Discussion Forum

Hey Luca,

As it is difficult to give an answer to your question directly, I would prefer to give you something like a check list to make you sure that you are defining the identical problem in two different tools.

In comparison cases, besides putting in the identical material parameters (damping, E, density), the definition of the boundary conditions plays an important role. I advise you to make sure that the boundary conditions that you are assingning to both models behave the same way. Please keep in mind that Comsol works with surfaces, areas, lines and points rahther than nodes (as it is the case with some other tools). Secondly, and specially if you are new to Comsol, please check your dimensions. As Comsol uses "meter" by default, one can easily make importing mistakes in the dimensions.

Hope it helps,
Onur

Hi

I have often compared COMSOL with other FEM tools for eigenfrequencies, mostly they agree with > 4-5 digits,

So I would only suggest as stated above, check again your boundary conditions.

But you might also have found a specific faulty situation for COMSOL, in which case try to submit it to the comsol support

Good luck
Ivar

Hello everyone,

I am calcualting eigenfrequncies of a cilindrical cantilever in the Stress strain mode. The amplitudes are arbitrary if I don't specify initial conditions but if I do, it should restrain the amplitudes. If I choose from the main menu physics/subdomain settings/element/Lagrange cuadratic I get amplitudes of 6. Since I am in SI units, it means 6 meters but the size my cantilever is 4 mm long and .25 mm radius. If I use ... element/Lagrange U2P1, the amplitude is 10^-12. It changes 12 orders of magnitude.
I go to solve/solver manager and check initial value expression and Use settings from initial value frame. Then I go to solve/get initial value and it gives me the initial conditions that I specified which is great but once I hit solve, it gives me 6 if I use a cuadratic lagrangain element and 10^-12 if I use U2P1. Any ideas on how I can restric the amplitude of the oscilations?

Thank you very much.

sorry 2nd IEexporer crash, full text below

Hi Alejandro

From my understanding, an "eigenfrequency analysis" is a basicaly a mathematical treatment of your model giving you two set of variables: the eigenvalues of your system (then transformed into frequencies in Hz for a structural analysis) and these are "absolute and precise", and the egenvectors or eigenmode shapes, but there is nothing in the definitions that gives any absolute value for the eigenmode amplitudes, these can only be compared as relative amplitudes: [m], [um], ... or whatever, it is simply a normalisation definition.

You should think of this as a system with infinite resonances (amplitudes) with an infinite energy put into the system.

So you should only compare the relative mode shape values.

Futhermore there are some special cases: if you do an analysis in free-free mode (non boundary conditions or BC's) the numerical importance of the 6 first "rigid body modes", compared to the other "elastic-modes" are very different, even the elastic modes are mostly down in the numerical noise level, close to "eps". Your stiffnss and Mass matrices (M&K) are ill conditionned and the results might not be very precise, this depends strongly on the algoritms used, how these detect ill conditioning and treat them.
On the other hand you have the fully constrained models (6 independet BC's) for which there is no or small rigid body displacements and mainly elastic modes, in this case the comparison of mode shapes is more precise, but only relative shapes.

In fact, depending on the normalisation scheme used, other FEM tools such as NASTRAN, ANSYS, or COSMOS gives you "mass particpation factors" in addition to eigenfrequencies and relative eigenmode shapes, these are the diagonal of the elastic mode mass matrix for a specific stiffness normalisation, which allows you to compare the modes on a global point of view, as the sum over all modes per degree of freedom (x,y,z in 3D) is simply the total mass of the system, you can then pick the largest modes up to you have 80 or 90% of the total mass and know that you have the most important ones (these are not necessarily the first ones based on a sorted frequency list), typically if you want to make a simpler model of a complex system this is the best way to go.
If you do a free-free model with these tools you will see that the total mass adds up in the 6 rigid body values, and the other elastics modes are in the 1E-25 level close to numerical noise.

See aso the excellent book: "Vibration Simulations Using Matlab and ANSYS" by M.R. Hatch (it could/should have been COMSOL and not ANSYS ;).
For an article on Mass participation factors try this one, or more recent the articles referring to it: J.T.Chen, H.K.Hong and C.S.Yeh, "Modal Reaction method for modal participation factors in supported motion problems", Communications in Numerical Methods in Engineering, Vol 9, pages:479-490, 1995.

If you want to look at the absolute amplitudes of your mode, you must consider to inject a finite PSD (power spectral density) acceleration i.e. in harmonic sweep mode (i.e. a provide a finite input energy), and add relevant damping (this is the difficult point: very model dependent on sizes, materials, environment (i.e. thin gas film skeeze modes ...), then you will get displacement that have a physical meaning, provided that the damping parameters are "correct" and sure you model truely representatif.

Hope this helps
Good luck
Ivar

Hi again

I would to propose some good litterature on modal analysis (and modal mass participation factors, see §4.5)

"Vibration Dynamics and Control", by Gienacarlo GENTA, Springer, 2009, ISBN 978-0-387-79579-9

But as I understood you know the author

there is also this other series (I have myself only vol3):

Vol3 Modelling of Mechanical Systems: Fluid-Structure Interaction, F. Axisa & J. Antunes, 2007, B&H-Elsevier, ISBN 978-0 750-66847-7

for the others, probably as good and well written

Vol2 is on "Structural Elements", and Vol 1 on "Discrete systems", all three by F. Axisa



Have a nice reading ;)
Ivar

Hello Ivar
I just read the bibliography proposed and now i search the books and i hope to find the solution, but i would ask a question about eigenfrequencies again. I have some problems with the first eigenfrequency of my model, in fact I realized the model using your advices, shell that is 'equation' connected with solid. In this way I found the right values for the 2nd and 3rd eigenfrequencies, but i also found the 1st eigenfrequency that is 2.9Hz against the right value of 3.9 Hz. Developing the same model using only shell element and assigning thickness i found the correct first frequency. Returning to 3D model(shell+solid) I note that if i activate the boundaries of solid block in shell physics my frequencies grow, i suppose that the reason is the increasing of stiffness.

Thank you in advance
Luca

Hi Luca

I'm starting to have replied to so many questions on the forum that I'm getting slightly confused what I have said to whom ;)

I now that I have posted somewhere a model linking shell beam to a solid but this model was/is slightly too simple as I'm only linking the solid rotation to the shell and not the opposite in a bidirectional way, furthermore as a shell is a surface, linking it to a solid in 3D over a line means that you get a too soft link.

First one should use a separate equation or a weak constraint to link the Solid and the Shell rotations in a bidirectional way, you can be inspired by the example of the torque load in a the structural use guide (I believe).

Furthermore, one should idealy define a surface imprint (about the size of the section of the shell/beam) on the boundary surface of the solid and link an integrated value over this surface for a better coherence of the model.

Not applying these improvements, can easily change the link stiffness, hence the resonance frequencies by I expect some 50% !

I'm away on business travels so I have no access to COMSOL these days (that's terrible for me ;)
I'll try to fetch together a better example once, but I'm missing some free time to do this.

Good luck
Ivar