Panel speaker simulation - harmonic mode

[pwray]

Hello

Thanks for the previous advice about using Harmonic Mode with smitc solver.
I think that I have successfully set up a mesh and sif for harmonic mode simulation, because I seem to be getting reasonable results.

1) First I meshed a panel (1200 x 350 mm) with an embedded 30mm diameter 'patch' (is that the right term?) to accept a pressure force representing an audio exciter. I first meshed the exciter area, and then the remainder of the panel, subtracting the inner area. The mesh seems to be continuous across the patch. Is that the correct approach?

2) I used smitc with harmonic mode, and tried both real and complex settings. I seem to be getting sensible results, such as:
* With the frequency set to an eigenfrequency, it gives that mode shape
* There is smaller amplitude the further that the "exciter" is from the antinode
* Frequencies below the fundamental seem to give something similar to a 'static' deflection of the panel under the exciter location
* For frequencies between resonances, you get some sort of hybrid (although one Ive seen seems unrealistic, I may ask a separate question about that).

3) The solver seemed to take a long time to converge, and often failed to converge, particularly for higher frequencies and in-between eigenfrequencies, both of which make sense to me. I tried the ILUT preconditioner and it helped greatly, particularly for the complex option, which converges much faster with ILUT than the real option with ILUT.

Questions:
1) It would be great if anyone can check that my mesh and the configuration of the exciter patch body is correct.
2) I tried to add Rayleigh damping (just with nominal values alpha=beta=0.1) I dont see any effect. (I would expect to see smaller displacements at eigenfrequencies, larger displacements in between eigenfrequencies, and faster convergence?) Is Rayleigh damping implemented for the smitc model?
3) Can I have Elmer output the velocity field to the result file?

Thanks,
Paul

[pwray]

Some images of the mesh (I could not attach to original post)

Capture1.PNG (13.34 KiB) Viewed 459 times

Capture.PNG (34.99 KiB) Viewed 459 times

[kevinarden]

Questions:
1) It would be great if anyone can check that my mesh and the configuration of the exciter patch body is correct.
2) I tried to add Rayleigh damping (just with nominal values alpha=beta=0.1) I dont see any effect. (I would expect to see smaller displacements at eigenfrequencies, larger displacements in between eigenfrequencies, and faster convergence?) Is Rayleigh damping implemented for the smitc model?
3) Can I have Elmer output the velocity field to the result file?

1, linear triangles are not good for solid mechanical solutions, second order elements are necessary if triangles are used. This can be done in gmsh with 2nd order elements, or in elmer solver with Elements = "P:2"
2. Damping normally is not included in static or eigenvalue solutions, I think it only is included in transient solutions.
3. I do not think there is a velocity term in static or eigen value solutions. Transient has accelerations and velocity.

[pwray]

Thanks Kevin,

1) OK, I'll try recombination to use quads, or second order triangles.
2) I'm not attempting to use damping with Eigen. I just ran eigen first to see where the modal frequencies and see mode shapes. I thought damping should work for harmonic, otherise displacements are unrealistically large or even infinite?
3) Again, Im using steady state harmonic. I think that the model would need to calculate velocity & acceleration in order to output displacement?

Paul

[kevinarden]

You may have to turn on the complex eigen solver to account for damping?
viewtopic.php?p=27617&hilit=eigen+damping#p27617

[pwray]

Thanks Kevin
Ive been using the default (complex system) by commenting out:
!Linear System Complex = False

And strangely it converges faster than linear when using ILUT preconditioning. So maybe something not right about that?
I will double-check that complex IS the default, by trying exlicit "Linear System Complex = True"

[pwray]

Regarding damping:
I have an effect when I specify the plain
Damping = Real
With a complex system, but no sign that Rayleigh damping is doing anything.

Regarding preconditioner:
It seems specifying simply 'ILUT' is only applied to a complex system?
ILU 0 for example seems to work for both real or complex

[kevinarden]

I looked at the code and Rayleigh damping is not included in Smitc. It is included in the shellsolver.

"3) The solver seemed to take a long time to converge, and often failed to converge, particularly for higher frequencies and in-between eigenfrequencies, both of which make sense to me. I tried the ILUT preconditioner and it helped greatly, particularly for the complex option, which converges much faster with ILUT than the real option with ILUT."

for solid mechanics I try to use the direct solvers, they are faster and avoid having to converge. The draw back is that the problem has to fit in RAM. Mumps is the perferred on, but there is also banded and umfpack
Linear System Solver = Direct
Linear System Direct Method = Mumps

There is an iterative solver called gcr that sometimes works well with solid mechanics
Linear System Iterative Method = gcr

[pwray]

Thanks,

I tried to run an eigen analysis using shell solver with a simple clamped rectangular plate.
I'm not getting sensible results, there seems to be too many degrees of freedom (too many very similar mode shapes), and some look like random patterns in the cells. Im not sure either how the results are output to the vtu file, so I may be interpreting it wrongly. I tried a quad mesh I generated from with gmsh, and the regular mesh you posted with similar results.

I tried iterative and direct. I dont yet have mumps installed, but tried umfpack.
I looked at a couple of the eigenvalue tests, but maybe my simple 2D setup should be done slightly differently.

I have attached the sif file. Do you see the problem?

[kevinarden]

I did not see a problem with the sif. I will do some validation runs with plate and shell solver

Plate 0.8 x 0.8 E=70.9 v=.28 density=2712, hard clamped edges (all DOFs fixed) t=0.015
Closed form solution frequency = 205
NASTRAN ABAQUS
Mode Eigen Freq Eigen Freq
1 1.62686E6 203 1.664E6 205
2 6.70305E6 412 7.018E6 422
3 6.70305E6 412 7.018E6 422
4 1.41776E7 599 1.512E7 619
5 2.13733E7 736 2.321E7 768