# [COMSOL] Cantilever Beam help

1. Aug 28, 2007

### 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...

2. Aug 29, 2007

### Lucas84

No one ?

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

3. Aug 29, 2007

### 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

4. Aug 29, 2007

### 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 [Broken]

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...

Last edited by a moderator: May 3, 2017
5. Aug 29, 2007

### 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.

6. Aug 29, 2007

### Mech_Engineer

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

7. Aug 30, 2007

### vidar

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 cant say at the time.

Last edited: Aug 30, 2007
8. Aug 30, 2007

### Lucas84

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)

Thanks : so the beam lenght 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...

Last edited: Aug 30, 2007
9. Aug 30, 2007

### 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.

#### Attached Files:

File size:
16.7 KB
Views:
542
File size:
16.4 KB
Views:
452
• ###### mode 3.JPG
File size:
17.7 KB
Views:
395
Last edited: Aug 30, 2007
10. Aug 30, 2007

### Mech_Engineer

Modes 4-6 pictures.

#### Attached Files:

File size:
25.4 KB
Views:
376
File size:
21.5 KB
Views:
368
• ###### mode 6.JPG
File size:
23.1 KB
Views:
310
11. Aug 30, 2007

### 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

#### Attached Files:

File size:
20.1 KB
Views:
369
File size:
19.8 KB
Views:
384
• ###### mode 9.JPG
File size:
18.2 KB
Views:
354
12. Aug 30, 2007

### Mech_Engineer

Mode 10 picture:

#### Attached Files:

• ###### mode 10.JPG
File size:
21.1 KB
Views:
405
13. Aug 30, 2007

### 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)...

14. Aug 30, 2007

### Mech_Engineer

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

15. Aug 30, 2007

### 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.

16. Aug 30, 2007

### 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

17. Aug 30, 2007

### Lucas84

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.

18. Aug 30, 2007

### 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.

#### Attached Files:

• ###### mesh.JPG
File size:
61.9 KB
Views:
388
Last edited: Aug 30, 2007
19. Aug 30, 2007

### 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.

#### Attached Files:

• ###### f-resp.JPG
File size:
33 KB
Views:
455
Last edited: Aug 30, 2007
20. Aug 30, 2007

### 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 everthing (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:
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).

Last edited: Aug 30, 2007