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 The information provided may be out of date.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.

2D vs 3D Frequency Response

Please login with a confirmed email address before reporting spam

Hello,
I am trying to compare the frequency response (displacement amplitude [y-axis] vs frequency [x-axis]) of a simple beam both in 2D and 3D to compare the differences in the responses.

The resonant frequency peaks align between the 2D and 3D model; however, the amplitudes of the peaks for the 3D model are 10 times higher than the 2D model.

How can I scale the 2D model to have not only the peaks align in frequency but in amplitude as well; in other words, how can I make the 2D model response match the 3D model response?

Thank you!


13 Replies Last Post Jun 12, 2012, 4:36 p.m. EDT
Ivar KJELBERG COMSOL Multiphysics(r) fan, retired, former "Senior Expert" at CSEM SA (CH)

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Apr 24, 2012, 7:48 a.m. EDT
Hi

how do you treat the damping ? and are you sure your frequency stepping are the same between 2D and 3D ?

--
Good luck
Ivar
Hi how do you treat the damping ? and are you sure your frequency stepping are the same between 2D and 3D ? -- Good luck Ivar

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Apr 24, 2012, 5:42 p.m. EDT
I havent incorporated any damping into either model (2D or 3D), would I need to in order to match the amplitude of the peaks?

I have made sure they have the same starting frequency, step, and ending frequency during the frequency sweep.

Thanks, Ivar!
I havent incorporated any damping into either model (2D or 3D), would I need to in order to match the amplitude of the peaks? I have made sure they have the same starting frequency, step, and ending frequency during the frequency sweep. Thanks, Ivar!

Ivar KJELBERG COMSOL Multiphysics(r) fan, retired, former "Senior Expert" at CSEM SA (CH)

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Apr 25, 2012, 9:23 a.m. EDT
Hi

the resonance peak height to Full Width at Half Maximum (FWHM) is the Q factor or half the damping value (check it out on Wiki)

en.wikipedia.org/wiki/Q_factor

If you have no damping (apprt from some numerical effects that might come from the solving stabilisation process you will not get any finite peak values

--
Good luck
Ivar
Hi the resonance peak height to Full Width at Half Maximum (FWHM) is the Q factor or half the damping value (check it out on Wiki) http://en.wikipedia.org/wiki/Q_factor If you have no damping (apprt from some numerical effects that might come from the solving stabilisation process you will not get any finite peak values -- Good luck Ivar

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Jun 8, 2012, 2:38 a.m. EDT
I have tried modifying the damping, but regardless of what I enter, the amplitudes still dont match up; so I've attached the models for clarification. Any help is appreciated!
I have tried modifying the damping, but regardless of what I enter, the amplitudes still dont match up; so I've attached the models for clarification. Any help is appreciated!

Ivar KJELBERG COMSOL Multiphysics(r) fan, retired, former "Senior Expert" at CSEM SA (CH)

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Jun 8, 2012, 3:29 a.m. EDT
Hi

if the model is too big, clear the solutiomn, mesh and reset the model then save and upload, it should pass ;)

--
Good luck
Ivar
Hi if the model is too big, clear the solutiomn, mesh and reset the model then save and upload, it should pass ;) -- Good luck Ivar

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Jun 8, 2012, 12:54 p.m. EDT
Ivar, you've been a life-saver! I was going to re-make the models without the solutions but that made it much easier! Here they are.

They simply have a point load in the center of each. Whenever I plot the frequency response (just to be clear--frequency, x-axis, and amplitude, y-axis) the resonant frequency peaks match up fairly well in terms of frequency but again not in amplitude.

I've added damping to the 3D model, but not the 2D model--and i've experimented with several variations (adding damping to both, just the 2D and no damping on either model) and still am unable to get the amplitudes to match.

Thanks again for your help!
Ivar, you've been a life-saver! I was going to re-make the models without the solutions but that made it much easier! Here they are. They simply have a point load in the center of each. Whenever I plot the frequency response (just to be clear--frequency, x-axis, and amplitude, y-axis) the resonant frequency peaks match up fairly well in terms of frequency but again not in amplitude. I've added damping to the 3D model, but not the 2D model--and i've experimented with several variations (adding damping to both, just the 2D and no damping on either model) and still am unable to get the amplitudes to match. Thanks again for your help!


Ivar KJELBERG COMSOL Multiphysics(r) fan, retired, former "Senior Expert" at CSEM SA (CH)

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Jun 8, 2012, 3:13 p.m. EDT
Hi

My comments are the following:
1) do not use point loads as these are singularities and give large errors around the point of application hence tend to perturbate the solver sequence and convergence estimator. It's easier to cut the beam in two in the length and apply a boundary load in both 2D and 3D along this cut line/surface
2) if you have only 1 element in the thickness, you could as well use a line/surface and beam or shell elements, so if you want to stay in "solid" ensure you have enough elements across the the beam thickness (I would say > 3). I mostly cut my biam geoemtry into 2 along the neutral line and then impose 2 mesh elements as minimum resolution per domain

I aso try to avoid free free models, as you can get other errors due to the free motion and rotation you allow. It's better to constrain your device some way to limits its free inertial motion

finally a material damping of 0.004 is rather low (realistic still) but it will hardly be observed, try 2-5%, then you should se your Bode plots as second order roll-off elements

--
Good luck
Ivar
Hi My comments are the following: 1) do not use point loads as these are singularities and give large errors around the point of application hence tend to perturbate the solver sequence and convergence estimator. It's easier to cut the beam in two in the length and apply a boundary load in both 2D and 3D along this cut line/surface 2) if you have only 1 element in the thickness, you could as well use a line/surface and beam or shell elements, so if you want to stay in "solid" ensure you have enough elements across the the beam thickness (I would say > 3). I mostly cut my biam geoemtry into 2 along the neutral line and then impose 2 mesh elements as minimum resolution per domain I aso try to avoid free free models, as you can get other errors due to the free motion and rotation you allow. It's better to constrain your device some way to limits its free inertial motion finally a material damping of 0.004 is rather low (realistic still) but it will hardly be observed, try 2-5%, then you should se your Bode plots as second order roll-off elements -- Good luck Ivar

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Jun 9, 2012, 12:27 a.m. EDT
Thanks for all your help, Ivar. I will try it out and see how it goes!
Thanks for all your help, Ivar. I will try it out and see how it goes!

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Jun 10, 2012, 6:17 p.m. EDT
I am not quite sure how to make the cuts in the models. Is there an easy way to do this? I am trying to essentially estimate a vibrational load that sweeps through the various frequencies, so I was using a point load previously
I am not quite sure how to make the cuts in the models. Is there an easy way to do this? I am trying to essentially estimate a vibrational load that sweeps through the various frequencies, so I was using a point load previously

Ivar KJELBERG COMSOL Multiphysics(r) fan, retired, former "Senior Expert" at CSEM SA (CH)

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Jun 11, 2012, 12:48 a.m. EDT
Hi

check the layer feature under the advanced tab note that you cannot have different layer thicknesses in different directions, all directions selected get the same layer thickness. to cut your beam in 1 along the length , append 2 1/2 rectangles, or duplicate your first one by a copy

--
Good luck
Ivar
Hi check the layer feature under the advanced tab note that you cannot have different layer thicknesses in different directions, all directions selected get the same layer thickness. to cut your beam in 1 along the length , append 2 1/2 rectangles, or duplicate your first one by a copy -- Good luck Ivar

Nagi Elabbasi Facebook Reality Labs

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Jun 11, 2012, 8:56 a.m. EDT
The main reason for the difference in results is the difference between the beam widths in 2D and 3D. For the 2D the out-of-plane width is 1.0 by default. If you change it to 0.0254 as in the 3D model the results will be closer. You should also change the 2D beam to plane stress instead of plane strain which is a closer approximation of your 3D beam. The damping, mesh density and singularity of point load are other reasons for the difference in results.

Nagi Elabbasi
Veryst Engineering
The main reason for the difference in results is the difference between the beam widths in 2D and 3D. For the 2D the out-of-plane width is 1.0 by default. If you change it to 0.0254 as in the 3D model the results will be closer. You should also change the 2D beam to plane stress instead of plane strain which is a closer approximation of your 3D beam. The damping, mesh density and singularity of point load are other reasons for the difference in results. Nagi Elabbasi Veryst Engineering

Ivar KJELBERG COMSOL Multiphysics(r) fan, retired, former "Senior Expert" at CSEM SA (CH)

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Jun 11, 2012, 3:17 p.m. EDT
Hi Nagi

Good point, I'm getting so used to COMSOL now that I start to automatically think "per meter" in 2D, (or per m^2 in 1D) but to get absolute values one should not forget to multiply by the TRUE depth ;)

--
Good luck
Ivar
Hi Nagi Good point, I'm getting so used to COMSOL now that I start to automatically think "per meter" in 2D, (or per m^2 in 1D) but to get absolute values one should not forget to multiply by the TRUE depth ;) -- Good luck Ivar

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Jun 12, 2012, 4:36 p.m. EDT
Thank you for your help guys! Nagi, that definitely helped to change the out-of plane width; peaks are very close--working on matching the models now using the previous suggestions. You guys are life-savers!

Thank you for your help guys! Nagi, that definitely helped to change the out-of plane width; peaks are very close--working on matching the models now using the previous suggestions. You guys are life-savers!

Note that while COMSOL employees may participate in the discussion forum, COMSOL® software users who are on-subscription should submit their questions via the Support Center for a more comprehensive response from the Technical Support team.