Discussion Forum

Hi

I'm not sure how you define your "breahting" mode, but when I make a 1m radius, default material (steel) sphere, and ask to solve for the 24 first eigenmodes, I can see differet modes showing up
(I use "boundary" map with "deformed shape" on, and not "slice" mode).

Now as you have not attached/fixed your sphere the first 6 modes are 0, and then as you have a fully symmetric sphere your modes have a high degeneracy so in the "24" modes there are only a few fundamental different modes. (the "same" frequencies differ slightly depending on the mesh finess/symmetry you use).

So I suggest that you try again

Good luk
Ivar

Hello, I am a newbie of Comsol and I tried to start with a very simple model of finding fundamental breathing mode of a solid sphere, but got frustrated - it seemed that I was not able to find the breathing mode (or don't know how to identify). The way I did is following:

Structural Mechanics Module ->Solid, Stress-Strain -> Eigenfrequency analysis -> create a solid sphere of 1m -> set boundary constraint condition as Free -> Set Subdomains with default setting (E=2.0e11); v=0.33; a=1.2e-5; p=7850), Material model as isotropic; Coordinate system as global coordinate system; ->initialize mesh - Solve eigenfrequency -> that is.

I used Slice (predefined quantities=total displacement) to check all the frequencies found from 0-4000Hz, but were not able to find the breathing mode...

did I do anything wrong here? Help please

free b/c is making problem. specify simply supported or b.c.

Hi

Most advanced FEM softwares, and COMSOL too, accepts free objects (fully unconstrained volumes without BC) for their eigenmode calculations, but then the first 6 dof (in 3D) are at "0" [Hz] or close to, as the unconstrined object can move/rotate freely along the first 6 dofs (x,y,z, Rx,Ry,Rz).
By default COMSOL provides you with the results of the first 6 modes, you have to manually set a higher limit, i.e 12 or more to see the modes above. See the solver setting page.

So normally you do not need to set any BC, especially how would you, on a sphere like that, without influencing the modes ?

Ivar

Hi

I'm not sure how you define your "breahting" mode, but when I make a 1m radius, default material (steel) sphere, and ask to solve for the 24 first eigenmodes, I can see differet modes showing up
(I use "boundary" map with "deformed shape" on, and not "slice" mode).

Now as you have not attached/fixed your sphere the first 6 modes are 0, and then as you have a fully symmetric sphere your modes have a high degeneracy so in the "24" modes there are only a few fundamental different modes. (the "same" frequencies differ slightly depending on the mesh finess/symmetry you use).

So I suggest that you try again

Good luk
Ivar

Dear Ivar,

thanks for your reply. I still had troubles in understanding results from Comsol. here are some more information on "breathing mode".
(1) the breathing mode of a sphere means sphere only experiences radial motion. the fundamental breathing mode of a free sphere corresponds to an expansion and contraction of the sphere along radial direction oscillations with the lowest frequency (n=0 mode). I attached an image here showing analytical calculation of n=0 and n=1 breathing mode of a sphere.
(2) As I described before I tried to use Comsol to calculate breathing mode of a sphere (R=1m with default material setting, see above), but I was not able to find the fundamental breathing mode. I attached result from comsol calculation here with lowest frequency at 1229Hz. as you can see from both slice and boundary images (total displacement) it was not so called breathing mode (which was supposed to have spherical symmetry in the motion).
would it be possible that I didn;'t use larger mesh size? becasue of limitation of my computer I was not able to set larger mesh size though.
(3) you mentioned about the "deformed shape" image in your message, but I can not find it with comsol 3.5a. would you describe a little bit more detail? I only found x-displacement, y-displacement, z-displacement, total displacement and etc in the predefined quantitied...
another question related to this: my understand is that Comsol did such calculation in cartesian (x-y-z) coordinate. can we select spherical coordinate instead?
(4) another thing I questioned about the result from comsol was that if you looked at my attached image of 1229Hz mode, the total displacement of sphere at that mode could be up to 3.5m for a R=1m sphere. does that make sense? it seemed to em the oscillation amplitude should not be that big...

Thanks again for your time and help,

-Michael

Hi
I do not have time just now to answer all your questions (I'm in fact at a Comsol course, RF this time), but I have a few easy points to give you here:

Eigenfrequencies calculations: the eigenfrequencies calculated are correct from the model point of view in Hz, but total displacements are arbitrary, as eigenmode can be arbitrary normalised. COMSOL has selected one way, rather different from some other fem tools such as NASTRAN and ANSYS, but it's still mathematically correct, so you should not concentrate on the absolute values of a mode shape, only their relative shapes.

As you are interested only in the radial displacements, try to create the integration variable
Duvw dist_smsld
over your spherical volume , then hit "Solve Update Model"

I assume you are in the smsld application mode, and there dist_smsld = sqrt(u^2+v^2+w^2) the total displacement, furtmore I'm assuming your radial origine is at x,y,z=0,0,0, you will need to adapt the formulas if this is not the case

Search for the first mode with largest radial displacement, i.e. plot Duvw over the modes by:
goto the "Postprocessing Domain Plot, General tab: select all modes, select "keep plot", Point tab: select any point, and type for the Expression Duvw then OK

see also the replies for the discussion of
"SD": 2D plane strain mode vs. 2D axial symmetry stress-strain mode

so far good luck
Ivar

Hi again,

For the cylindrical coordinates, here you can find some more info:

www.comsol.com/support/knowledgebase/939/

It's true that COMSOl proposes by default only the cartesian in 3D strutural.

Now what are you really wanting to do ?
- use COMSOL to verify your PDE equations
- use COMSOL to give you some nice pictures of the sphere
- ...

because as you have a fylly symmetric problem, you can simplify the equations and attack it as a 1D PDE case (without the nice photos though).

Back to your 3D simulation, I repeated it quickly, default 1m radius sphere, no BC, default material steel. I meshed it rather "finer" with 55000 elements and 231873 DoF's. It took 352 seconds on 8 core for 9 GB ram in direct defauilt settings mode. I asked for 26 first eigenmodes, and what do you see:

Observe the mode shapes in "Slice" mode with 3/1/1 slices and alternatively in "Boundary", with "Deformed" shape ON

I get 6 modes close to "0" Hz, these are the 6 free-free DoFs, as expected;
then 5 modes around 1232+/-0.5 Hz, the shape appears rather spheric with several hills appearing, allthough the numerical values shown are large, but this could be a mode normalisation effect
then 5 modes around 1305+/-0.5 Hz, the sphere show large elliptic deformations, more like an egg,
then 2 modes around 1767 Hz, 1 at 1777, 2 at about 1900, 2 at 1903, 2 at 1905 and one or more at 1912 Hz

with a larger mesh and less elements you will just see more dispersion on the frequencies

So I add the subdomain Integration variable as "Duvw dist_smsld" and hit "Solve Update Model" and do an Global Plot on all eigenmodes of Duvw, the result is not very clear, so my suggestion of yesterday was too hasty.

So let us go more systematically:
In Options Expression Scalar expressions I add the 3 following rotation definitions based on small deformation hypothesis (F=I+D+W where I is the identity or translation, D is symmetric deformation tensor and W the rigid body rotations antisymmetric tensor. Ref, i.e. Timoshenko on Elasticity):

thu 0.5*(wy-vz)
thv 0.5*(uz-wx)
thw 0.5*(vx-uy)

then OK.

In the Options Integration Coupling Variables Boundary Variables I define for all 8 surfaces (You can do the same on the sub-domain, with Vol instead of Area, and skip the small "b" for bounday in the names)

Area 1
Ub u/Area
Vb v/Area
Wb w/Area
Ub_2 u^2/Area
Vb_2 v^2/Area
Wb_2 w^2/Area
Dbuvw_2 (u^2+v^2+w^2)/Area
Thub thu/Area
Thvb thv/Area
Thwb thw/Area
Thub_2 thu^2/Area
Thvb_2 thv^2/Area
Thwb_2 thw^2/Area

Then when I do a Global Plot, on all eigenmodes >1Hz (with line settings labels) of these variables this gives me some indications on how to interprete these modes. But again I'm not impressed by what I get out, apart that some correlation of mode duplicity shows up: 6-5-5-2-1-2-2-2-1 for the 26 first modes.

In present state I must admit that I do no have the best clue how to identify with COMSOL the spherical breathing modes nor the torsional modes one could expect to observe, and that the modes shapes in spherical symmtry apper somewhat unexpected for me.

So you have a nice problem here, it requires some more studying

More nexxt time
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.

Hi Alejandro

You can find some suggestions concerning your questions in the other session: "eigenfrequencies analysis"
Ivar

Hi again

Your "breathing modes" are giving me some challenges, and I'm not through yet, but getting closer. First of all, I notice that few of my books come close, as spherical coordinates are not or hardly considered. In the mean time I have done the following:
Run the same simulation with COSMOSWorks, just to compare: we get the same frequency values (wihin a few Hertz), but slightly more expressive images, I beleive due to their different "modal mass normalisation". So I see that the first five mode above the 6 free-free rigid-body modes is probably a rotation mode, the second series are probably to be defined as breathing modes, but giving ellispoidal shapes, higher up thetraedral, then cubic etc.
No way to get a perfect symmetric radial expansion mode, which I suspect that is due to meshing and symmetry disruptions due to the binairy numerical appoximations.

By making several runs with COMSOL for different E, nu, R, just to validate the eigenfrequency dependence I get that the modes are scaling as (2*pi*f)^2=w^2=a^2*(G/rho)*(2*pi*R^2) with a=1,1.12, 2.20, 2.38, 2.51 ... (whre G=E/2/(1+nu), E the Young Modulus, nu Poisson coefficient, rho the density, R the sphere radius.

My conclusion for COMSOL: eigenfrequencies are correct, mode shapes are difficult to understand because of the large difference with the free-free modes and elastic modes numerical values in teh K&M stiffness and mass matrices, due to their ill-conditionning.

Now I have gone slightly further, but without having had the time to check, so pls verify carefully, I might have missed soemthing goingtoo quick. Taking the Timoshenko and MAPLE 13 I have evaluated the diff equations and extracted the radial part (if not missed something) as per my pdf file attached.
Then instead of going further in MAPLE, I took this equation "NS1r" for the radial part into the PDE mode of COMSOL:

I select "Multiphysics, 1D and use "r" instead of "x" as reference coordinate, PDE, Coefficient Form (c), Eigenmode calculations, with "u" as dependent variable.
I define the constants E=200E9[Pa], nu=0.33, rho=7850[kg/m^3], G=E/2/(1+nu) the sear modulus, Lam=G*nu/(1-2*nu) the Lamé modulus, R=1[m] the sphere radius.
In draw mode: I make a single line from "0" to "1" the radial length
In the Boundary Conditions: I select the two points "1,2" and set Neumann boundary conditions, defaults values (I remain in free-free mode)
In the Subdomain settings I set: c=(Lam+2*G), a=0, f=0, ea=rho*4/3*pi*R^3 (the sphere density times the volume = mas), da=0, alpha=2/r, beta=gamma=0, just as in my pdf file from the MAPLE algebra (I hope there is no typo here).
I mesh by default, and refine a few times, then solve.
Now to read the frequencies, on should recall that f[Hz]=1/2/pi*j*lambda where j=sqrt(-1) and I get some 1303 Hz, very close to the second family of modes obtained with the full 3D analysis, the one with elliptic shapes, clearly a radial driven expansion, modes frequency increase is clearly multiple harmonics.
Your image of the modes where with a fixed cetral point (I'm calculating here in free-free mode) soone need to adapt the BC's of point 1 to be in the same conditions (Dirichlet q=1, h=1 other =0), but they remain rather simular (how well is difficult to tell, the sign and absolute value being anyhow arbitrary due to the arbitrary normalisation possibility). Now by fixing the central point we change the first eigenfrequency value, but the spacing remains the same.

I'm rather stuck here, but you can find sime interesting developments and illustrations in the excellent book "Modelling of Mechanical Structures, Vol 3, Fluid Structure Interactions" by F. Axisa & J. Antunes, 2007, ISBN 978-0-750-66847-7, the only place where I expect to find more on radial modes of spheres, because immersed in a liquid a sphere or a spherical shell would undergo a purely radial symmetry compression. But I just received the book a day ago, this implies stufdying associated Legendre equations and Bessel equations.

In the mean time It's a nice example (and training for me) on how to use COMSOL to play with 1D PDEs, not only full 3D models.

Pls check crefully and give me feedback on any errors or omissions

Have fun
Ivar

Thank you. I will go through your response carefully.