Discussion Forum

Hi

this model can be more or less tricky, if you have only a global constant temperature difference you can use Solid Physics with the material properties and define these as Temperature dependent (essentially E(T) and rho(T)) but then be sure you are in the "material frame" (linear geometry calculations).

Because if you use the full HT and/or work in the "spatial frame", you need a constant density (independent of T) as the T dependence arrive with COMSOL via the geometric deformation (determinant of the Jacobian) calculation that are then turned on in COMSOL. If you use default T dependence on rho you might end up with twice the thermal volume contraction effect, be aware !

All this because the law states conservation of mass, but at the small elementary volume dV=dx*dy*dz one define the Ddensity "rho" as input parameter and not the mass. And the density changes since the volume changes with temperature, but not the global molecular mass encircled by your closed volume.

Last case you have heat flow AND temperature gradients, then you must ensure that your T variable is taken for each elementary volume considered. This is the case for the default set up of Solid with HT combined.

To get the different eigenfrequencies, make a Parametric Sweep with two or more values for your T (or define T via a separate or coupled HT model)

I hope I made myself clear ;)

--
Good luck
Ivar

Hi,

For a beam which is fixed at one end only, all those small details about how different material properties vary with T becomes extremely important. Length, cross section area, etc are also all temperature dependent due to the thermal expansion.

But if the beam is fixed in both ends, then the thermal stress caused by the restrained expansion will give rise to a change in eigenfrequency which is at least one order of magnitude larger than the effects of material temperature dependence. So in that case , what you need is a prestressed eigenfrequncy analysis.

Regards,'Henrik

Hi Henrik

Indeed, I forgot to mention that case,

And then there is also the one I have had most trouble to set up (mainly because I do not have the acoustic module): eigenmodes of a structure partly immersed in a fluid, with a heat flux on top ;)

But there is the Blog of Nagi Elabbasi that gives also some nice tricks :
www.comsol.eu/blogs/natural-frequencies-immersed-beams/

and for the heat flow and deformed solids, the blog of Peng-Chhay Ung:
www.comsol.eu/blogs/heat-transfer-deformed-solids/

--
Good luck
Ivar

Hi ivar and others,

I have simulated a mems capacitive accelerometer. Now I want to find its cross axis sensitivity (how much it will displace in other direction when it is accelerated in one direction?). I dont know how to find it in COMSOL. Waiting for your kind response.

Thanks.

Dear Henrik,

Right now I'm working on clamped beam temperature sensitivity problem. I try to use pres-tress egigenfrequency study, but it always gives me errors. I was wondering if you can give me a simple example contains solid mechanics (clamped beam) and heat transfer in eigenfrequency study.

Thanks a lot!

Wenyuan

Hi

You have a delicate geometry there, as if you have thermal expansion your device will buckle and you enter a non-linear regime, not really compatible with a linear eigenfrequency analysis either.

Still it gives some insights, for me you should add two Parameters with i.e.
T0 = 20[degC]
Tanalyse = T0+10[K]

Then you add a sub node to the Linear Elastic Material node for Thermal heat expansion with T0 in the reference temperature and Tanalyse as current temperature.

Add a Study case: Prestressed Eigenfrequency, and manually add Parametric Sweep (PS) node in front of the Stationary solver node.
Set the PS parameter to Tanalyse and use the values "range(T0,1,T0+10)" or "20 21 22 30" and important, set the units "degC", with the two temperature scales "K" versus "degC" it's very easy to get the T values all messed up => always double check T and its units of your results ;)

Then solve.
You will probably get imaginary frequencies at least for large temperature differences, take the absolute value, but the imaginary values show that there are other phenomena that are interfering here, probably some "numerical damping" too. For small temperature changes you should be able to observe the change in frequency, check carefully your mode shapes as they might change order as T increases.

You will notice three Data Sets so you can also look at the last stationary study results too (add a 3D plot) this is important to check as nonlinear deformation effects will show up here, NOT on the eigenfrequency displacements since these are arbitrary (large) due to the properties of eigenfrequency analysis !

Remains that for your case you should turn on the "include geometrical nonlinearity" solver check for the stationary case as your small device does undergo "large deformations" for larger temperature changes,
then remains an unsolved question for me: should this check boy should still be used for the eigenfrequency node? now with V5.1 it is set on by default, so I'll leave it as is...

Last remark, for you beam with a rectangular link to the restraining pads, you will develop unphysical stress concentrations in these sharp corners, these are "numerically correct" but always difficult to justify when one presents the results, therefore you could add a little fillet, that you will anyhow have from the MEMS processing (perhaps not if you do use wet etching, but then you will really also have a crystalline sharp edge with very high localised stresses

--
Good luck
Ivar

Dear Kjelberg,

Thank you for replying me back. It is really helpful. Right now I'm working on temperature sensor simulation. My partner designed half cross bridge(silicon nitrite, length = 8mm, width = 1mm, thickness=1um ) with rectangular frame(silicon). After heated up the whole device the resonant frequency was increasing first and then drop down. We are assuming the frame is expending first, which apply external stress to the bridge (cause frequency increase). When the temperature increases a lot, the bridge's frequency is dropping down. I want to simulation this kind of phenomenon.

After redesign the same geometry on comsol, the resonant frequency is 11 Hz, but the real experiment is around 296Hz. In order to archive experimental data, I add external stress (11e7 n/m^2). After done that, I add thermal expansion to the bridge and frame separately. However, both turns out drooping the resonant frequency. Since I fix the frame boundary, there won't have any expansion. If I don't fix the frame boundary, the whole frame will vibrate. Could you give me some hints please?

Thanks in advance~

Wenyuan

Hi

you seem to have a delicate issue there, for me it's not clear why the frequency should increase and then drop ? which physical phenomena is responsible for that ?

are you sure you are considering already all the different material properties, and have these expressed in the material data ? such as temperature dependence of alpha, E, ... and that your surrounding is correctly modelled i.e. fixations, and their T dependence.

When you have a multilayer MEMS device one often get high pre-stress in the layers due to their thermal expansion coefficients and the manufacturing process, sometimes one must include this too to get correct values

If you device is "small" which is the case for MEMS then you might also have issues with the surrounding air and air load, coupling to the vibration mode, the air properties are themselves very temperature dependent (viscosity = f(T) and local rho density)

Buckling is a non linear phenomena it's often delicate to simulate and you should ensure you use (if applicable) the non linear geometrical deformations. It might be that you see such a change when switching from a linear to a non-linear regime for the frequency response.

So there are many causes and elements in play, often its worth to identify as many as possible, analyse their mutual influence, and identify a few simple experiments to assess the most important effects separately, as when everything is mixed it's difficult to identify the major players

And I agree, if you are making a sensor, you better understand well the physics involved, else you might get a surprise when producing them, as one minor process change might completely change the responses

--
Good luck
Ivar

Dear Ivar,

Thank you for replying back. I talked with my partner. He said the resonant frequency is increasing initially is because the silicon frame expand faster than silicon nitrite bridge, which cause external stress to the bridge. After temperature increased, the bridge expand faster than frame, so the resonant frequency decrease (w = sqrt(k/m)). I was wondering if you can teach me how to use heat transfer in solid physics to solve this problem.

Thanks,

Wenyuan Zhu

Hi

For the solvers: You need to run a pre-stressed eigenfrequency study (combination of a stationary study to set the stress level from the thermal expansion, and thereafter an eigenfrequency study starting at the previous stationary solution (using the results of the previous study as the linearization point. to scan a series of temperature values, you need to precede the two studies with a Parametric sweep n a parameter you can call T for the constant temperature.

For the physics you need the structural, and add the thermal expansion sub-node to the elastic material node (I assume you do not solve for any thermal flux, and that the temperature is the same over all the model, if not you need to use the TS physics (thermal stress, that is a combination of Solid and HT).

Finally for the material you need to be sure you have all material parameter well defined, possibly also with their T dependence. Then you must define the reference temperature at which you are in correct geometrical dimension and in a stress-free state.

If you dig into the Model/application library, I believe I remember there is such an example somewhere

--
Good luck
Ivar

Dear Kjelberg,

Right now I'm working only on the bridge with magnet. I have a problem with external stress and pre-stress frequency domain analysis. For the external stress in the linear elastic material, the equation of external stress is not consistent. Also, if I use Sext = sigma(ext), it won't have any changes to the study. However, if I use the Sext = JF^-1 sigma(ext) F^-T, it works for eigenfrequecny and stationary study. I have two questions for you. Firstly, why Sext = sigma(ext) doesn't work. Secondly, How can I apply external stress to frequency domain study? The pre-stress study doesn't work. I change everything include adding harmonic load, phase....

Thanks in advance,

wen