Discussion Forum

Hi

1) first of all you should NOT use a "point" except in 1D as this will give you a singularity and poor values. Use rather a boundary (surface in 3D edge in 2D) of finite length (> 2-3 mesh elements per side) you can cut it out on the boundary or use a Gaussian shaping function.

2) apply a boundary load (with amplitude versus frequency from an interpolation table or an equation) and a frequency domain solver, this will interpret ALL boundary loads as harmonic amplitudes, and define your frequency range() in the solver settings

Note by applying a boundary force you do not change the eigenfrequency as you do not add any true local mass to the system. But if you intend to model a shaker applying a force via some extra connection, the mass of this connection could interfere with your structure modal shapes

--
Good luck
Ivar

Hello,

Thanks for the help. But I tried to add a boundary load to the top of a cantilever. But when I do the Frequency test the cantilever won't move at all.


I'm trying to add a force that will act in a periodical manner (that I can adjust it by changing the frequency in which this force is applied to the cantilever ) so that it will make my it move in a up-and-down direction.

I'm uploading my model so you can take a look of what I'm doing it wrong.

Bare with me because I'm really new to this program.


Much appreciated for your help.

Victor Soares

Hi

you should rather use a classical frequency domain scan, as you have no prestressed load case for the stationary solver, and your harmonic "perturbation" is not "small compared to the prestressed state

One trick to ease the meshing for long thin beams: Use the geometry "layer" tab and split your beam in the middle with one or three layers, then mesh in "normal mode"

When you do frequency domain sweeps, its often quicker to use a log scale à la "10^{range(0,0.5,3)}", and run a eigenfrequency scan first to define the resonances, approach these with a finer step around the resonance. Often the solver will not step through a resonance as there is no damping and Q=> INF

--
Good luck
Ivar

Good evening,


I'll try this when I get home.

But is there a tutorial so I can learn how to add a Boundary Load on top of my beam, in a square near the end. So I can set a frequency in which this load would act in order to make my structure go up and down ?

Hi
check the library models, and read the doc about the frequency domain solver cases, and look at the equations in the main physics nodes when you switch from atime solver to a stationary solver to a frequency doamin solver. I find it easier to understand when looking a the general formulas used.

--
Good luck
Ivar

Hi Ivar,

I have been trying to do a Frequency Domain analysis of a simple cantilever beam and it has taken me ages till I found your post and read it.

The fact is that I tried to define the harmonic load with a boundary load and the "Harmonic Perturbation" option activated. All the results that I got were 0. After desactivating it, the model worked perfectly.

I find this "Harmonic Perturbation" option confusing, and even though I looked for it in the documentation I do not still understand what it is used for. In which situation are those "Harmonic Perturbations" used?

Thank you for your help

Regards

Mikel

Hi,

The concept of Harmonic Perturbation is essentially a tool for being able to split loads in one stationary 'pre-stress' component giving a base state and one superimposed harmonic perturbation.

If you run an analysis where you have two study steps where the first one is stationary and the second one is frequency domain, then the loads marked 'Harmonic Perturbation' are ignored in the first step, while those without this mark are ignored in the second step.

If we go a bit more into details:

Whether a load is considered as being a perturbation load or not is internally controlled by the 'linper()' operator. If you look in Equation view at a load marked as Harmonic Perturbation, you will see that this operator has been added to the given load.

For the rest of the discussion we assume that you have two loads. One has the value 4711, and the other one 17, but has Harmonic perturbation marked. You could actually write the same load as a single load (without marking it as Harmonic perturbation) as 4711 + linper(17) .

Now 4711 would be used as load for the pre-stress case and 17*cos(omega*t) would be used in the frequency domain analysis. Note that the harmonic variation is always implicit in a frequency domain analysis.

In the 'General' section in the settings for the Stationary solver (the one used for a frequency domain solution), there is a setting 'Linearity' which controls whether to use the perturbation loads or not. It is automatically set to 'Linear perturbation' when you add a study of the 'pre-stressed' type, but not if you just add a Frequency Domain study. The consequence is that for a pure Frequency domain analysis the load above would as a default be interpreted as 4711*cos(omega*t).

A mode superposition based frequency domain analysis is as a default considered as a perturbation type analysis. In that case it is the setting of 'Linearity' in the Modal Solver settings which controls which load to use.

Regards,
Henrik

Hi Ivar,
Can we also input the phase of the applied boundary load (complex value of boundary load?) in comsol?

Thanks,
Xiang

Hi Henrik,
Are we able to have complex input in frequency domain analyis?
If we can, we will able to provide the phase information of the applied load.

Thanks,
Xiang

Hi Henrik,
Are we able to have complex input in frequency domain analyis?
If we can, we will able to provide the phase information of the applied load.

Thanks,
Xiang

Yes, you can either write the load in complex form like 10.2e3*(1+0.4*i)[N] or right-click on the load and add a Phase subnode where you supply the phase angle.

Regards,
Henrik

Thanks, does comsol assume F_amplitude as a real number by default? Can have complex amplitude input in comsol? When we solve some problems, we may also get complex amplitude solution. Say u=u_amp*e(i*phi)*e(i*2*pi*f*t), if u_amp is an imaginary number, then if we take the real part of u, u = u_amp*i*sin(2*pi*f*t+phi). Does comsol also allow complex amplitude input?

Thanks,
Xiang