This website uses cookies to function and to improve your experience. By continuing to use our site, you agree to our use of cookies.

**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.

## Damping problem in the undamped vibration analysis of a cantilevered beam in Comsol Multiphysics

Posted Jul 27, 2009, 5:53 PM EDT 6 Replies

Please login with a confirmed email address before reporting spam

I'm trying to do the undamped vibration analysis of a cantilevered beam in Comsol Multiphysics. Although i choose "no damping" in materials tab in subdomains menu, it solves the problem as if the material is damped. This happens when i choose "BDF" as time dependent solver and set "weak constrains" as on.

And if i set "weak constrains" as off in plane stress application mode properties, the solution becomes completely wrong(not a vibration signal anymore).

I tried to change the time dependent solver. When i use generalized alpha, solution becomes "random" undamped oscillation for solving the problem in short time limit(like solving to max 2 seconds). If i increase the upper time limit (like solving to 10 seconds) then the solution becomes unstable.

Although my problem is a simple vibration problem, i couldn't figure out what I'm missing. Even I'm thinking that it could be a bug(its easy to blame software: p): ]

Any ideas would be appreciated..

Thanks in advance..

Ouz

P.S.

my problem is a simple rectangular aluminium beam which is fixed by one of its short boundaries. I defined a function as an input and set it as a load on the upper point of unfixed short boundary.

Please login with a confirmed email address before reporting spam

I think that you observe damping because of the *numerical damping* of the integration scheme you are using.

Give a look to manual in the part "Solving the model/The solvers and their settings/Time dependent solver".

You will see that any numerical scheme contains a certain amount of numerical damping (that is, a damping that has no physical basis but it is needed just to stabilize the scheme).

Within BDF you control damping by choosing the integration order, while using generalized alpha you have much more freedom to control it using several settings.

In any physical situation material damping always exists and therefore it would be better to add it to your simulation.

If your actual beam is underdamped (that is it can vibrate even if damping is present) just choose a value of physical damping that stabilize your oscillation. Using BDF scheme, a certain amount of numerical damping will be superimposed to the phycisal one. To minimize the contribution of the scheme, just reduce the time step as suggested by the manual. A "Trial and error" approach will help you to set both the physical and the numerical damping properly.

If you give me more information about your model, I think I can give some more hint.

Hi!

Alessandro

Please login with a confirmed email address before reporting spam

I'm working on modeling of eddy current damping effects on the vibration of conducting cantilevered beams.

I want to compare the case in which eddy current damper is active to the case in which there is no damping in the material of beam. I know it will be just theoretical but I think it will be much impressive in the plots when comparing the cases.

I tried what you told me about solver options and look at the user manual. I chose the timestep as 0.0001 which is 200 times of the (lowest) mode that i'm interested in. I got an -almost- undamped vibration response (an almost pure sinusodial) but there was a transient damping at the start of the signal(superposing of a decayed sinusoid. I think it is higher frequency mode).

But I couldn't get the pure sinusodial signal that i got from ANSYS before,yet. Is there any chance that i can do it in Comsol?

The model geometry is a simple rectangle which one of its short edge is fixed as setting Rx=0 Ry=0 in boundaries tab.

I defined the input with these command lines on top point of the free edge :

% Functions

clear fcns

fcns{1}.type='interp';

fcns{1}.name='inpt';

fcns{1}.method='cubic';

fcns{1}.extmethod='extrap';

fcns{1}.x={'0','0.001','0.002','0.003','0.01'};

fcns{1}.data={'10','10','0','0','0'};

fem.functions = fcns;

I have another question.

Is it possible to model this problem in 1 dimension in structural options of multiphysics module or i need to model it in PDE coefficients options if i want to model it in 1 dimension?

Thanks in advance..

Ouz

Please login with a confirmed email address before reporting spam

your choise of the time step seems right. In structural mechanics time dependent simulations I usually set a time step which is about 1/100 of the period of vibration of the dominant mode and usually the simulation runs correctly.

In any case, as suggested by the manual, you have also to tune the absolute tolerances of the scheme so that their values are at least one order of magnitude less then the expected values of your displacements. This will ensure the convergence of the scheme.

According to your post, the external force acting on the free end is a square impulse. Such excitation, from a physical point of view, will excite almost all modes of vibration (the fourier transform of a signal which is "short" in time, will have a large frequency span, thus covering a range in which the frequencies of many modes of vibration fall) and I think that what you observe at the beginning of times is rightly a contribution due to higher modes.

I think that, if physical damping is absent, it is becouse of the time step I have chosen (may too large to capture the vibration of higher modes) that you observe a rapid decay of such contributions. Just the fundamental mode survives and this is what you observe.

In any case it seems to me that your goal is just to verify the effect of your physical damping (due to eddy currents) to the vibration of your beam. If I'm right about your intention, I think it is better to model the problem in frequency domain, through an eigenfrequency analysis. In the undamped case, the displacement in an eigenfrequency analysis is *assumed* to be a perfect sinusoid and therefore no time domain analysis is needed.

A good way to reduce the computational cost of your analysis (this my answer to your second question) is to employ beam theory. Set space dimension to 2d and go in "Structural Mechanics module/In-plane Euler beam". If your cantilever width and thickness are w and t, set in "subdomain settings/cros-section" A = w*t, Iyy = 1/12*w*t^3, heightz = w (where I assume that the width of your beam is along z-axis, that is along a line normal to your geometrical xy plane).

The advantage of beam theory is that you will have a 1-dimensional mesh (the geometrical model of your beam is just a line) and therefore you will save a lot of computational cost.

Clamp condition and external forces should appear in "point settings".

Good luck!

Alessandro

Please login with a confirmed email address before reporting spam

I can only confirm that you must always play attention to the boundery conditions, AND the derivatives theroff, particularly when you work in time domain, I always leave out 1-2 full periods of the beginning ot the time simulations to let the phsysics/mathematics stabilise. This is due to the fact that one mostly do not apply correctly the step functions, by smoothing them and checking that the derivatives are also continue, hence you get a shock start and you must get this damped (if it does not just run unstable).

You will see these oscillations too if you run simple analytical checks with a tool such as MaplSim (what I use for my regular model checks) as I always check my models independently at a few "easy" points.

The question remains for my why one is not used to see this too i ANSYS ? I beleive ANSYS is applying some "initial damping" without really telling us, for me this tool has always had a "balck" box approach, not that it's globally wrong, but it applies some "stabilisation" tricks, that simplifies life, but get us to forget about the true physics.

Have fun

Ivar

Please login with a confirmed email address before reporting spam

I think I should work a little more on damping of the beam. It still does not settle as in the experiments..

Ouz

Please login with a confirmed email address before reporting spam

my paper problem is shock response analysis of packaged accelerometer.could you tell me how to give the shock input to the system.and how to find the stress response analysis.

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.