Discussion Forum

Below is an image of the 3 options which I could already simulate

- Time Dependent Modal const. force of 1[N] (a damping is very easy to recognize)
- Time Dependent const. force (no damping can recognize, but a shift/offset by the constant force)
- Time Dependent gp force (gp: Gaussian Pulse, a shift by the constant force was avoided but still no damping can recognize)

cya Thomas

Hello again,

I tried to vary the system, but without getting new results. I tried to vary the system, but without getting new results. It would be great if someone could look at my simulation and tell me why in Study 3 (Time Dependent without Modal) is no damping or why i can't use Boundary Load gp force with a gaussian pulse in Study 1 (Time-Dependent Modal).
Many thanks for your help and i hopefully get a reply soon ;)
sincerely Thomas

Hello again,

it is perhaps possible that the system can be provided with a start condition.
For example an initial velocity, which is then slowed down by the damping.
Or an initial deflection which oscillates back by the spring constant and then ends at neutral position (without an deflection) by attenuation?

Thanks again

cya Thomas

Hi Thomas,

That is an interesting problem. The way your model is set up you should not be getting any damping! The damping you get in the modal analysis Study is because of low convergence tolerances that lead COMSOL to take a big enough step size that causes NUMERICAL damping. If you reduce the convergence tolerances you will get less of that numerical damping.

To get more physically accurate damping you need to add damping ratios to the modal analysis. For the non-modal analysis you can use Rayleigh damping, or a material model that has built in damping, such as viscoelastic.

Nagi Elabbasi
Veryst Engineering

Hello Nagi,

Thanks for your answer. I use the material data from MatWeb and unfortunately there is no information about the damping.

matweb.com/search/DataSheet.aspx?MatGUID=f7a64cd5a3534bf0a85d836da650f022&ckck=1

Maybe you can give me a tip/hint so I should proceed further and to simulate the damping of the system.

many thanks and best regards

Thomas

Hi Thomas,

I cannot open your MatWeb link but it’s true that it’s rare to find damping data in material data sheets. It’s also hard to model damping accurately, so frequently it’s oversimplified. In many applications that oversimplification is justified, but if, for example, the main objective of a simulation is to find how many cycles a part will vibrate before it stops then an oversimplification of damping is not recommended!

There are experimental methods that evaluate the logarithmic decrement, loss factor, phase angle, or “tan delta” of a material, which are measures of damping. The loss factor is usually a function of frequency and is low for most metals (1e-4 to 1e-3) and higher for most polymers (0.01 to 1). For polymers, you can use DMA (Dynamic Mechanical Analysis) for frequencies below ~200 Hz and ASTM E756 for higher frequencies. Other techniques are available for metals.

When you have the damping data you can use it to calculate modal damping factors for modal analyses. For non-modal analyses you can also use that data to select viscoelastic material parameters, or Rayleigh damping constants. Unfortunately, it’s hard to match experimental damping data over a wide frequency content so you should focus on matching the damping for the frequency content present in your system.

I hope that helps.

Nagi Elabbasi
Veryst Engineering

Hi

thank you for your help.
In our experiments we want evaluate eigenmodes frequencies in the range up to 24kHz, eigenmodes that are excited by a pulse (small impact).
Additional we try to evaluate the damping performance, but in my opinion, it is sufficient to investigate only the lower frequency range(because of the geometry and because this has the greatest impact on the damping).

Enclosed a functioning link to the material parameters of SAWBONE 10PCF (Polyurethane Foam)

matweb.com/search/DataSheet.aspx?MatGUID=f7a64cd5a3534bf0a85d836da650f022

Thanks a lot yours sincerely

Thomas

Hi Nagi & Thomas

thanks for taking up this issue, and thanks Nagi for the precision on the solver tolerance settings, I hadn't noticed that the relative tolerance settings from "Set 2:Time Dependent Modal" is DISCONNECTED from the lower sub-node "Modal Solver 1" node absolute and relative tolerances variables.

These large numerical damping had made me give up last time I was working in Modal time domain, now it looks much better :)

Material damping is indeed a delicate issue, and reliable data is missing, even when searching hard with Google ;)
But for your styro-foam material it's really not a "linear elastic material", so is even a linear eigenfrequency solver valid ? probably you should also check it, if it should not be run with a pre-stress load case too, but Nagi these polymer that's your domain, no ? perhaps your company could provide us with generic DMA analysed thermo-elasto-damping ... values

--
Good luck
Ivar

Hi Ivar, good to hear from you! Damping is indeed a delicate issue. Yes foams are nonlinear materials but you can still do a linear eigenfrequency analysis. I recommend doing a pre-stress analysis step first, as you suggested, especially if the foam is experiencing large strains. We do not do DMA or ASTM E-756 testing in-house. We rely on a few good labs for that type of testing. Also there are unfortunately no reliable generic experimental damping data for foams, as you would find for say Titanium. But in the absence of experimental data I suggest a damping value around 0.25, or searching even harder on Google :) And one last comment. You mentioned an interesting issue of “thermo-elastic damping”. That is a different source of damping, as you know, relevant mainly for small scale, high frequency applications, so it’s common in MEMS.

Thomas, you will find several examples on pre-stressed eigenfrequency analysis in the COMSOL model library. You will also find a good example on thermoelastic damping, in case you need it. I agree, based on what I know about your model, that you should focus on the damping of the low frequency range.

Nagi Elabbasi
Veryst Engineering

Hello Nagi,
Hello Ivar,

Thanks for your help. I am learning a lot (very quickly) ;)
I will look the examples and hope that I can apply them on my simulation.
I still noticed that the frequencies (Timing diagrams) behave differently. I have reduce the convergence tolerances and both graphs of the total displacement are not comparable (Study 1 and Study 3 are completely out of phase at t=0.25s), what is the reason?

Thank you for your help

cya Thomas

Additionally I have added damping (random value for a first try, Linear Elastic Material 1-> Damping 1).
In Study 1 I used a constant force of 1 [N] (Boundary Load const. force and deactivated Boundary Load gp force) and at the solver (Modal Solver 1) i used a Load factor "an1(t[1/s])" (gaussian impuls)
and in Study 3 i used the gaussian impuls Boundary Load gp force and i have deactivated Boundary Load const. force.

The result already looks very good, I just have to find the right damping factor and eliminate the phase shift of both simulations

Hi Thomas, you’re welcome! The phase shift you observed may be a result of the numerical integration in the non-modal transient analysis. Basically time integration not just introduces some numerical damping, it also introduces a phase lag that results in a reduction in frequency! Both effects decrease as the time step size is reduced. I tried briefly to reduce the step size but could not eliminate that phase lag, so there may be another reason behind it for this problem.

I have a comment on the two displacement curves you plotted though (modal and non-modal). They involve a half-cycle phase shift over a period of 13 cycles, and the peak displacement amplitudes are very similar. For many dynamic applications that level of accuracy is good enough.

Nagi Elabbasi
Veryst Engineering

Hi

there is a bit more to say here:

first of all you are using 5.0, while I get an error message in my 5.1.0.180:

Time-dependent equation residual vector is not supported for modal analysis.

==> update this is "simply" that the TIM solver does not accept a "time dependent load" only a constant time INdependent load !

So I cannot run the modal solver, even if I define a new Solver. This is new to me so I'll have to dig further here, so I cannot compare the values of your latest model

Second I see that your time dependent analysis (study 3) is done in "free" time stepping and that from the log you are interpolating many results between true solver steps, for oscillatory models like this you should rather use the "intermediate" time stepping to ensure that the solver takes one time step in-between each saved result.
I see also you select all 6 modes, while the two last Twist Theta_Z and Elongation/compression Dz at 379 and 614 Hz respectively will not be much excited, so the time stepping at 5E-4 s or 2kHz should resolve adequately the 4 first modes (even the 6) if the solver steps for each. This takes some more time to get to the solution, but still it's reasonable.

I suspect (and see from my comparison) that your solver-relative phase delay also comes from the time dependent solver settings!

You could check further by taking an FFT of the resulting oscillations, there are operators to do this inside COMSOL, even if it has disappeared from the Derived Values - Data Series Operation, it's now a solver process you can add to the time stepping solver (see the doc FFT Solver)

--
Good luck
Ivar

Ivar, good point. The Time-Dependent Modal solver appears to only work with time-independent loads which is quite restrictive. It turns out that it can work with time varying loads but that feature is quite hidden in my opinion! COMSOL should highlight it better, and maybe mention it also in one of the Tutorial examples.

You have to remove the time-dependent factor from the load definition(s) and add it to the Modal Solver > Advanced > Load Factor. It still means that you can only have one time dependent factor for all loads in the model but in many cases, such as this problem, that is sufficient.

Nagi Elabbasi
Veryst Engineering

Hi

indeed I find it also poorly documented or lets say poorly illustrated, even from the theoretical section it's difficult to understand what applies where and where to apply the "f(t)*L0" in the GUI fields.

For a frequency domain analysis, one would then apply the PSD spectra, but transformed correctly, into this load factor.

Again COMSOL is giving us the theoretical tools, in a superb way, but they seem to lack the practical engineers to propose simple and more handy ways to handle common analysis tasks, in the postprocessing section.
With the newer version of COMSOL one set up a multi-physics model, and solve it, so quickly, that I now spend 80% of my time clicking along the Post-processing section, mostly for very tedious and repetitive tasks, in this last section of the Model Tree, for me, the most effective improvements are still "to be done". Hopefully it will arrive once too :)

UPDATE:
You can find the example for the time domain in the Application Library "elbow_bracket.mph" example but you must dig all the way down and open the "Advanced" tab of the Modal 1 Solver node.

Unfortunately I can find no example for the frequency Domain modal with a PSD defined load. COMSOL could easily implement this in the "vibrating_deep_beam.mph" example of the Application library (but I might have missed something) again one must dig all the way down to the "Advanced" setting to check. So as usual with COMSOL: it's there, but sometimes well hidden ;)

--
Good luck
Ivar

Hello,

I am using Comsol 5.3 and trying to model a piezoelectric transducer. I have defined an analytic function as figure 1. I want to load the piezoelectric voltage with this pulse so I added it to the electric potential as shown in figure 2.

When I run the time-dependent study, I get the error that is shown in figure 3. I have tried to add "an1(t)" to Modal Solver > Advanced > Load Factor, but it did not work.

What is this error message implying to?

Thanks,
Hamed