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.

free-free beam natural frequency

hallo friend
I first conducted a simulation to calculate the natural frequency of the first mode of a beam of 4m length, 40cm height and 70cm in width. the theoretical calculation gives me f1 = 128 Hz but Comsol gives me 0 Hz
do you have an idea about the problem?

thank you in advance

6 Replies Last Post Sep 29, 2011, 7:39 AM EDT
Posted: 8 years ago Dec 14, 2009, 9:29 AM EST
Hi

a "0" for a structural mode means a (or several) DoF that is not blocked, if you have 6 of them at about "0" Hz, its typically that you are looking at the first 6 (x,y,z, Rx,Ry,Rz) free-free modes, and your 128 Hz will show up as mode no 7 (increase the number of mods in the solve tab to see this)

This was assuming a 3D model, if you are in 2D its 3 modes x,y,Rz that would be at "0".

If you have only 1 or 2 modes at "0" Hz then typically you have not constrained enough DoF to block one face.

I did a quick check in 3D default values (steel) I get 125.65, 206.30, Hz for mode "7 & 8". But if I fixee one of the small faces I get 20.49, 35.17 and 123.2, 161.72 Hz for the first 4 modes respectively in Rz and Ry . First, is the meshing fine enough ? by doing an overkill going from 1'794 to 273'873 Dof the frequencies changes to respectively 125.39 and 206.14 in free-free and 20.41, 35.05, 122.26, 156.20 Hz in clamped- free mode, so default values are about OK

Furthermore, one must be carefull to observe the mode shapes, in free-free and in clamped-free they differ, the two first in clamped-free cannot show up in free-free because of symemtry reasons. In fact a free free mode beam behaves as a symmetric L/2 length beam hence there is a factor 4 in frequency difference for this mode between clamped-free and free-free for this specific mode, try to set a symmetry boundary codition on the small edge instead of fixed, and compare to the free-free values.

Analytically in a simplified way the first eigenmodes are typically for clamped-free f=gamma/2/pi*sqrt(K/M) with k=3*E*I/L^3 with L the beam length, E the young modulus, M the total mass (mostly expressed as m*L=M the mass per length or M=rho*h*b*L with rho the density) I=h*b^3/12 the inertia with h width, b thickness (in the normal direction of rotation) amd gamma is a (mass) partcipation factor depending on the way the beam is clamped (sqrt(gamma)=(1.875, 4.694, 7.855) for the first clamped-free modes, while sqrt(gamma)=(4.730, 7.8532) for the first free-free modes (note: these are for the same given flexure mode, while the 2 cases from COMSOL are the first modes in two perpendicuzlar directions). This gives typically for E=200[GPa] and rho= 7850[kg/m^3] the value of steel: f1 = gamma*b/4/pi/L^2*sqrt(E/rho) = 5.8[Hz]*1.875^2 = 20.38[Hz] in clamped-free and 5.8[Hz]*4.73^2=129.71[Hz] in free-free

All above in simplified non-shear theory, ignoring "nu" which is an acceptable first approcimation.

Furthermore as the heigt to width ratio is only 0.7/0.4=1.75 we should see a mode difference of this ratio (sqrt(h*b^3/b*h^3)=b/h = 1.75), indeed 35.17/20.49=1.716 and 206.3/125.65=1.64, good enough

Well as you have not precised your boundary conditions, neither the material, I might be wrong with some of the numerical values, but the rest I believe is more or less OK, no? There is quite a lot to say about mode shapes...

For the theor, have a look at "Formulas for Natural Frequency and mode shape" R.D. Blevin, Kruger, 1979, reprint 2001, ISBN 1-57524-184-6

Hope this helps
Ivar
Hi a "0" for a structural mode means a (or several) DoF that is not blocked, if you have 6 of them at about "0" Hz, its typically that you are looking at the first 6 (x,y,z, Rx,Ry,Rz) free-free modes, and your 128 Hz will show up as mode no 7 (increase the number of mods in the solve tab to see this) This was assuming a 3D model, if you are in 2D its 3 modes x,y,Rz that would be at "0". If you have only 1 or 2 modes at "0" Hz then typically you have not constrained enough DoF to block one face. I did a quick check in 3D default values (steel) I get 125.65, 206.30, Hz for mode "7 & 8". But if I fixee one of the small faces I get 20.49, 35.17 and 123.2, 161.72 Hz for the first 4 modes respectively in Rz and Ry . First, is the meshing fine enough ? by doing an overkill going from 1'794 to 273'873 Dof the frequencies changes to respectively 125.39 and 206.14 in free-free and 20.41, 35.05, 122.26, 156.20 Hz in clamped- free mode, so default values are about OK Furthermore, one must be carefull to observe the mode shapes, in free-free and in clamped-free they differ, the two first in clamped-free cannot show up in free-free because of symemtry reasons. In fact a free free mode beam behaves as a symmetric L/2 length beam hence there is a factor 4 in frequency difference for this mode between clamped-free and free-free for this specific mode, try to set a symmetry boundary codition on the small edge instead of fixed, and compare to the free-free values. Analytically in a simplified way the first eigenmodes are typically for clamped-free f=gamma/2/pi*sqrt(K/M) with k=3*E*I/L^3 with L the beam length, E the young modulus, M the total mass (mostly expressed as m*L=M the mass per length or M=rho*h*b*L with rho the density) I=h*b^3/12 the inertia with h width, b thickness (in the normal direction of rotation) amd gamma is a (mass) partcipation factor depending on the way the beam is clamped (sqrt(gamma)=(1.875, 4.694, 7.855) for the first clamped-free modes, while sqrt(gamma)=(4.730, 7.8532) for the first free-free modes (note: these are for the same given flexure mode, while the 2 cases from COMSOL are the first modes in two perpendicuzlar directions). This gives typically for E=200[GPa] and rho= 7850[kg/m^3] the value of steel: f1 = gamma*b/4/pi/L^2*sqrt(E/rho) = 5.8[Hz]*1.875^2 = 20.38[Hz] in clamped-free and 5.8[Hz]*4.73^2=129.71[Hz] in free-free All above in simplified non-shear theory, ignoring "nu" which is an acceptable first approcimation. Furthermore as the heigt to width ratio is only 0.7/0.4=1.75 we should see a mode difference of this ratio (sqrt(h*b^3/b*h^3)=b/h = 1.75), indeed 35.17/20.49=1.716 and 206.3/125.65=1.64, good enough Well as you have not precised your boundary conditions, neither the material, I might be wrong with some of the numerical values, but the rest I believe is more or less OK, no? There is quite a lot to say about mode shapes... For the theor, have a look at "Formulas for Natural Frequency and mode shape" R.D. Blevin, Kruger, 1979, reprint 2001, ISBN 1-57524-184-6 Hope this helps Ivar

Posted: 8 years ago Dec 14, 2009, 7:49 PM EST
hallo;

you wrote: a "0" for a structural mode means a (or several) DoF that is not blocked, if you have 6 of them at about "0" Hz, its typically that you are looking at the first 6 (x,y,z, Rx,Ry,Rz) free-free modes, and your 128 Hz will show up as mode no 7 (increase the number of mods in the solve tab to see this)

end.

that mean the first natural frequency occurs at the 7 mode in the case of free-free beam.

thank you very much
hallo; you wrote: a "0" for a structural mode means a (or several) DoF that is not blocked, if you have 6 of them at about "0" Hz, its typically that you are looking at the first 6 (x,y,z, Rx,Ry,Rz) free-free modes, and your 128 Hz will show up as mode no 7 (increase the number of mods in the solve tab to see this) end. that mean the first natural frequency occurs at the 7 mode in the case of free-free beam. thank you very much

Posted: 8 years ago Apr 16, 2010, 5:18 AM EDT
Hi

sorry for the late reply, but you are perfectly right, in a 3D representation of a free-free-structure it is the 7th mode that is the first interesting (non-trivial one), as the first 6 represent the free motion: 3 displacements and 3 rotations in a 3D space.



For you second question about stress concetration, I need a little more info.

Are you studying stress concetrnation at a "sharp edge" ?

in which case FEM will tend to give you "infinity" as you have a singularity at the edge. These singularities on "sharp edge effects" are typical for structural or even ACDC electric or magnetic fields.

one must "soften" the edges, to a reasonnable "engineering" level (note that: if you put a radius, the FEM meshing will simplify it to a polygonal shamfer).

If you need some litterature, I can only advise to study through:

"Peterson's Stress Concetration Factors" by W.D. Pilkey, Wiley&Sons, 1997.

For Eigenmodes take a look at:

"Formulas for natural frequencies and mode shapes" R.D. Blevins Krieger, 2001

These are classical approaches, but are the best exercices you might get to fit to FEM. It would be a nice project that someone went systematically through these two books and ported the examples to a FEM tool like COMSOL and reported the differences

Have fun Comsoling
Ivar
Hi sorry for the late reply, but you are perfectly right, in a 3D representation of a free-free-structure it is the 7th mode that is the first interesting (non-trivial one), as the first 6 represent the free motion: 3 displacements and 3 rotations in a 3D space. For you second question about stress concetration, I need a little more info. Are you studying stress concetrnation at a "sharp edge" ? in which case FEM will tend to give you "infinity" as you have a singularity at the edge. These singularities on "sharp edge effects" are typical for structural or even ACDC electric or magnetic fields. one must "soften" the edges, to a reasonnable "engineering" level (note that: if you put a radius, the FEM meshing will simplify it to a polygonal shamfer). If you need some litterature, I can only advise to study through: "Peterson's Stress Concetration Factors" by W.D. Pilkey, Wiley&Sons, 1997. For Eigenmodes take a look at: "Formulas for natural frequencies and mode shapes" R.D. Blevins Krieger, 2001 These are classical approaches, but are the best exercices you might get to fit to FEM. It would be a nice project that someone went systematically through these two books and ported the examples to a FEM tool like COMSOL and reported the differences Have fun Comsoling Ivar

Posted: 8 years ago Apr 16, 2010, 9:34 AM EDT
this what i'm studying:
www.comsol.fr/showroom/gallery/988/


Single Edge Crack: the KI parametre converge just for 1000 elements

but the maximum value of Von Mises stress increase all time and do not converge

thank you in advance
this what i'm studying: http://www.comsol.fr/showroom/gallery/988/ Single Edge Crack: the KI parametre converge just for 1000 elements but the maximum value of Von Mises stress increase all time and do not converge thank you in advance

Posted: 6 years ago Sep 29, 2011, 2:51 AM EDT
Dear Sir do you have the soft copy of that book? i have searched it but havenot found it in library and also on net. Sir i want to find the resonance frequency of longitudinal free free microbeam. I have used the formula f=(1/2L)*sqrt(E/p) but when i simulated the beam the resonant frequency is not correct. So if you any formula for finding the resonant frequency in longitudinal beam than please tell it to me.
Regards
Abid
Dear Sir do you have the soft copy of that book? i have searched it but havenot found it in library and also on net. Sir i want to find the resonance frequency of longitudinal free free microbeam. I have used the formula f=(1/2L)*sqrt(E/p) but when i simulated the beam the resonant frequency is not correct. So if you any formula for finding the resonant frequency in longitudinal beam than please tell it to me. Regards Abid

Posted: 6 years ago Sep 29, 2011, 7:39 AM EDT
Hi

unfortunately i do only have paper books (yet ;), but if you try on Wiki or on the web I'm sure you can find the relevant analytical formulas

--
Good luck
Ivar
Hi unfortunately i do only have paper books (yet ;), but if you try on Wiki or on the web I'm sure you can find the relevant analytical formulas -- Good luck Ivar

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.