cantilever with our piezos, 100 mV).

5. Used the same driving force for a frequency domain study at a heigher mode (mode 8). Recalculated beta for this mode, should also correspond to a Q-value of 500 (found in experiment).

That's it. Maybe it is still the wrong implementation of damping? According to the struc. mech. module it is very commen to set alpha to 0.

Any idea what could have gone wrong?

p.s.

* I turned on the non-linear solver - it didn't make a difference.
* Thank you a lot for taking time to discuss these problems, your advise helped me a lot building the simulation.

Hi

From what I read, I believe that you are missing some loss factor in your model. the Rayleigh damping are damping of the structures (acting on M&K see the COMSOL users manuals). You said you are in vacuum so there you have removed any aerodynamic damping (apart you talk about a 1 Pa boundary load, not sure what you mean about that it might be in one of the previous exchanges, Nagi proposed a simplified way in one of the Blogs, but you have also the acoustic module that gives ambient pressure exchange, apart I though you were in high vacuum so I might miss the point here).

You said previously you have Eddy current damping so your Q factor was smaller than expected, that is velocity dependent so clearly non linear with frequency as the linear velocity ranges as
(2*pi*f)^2*amplitude but you do not model that as an Eddy current model probably not obvious how to in your case. If you only rely on alpha and beta (M and K terms) be aware they have different effects versus frequency too.

The easiest is to make a "toy model" of two beams and with a frequency sweep you check the alpha and beta behaviors w.r.t. frequency. That might give you some clues. Particularly as your nano beams have larger frequency spans than classical building structures :)

Scaling in physics plays us tricks, hypothesis and common ways to do analysis for large structures are not always the good one and correctly applicable to the nano-scale. It's NOT that the physics has changes, it's the influences of the different physics that are fundamentally different. What might be neglected in one case are predominant in the other. Therefore several older FEM tools, perfectly OK for larger structures gives wrong results for the nano-scale because they do not use enough physics and their black box approach makes the users miss all these points.
With COMSOL it's different, because it's really the user that must select his Physics, the equations do not change but the addition of some extra terms are there and easily available. Still it's the programmer/users task to find which physics to use, that COMSOL cannot tell, with most older tools you can simply NOT add these terms at all, without rewriting the program.
Check the books & literature, and the MEMS doc on the scaling and their effects.

I suspect this boils down to that you do have not a constant "beta", but a "beta" as function of the frequency, to cope for another missing explicit damping physics effect.

Here is a toy model, still everything is to be tested and understood ;)
Run the two studies, then clear and update all Derived values => study the Bode plots
--
Good luck
Ivar

Hi Ivar,

Thank you!!

I'm in high vacuum indeed, the 1 Pa boundary load correspond to the cantilever's driving force exerted by my piezos. As you could see in the graphs I sent you I actually already used a frequency dependent beta to model the damping at the 2 different resonance frequencies, although I have set alpha to 0 at both frequencies.

I could include alpha now to the game (why do they say in the struc mech module that it is commen to set alpha to 0?), and tune alpha and beta at 2 different modes. Maybe that solves my problem of applying the correct damping...

I wish to play with your toy model, only I can't open it since I am using Comsol 5.0...

P.s. with bode plots you just mean the displacment amplitude and phase VS drive frequency right? How are these defined in Comsol by the way, with respect to what? For tip motion, isn't it better to look at displacment fields?

Best,

Rembrandt

Hi

Unfortunately I have only 5.2 active ...

I make my Bode plots as abs(v) of a point at the tip of the beam and the arg() or atan2(imag(v),real(v)) all versus frequency, then I like to use log-log and log plot scales.

I made three beams, in 2D, in steal, 1 m long, 0.02 m thick, one no damping, one with alpha = 100 and the other with beta = 1/100 arbitrary values. Beams are fixed at one end, have 1kPa/m^2 Y load at the other end. I do a fist frequency plot, and a second frequency domain sweep, I tried from 10 to 200 Hz by 1 Hz. but one should also look at higher frequencies to better understand the differences of alpha and beta.

So if you span several modes and a large frequency band you should optimize both alpa and beta to get best values.

--
Good luck
Ivar

Hello there again :-)

Still can't see that since I have COMSOL 5.0... but I appreciate your help!

I actually did a new frequency study, now just using a isotropic loss factor which was equivalent to the Q-value I want. The result is exactly similar when I used Rayleigh damping with alpha set to 0. I think setting alpha to 0 is equivalent to using just an isotropic loss factor - I read something like that in the struc. mech. module.

I reread all our messages, and I think I still need to try to involve alpha to the game:
Tune alpha and beta for the 2 seperate modes such that I get a flat Q. I hope that will be the key to my problem.

I know how to plot Q VS frequency when I do the frequency domain plot, but how to find a good combination between alpha and beta? The stuff I found on the internet was not helping a lot...

You talked about some old Matlab code that could easily find the right combination (but you lost it). Is there a way to do this optimlization in Comsol?

Best,

Rembrandt

OK, I found some combinations for mode 1 where I get a pretty flat Q (damping increases linear with frequency, but with a small slope), but any idea if any solution with a flat Q is a 'good' combination? I noticed that for Q = 500 and omega = 3043 Hz, beta converges to a certain value, ie:

beta alpha
100 -925984893.9
1E+01 -92598483.91
1E+00 -9259842.914
1E-01 -925978.814
1E-02 -92592.404
1E-03 -9253.763
1E-04 -919.8989
1E-05 -86.51249
1E-06 -3.173849
1E-07 5.1600151
1E-08 5.99340151
1E-09 6.076740151
1E-10 6.085074015
1E-11 6.085907402

Any experience with this?

Best,

Rembrandt

OK, I'm a bit further (this question has become a quite obsession) - I did some literature research about damping and I figured out a way to get my alpha and beta tuned - I used 2 frequencies close to the resonance frequency and solved for alpha and beta while keeping the damping parameter constant for both frequencies. I managed to obtain a very flat Q-factor at both modes and till my surprise I still found a very small tip displacement at my higher mode (let's say a factor 10k too small which would be sufficient to fully understand our data).
Is it perhaps possible that my higher mode is 'coupled' to my first mode, even when I drive the system exactly at the higher mode? It could be that the tip displacement motion is is still dominated by the first mode... Is there any way to find out with COMSOL how much 2 modes are coupled?

Thank you very much in advance, I'm looking forward to your insights :-)

p.s. maybe this is not a minor thing, but I forgot to mention that at the first mode I need to adjust the relative tollerence of the solver - otherwise I get diverging solutions. What is exactly the relative tollerence and what does it say about the quality of the simulation?

Best,

Rembrandt