Troubleshooting Cantilever Beam Simulation in COMSOL

[Lucas84]

Hi everyone,

I've just started to use COMSOL for the study of a simple cantilever beam and I'm facing some problems while calculating the eigenfrequencies and the frequency-response.

I use the 3D MEMS Module>Solid, Stress-Strain. I create a 500e-6,100e-6,10e-6 box. From the Sub-domain menu in Physics I select the default settings for Silicon and from the boundary settings I'm fixing the face 1. In properties I select "large deformation" and "eigenfrequency".

Then I let COMSOL solve the problem, and here appears the first issue : I get an apparently good resonant frequency (49Khz) but the z displacement give 3.33m ! Why ? Is it due to the fact that air damping is not included or something like this ?

Second issue : now I use the frequency-response solver. I fix a Fz load on the upper surface so that (if I'm not wrong) the simulated force will be a Fzsin(2*3.14*f*t). In the Solver parameter I specify a range of frequency around the resonant frequency. I solve the problem, go to Postprocessing menu choose Cross-Section Plot Parameters>Plot and in the predefined quantities select z displacment. Normaly I should obtain a curve with a maximum at the resonant frequency. Instead I have a linear curve. Once again what went wrong.

As I'm a beginner I have a lot of other question, but for the moment I really need help on those specific issues...

Thanks...

 

[Lucas84]

No one ?

Please...I saw in a previous post that some of the people around here had a good knowledge of COMSOL...

Please, please, help me...

 

[AlephZero]

I've never used COMSOL, but:

"I get an apparently good resonant frequency (49Khz) but the z displacement give 3.33m"

If you are doing a vibration analysis, the amplitude of the mode shapes is arbitrary. There may be options to normalize the amplitude by doing things like

* Specify the size of the displacement at one point
* Make the largest displacement = 1.0

The default option may well be what is called "mass normalization", where if the modeshape vector is X, the amplitude is set so that X^T.M.X = 1. If you know the theory of using modal coordinates for frequency response analysis, etc, you will probably see the reason for making that choice. If not, don't worry about it.

"Normally I should obtain a curve with a maximum at the resonant frequency. Instead I have a linear curve"

I'm guessing here, but a classic error is specifying frequency in the wrong units. Check whether the input is supposed to be in rad/sec or Hz.

Try plotting the response over a wide frequency range, e.g. 0 to 200 KHz, if you have a resonance at 49KHz. That should make it more obvious what's going on.

Hope this helps

 

[Lucas84]

First of all thank you very much for your help alephzero.

I've look at COMSOL help, and the input is in Hz as well as the results. However, I did a simulation on a wide range of frequency and here's what I got :

http://img408.imageshack.us/img408/5463/resonancexq3.jpg

It gives me a resonant frequency at 0Hz, 2.4MHz and 7Mhz while the eigenfrequency analysis gives me 49kHz, 307kHz, 861kHz, 1.7Mhz, 2.8Mhz...for the z resonance.

So there's obviously something I missed...But I don't see what...

However, thanks again for your help...

 

[AlephZero]

The lowest vibration frequencies of a cantilever clamped at one end are in the ratio 1 : 6.27 : 17.55.

That matches your frequencies of 49, 307, and 861 Khz very closely.

In your frequency analysis, the resonance at 0 Hz suggests you didn't apply any constraints, so the frequencies will be different (and larger).

The frequencies for a free cantilever are in the ratio 0 : 1 : 2.75 : 5.40

and that matches your resonances at 0, 2.4, 7.0 MHz fairly well (not as closely as the cantilever frequencies)

However the first "free" frequency should be 6.37 times the first "clamped" frequency. Yours is 50 times higher. I can't guess a reason for that.

Checking the constraints seems a good thing to do.

If all else fails, back off from the real problem and make a mass-on-a-spring model, so you are confident what the answers are supposed to be.

Ref. for frequency data: W.T.Thomson, Vibration Theory and Applications, 1966.

 

[Mech_Engineer]

If you gave us the beam's properties, I would be willing to do a "confirmation" in ANSYS.

 

[vidar]

I get an apparently good resonant frequency (49Khz) but the z displacement give 3.33m !

Im facing a similar problem when trying to simulate a cantilever bent under its weight. I recognized a unslightly to large displacement compared with the data of a simulation done with some other software. wether its the fault of comsol or the other software I can't say at the time.

 

[Lucas84]

The lowest vibration frequencies of a cantilever clamped at one end are in the ratio 1 : 6.27 : 17.55.

That matches your frequencies of 49, 307, and 861 Khz very closely.

In your frequency analysis, the resonance at 0 Hz suggests you didn't apply any constraints, so the frequencies will be different (and larger).

The frequencies for a free cantilever are in the ratio 0 : 1 : 2.75 : 5.40

and that matches your resonances at 0, 2.4, 7.0 MHz fairly well (not as closely as the cantilever frequencies)

However the first "free" frequency should be 6.37 times the first "clamped" frequency. Yours is 50 times higher. I can't guess a reason for that.

Checking the constraints seems a good thing to do.

If all else fails, back off from the real problem and make a mass-on-a-spring model, so you are confident what the answers are supposed to be.

Ref. for frequency data: W.T.Thomson, Vibration Theory and Applications, 1966.

Thanks again for your help AlephZero..So, I've applied for both simulation (eigenfrequency and frequency-response) a Rx=0/Ry=0/Rz=0 constraint on the clamped surface. But I don't get the same result. The only option I've changed between those two simualtions is the Load. However, there might be a specific option for the frequency-response constraint that I missed...Then I'll try the mass-on-spring model...

EDIT : I'm just wondering if applying a Rx=0/Ry=0/Rz=0 constraint is sufficient (the end condition for a clamped beam being dv/dx=0 and v=0 where v is the displacement)

If you gave us the beam's properties, I would be willing to do a "confirmation" in ANSYS.

Thanks : so the beam length is 500 micrometers, 100 micrometers width and 10 micrometers thickness. It's a silicon beam. I use the default mechanical properties in COMSOL : Young Modulus = 131E9, density = 2330, poisson ration = .27. It's a clamped-free beam. And I use an arbitrary harmoni load on the upper surface. THat's all...I hope I didn't forget something...

 

[Mech_Engineer]

Ok did a quick modal analysis in Ansys based on the basic dimensions you gave me, and a "fixed support" on one end of the beam. As with other modal analyses, ignore the "max displacements" as they are pretty much gibberish.

Material Properties (Matweb Silicon):

http://www.matweb.com/search/SpecificMaterial.asp?bassnum=AMESi00

Young's Modulus: 112.4 GPa
Poisson's Ratio: 0.28
Density: 2329 Kg/m^3

Calculated Modes:

Mode 1: 45.332 kHz
Mode 2: 283.34 kHz
Mode 3: 436.75 kHz
Mode 4: 439.76 kHz
Mode 5: 792.26 kHz
Mode 6: 1343.4 kHz

Pictures of first three modes attached, next three in next post.

 

[Mech_Engineer]

Modes 4-6 pictures.

 

[Mech_Engineer]

... and just for fun, modes 7, 8, 9, and 10:

Mode 7: 1549.8 kHz
Mode 8: 2316.2 kHz
Mode 9: 2362.1 kHz
Mode 10: 2554.2 kHz

 

[Mech_Engineer]

Mode 10 picture:

 

[Lucas84]

Ok for the eigenfrequencies, using MATweb silicon mechanical properties with COMSOL I get :

Mode 1: 45.467 kHz
Mode 2: 284.68 kHz
Mode 3: 437.23 kHz
Mode 4: 447.07 kHz
Mode 5: 798.66 kHz
Mode 6: 1369.5 kHz

Which is approximatively the same thing (why is there a small difference between the softwares I don't know)...

 

[Mech_Engineer]

Ok for the eigenfrequencies, using MATweb silicon mechanical properties with COMSOL I get :

Mode 1: 45.467 kHz
Mode 2: 284.68 kHz
Mode 3: 437.23 kHz
Mode 4: 447.07 kHz
Mode 5: 798.66 kHz
Mode 6: 1369.5 kHz

Which is approximatively the same thing (why is there a small difference between the softwares I don't know)...

The differences probably have to do with mesh density, boundary conditions, elements used, etc. They are close enough to call them good IMO.

 

[Mech_Engineer]

How many elements do you have in your mesh? Are they mapped face, or varied tetrahedrons? How are you applying the boundary condition; is it by attaching it to an area, or individual elements? Meshing is the most important part of any finite element model, followed closely by BC's.

On another note, ANSYS does not require a load to be applied in modal analysis, just apply your BC's and go... perhaps this accounts for some of the difference as well.

 

[Mech_Engineer]

The large variation in the two sets of material properties tells me you should verify EXCATLY what Silicon you are using, and get the mat properties for it before using your numbers for any sort of design work.

I solved the same problem using your material properties, and came up with the following results:

Mode 1: 48.895 kHz
Mode 2: 305.62 kHz
Mode 3: 471.39 kHz
Mode 4: 476.35 kHz
Mode 5: 854.49 kHz
Mode 6: 1454.8 kHz
Mode 7: 1671.3 kHz
Mode 8: 2507.4 kHz
Mode 9: 2551.2 kHz
Mode 10: 2754.1 kHz

 

[Lucas84]

How many elements do you have in your mesh? Are they mapped face, or varied tetrahedrons? How are you applying the boundary condition; is it by attaching it to an area, or individual elements? Meshing is the most important part of any finite element model, followed closely by BC's.

On another note, ANSYS does not require a load to be applied in modal analysis, just apply your BC's and go... perhaps this accounts for some of the difference as well.

Up to know, I didn't really pay attention to the meshing, I let COMSOL do it automaticly. From what I know, its a varied tetrahedrons meshing, but I don't know how many elements I've got.

I didn't apply any load for the modal analysis. What I said in my previous post was that the modal analysis seems good, the problem was when I was doing a frequency-response analysis. In this analysis I had some strange results.

 

[Mech_Engineer]

Well, what does your mesh look like? It's possible to run into problems if your mesh has only one element through the thickness of the beam (esepecially when using low-order elements), or other things like that. Letting your software automatically mesh the geometry without at least taking a critical look at it can end in tears...

Here's a picture of the one I used (mapped face, obviously). It has 155369 nodes, 32000 elements.

 

[Mech_Engineer]

Here is the frequency respone of the beam based on a frequency acceleration (rather than a force) on the part. The calculated z-displacement is at the unconstrained end of the beam. We can see that there is a spike at the first mode.

 

[AlephZero]

Hey, isn't this supposed to be practical enginneering? Don't get bogged down about the odd percent or two difference between different FE systems! Leave that to the system developers and FE formulation gurus...

You don't need a 155,000 node mesh for this model. 10 beam elements (11 nodes) would be plenty. The bottom line is there's nothing wrong with the OP's vibration analysis, for practical purposes. It looks like the COMSOL analysis is just finding the bending modes in one plane, while the other runs are finding everything (bending in the other plane, torsion, axial...) Big deal. If the OP is only going to excite the bending modes in one plane, that's all you need to get the right answers.

However, I think there some clues that fit together:

First clue:

... and just for fun, modes 7, 8, 9, and 10:
Mode 7: 1549.8 kHz
Mode 8: 2316.2 kHz
Mode 9: 2362.1 kHz
Mode 10: 2554.2 kHz

Mode 9 at about 2.4MHz looks like an axial mode to me.

Second clue: the OP's whole response curve looks rather strange. In particular, the "resonance" at 7Mhz looks a very strange shape unless you have some exotic nonlinear damping in the model (and since damping hasn't been mentioned, I guess either you don't have any damping at all in the model, or you have a default value from the built-in material properties, not something fancy).

Third clue: The displacement scale on the OP's response plot is "times 1e-17". That's a pretty small displacement, whatever units you are working in.

My bet is, the OP applied the sinewave loading in the wrong direction. The load was axially along the beam, not nornal to it. So the bending modes never got excited at all. Plotting a displacement normal to the beam, what you see are "rounding errors" which look rather like a response curve reflected in a distorting mirror.

To the OP: try doing a linear static analysis, and compare the answers to simple beam bending theory. And compare them to the zero-frequency response in Mech Engineer's plot (post #19).

 

[Mech_Engineer]

You don't need a 155,000 node mesh for this model. 10 beam elements (11 nodes) would be plenty. The bottom line is there's nothing wrong with the OP's vibration analysis, for practical purposes. It looks like the COMSOL analysis is just finding the bending modes in one plane, while the other runs are finding everything (bending in the other plane, torsion, axial...) Big deal. If the OP is only going to excite the bending modes in one plane, that's all you need to get the right answers.

Perhaps there are way too many elements in the model, but even so it only took about 10 minutes to solve and adds valuable (and accurate) insight into modes that could not be seen in a 2-d model. Overkill is fun

First clue:

Mode 9 at about 2.4MHz looks like an axial mode to me.

Actually it's another bending mode in the "thick" direction of the beam. It's easier to see from the top, but I messed up in making the picture.

[Mode 1] : [Mode 2] :: [Mode 3] : [Mode 9]

 

[Lucas84]

Ok, first of all once again thanks for your help.

So if we go back to the topic my main issue is the frequency-response analysis. I would like to obtain the same result as Mech_Engineer did (which look pretty good to me). As Alephzero suggest I've tried every direction for the applied force : nothing.

Here is the frequency respone of the beam based on a frequency acceleration (rather than a force) on the part. The calculated z-displacement is at the unconstrained end of the beam. We can see that there is a spike at the first mode.

How did you do exactly (for the frequency accelaration, what option did you use etc...). Do you know how to do it with COMSOL ?

EDIT : There's obviously somethin wrong in my frequency-response simulation, here's the shape of the cantilever given by the eigenfrequency analysis for the first mode :

http://img239.imageshack.us/img239/953/23520520vl9.jpg

But if I do the frequency-response analysis at the same frequency here's the shape I obtain :

http://img510.imageshack.us/img510/1228/16990208ar5.jpg The second one looks wrong in my opinion, now the question is why does it look like that...

 

[AlephZero]

The eigenfrequency mode shape looks OK to me.

In the frequency response, it looks like you have the slope equal to 0 at the wrong end of the beam. Maybe you restrained the X displacements at the wrong end somehow?

It's hard to tell without zooming in on the picture, but that's my guess.

 

[AlephZero]

Perhaps there are way too many elements in the model, but even so it only took about 10 minutes to solve and adds valuable (and accurate) insight into modes that could not be seen in a 2-d model. Overkill is fun

Sure, it's harmless here.

The troubles start when you want to model something with 1,000 interconnected beams and you try to put 155,000 nodes in each beam, of course - then it helps a lot to know how few elements you can get away with and still get useful results

 

[Chris Hillman]

Speaking of cantilevers

Just thought I'd mention some light reading which by coincidence I just came across: Henry Petroski, "The Cantilever", American Scientist, September-October 2007.

 

[AlephZero]

Just thought I'd mention some light reading which by coincidence I just came across: Henry Petroski, "The Cantilever", American Scientist, September-October 2007.

http://www.americanscientist.org/template/AssetDetail/assetid/55852;jsessionid=baa9...

Actually, it misses one key fact in the Galileo story. It wasn't pure academic research at all. He was hired to work on the problem, by a stonemason who was trying to produce stone columns for buildings, but was having big problems the columns breaking when they tried to move them around. In other words, columns "designed" to take a compressive end load were failing when they were being transported as a simply-supported cantilevers loaded by their own weight.

EDIT: Hmm... Something strange about that link. I found in with
google "American Scientist" cantilever
and read it OK. But now I can't get back to it because it says I'm not a subscriber. I don't how what happened there - if you want to read it, maybe try Googling for it.

 

[Lucas84]

Hi again everybody,

First of all I wanted to apologize for my late answers : I know that nobody care but I just have the Internet (and COMSOL) at the office and besides with the jet lag (I'm from France) it's not easy to answer instantly (and correctly). Anyway...

I'm sorry to say that but I'm still stuck. So my first question would be : is there any COMSOL user out there. Beacause I would rather say that this isssue could be solved if someone knew what specialy insane option make the software go crazy where normally everything should go fine...And once again how do I apply an acceleration rather than a force in COMSOL like Mech_Engineer did ?

The eigenfrequency mode shape looks OK to me.

In the frequency response, it looks like you have the slope equal to 0 at the wrong end of the beam. Maybe you restrained the X displacements at the wrong end somehow?

It's hard to tell without zooming in on the picture, but that's my guess.

My guess would be that (and I'm quite pretty sure of that) all hings on the applied force because nothing has been changed from the eigenfrequencies analysis and the frequency-response except that. So yes, once again all is about that applied force. What I did was to apply a surface force on the top one which was equal to : 0,0003495 N/m² (rho(=2330)*thickness(10 micrometers)*acceleration(15m/s²)) and I'm sure that there's something not right in it...

So yes once again HELP !

 

[Chris Hillman]

Galileo good, Google-cloaking bad

Actually, [the American Scientist article] misses one key fact in the Galileo story. It wasn't pure academic research at all. He was hired to work on the problem, by a stonemason who was trying to produce stone columns for buildings, but was having big problems the columns breaking when they tried to move them around. In other words, columns "designed" to take a compressive end load were failing when they were being transported as a simply-supported cantilevers loaded by their own weight.

Interesting! Do you have a citation for that?

Speaking of good reading, Galileo's books remain entertaining (and in places, strikingly modern examples of "popular science"), e.g. On Motion (1590), Mechanics (1600) have been republished by University of Wisconsin Press, and Dialog on the Two New Worlds has been recently republished by University of California Press. (Translated titles vary from translation to translation!)

EDIT: Hmm... Something strange about that link. I found in with
google "American Scientist" cantilever
and read it OK. But now I can't get back to it because it says I'm not a subscriber. I don't how what happened there - if you want to read it, maybe try Googling for it.

Alas, sounds like American Scientist might be guilty of an increasingly common but highly disreputable practice:

http://golem.ph.utexas.edu/category/2007/07/web_spamming_by_academic_publi.html

I think you got to buy the magazine, but it's cheap and there are many other good articles in that issue. Before you ask, I myself have no connection to or financial interest in American Scientist, but it's "popsci for scientists" so IMHO head and shoulders above more expensive rags like the sensationalistic and increasingly cranky New Scientist, which I urge all PF denizens to boycott.

 

[AlephZero]

Interesting! Do you have a citation for that?

No, but I'm 99.9% sure I got it from a reputable book on the history of science, engineering, and/or technology.

This link is circumstantial corroboration: http://esag.harvard.edu/rice/e0_Solid_Mechanics_94_00.pdf Page 4:

He [Galileo] also investigated how the breaking of heavy stone columns, laid
horizontally in storage as beams, depended on the number and condition of their supports.

 

[Lucas84]

Ok so if I understood no one can help...Ok then, thanks anyway (even if I'm the same place as I was a week ago)

 

[bilz]

I was wondering how would you solve this problem (Eigenfrequency Analysis) if you were to include ''air damping'' any user of COMSOL has any idea? because i kinda have the same problem. i want to include air damping in my eigenfrequency analysis...

 

[akancha]

First of all thank you very much for your help alephzero.

I've look at COMSOL help, and the input is in Hz as well as the results. However, I did a simulation on a wide range of frequency and here's what I got :

I have a question concerning performing the simulation over a wide range of frequency in comsol. You mentioned you could do it in the comsol, can you tell me how? When I did the eigenfrequency analysis, it shows me a set of frequencies from which I have to select but not the frequencies of my choice. Thanks for your response!