Note: This discussion is about an older version of the COMSOL Multiphysics® software. The information provided may be out of date.
Discussion Closed This discussion was created more than 6 months ago and has been closed. To start a new discussion with a link back to this one, click here.
beam vibration by a shaker
Posted Aug 27, 2011, 7:25 a.m. EDT Acoustics & Vibrations, Structural Mechanics Version 4.3b, Version 4.4 76 Replies
Please login with a confirmed email address before reporting spam
Hello, eneryone.
I am doing a project simulating a simple beam structure vibrated by a shaker. The left end of the beam is fixed with the shaker. If I want to set the beam vibration acceleration at 10 m/s^2, how can deal with this boundary condition?
Thank you all in advance!
Yuan Xue
I am doing a project simulating a simple beam structure vibrated by a shaker. The left end of the beam is fixed with the shaker. If I want to set the beam vibration acceleration at 10 m/s^2, how can deal with this boundary condition?
Thank you all in advance!
Yuan Xue
Attachments:
76 Replies Last Post Apr 28, 2015, 11:56 a.m. EDT
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
You can apply a prescribed acceleration to the beam end that is fixed to the shaker. If you want the steady state response you should do a frequency domain analysis, set the frequency in the Study settings and just prescribe an acceleration of 10.0. Otherwise, you should perform a time dependent analysis and prescribe the acceleration such as 10.0*sin(omega*t).
Nagi Elabbasi
Veryst Engineering
Nagi Elabbasi
Veryst Engineering
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
take a little care the prescribed acceleration: it is a body load.
I would rather say a shaker is applying a force boundary load, hence running a harmonic solver would give you the frequency response. And with a little fiddling you can get a Bode plot, as these are not (yet I hope) implemented as such
--
Good luck
Ivar
take a little care the prescribed acceleration: it is a body load.
I would rather say a shaker is applying a force boundary load, hence running a harmonic solver would give you the frequency response. And with a little fiddling you can get a Bode plot, as these are not (yet I hope) implemented as such
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
I don’t think so Ivar. Prescribed acceleration in the Solid Mechanics modules is a boundary condition, just like prescribed displacement except that it is only applicable to time dependent and frequency domain problems.
Nagi Elabbasi
Veryst Engineering
Nagi Elabbasi
Veryst Engineering
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Nagi
You are right I was a bit quick there, there is also a boundary acceleration condition.
I got caught the other day on the use of the domain one ;)
One must always reread the hypothesis behind the different BC and physics, some are not trivial ;)
But now, to come back to the MEMS shaker test:
If you apply a shaker test (on a beam just to have an example) you have basically (at least) 2 possibilities:
1) you place the full system on the shaker and you apply a body load from the acceleration of the shaker (your fixed point is also shaking ! hence this is not "just" using the acceleration boundary or domain body load on a fixed lever
2) you attach a boundary to the shaker and you apply locally an excitation force, but the fix point is "fixed" inertially
the responses are different see below.
Take a beam 1, 0.1, 0.01 m^3 (x,y,z) size in structural steel. Attach "fixed" boundary 1 (the first small 0.1x0.01m^2 or y,z plane side), load boundary 6 (the other end of the beam) with an acceleration and then with a Force (both in Z), and do a harmonic scan of the type f=10^{range(0,0.01,2)}
then plot in log/log (or adapt to dB) mode the average "w" or "disp" value of the excited boundary "6" you will not get the same response.
Then, try a domain acceleration => its all wrong so long you do not replace the "fixed" boundary condition by something adapted to the acceleration motion,
something to think over ;)
That is why using COMSOL is fun, you can test quickly on simple examples without braking anything
--
Good luck
Ivar
You are right I was a bit quick there, there is also a boundary acceleration condition.
I got caught the other day on the use of the domain one ;)
One must always reread the hypothesis behind the different BC and physics, some are not trivial ;)
But now, to come back to the MEMS shaker test:
If you apply a shaker test (on a beam just to have an example) you have basically (at least) 2 possibilities:
1) you place the full system on the shaker and you apply a body load from the acceleration of the shaker (your fixed point is also shaking ! hence this is not "just" using the acceleration boundary or domain body load on a fixed lever
2) you attach a boundary to the shaker and you apply locally an excitation force, but the fix point is "fixed" inertially
the responses are different see below.
Take a beam 1, 0.1, 0.01 m^3 (x,y,z) size in structural steel. Attach "fixed" boundary 1 (the first small 0.1x0.01m^2 or y,z plane side), load boundary 6 (the other end of the beam) with an acceleration and then with a Force (both in Z), and do a harmonic scan of the type f=10^{range(0,0.01,2)}
then plot in log/log (or adapt to dB) mode the average "w" or "disp" value of the excited boundary "6" you will not get the same response.
Then, try a domain acceleration => its all wrong so long you do not replace the "fixed" boundary condition by something adapted to the acceleration motion,
something to think over ;)
That is why using COMSOL is fun, you can test quickly on simple examples without braking anything
--
Good luck
Ivar
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Thank you Nagi and Ivar. Your answer is really helpful to me.
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
I think u can better put a prescribed displacement ...
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi, John. Yes. It seems better to put a prescribed displacement according to my expected input acceleration. When I set a sinusoidal prescribed displacement at the left end of the beam, do the time-dependant analysis, I can get the expected sinu displacement at the point.
However, when I do frequency domain analysis, I cannot get the result that the displacement reach the highest at resonant frequency of the beam. Here is what I got.
However, when I do frequency domain analysis, I cannot get the result that the displacement reach the highest at resonant frequency of the beam. Here is what I got.
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
if you impose an acceleration or a prescribed displacement the response is fixed your harmonic displacement is given or driven via acc=iomega^2*disp
Tryo use a boundary force of 1[N] then you will see the bodeplot if you plot the average tip displacement versus frequency (see my previous graph image above)
--
Good luck
Ivar
if you impose an acceleration or a prescribed displacement the response is fixed your harmonic displacement is given or driven via acc=iomega^2*disp
Tryo use a boundary force of 1[N] then you will see the bodeplot if you plot the average tip displacement versus frequency (see my previous graph image above)
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
This post is a little bit old but maybe someone can help me.
I am trying to do this exact same thing but with a prescribed displacement reprsenting the shaker and I am a bit confused, I try to apply the displacement to the fixed end of the beam and it clear overrides my fixed constraint and my simulation fails.
Am I missing something?
Is there something other than a prescribed displacement that I should be applying?
Thank you in advance.
Mikkel
I am trying to do this exact same thing but with a prescribed displacement reprsenting the shaker and I am a bit confused, I try to apply the displacement to the fixed end of the beam and it clear overrides my fixed constraint and my simulation fails.
Am I missing something?
Is there something other than a prescribed displacement that I should be applying?
Thank you in advance.
Mikkel
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
if you have a time dependent displacement signal (lets say for a vertical motion), I would try 1) to model a fixing feature as a slab, then on the vertical edge apply a roller condition 2) perpendicular ones for 3D and impose a vertical "z" prescribed motion on this rigid interface. Then your DUT (device under test) wil lsee a vertical motion, hence also acceleration. I would also add a vertical body load to give the constant gravity as "-solid.rho*g_const"
However, often you can transfor this into a fully fixed feature (I would anyhow add afixation item and let it out for the tress plots just to be sure you have a fully representative I/F (interface) and now stress concetration items) and then add a varying body load deendign on your acceleation spectra
And I would use tha lastest version, 4.0 was really a "first version" of the new interface, many things have been improved since
--
Good luck
Ivar
if you have a time dependent displacement signal (lets say for a vertical motion), I would try 1) to model a fixing feature as a slab, then on the vertical edge apply a roller condition 2) perpendicular ones for 3D and impose a vertical "z" prescribed motion on this rigid interface. Then your DUT (device under test) wil lsee a vertical motion, hence also acceleration. I would also add a vertical body load to give the constant gravity as "-solid.rho*g_const"
However, often you can transfor this into a fully fixed feature (I would anyhow add afixation item and let it out for the tress plots just to be sure you have a fully representative I/F (interface) and now stress concetration items) and then add a varying body load deendign on your acceleation spectra
And I would use tha lastest version, 4.0 was really a "first version" of the new interface, many things have been improved since
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Ivar,
Thank you for the response.
What I actually have is Acceleration vs frequency data that i would like to input, so I'm looking to run a frequency study but instead of having a single constant acceleration I would like to have it varying depending on the frequency value.
It seems like this might be possible but I was getting stuck even applying just an acceleration.
Mikkel
Thank you for the response.
What I actually have is Acceleration vs frequency data that i would like to input, so I'm looking to run a frequency study but instead of having a single constant acceleration I would like to have it varying depending on the frequency value.
It seems like this might be possible but I was getting stuck even applying just an acceleration.
Mikkel
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I believe it should be possible with a fequency sweep (harmonic) solver and link the bondary acceleration amplitude to the frequency by an appropriate equation
--
Good luck
Ivar
I believe it should be possible with a fequency sweep (harmonic) solver and link the bondary acceleration amplitude to the frequency by an appropriate equation
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Thanks again Ivar, your suggestion of using the rollers seems to have worked out very well
Mikkel
Mikkel
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
if you have a time dependent displacement signal (lets say for a vertical motion), I would try 1) to model a fixing feature as a slab, then on the vertical edge apply a roller condition 2) perpendicular ones for 3D and impose a vertical "z" prescribed motion on this rigid interface. Then your DUT (device under test) wil lsee a vertical motion, hence also acceleration. I would also add a vertical body load to give the constant gravity as "-solid.rho*g_const"
However, often you can transfor this into a fully fixed feature (I would anyhow add afixation item and let it out for the tress plots just to be sure you have a fully representative I/F (interface) and now stress concetration items) and then add a varying body load deendign on your acceleation spectra
And I would use tha lastest version, 4.0 was really a "first version" of the new interface, many things have been improved since
--
Good luck
Ivar
According to my experience with this kind of problems, an "accelaration bc" set at the constrained surface/edge of the structure leads to an oscillatory motion about a non-zero value of the displacement.
To set an input acceleration to a model I just use a body load equal to "-solid.rho*input_acc" and then use the "canonical" fixed BC at the constrained surface/edge of the structure.
It works properly.
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Alessandro
I agree with you that the easiest is often to model the device fixed, and virtually shake the full modelling environment with a body load. Ideally in Frequency domain with the envelope PSD spectra (assuming the coupling is linear)
Simialr to a rotating object model as fixed and where one rotates the referential frame via a rotating/radial boady load
--
Good luck
Ivar
I agree with you that the easiest is often to model the device fixed, and virtually shake the full modelling environment with a body load. Ideally in Frequency domain with the envelope PSD spectra (assuming the coupling is linear)
Simialr to a rotating object model as fixed and where one rotates the referential frame via a rotating/radial boady load
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello everyone,
I've got a similar problem with a simulation of a vibration test. For easy understanding and a fast simulation I have simplified the model to a beam with the dimensions 1m * 0,02m * 0,02m (x, y ,z), which is fixed on the left end. Now this cantilever should be excited by an acceleration, but I don't know how to define this acceleration in the simulation. The first try was to define a boundary "prescribed acceleration" at the fixed end of this beam, but then the first condition gets overwritten, which is definitely wrong. I've also tried to simulate the beam of Ivar and the same results came out, but this is not the same task. I need a frequency-acceleration plot of this model, where the acceleration amplitudes of this cantilever can clearly be seen due to the eigenfrequencies of it. For example (acceleration of 5 m/s²), for the first 10 Hz there is almost a constant acceleration of 5 m/s², but at the first eigenfrequency of about 16 Hz there is a gain of xxx Q. After that the acceleration goes down and gets higher again at the second eigenfrequency, and so on.
So, how can I simulate this task, where should the acceleration act and also which kind of acceleration should act?
Thank you in advance for your help!!
Kind regards
I've got a similar problem with a simulation of a vibration test. For easy understanding and a fast simulation I have simplified the model to a beam with the dimensions 1m * 0,02m * 0,02m (x, y ,z), which is fixed on the left end. Now this cantilever should be excited by an acceleration, but I don't know how to define this acceleration in the simulation. The first try was to define a boundary "prescribed acceleration" at the fixed end of this beam, but then the first condition gets overwritten, which is definitely wrong. I've also tried to simulate the beam of Ivar and the same results came out, but this is not the same task. I need a frequency-acceleration plot of this model, where the acceleration amplitudes of this cantilever can clearly be seen due to the eigenfrequencies of it. For example (acceleration of 5 m/s²), for the first 10 Hz there is almost a constant acceleration of 5 m/s², but at the first eigenfrequency of about 16 Hz there is a gain of xxx Q. After that the acceleration goes down and gets higher again at the second eigenfrequency, and so on.
So, how can I simulate this task, where should the acceleration act and also which kind of acceleration should act?
Thank you in advance for your help!!
Kind regards
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
what about using a body load of solid.rho*acceleration. If you want to do a sinus load case, try the frequency harmonic solver with a frequency span start-stop, and perhaps a frequency dependent acceleration.
I'm too missing a simple template as part of COSMOL by default to enter a PSD curve for load definition, so one need to make a function and a parametric PSD input shape, and it works ;)
--
Good luck
Ivar
what about using a body load of solid.rho*acceleration. If you want to do a sinus load case, try the frequency harmonic solver with a frequency span start-stop, and perhaps a frequency dependent acceleration.
I'm too missing a simple template as part of COSMOL by default to enter a PSD curve for load definition, so one need to make a function and a parametric PSD input shape, and it works ;)
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Ivar,
thank you very much for your answer. I've tried to use a body load and have a question about the simulation results. The acceleration peaks are not realistic, aren't they? And how do I get realistic stress results? If I choose von Mises stress at the eigenfrequencies the stress is much too high. The results are important, because with these values it is possible to choose the right material and/or geometry. The same thing happens if I choose a geometry of 1*0,2*0,2m, where the maximum acceleration is about 1400g...
Another question to your answer, how can I apply a harmonic body load and where can I find the frequency harmonic solver? If I right-click on body load and choose "Harmonic Perturbation" it should be harmonic, but if the simulation gets computed the acceleration is really small (about 1e-4). Do I have to set something else? Or do I have to choose the "Frequency-Domain Modal" Analyses? Because there I get some results, which aren't too low or high...
Last question, how is it possible to generate a PSD curve? I think this is just possible in the time-dependent analyses, isn't it?
Thank you very much for your help!!!!
PS: You can find a acceleration over frequency plot in the attachment of the cantilever example (1*0,02*0,02m) with 5 m/s² body load (steel). Are the results right?
thank you very much for your answer. I've tried to use a body load and have a question about the simulation results. The acceleration peaks are not realistic, aren't they? And how do I get realistic stress results? If I choose von Mises stress at the eigenfrequencies the stress is much too high. The results are important, because with these values it is possible to choose the right material and/or geometry. The same thing happens if I choose a geometry of 1*0,2*0,2m, where the maximum acceleration is about 1400g...
Another question to your answer, how can I apply a harmonic body load and where can I find the frequency harmonic solver? If I right-click on body load and choose "Harmonic Perturbation" it should be harmonic, but if the simulation gets computed the acceleration is really small (about 1e-4). Do I have to set something else? Or do I have to choose the "Frequency-Domain Modal" Analyses? Because there I get some results, which aren't too low or high...
Last question, how is it possible to generate a PSD curve? I think this is just possible in the time-dependent analyses, isn't it?
Thank you very much for your help!!!!
PS: You can find a acceleration over frequency plot in the attachment of the cantilever example (1*0,02*0,02m) with 5 m/s² body load (steel). Are the results right?
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I'm not by my WS so I cannot test it out, but why shouldt the amplitudes be correct ? If you apply a body load of g_const*solid.rho its gravity load, and this has always worked for me ;)
What you might see is the Q facor amplification, when you excite the resonance, have you added some damping in your system ? to make it more ralistic ?
Normally, the stress is related to the displacement, so if the displacement is not realistic, certainly the stress is neither not correct.
Have you found the frequency domain solver, check the equation view to see what you can do and what is considered.
One can transfor a PSD to an equivalent frequency sinus sweep response (in LTI system) check the web on virations loads, our the litterature
--
Good luck
Ivar
I'm not by my WS so I cannot test it out, but why shouldt the amplitudes be correct ? If you apply a body load of g_const*solid.rho its gravity load, and this has always worked for me ;)
What you might see is the Q facor amplification, when you excite the resonance, have you added some damping in your system ? to make it more ralistic ?
Normally, the stress is related to the displacement, so if the displacement is not realistic, certainly the stress is neither not correct.
Have you found the frequency domain solver, check the equation view to see what you can do and what is considered.
One can transfor a PSD to an equivalent frequency sinus sweep response (in LTI system) check the web on virations loads, our the litterature
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi,
thank you very much for your fast answers! Ok, good to know. I just thought the amplitudes are too high, but at the moment no damping has been included in the simulations.
You said the stress is related to the displacement, which is clear. But I've seen some other comments and questions in this forum where you say, that Comsol just calculates the eigenfrequencies of the respective part and therefore the displacements are not really correct, they are normalized by an factor. In this case it's the same problem, I get deformations of about 4 meters, where the cantilever has just a length of 1m. Do you maybe know where it is possible to see realistic deformations and stress? Or where you can set this normalization factor to get realistic results?
At the frequency domain solver it is just possible to choose the available study type. What do you mean here?
Thank you very much for your help!!
PS: Sorry for so many questions, I'm completely new to Comsol
thank you very much for your fast answers! Ok, good to know. I just thought the amplitudes are too high, but at the moment no damping has been included in the simulations.
You said the stress is related to the displacement, which is clear. But I've seen some other comments and questions in this forum where you say, that Comsol just calculates the eigenfrequencies of the respective part and therefore the displacements are not really correct, they are normalized by an factor. In this case it's the same problem, I get deformations of about 4 meters, where the cantilever has just a length of 1m. Do you maybe know where it is possible to see realistic deformations and stress? Or where you can set this normalization factor to get realistic results?
At the frequency domain solver it is just possible to choose the available study type. What do you mean here?
Thank you very much for your help!!
PS: Sorry for so many questions, I'm completely new to Comsol
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
eigenfrequency analysis is normalised and amplitude are arbitrary (you can select three different types of normalisation in v4.2a also to give mass participation factors) see the solver sub node for eigenfrequency.
A frequency domain (harmonic development) is giving you "correct" amplitudes, if you have enough damping to have finite Q factors. The difficulty is really to decide what to use for the damping, as this is very model dependent, you have material damping, assemby damping and perhaps also eddy current damping, induced fluid flow damping ...
By default there is no damping (apart perhaps something from numerical effects) there is a specific chapter in the reference doc, I believe on that too
--
Good luck
Ivar
eigenfrequency analysis is normalised and amplitude are arbitrary (you can select three different types of normalisation in v4.2a also to give mass participation factors) see the solver sub node for eigenfrequency.
A frequency domain (harmonic development) is giving you "correct" amplitudes, if you have enough damping to have finite Q factors. The difficulty is really to decide what to use for the damping, as this is very model dependent, you have material damping, assemby damping and perhaps also eddy current damping, induced fluid flow damping ...
By default there is no damping (apart perhaps something from numerical effects) there is a specific chapter in the reference doc, I believe on that too
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello,
thank you very much for your answer. I have version 4.2, and maybe you mean "RMS", "Max" and "Mass matrix" in the section "Eigenvalue Solver" at "Scaling", is that correct? If I choose these three different types I get complete different results, and by choosing "Mass matrix" a "more correct" result. Do I have to choose this type for stress calculation? I want to state a sentence in the documentation of COMSOL, where the Mass matrix scale type "... is a common choice for the scaling of eigenvectors within the structural mechanics field."
I understand that the choice of damping is dependent on many factors as I have read this in the internet. But, if I calculate alpha and beta and use these values for the calculation, the stress and also displacements are wrong again. I'm doing something wrong, but I don't know what...
Thank you very much!!!
thank you very much for your answer. I have version 4.2, and maybe you mean "RMS", "Max" and "Mass matrix" in the section "Eigenvalue Solver" at "Scaling", is that correct? If I choose these three different types I get complete different results, and by choosing "Mass matrix" a "more correct" result. Do I have to choose this type for stress calculation? I want to state a sentence in the documentation of COMSOL, where the Mass matrix scale type "... is a common choice for the scaling of eigenvectors within the structural mechanics field."
I understand that the choice of damping is dependent on many factors as I have read this in the internet. But, if I calculate alpha and beta and use these values for the calculation, the stress and also displacements are wrong again. I'm doing something wrong, but I don't know what...
Thank you very much!!!
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
indeed these are the three critical in eigenfrequency studies (I'm not always behind my WS so sometimes my mind get the names wrong).
But the frequency should not change, the amplitude: yes, as this changes with the normaisation, but the "shape" remains, and that is all wat you can get out of an egenfrequency solver. (Frequency domain solver is another story)
Therefore, the stress in an eigenfrequency is also "wrong" in "absolute" values, but relative values can give you info where you have stress concentration. Again frequency domain solver gives you correct values energy in - out, so if you have a representative damping in frequency domain you get a reasonable amplitude and stress (but do not forget the damping ;)
--
Good luck
Ivar
indeed these are the three critical in eigenfrequency studies (I'm not always behind my WS so sometimes my mind get the names wrong).
But the frequency should not change, the amplitude: yes, as this changes with the normaisation, but the "shape" remains, and that is all wat you can get out of an egenfrequency solver. (Frequency domain solver is another story)
Therefore, the stress in an eigenfrequency is also "wrong" in "absolute" values, but relative values can give you info where you have stress concentration. Again frequency domain solver gives you correct values energy in - out, so if you have a representative damping in frequency domain you get a reasonable amplitude and stress (but do not forget the damping ;)
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello Ivar,
thank you very much for your fast answer. To summarize, it is just possible to calculate the respective eigenfrequencies of each part in the eigenfrequency analyses and nothing else.
You mentioned that in the frequency domain analyses it would be possible to get "correct" stress results. For example, if I want to simulate this cantilever the first eigenfrequency is at 16.35Hz and now it is possible to determine the stress and deformation there, but with a frequency domain analyses. Therefore it is necessary to define a range of (for example) range(10,0.1,20) to calculate the maximum stress there. And, of course, I define damping by the isotropic structural loss factor of 0.04, because I know that ζ has an value of 0.02 (2%) and η can be calculated with 2 multiplied with ζ.
Is everything correct? I hope so, because then I would understand it now ...finally!!! :-)
Thank you very much in advance!!
thank you very much for your fast answer. To summarize, it is just possible to calculate the respective eigenfrequencies of each part in the eigenfrequency analyses and nothing else.
You mentioned that in the frequency domain analyses it would be possible to get "correct" stress results. For example, if I want to simulate this cantilever the first eigenfrequency is at 16.35Hz and now it is possible to determine the stress and deformation there, but with a frequency domain analyses. Therefore it is necessary to define a range of (for example) range(10,0.1,20) to calculate the maximum stress there. And, of course, I define damping by the isotropic structural loss factor of 0.04, because I know that ζ has an value of 0.02 (2%) and η can be calculated with 2 multiplied with ζ.
Is everything correct? I hope so, because then I would understand it now ...finally!!! :-)
Thank you very much in advance!!
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
for me eigenfrequency gives three iformations:
- the (eigen)frequencies in Hz,
- the relative modal shapes but (not absolute amplitudes) and also the relative stress concentrations (but not amplitude absolute values),
- and finally the modal mass participation factors, which is another way to look at the realtive energy distribution between modes.
Again its all relative, except for the "asolute" frequency values.
The freqency domain analysis gives you an absolut response (provided damping is correctly defined) per Newton or what ever excitation value/density you give as excitation. Check your equations to see the driveing BCs
Also damping values depend on what you know or have measured, rather model dependent, but as you say these are often distribted between a frequency dependent damping factor and some structural or viscuous damping
--
Good luck
Ivar
for me eigenfrequency gives three iformations:
- the (eigen)frequencies in Hz,
- the relative modal shapes but (not absolute amplitudes) and also the relative stress concentrations (but not amplitude absolute values),
- and finally the modal mass participation factors, which is another way to look at the realtive energy distribution between modes.
Again its all relative, except for the "asolute" frequency values.
The freqency domain analysis gives you an absolut response (provided damping is correctly defined) per Newton or what ever excitation value/density you give as excitation. Check your equations to see the driveing BCs
Also damping values depend on what you know or have measured, rather model dependent, but as you say these are often distribted between a frequency dependent damping factor and some structural or viscuous damping
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello Ivar,
at the moment everything is clear, so thank you very much for your help!! Have a nice day!
Kind regards
at the moment everything is clear, so thank you very much for your help!! Have a nice day!
Kind regards
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I notice I have forgotten to say that adding damping to eigenfrequency gives you imaginary frequencies, as you have phase lag, use the abs() or phasor approach.
This applies also to frequency domain responses
--
Good luck
Ivar
I notice I have forgotten to say that adding damping to eigenfrequency gives you imaginary frequencies, as you have phase lag, use the abs() or phasor approach.
This applies also to frequency domain responses
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
and to add a little more, the prescribed acceleration on a "otherwise fixed" base, works OK with the Frequency Domain solver, but I cannot get it to work with Frequency Domain Modal solver, as I havnt found out yet how to apply a harmonic perturbation on the "acceleration".
And I want to correct my too quick remark earler hereabove, a distributed force load (or body load), and a prescribed acceleration are not look fully the same, as the transfer functions varies. For a prescribed base acceleration you need to analyse the difference between the point on the object and a reference point on the moving/accelerated "base"
A third method (at least present in 4.2a) that does work in Frequency Domain Modal is to apply a Force on teh otherwise rigid base, such as total_mass*g_const.
Note there is something else with the Frequency Domain - Modal studies refgarding the amplitudes. as there are two places where to define amplitudes (and damping), at the BCs and at the modal solver node
This needs some more testing before I can say I master it fully ;)
--
Good luck
Ivar
and to add a little more, the prescribed acceleration on a "otherwise fixed" base, works OK with the Frequency Domain solver, but I cannot get it to work with Frequency Domain Modal solver, as I havnt found out yet how to apply a harmonic perturbation on the "acceleration".
And I want to correct my too quick remark earler hereabove, a distributed force load (or body load), and a prescribed acceleration are not look fully the same, as the transfer functions varies. For a prescribed base acceleration you need to analyse the difference between the point on the object and a reference point on the moving/accelerated "base"
A third method (at least present in 4.2a) that does work in Frequency Domain Modal is to apply a Force on teh otherwise rigid base, such as total_mass*g_const.
Note there is something else with the Frequency Domain - Modal studies refgarding the amplitudes. as there are two places where to define amplitudes (and damping), at the BCs and at the modal solver node
This needs some more testing before I can say I master it fully ;)
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello Ivar,
thank you for your comments. But, as you said before, to simulate a vibration test it is necessary to use a body load with rho*acceleration, is that right? I have also a question about such a simulation: If I have an assembly with 10 parts, and there are 3 different materials used, how should I define the body loads? For example if one part is made of steel and another one is made of titan, then they have different densities and also the body load would be a different one of each part. How can this problem get solved?
Another question to a simulation of an assembly. Do I have to set the boundary conditions of each part in Comsol, or does Comsol use these BC's of the constructing program (in this case of Solid Edge)? With BC's I mean how the parts can move and in which direction they cannot.
Thank you very much in advance for your answer!
thank you for your comments. But, as you said before, to simulate a vibration test it is necessary to use a body load with rho*acceleration, is that right? I have also a question about such a simulation: If I have an assembly with 10 parts, and there are 3 different materials used, how should I define the body loads? For example if one part is made of steel and another one is made of titan, then they have different densities and also the body load would be a different one of each part. How can this problem get solved?
Another question to a simulation of an assembly. Do I have to set the boundary conditions of each part in Comsol, or does Comsol use these BC's of the constructing program (in this case of Solid Edge)? With BC's I mean how the parts can move and in which direction they cannot.
Thank you very much in advance for your answer!
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
First how to simulate body loads with different materials ?
that is easy: as you define the load as a density in N/m^3 or simply g_const*solid.rho
This way you distribute the load on each mesh element depending on its local density (also valid for a density that might vary with the position in a domain). You can also say that you know the totoal mass, and acceleration F= Mass*g_const. Then COMSOL will distribute that AVERAGE force value onto each element, not exactly the same and certainly not for different domains with different densities
2nd point acceleration or body load ?.
I say that both work with a frequency domain sweep, but the prescribed acceleration does not work (for me, I might have missed something) for the frequency domain - modal analysis, as I cannot set the harmonic perturbation option on prescribed acceleration loads.
I was too quick in my first reply, and forgotten that a body force random excitation is not exactly the same as a random prescribed acceleration (from the base) excitation. The transfer functions differ, in one case its x, in the other case its (x-xbase) relative motion you are looking after.
But if you have a complex model Frequency domain might be heavy to solve, while frequency modal is rather quick and precise enough if you sort out the main modes
--
Good luck
Ivar
First how to simulate body loads with different materials ?
that is easy: as you define the load as a density in N/m^3 or simply g_const*solid.rho
This way you distribute the load on each mesh element depending on its local density (also valid for a density that might vary with the position in a domain). You can also say that you know the totoal mass, and acceleration F= Mass*g_const. Then COMSOL will distribute that AVERAGE force value onto each element, not exactly the same and certainly not for different domains with different densities
2nd point acceleration or body load ?.
I say that both work with a frequency domain sweep, but the prescribed acceleration does not work (for me, I might have missed something) for the frequency domain - modal analysis, as I cannot set the harmonic perturbation option on prescribed acceleration loads.
I was too quick in my first reply, and forgotten that a body force random excitation is not exactly the same as a random prescribed acceleration (from the base) excitation. The transfer functions differ, in one case its x, in the other case its (x-xbase) relative motion you are looking after.
But if you have a complex model Frequency domain might be heavy to solve, while frequency modal is rather quick and precise enough if you sort out the main modes
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello Ivar,
thank you very much for your well explained answer. But I have a last question about simulating an assembly : Do I have to set the boundary conditions of each part in Comsol, or does Comsol use these BC's of the constructing program (in this case of Solid Edge or CATIA)? With BC's I mean how the parts can move and in which direction they cannot.
Kind regards
thank you very much for your well explained answer. But I have a last question about simulating an assembly : Do I have to set the boundary conditions of each part in Comsol, or does Comsol use these BC's of the constructing program (in this case of Solid Edge or CATIA)? With BC's I mean how the parts can move and in which direction they cannot.
Kind regards
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
careful with what you call "assembl"y, in the CAD its a series of "parts", "bodies" or "Objects" for COMSOL, that transform into "domains" in COMSOL (sometimes into several domains per body all depends how they possibly interfere).
On the other hand "assembly" mode of the geometry in COMSOL is something DIFFERENT, it means that the common boundaries between the domains are not automatically knit together with a continuation boundary condition, as it will be in COMSOL "Geometry UNION" mode (note objects like bodies = volumes (in 3D), surfaces, lines and vertexes are CAD items, while once analysed by COMSOL these are transformed into geometrical ENTITIES: Domains, Boundaries, Edges and Points onto which you attach your physics (mainly onto domains and boundaries), and onto which you get the mesh to discretize your model for the solving process.
When you import a "CAD assembly" made of different parts in contact over a common boundary, then if you use COMSOL "Geometry Union" mode these will be "glued" together, even you will find only one common (internal) boundary belonging to each domain
Hope this is clear ;)
--
Good luck
Ivar
careful with what you call "assembl"y, in the CAD its a series of "parts", "bodies" or "Objects" for COMSOL, that transform into "domains" in COMSOL (sometimes into several domains per body all depends how they possibly interfere).
On the other hand "assembly" mode of the geometry in COMSOL is something DIFFERENT, it means that the common boundaries between the domains are not automatically knit together with a continuation boundary condition, as it will be in COMSOL "Geometry UNION" mode (note objects like bodies = volumes (in 3D), surfaces, lines and vertexes are CAD items, while once analysed by COMSOL these are transformed into geometrical ENTITIES: Domains, Boundaries, Edges and Points onto which you attach your physics (mainly onto domains and boundaries), and onto which you get the mesh to discretize your model for the solving process.
When you import a "CAD assembly" made of different parts in contact over a common boundary, then if you use COMSOL "Geometry Union" mode these will be "glued" together, even you will find only one common (internal) boundary belonging to each domain
Hope this is clear ;)
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi,
I think I understand you. To summarize: If importing an assembly of any CAD program, which consists of more than two parts, then it is necessary to select the command "Form Union" in COMSOL, because with selecting "assembly" the parts would "fly" around freely, if there is no BC on the respective part (I've tried such a simulation, this was the result). For example, if a bearing and a shaft are assembled, then it is necessary to select "form union", because then it's clear for COMSOL that the bearing can't move down or through the shaft. Is that correct?
Thank you very much in advance!!
I think I understand you. To summarize: If importing an assembly of any CAD program, which consists of more than two parts, then it is necessary to select the command "Form Union" in COMSOL, because with selecting "assembly" the parts would "fly" around freely, if there is no BC on the respective part (I've tried such a simulation, this was the result). For example, if a bearing and a shaft are assembled, then it is necessary to select "form union", because then it's clear for COMSOL that the bearing can't move down or through the shaft. Is that correct?
Thank you very much in advance!!
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
almost: in union mode there is only one COMMON boundary between the two domains, and every flux entering from one side exits on the opposite, including stress, heat, current, flow .....
but COMSOl has some special internal boundaries that allows to change this "thin resistive layer for heat and current etc.
In assembly mode there are two boundaries and it is up to the user to define the links between these two, COMSOL by default does not assume anything at all (apart it's nice and will make "pairs sets" out of those overlapping, making it easier for us to select the "pairs" to later add our physics on the boundaries
--
Good luck
Ivar
almost: in union mode there is only one COMMON boundary between the two domains, and every flux entering from one side exits on the opposite, including stress, heat, current, flow .....
but COMSOl has some special internal boundaries that allows to change this "thin resistive layer for heat and current etc.
In assembly mode there are two boundaries and it is up to the user to define the links between these two, COMSOL by default does not assume anything at all (apart it's nice and will make "pairs sets" out of those overlapping, making it easier for us to select the "pairs" to later add our physics on the boundaries
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello Ivar,
thank you for your answer. I will try a simulation like this, but that could take a few days.
Have a nice weekend!
thank you for your answer. I will try a simulation like this, but that could take a few days.
Have a nice weekend!
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello All,
I am trying to simulate frequency response of a MEMS cantilever coated with a piezoelectric material. I have been successful in calculating the natural frequencies. The job remaining is to be able to capture frequency response of the model under the application of a constant acceleration (say 10 m/s^2). What I do not understand is where should I apply the acceleration (i.e. which boundaries!).
I am attaching the model herewith. It will be kind of you to suggest changes in my model.
Thanks
I am trying to simulate frequency response of a MEMS cantilever coated with a piezoelectric material. I have been successful in calculating the natural frequencies. The job remaining is to be able to capture frequency response of the model under the application of a constant acceleration (say 10 m/s^2). What I do not understand is where should I apply the acceleration (i.e. which boundaries!).
I am attaching the model herewith. It will be kind of you to suggest changes in my model.
Thanks
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I'm neither not fully happy with the structural prescribed acceleration, velocity and displacement nodes, because I have issues with how to mix them, if I only want a described acceleration along z and fixed =prescribed dispalcement along x,y I have issues mixing them, as one overrides the other on a global basis, while I want only on a coordinate by coordinate basis.
For your case I would add a body load with a force of "acceleration*pzd.rho" and then do a frequency domain sweep but with a range of the type: 10^{range(1,0.05,4)} and plot in log scale the average displacement of your free tip.
If you accelerate you need also to consider w - w0 or just w
--
Good luck
Ivar
I'm neither not fully happy with the structural prescribed acceleration, velocity and displacement nodes, because I have issues with how to mix them, if I only want a described acceleration along z and fixed =prescribed dispalcement along x,y I have issues mixing them, as one overrides the other on a global basis, while I want only on a coordinate by coordinate basis.
For your case I would add a body load with a force of "acceleration*pzd.rho" and then do a frequency domain sweep but with a range of the type: 10^{range(1,0.05,4)} and plot in log scale the average displacement of your free tip.
If you accelerate you need also to consider w - w0 or just w
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello,
For some reason I am still not able to simulate the frequency response. I have a cantilever beam which has 3 layer (very thin though 80 nm) of 3 different materials. I have calculated the resonance frequency but the frequency response still does not work. I work in a frequency domain far away from the resonance frequency of the resonator. BUT STILL does not work. "Failed to find a solution for the initial parameter. The relative error (X) is greater than the relative tolerance Returned solution has not converged." It's frustrating!!!!!!! I have tried refining the mesh size, but it does not work either. I am planning to build an accelerometer based on this model.
I am attaching my model. Please, please suggest what should I do!! Also suggest any correction in the "PIEZOELECTRIC DEVICE" node, for obtaining voltage and charges.
Thank you,
Sankha
For some reason I am still not able to simulate the frequency response. I have a cantilever beam which has 3 layer (very thin though 80 nm) of 3 different materials. I have calculated the resonance frequency but the frequency response still does not work. I work in a frequency domain far away from the resonance frequency of the resonator. BUT STILL does not work. "Failed to find a solution for the initial parameter. The relative error (X) is greater than the relative tolerance Returned solution has not converged." It's frustrating!!!!!!! I have tried refining the mesh size, but it does not work either. I am planning to build an accelerometer based on this model.
I am attaching my model. Please, please suggest what should I do!! Also suggest any correction in the "PIEZOELECTRIC DEVICE" node, for obtaining voltage and charges.
Thank you,
Sankha
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
first a few suggestions to make it easier to work on your model
1) learn how to use the "Layers" in the geometry block tabs, you will build your models quicker
2) Add a second view and turn off the "Preserve aspect ratio" its easier to check your model
3) I didnt expect Au to be Piezoelectric, and as its really thin you could model it as a "thin" layer
4) you have really few elements in the thickness, I would not work without a minimum of 3 per layer
5) your electric potential is not connected
6) if you have done many changes, it's sometimes worth to rebuild the model from scratch as COMSOL sometimes get disoriented in it's internal settings
If I add a stationary study and connect your potential to the top surface it gives some results, but it fails if I choose the plane underneath the GND plane, but I cannot say I fully understand the three first layers
Sorry but I'm not sure what is wrong here, apart I would suggest to use a more up to date version
--
Good luck
Ivar
first a few suggestions to make it easier to work on your model
1) learn how to use the "Layers" in the geometry block tabs, you will build your models quicker
2) Add a second view and turn off the "Preserve aspect ratio" its easier to check your model
3) I didnt expect Au to be Piezoelectric, and as its really thin you could model it as a "thin" layer
4) you have really few elements in the thickness, I would not work without a minimum of 3 per layer
5) your electric potential is not connected
6) if you have done many changes, it's sometimes worth to rebuild the model from scratch as COMSOL sometimes get disoriented in it's internal settings
If I add a stationary study and connect your potential to the top surface it gives some results, but it fails if I choose the plane underneath the GND plane, but I cannot say I fully understand the three first layers
Sorry but I'm not sure what is wrong here, apart I would suggest to use a more up to date version
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Ivar,
First let me thank your for your quick and detailed response. I have few questions regarding your suggestions,
1) I am a beginner with Comsol and I do not know what should be the GND, floating potential, terminal settings. I find the manual insufficient to make users understand these features. They do not have any solved examples on the website. I have searched through this blog to find out worked out models shared by other users but unfortunately there are very few and what is worse is that they are in Comsol 4.2. I would request you to share with us some model on "Piezoelectric accelerometers". This would help many other users who are beginners.
2) I have ZnO as piezoelectric material. Gold is used as an electrode. I can model it as a thin layer. But I can not fild 'thin layer' primitive under the geometry node. Is this something available in the newer versions? I have 4.1.
3) I have tried using 3 elements along the thickness of every element. The natural frequency and the mode shape is the same, but the software is still incapable of performing a frequency sweep.
4) The bottommost and the topmost layers are polymer, so they are not conductors. Frankly, I do not know what electrical connections need to be used for obtaining the voltage and charge generated in the piezolayer during frequency sweep.
I do not want to give up.
-Sankha
First let me thank your for your quick and detailed response. I have few questions regarding your suggestions,
1) I am a beginner with Comsol and I do not know what should be the GND, floating potential, terminal settings. I find the manual insufficient to make users understand these features. They do not have any solved examples on the website. I have searched through this blog to find out worked out models shared by other users but unfortunately there are very few and what is worse is that they are in Comsol 4.2. I would request you to share with us some model on "Piezoelectric accelerometers". This would help many other users who are beginners.
2) I have ZnO as piezoelectric material. Gold is used as an electrode. I can model it as a thin layer. But I can not fild 'thin layer' primitive under the geometry node. Is this something available in the newer versions? I have 4.1.
3) I have tried using 3 elements along the thickness of every element. The natural frequency and the mode shape is the same, but the software is still incapable of performing a frequency sweep.
4) The bottommost and the topmost layers are polymer, so they are not conductors. Frankly, I do not know what electrical connections need to be used for obtaining the voltage and charge generated in the piezolayer during frequency sweep.
I do not want to give up.
-Sankha
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I agree with you that in the beginning it's slightly confusing. This I believe comes from the fact that very few users take the time to learn the COMSOL notations and manage to get it linked to our (diverse) way of doing math and physical math. I can also recommend the introduction and advanced courses by COMSOL, I learned a lot with these.
My main suggestion is: start simple, build your models step by step, understand the essentials, then go to the more complex.
For the versions certainly the to come 4.3 will be a big step towards better stability and many new functionality w.r.t your old 4.1
To come back to your model, you need to better understand the differences of the main physics nodes and sub nodes. Which dependent variables are needed where. Linear material, PZT material, ...
And w.r.t meshing, ensure you always have 2-3 elements in the thickness with layers, otherwise you cannot resolve the fields and gradients across the thickness, which means you are better off with a "thin layer physics" where the thickness is a parameter. This reduces the mesh size and DoFs too and often gives better results (than a poorly meshed membrane), not to say quicker solving
Normally one uses the PZD physics (pre-cooked by COMSOL) define the non-pzt material domains as linear elastic, and keep ONLY the PZT paterial in the default PZD anisotropic physics domain. Then one should use GND and a terminal on the appropriate boundaries for the electrodes (à PZT behaves mechanically different if the wires are connected or free). And do not forget that with multiple physics you need enough BC PER physics and dependent variables to get an unique solution of your PDEs
--
Good luck
Ivar
I agree with you that in the beginning it's slightly confusing. This I believe comes from the fact that very few users take the time to learn the COMSOL notations and manage to get it linked to our (diverse) way of doing math and physical math. I can also recommend the introduction and advanced courses by COMSOL, I learned a lot with these.
My main suggestion is: start simple, build your models step by step, understand the essentials, then go to the more complex.
For the versions certainly the to come 4.3 will be a big step towards better stability and many new functionality w.r.t your old 4.1
To come back to your model, you need to better understand the differences of the main physics nodes and sub nodes. Which dependent variables are needed where. Linear material, PZT material, ...
And w.r.t meshing, ensure you always have 2-3 elements in the thickness with layers, otherwise you cannot resolve the fields and gradients across the thickness, which means you are better off with a "thin layer physics" where the thickness is a parameter. This reduces the mesh size and DoFs too and often gives better results (than a poorly meshed membrane), not to say quicker solving
Normally one uses the PZD physics (pre-cooked by COMSOL) define the non-pzt material domains as linear elastic, and keep ONLY the PZT paterial in the default PZD anisotropic physics domain. Then one should use GND and a terminal on the appropriate boundaries for the electrodes (à PZT behaves mechanically different if the wires are connected or free). And do not forget that with multiple physics you need enough BC PER physics and dependent variables to get an unique solution of your PDEs
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello Ivar,
Thanks for your detailed answer. I have implemented your suggestions and when I introduce 3 layers across the thickness of every layer the frequency sweep works. To do this I had to reduce the mesh density, otherwise my compute would just stop working! But for the software to finish the job I have to reduce the relative tolerance in the stationary solver to 0.1 (usually its 10^-6). I do not if I am compromising with the accuracy of simulations by doing this. I should mention that, the mode shape and natural frequencies of the resonator is unaffected by this change! But, I do not know whether this affects displacement fields!
In your last post you mentioned that perhaps I am better off using thin layers instead of using blocks for thin films. By thin layer, do you refer to 'shell elements' ? Can you post a very simple example where in such a feature (e.g. shell elements) has been implemented. I tried to find this primitive under the geometry node, but could not locate!
Thank you for your help.
-Sankha
Thanks for your detailed answer. I have implemented your suggestions and when I introduce 3 layers across the thickness of every layer the frequency sweep works. To do this I had to reduce the mesh density, otherwise my compute would just stop working! But for the software to finish the job I have to reduce the relative tolerance in the stationary solver to 0.1 (usually its 10^-6). I do not if I am compromising with the accuracy of simulations by doing this. I should mention that, the mode shape and natural frequencies of the resonator is unaffected by this change! But, I do not know whether this affects displacement fields!
In your last post you mentioned that perhaps I am better off using thin layers instead of using blocks for thin films. By thin layer, do you refer to 'shell elements' ? Can you post a very simple example where in such a feature (e.g. shell elements) has been implemented. I tried to find this primitive under the geometry node, but could not locate!
Thank you for your help.
-Sankha
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
certainly if you reduce the relative tolerance your results will be less accurate, having enough RAM is mandatory for more complex models, unfortunately.
For me the thin film was i.e. to reduce a conductor layer to a surface with a perfect thin film condctor or other type of surface physics, not really shells. I would wait for the new release 4.3 to use a mix of shell and solids, to much homework to correctly knit these together in 4.2
--
Good luck
Ivar
certainly if you reduce the relative tolerance your results will be less accurate, having enough RAM is mandatory for more complex models, unfortunately.
For me the thin film was i.e. to reduce a conductor layer to a surface with a perfect thin film condctor or other type of surface physics, not really shells. I would wait for the new release 4.3 to use a mix of shell and solids, to much homework to correctly knit these together in 4.2
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello Ivar,
I have two questions.
1) My computer has 6 GB RAM. When I try to run models which have more than 10000 elements my computer just stops working. I shut off every other program so that COMSOL gets all the processor and RAM. Still this thing happens! Is it possible to allocate memory for COMSOL, so that even if it needs extra memory my computer will still work and COMSOL will work too, but it will take longer to complete the simulation?
2) I understood what you mean by "Thin film". My question is, is this a new primitive? Because in 4.1, I could not find it!
Sankha
I have two questions.
1) My computer has 6 GB RAM. When I try to run models which have more than 10000 elements my computer just stops working. I shut off every other program so that COMSOL gets all the processor and RAM. Still this thing happens! Is it possible to allocate memory for COMSOL, so that even if it needs extra memory my computer will still work and COMSOL will work too, but it will take longer to complete the simulation?
2) I understood what you mean by "Thin film". My question is, is this a new primitive? Because in 4.1, I could not find it!
Sankha
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
if you do not see it it must be a newer feature, COMSOL has been updating heavily the number of nodes available for each release
ow I'm astonished that with 6Gb of RAM you do not manage to run quite complex models. Sure you have a 64 bit OS that really uses all that RAM, or it might be again an improvement with the later versions, COMSOL has also been improving the RAM use per solver
--
Good luck
Ivar
if you do not see it it must be a newer feature, COMSOL has been updating heavily the number of nodes available for each release
ow I'm astonished that with 6Gb of RAM you do not manage to run quite complex models. Sure you have a 64 bit OS that really uses all that RAM, or it might be again an improvement with the later versions, COMSOL has also been improving the RAM use per solver
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi,
I need to apply based excitation in harmonic motion at the fixed end of the beam. may I know how can I accomplish this?
Thanks
I need to apply based excitation in harmonic motion at the fixed end of the beam. may I know how can I accomplish this?
Thanks
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
you have the prescribed acceleration or the "big mass" approach, you set your device on a huge rigid mass and apply a body load acceleration on this mass (and the full model).
You can also apply a body load, but then one place your object is fixed and is not moving, this is not really a "base acceleration" case
--
Good luck
Ivar
you have the prescribed acceleration or the "big mass" approach, you set your device on a huge rigid mass and apply a body load acceleration on this mass (and the full model).
You can also apply a body load, but then one place your object is fixed and is not moving, this is not really a "base acceleration" case
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi, I am doing the simulation with the cantilever coated by piezo material. When I do the frequency sweep, the cantilever tip displacement and output voltage reach its highest at the resonant frequency. My question is why there is a voltage leap from the negative to positive.
Thank you!
Thank you!
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
it has probably to do with the phase lag of your signal which inverses, before the resonance you are driving it, after its the resonance that is ahead of your excitation
Difficult to say more without running a full case
--
Good luck
Ivar
it has probably to do with the phase lag of your signal which inverses, before the resonance you are driving it, after its the resonance that is ahead of your excitation
Difficult to say more without running a full case
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
It is probably a phase issue as Ivar mentioned. Even without piezo effects, before resonance phase angle between force and displacement is 0 and after resonance it is 180 degrees (there is a gradual transition when there is damping).
Nagi Elabbasi
Veryst Engineering
Nagi Elabbasi
Veryst Engineering
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
indeed for force versus displacement, but if I got it right here it was V out versus force ?
--
Good luck
Ivar
indeed for force versus displacement, but if I got it right here it was V out versus force ?
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Is it because Force and the induced Voltage are always in the same phase?
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
if you have a PZT beam, fixed at one end and loaded by a varying force load at the other end, then the force will introduce a deformation of the beam, hence a stress build-up. This stress buildup will generate charges that will populate the electrodes hence induce an electric field across the PZT, this field will vary if the electrodes are free, or grounded (short) or hooked up to some other intermediate or complex impedance. Now the electric field will act on the stiffness tensor and change the deflection hence the response and off we are with a chicken an the egg story: who came first ?
So I would say your foce induces a flexing whcih nitroduces a stress change with induces a potential. But you can loop the other way too ;)
Normally you can simulate the eigenfrequency change if your electrodes are shorted or pen loop, the difference in frequency gives yout the elecric to mechani coupling factor "k"
As you have losses in the PZT and perhaps in the driving circuit of your PZT you will get complex responses so you mst study the behaviour with Bode plots for the amplitude "abs(...)" and the phase "atan2(imag(...),real(...))"
--
Good luck
Ivar
if you have a PZT beam, fixed at one end and loaded by a varying force load at the other end, then the force will introduce a deformation of the beam, hence a stress build-up. This stress buildup will generate charges that will populate the electrodes hence induce an electric field across the PZT, this field will vary if the electrodes are free, or grounded (short) or hooked up to some other intermediate or complex impedance. Now the electric field will act on the stiffness tensor and change the deflection hence the response and off we are with a chicken an the egg story: who came first ?
So I would say your foce induces a flexing whcih nitroduces a stress change with induces a potential. But you can loop the other way too ;)
Normally you can simulate the eigenfrequency change if your electrodes are shorted or pen loop, the difference in frequency gives yout the elecric to mechani coupling factor "k"
As you have losses in the PZT and perhaps in the driving circuit of your PZT you will get complex responses so you mst study the behaviour with Bode plots for the amplitude "abs(...)" and the phase "atan2(imag(...),real(...))"
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi,
I've tried applying 'prescribed acceleration' to the fixed end of the beam and managed to get the 'voltage vs freq' plot. However, when i do analysis of the beam's deformation at every single frequency, I've found out that the fixed end of the beam moves. It stays fixed only at the natural frequencies. I believe this might be due to 'fixed constraint' is overridden by 'prescribed acceleration'. If 'fixed constraint' overrides 'prescribed acceleration', there will be no output voltage generated.
If I changed the 'prescribed acceleration' to 'body load' of "pzd.rho*acceleration", the fixed end stays fixed throughout the simulation. However, I noticed that the list of eigenfrequencies changed and I'm not sure why.
If I want to plot the voltage distribution at every point accross the length of the beam, should i choose "electric field-Z component"?
Thanks
I've tried applying 'prescribed acceleration' to the fixed end of the beam and managed to get the 'voltage vs freq' plot. However, when i do analysis of the beam's deformation at every single frequency, I've found out that the fixed end of the beam moves. It stays fixed only at the natural frequencies. I believe this might be due to 'fixed constraint' is overridden by 'prescribed acceleration'. If 'fixed constraint' overrides 'prescribed acceleration', there will be no output voltage generated.
If I changed the 'prescribed acceleration' to 'body load' of "pzd.rho*acceleration", the fixed end stays fixed throughout the simulation. However, I noticed that the list of eigenfrequencies changed and I'm not sure why.
If I want to plot the voltage distribution at every point accross the length of the beam, should i choose "electric field-Z component"?
Thanks
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
indeed if you apply a prscribed acceleration, your object CANNOT be fixed these are antogonists. What you can do is to apply a body load of the type "material.rho*my_acceleration" and keep the fixed section "fixed".
I'm neither not fully happy as today I have not found a clean way to apply a shaker type PSD on a model, in a simple way. there are several threads about this on the Forum, try a search
--
Good luck
Ivar
indeed if you apply a prscribed acceleration, your object CANNOT be fixed these are antogonists. What you can do is to apply a body load of the type "material.rho*my_acceleration" and keep the fixed section "fixed".
I'm neither not fully happy as today I have not found a clean way to apply a shaker type PSD on a model, in a simple way. there are several threads about this on the Forum, try a search
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Ivar,
From the attached figure, does my model represent a beam subjected to base excitation? (the beam is attached to a big rigid mass). I've applied body load before to the rigid mass but the output voltage generated is maximum at the fifth eigenfreq. If I changed it to prescribed acceleration and applied it on top of the rigid mass, I can see that the maximum value of voltage is at the first eigenfreq (which is theoretically correct according to my understanding)
thanks
From the attached figure, does my model represent a beam subjected to base excitation? (the beam is attached to a big rigid mass). I've applied body load before to the rigid mass but the output voltage generated is maximum at the fifth eigenfreq. If I changed it to prescribed acceleration and applied it on top of the rigid mass, I can see that the maximum value of voltage is at the first eigenfreq (which is theoretically correct according to my understanding)
thanks
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
However, by applying prescribed acceleration, the value of voltage is hundreds volts, which is I think is not correct
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
from you image, you should not use fixed and acceleration simulatneously, but you must use two roller conditions on two opposite sides of your sqare mass at right angle to the acceleration direction. Be sure you large mass is "large" compared to the beam, and then get the correct estimate of the true load on the beam
100V is not necessarily that much, you can get a sparck (>1kV) easily with a stressed PZT, but this also depends strongly on the impedance you connect up on your PZT
--
Good luck
Ivar
from you image, you should not use fixed and acceleration simulatneously, but you must use two roller conditions on two opposite sides of your sqare mass at right angle to the acceleration direction. Be sure you large mass is "large" compared to the beam, and then get the correct estimate of the true load on the beam
100V is not necessarily that much, you can get a sparck (>1kV) easily with a stressed PZT, but this also depends strongly on the impedance you connect up on your PZT
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I think I'd better stick with your initial suggestion that is to apply body load. I use steel as the large mass due to its stiffness and aluminum beam. I apply fixed constraint to the faces of the mass except for the one that is attached to the beam.
I'm currently using one physics only that is piezoelectric device. I apply floating potential to the top of the PZT and ground at the bottom of the layer and this is how I extract the voltage generated Do I need to add another physics(i.e electrical circuit) for the impedance?
Thanks
I think I'd better stick with your initial suggestion that is to apply body load. I use steel as the large mass due to its stiffness and aluminum beam. I apply fixed constraint to the faces of the mass except for the one that is attached to the beam.
I'm currently using one physics only that is piezoelectric device. I apply floating potential to the top of the PZT and ground at the bottom of the layer and this is how I extract the voltage generated Do I need to add another physics(i.e electrical circuit) for the impedance?
Thanks
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
indeed fixing your block and applying a body load as an acceleration is o good way, in a frequency domain sweep you can get the frequency response too of your system. If you leave a floating potential its as if you have an open circuit, you voltage will be given by the charge build-up and the PZT beam capacity. If you add a CIR physics with an electric impedance of some kind, i.e. representing the entry impedance of your system, then you will see the response and voltage build up of your device in loaded conditions. One way to optimise the energy transfer is to play with the bandpass of your load impedance and the response of the beam
--
Good luck
Ivar
indeed fixing your block and applying a body load as an acceleration is o good way, in a frequency domain sweep you can get the frequency response too of your system. If you leave a floating potential its as if you have an open circuit, you voltage will be given by the charge build-up and the PZT beam capacity. If you add a CIR physics with an electric impedance of some kind, i.e. representing the entry impedance of your system, then you will see the response and voltage build up of your device in loaded conditions. One way to optimise the energy transfer is to play with the bandpass of your load impedance and the response of the beam
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
Thanks a lot. you've been really helpful
Thanks a lot. you've been really helpful
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi everybody.
I have with great interest read this thread.
I would like to simulate the steady-state response of a vertically base-excited cantilever beam.
The driving could e.g. be A*cos(Omega*tau) where A is the amplitude, Omega is the frequency, and tau is time.
(no PZT or multilayer or anything "fancy" - just an isotropic beam of steel).
I can see from this thread, that several challenges occur when modeling a vertically base-excited cantilever beam. I am completely new to Comsol, and have no experience with it what so ever. It has, in this thread, been proposed to add a comparably large rigid body mass. It seems inappropiate in my case - I would definitely prefer only to consider a cantilever which is driven by an external load (i.e. shaker) and that the resulting values (eigenfrequencies, absolute amplitude etc.) are directly comparable with experimental results.
The modeling itself should, I guess, be a very simple task for an experienced user and require a minimum of time. Could anybody please provide my with a working example?
It will of course require subsequent work from me, but I need to start from "steady ground" :)
Help is highly appreciated!
Kind regards,
Stefan
I have with great interest read this thread.
I would like to simulate the steady-state response of a vertically base-excited cantilever beam.
The driving could e.g. be A*cos(Omega*tau) where A is the amplitude, Omega is the frequency, and tau is time.
(no PZT or multilayer or anything "fancy" - just an isotropic beam of steel).
I can see from this thread, that several challenges occur when modeling a vertically base-excited cantilever beam. I am completely new to Comsol, and have no experience with it what so ever. It has, in this thread, been proposed to add a comparably large rigid body mass. It seems inappropiate in my case - I would definitely prefer only to consider a cantilever which is driven by an external load (i.e. shaker) and that the resulting values (eigenfrequencies, absolute amplitude etc.) are directly comparable with experimental results.
The modeling itself should, I guess, be a very simple task for an experienced user and require a minimum of time. Could anybody please provide my with a working example?
It will of course require subsequent work from me, but I need to start from "steady ground" :)
Help is highly appreciated!
Kind regards,
Stefan
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
In any case you should not talk about comparing eigenfrequencies, as these do not depend on external forces, only on the material, geometry shapes
And amplitudes depends on damping, which is a delicate issue, often ignored, but essential for any amplitude evaluation, you must add thedamping as specific material property nodes, the only thing is to know what to use as values !
Finally use rather the harmonic development and not the time series, as ou have then all the initial transient behaviour to consider
--
Good luck
Ivar
In any case you should not talk about comparing eigenfrequencies, as these do not depend on external forces, only on the material, geometry shapes
And amplitudes depends on damping, which is a delicate issue, often ignored, but essential for any amplitude evaluation, you must add thedamping as specific material property nodes, the only thing is to know what to use as values !
Finally use rather the harmonic development and not the time series, as ou have then all the initial transient behaviour to consider
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
In any case you should not talk about comparing eigenfrequencies, as these do not depend on external forces, only on the material, geometry shapes
And amplitudes depends on damping, which is a delicate issue, often ignored, but essential for any amplitude evaluation, you must add thedamping as specific material property nodes, the only thing is to know what to use as values !
Finally use rather the harmonic development and not the time series, as ou have then all the initial transient behaviour to consider
--
Good luck
Ivar
Hi Ivar,
Thank you for the fast response.
Comparison of eigenfrequencies is regards to existing lab results and, as you say, of course not dependent on external driving.
Obviously you are (also) right about damping - I only consider real physical systems why damping is larger than zero.
I have already obtained experimental damping coefficients for the system at hand - I will look at the implementation of damping coefficients in Comsol as you suggested soon...
Furthermore, I do not understand what you mean by "use rather the harmonic development and not the time series". I have already developed analytical approximate expressions for the steady-state response using perturbation analysis. For these, and relating numerical solution given by a Runge-Kutta solver, I have an estimate for the time period after which the transients are negligible. Thus, I can simulate the system with transients - but as for now, I do not know how to impliment/be able to analyse a time series in Comsol?
Most importantly, I would like you to elaborate on "use rather the harmonic development and not the time series" if possible - and preferably in relation to Comsol.
Kind regards,
Stefan
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
Check the doc about frequency domain solving, and look at the equations, you will understand, it solves far quicker in constant regime sinus type excitation
--
Good luck
Ivar
Check the doc about frequency domain solving, and look at the equations, you will understand, it solves far quicker in constant regime sinus type excitation
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi,
I've applied body load to represent base excitation, and assigned "added mass" BC at the free end of the cantilever ( to represent tip mass). Howver, it shows that the voltage output at the eigenfreq keeps decreasing as the "added mass" increases. I believe by adding the tip mass, the voltage will be increased.
Thanks
I've applied body load to represent base excitation, and assigned "added mass" BC at the free end of the cantilever ( to represent tip mass). Howver, it shows that the voltage output at the eigenfreq keeps decreasing as the "added mass" increases. I believe by adding the tip mass, the voltage will be increased.
Thanks
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
if you add an "added mass then you must also add a boundary force, as the body load applies ONLY forces to the DOMAIN, not to the added mass that is a separate "fictuous " entitiy do not forget that ;)
--
Good luck
Ivar
if you add an "added mass then you must also add a boundary force, as the body load applies ONLY forces to the DOMAIN, not to the added mass that is a separate "fictuous " entitiy do not forget that ;)
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
The added mass reduces the natural frequency so the voltage may be dropping because the frequency you specified in the frequency domain analysis is no longer close to the beam’s natural frequency.
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi,
thanks for the reply. in the frequency analysis, I've specified a range of frequency, the eigenfrequency lies within that range.
Thanks.
thanks for the reply. in the frequency analysis, I've specified a range of frequency, the eigenfrequency lies within that range.
Thanks.
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Ok, one more thing to check. Conceptually, if you apply a certain body load and you change the structure by adding mass the deformations should in general be lower and also the voltage.
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hmm,may I know why? Because from what I understand, Adding tip mass to the structure increases the strain,which eventually increases the deformation. Body load is assigned on the "large" mass attached to the beam and added mass is assigned at the other end of the beam,together with boudary load
Thanks
Thanks
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello all,
This is a very interesting discussion so far and I am trying to make a vibration model along similar lines.
I work with a similar excitation, but with a metal beam fixed at both ends (with compliant mounts) and a shaker applies vibration at the center of the beam with a static preload to hold it in place. Experimentally, I noticed that the resonances observed are of the entire system (shaker + beam) and not the beam alone. The frequencies I use are in several kilohertz where the shaker dimensions do matter.
So, in most of the discussions above where the shaker was attached to the beam, isn't it an issue to consider? Is there a way to include this non-linearity in the comsol model?
This is a very interesting discussion so far and I am trying to make a vibration model along similar lines.
I work with a similar excitation, but with a metal beam fixed at both ends (with compliant mounts) and a shaker applies vibration at the center of the beam with a static preload to hold it in place. Experimentally, I noticed that the resonances observed are of the entire system (shaker + beam) and not the beam alone. The frequencies I use are in several kilohertz where the shaker dimensions do matter.
So, in most of the discussions above where the shaker was attached to the beam, isn't it an issue to consider? Is there a way to include this non-linearity in the comsol model?
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
in all generality the "thumb" rules:
2*pi*freq = sqrt(k_stiff / mass) = sqrt(k_rot / Inertia),
and for a beam under gravity load, for the first mode gies about the max deflection
2*pi*freq = sqrt(g_const / Dz_deflection)
I a rather good approximation. So if you add a mas via your attachment to a shaker, it is clesr that you will influence the mode to. That is why one often attach the FULL system to the shaker, or we shake the base and not the directly part of structure itself under test. At least not with any mass of significance w.r.t. the object mass
--
Good luck
Ivar
in all generality the "thumb" rules:
2*pi*freq = sqrt(k_stiff / mass) = sqrt(k_rot / Inertia),
and for a beam under gravity load, for the first mode gies about the max deflection
2*pi*freq = sqrt(g_const / Dz_deflection)
I a rather good approximation. So if you add a mas via your attachment to a shaker, it is clesr that you will influence the mode to. That is why one often attach the FULL system to the shaker, or we shake the base and not the directly part of structure itself under test. At least not with any mass of significance w.r.t. the object mass
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi all
I am working in such a thing you talking about please how can I make a vibrating sphere inside water can anyone help me for that
thanks,
MSH
I am working in such a thing you talking about please how can I make a vibrating sphere inside water can anyone help me for that
thanks,
MSH
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi all
I am working in such a thing you talking about please how can I make a vibrating sphere inside water can anyone help me for that
thanks,
MSH
I am working in such a thing you talking about please how can I make a vibrating sphere inside water can anyone help me for that
thanks,
MSH
Please login with a confirmed email address before reporting spam
Posted:
10 years ago
Hi Ivar,
Firstly (I know that this post is now a bit old...), thank you for your precise answers. I read the discussion carefully but at a given point I'm no more able to understand your explanations...
I have a DUT on shaker measurement, in order to know the physical property of this material (Young's, Poissons's, loss factor), I would like to match to simulation with the measurement. On one face of my solid I assign a prescribed acceleration (around 5 m/s^2), on the other side a body load (comes from added known mass in the real measurement) and add the gravity to the solid. The excitation is 10^{range(0,0.1,3)} my question is for the post-processing part.
I want to perform the transfer function of the acceleration from the topmost part of the solid (accelerometer placed on the top of the added mass in the real measurement) on the acceleration from the base of my solid (an other acceleration from an accelerometer placed on the base of the shaker).
How can I extract the average acceleration of the topmost surface, the average acceleration of the base surface and make the ratio?
I know that my question is really basic, I'm far from an expert in COMSOL but this discussion is really useful!
Thank you in advance, Luis.
Firstly (I know that this post is now a bit old...), thank you for your precise answers. I read the discussion carefully but at a given point I'm no more able to understand your explanations...
I have a DUT on shaker measurement, in order to know the physical property of this material (Young's, Poissons's, loss factor), I would like to match to simulation with the measurement. On one face of my solid I assign a prescribed acceleration (around 5 m/s^2), on the other side a body load (comes from added known mass in the real measurement) and add the gravity to the solid. The excitation is 10^{range(0,0.1,3)} my question is for the post-processing part.
I want to perform the transfer function of the acceleration from the topmost part of the solid (accelerometer placed on the top of the added mass in the real measurement) on the acceleration from the base of my solid (an other acceleration from an accelerometer placed on the base of the shaker).
How can I extract the average acceleration of the topmost surface, the average acceleration of the base surface and make the ratio?
I know that my question is really basic, I'm far from an expert in COMSOL but this discussion is really useful!
Thank you in advance, Luis.