Discussion Forum

Hi

you need to explain us the relation you are looking for, as applying a current will give you some joule effect, hence heaing of a conductive media, but that does not explain which frequency you want. Is it a DC current you are using and the eigenfrequency you are looking for under thermal stress ?

or is it a AC current and you are inducing a vibration from the current change and the expansion effect ?

In any case, if its eigenfrequency changes of a pre-stressed beam, you need to use matlab in V3.5 (but nicely "pre-cooked" in v4.2)

Check the forum on how to do an eigenfrequency under pre-stress by a search on the forum (for 3.5)

Else you should consider a frequency domain sweep or a transient analysis, check the doc for the subtile differences ;)

--
Good luck
Ivar

sir,
Thanks a lot for your timely response. It is a DC current which I am applying and i need to know how to find out the frequencies under applied various DC current Voltages?
to be more specific: my problem is some thing simple like i take a beam fixed between two electrodes and apply a certain DC current voltage V across the beam. now i also vary the temperature. because of both voltage and temperature changes the beam deflects, hence i would like to note the frequency at various voltages under a fixed temperature and also frequency at various temperatures at fixed voltage..

Please direct me in this prob or give me a reference of any example
and i would be very grateful to you in this regard

Thanks and regards
R Abhishek.

Hi

then I understand that it is the pre-stressed eigenfrequency you are after, this implies matlab with v3.5 check/search the Forum, it has already been discussed, and there are a few matlab file examples here too

--
Good luck
Ivar

Dear Sir
hope you will be fine. Sir is there any method to put the DC current in the resonator and find the change in the temperature in it. I mean any model in which we just change in the temperature. and also if we can find the change in
Regards
Abid

Hi

if I understand you correctly you want to couple solid (structure) with joule heating = current and your dependent variables is then "u", V and T. This means typically using the "TEM" physics = "Joule heating and thermal exansion" (u,T&V) which is a predefined physics (probably in the "solid" add-in). Another combinations would be thermal stress "TS" for u&T + "JH" joule heating for V separately.

When you define a multiphysics model you should list the dependent variables you need and check with the ones of COMSOL (you need to select them to see that, but you can also use the help module) you should avoid duplicates (i.e. find combinations with just one "T" temperature variable)

--
Good luck
Ivar

Thanks for reply sir, sorry i think i havent explain the question exactly. I am applying the drain voltage in parametric study so my drain voltage is changing which changing the current in the resonator. And i want to find the change in temperature in it and also the resonance frequency of the resonator which will be the function of current or we can say it will be the function of temperature. any suggestion this regards.
Regards
Abid

Hi

certainly your overall temperature depends on the heat dissipation from Joules heating, on one side, and from the loss and convection (perhaps also some conduction) of the surrounding air on the other side, so both most be resolved.

What puzzles me is the "small" air region as you will have exchange from a much greater air volume, and I'm not sure I understand the BC conditions, and if there are enough BC's defined. But as your model looks far from trivial, It's rather normal that I (or most others) cannot grasp everything that easily
--
Good luck
Ivar

Dear Ivar,

I am dealing with about the same problem and have a follow-up question. My situation regards a hinge of which I am actively trying to alter the stiffness by use of thermal stress induced by Joule Heating. My model is quite elaborate by now but finally works as expected. I use strong coupling between the three physics involved (SM, EC, HT) i.e. all three are solved simultaneously in the same study. For more detail see the attached file.

I too want to find out if the resonance frequency changes significantly due to these induced stresses. For that reason I have already applied a prestressed eigenfrequency analysis which shows that the first eigenfrequency goes up from about 65690 to about 65700 Hz, a tiny change for high frequencies but realistic since my hinge is very small (2mm x 1mm). Note that I model it in 2D. What would be the difference in doing a prestressed frequency domain analysis? I have read all tutorials, help files etc and think I have a good understanding of the difference between eigenfrequency & freq analysis. From a previous post of you I find this a good description:
---------------------------------------------------
An eigenfrequency analysis is taking a model, stripping external forces/loads, linearising the model and searching for the eigenmodes of the equation sets

A frequency response is obtained by applying a sinus excitation, giving an amplitude, a phase and then scanning the frequency. If you load is applied such to excite the fundamental modes you should get a peak for your previously calculated eigenfrequencies
---------------------------------------------------
However, I don't get what the differences are in a prestressed analysis, as the joule heating effect is statically incorporated in both cases right? And in both cases you linearize around the solution from the stationary analysis, correct?

Thing is that the prestressed eigenfrequency analysis gives results as mentioned above, but with the prestressed frequency domain analysis I keep getting the error:
----------------------------------
Failed to evaluate variable.
- Variable: mod1.ec.DX
- Geometry: 1
- Domain: 1 3
----------------------------------
So the X or Y component of the electrical displacement field cannot be evaluated. Does this have to do with Comsol's inability to sweep a voltage? This error pops up in the 'frequency domain-perturbed' solver, the stationary solver works. If I uncheck the electric physics, I can plot a resonance plot but don't see any resonance peak.

So main questions:
- what is different between prestressed eigenfreq and prestressed freq dom? What properties are taken into account more in the latter analysis?
- is the stress induced by the joule heating effect due to constant DC current indeed static enough to be used in a perturbation analysis (prestr freq dom)?
- exactly what physics should be checked in the second study step for a prestressed analysis. For prestr eigenfreq I have let everything remain checked as happens by default.

I know it is a lot but I tried to give you a good overview of my situation, thoughts and questions to prevent post on post on post :)

Hopefully you can help me, I have done all the research I possibly could but cannot find satisfying answers and really need to get some results :)

Thanks in advance.

Regards, Arjan

Hi

you have many questions there, here are some of my thoughts, but I might not cover everything:

Your analysis, you say you observe 10Hz change, nice, but on 65000 Hz baseresonance, that is rather small and you should ideally check that its not "just" numerical noise", so my way in thoses cases is a) to run a model with 2x as dense mesh, to be sure I know the mesh denisty behaviour, then I would not only run for one prestress value but for at least 3, such as 0.5x my nominal value, 1x, and 2x my nominal value, to be sure I get a linear or close to fisrt order trend, only with 2 points its difficult to tell anything about relative precision.

Now for you analysis of eigenfrequency and frequency domain, I believe you are right, the eigenfrequency ignores ALL external loads (right side of main PDE equation) and solves the energy equation for the model as is, the frequency domain, applies a harmonic development of all equations such that ALL right hand side elements (boundaries loads) are considered as oscillatory components.

When you want to apply a prestress, you need to first with a stationary solver case apply all your static loads, then use the results of this first solver sequence as the "initial condition" for the eigenfrequency, respectively frequency domain solver case, such that the stationary stress is included and used as starting "linearisation" point, then for the second frequency domain case you need to add/dissable theBC such that you keep only the amplitude of the oscillating one (else all will be applied).

This is different from a transient case, where the stationary solver load case will stress your model, then if you use this as a time series solver, and remove the loads, he model will return to stress less case, by oscillating in time

When you have many physics, and many solvers in the same study, you do not need to solve for all (it might not be relevant), this depends on your model, I suspect your error could come from that, and also, not all physics are made compatible with all solver cases (frequency domain, and 'frequency domain-perturbed' do not work for all physics) to ceck open a new model ans select one physics then see the solver proposed, note it down, go bac change the active physicss, and see what are the default, etc, or just check in the doc, in v4.3 you have the list of physics and applicable solver cases. I suspect this is related to your DX error

--
Good luck
Ivar

Hello Ivar,

Thank you very much for you elaborate answer. Your advice on the mesh density makes sense and seems to work. Roughly these are the results:

mesh density: -- eigenfreq -- prestressed eigenfreq -- delta freq
--------------------------------------------------------------------------------------------
extr. coarse-------- 66253 ------ 66263 ---------------------------- 10
coarser ----------- 66406 ------ 66415 ----------------------------- 9
normal ----------- 65692 ------ 65702 ---------------------------- 10
finer --------------- 65328 ------ 65338 ---------------------------- 10
extremely fine -- 63422 ------ 63432 ---------------------------- 10

Since any FEM model is overconstraint ("more stiff") by definition, it seems right to me that the eigenfrequencies decrease as the mesh gets refined. I therefore think the almost constant bias frequency of 10 Hz is reliable and its small value related to the modest voltage I have put on now (1 mV). Would you agree with me?

Second, with your suggestions I have managed to get the prestressed frequency domain analysis to work. I have incorporated the Joule Heating stress through the stationary analysis (with all physics i.e. SM, EC, HT checked). Then in the perturbated frequency domain step I unchecked EC and HT and have made the point load in SM into a harmonic perturbation load (right-click). This working model I attached.

As regards the interpretation of the result, I'm a bit puzzled. In the attached model you can see both the freq domain response for the unstressed and the pre-stressed case. The unstressed case is nicely at 65692 as predicted by the unstressed eigenfrequency analysis, but the pre-stressed peak is almost at 70000 Hz. Quite a difference with the + 10 Hz from the prestressed eigenfrequency analysis.

Would you have an idea what parts of my model might be taken along in the prestressed freq domain analysis that are not present in the prestressed eigenfreq domain analysis? And do you think this 4400 Hz difference seems logical again given the only 1 mV voltage applied? Stress in the material is significant, approaching the yield stress.

Thanks a lot!
Regards, Arjan

Hi

one thing, avoid using "point" loads, use a boundary load, as anything of lower dimension than a boundary will give singularities. Then as you have an elongated shape, for coarser mesh the results are not very good as your model does not have enough mesh elements in the beam thickness, that is why the frequency changes quite a lot w.r.t mesh density, you could also consider a mapped or sweep mesh but have at least 3-5, if possible more, in the thickness

--
Good luck
Ivar