structure frequency responses under vibration forces

[alexbrown]

Hi Mika,

Many thanks for the kind advice. I checked the results from facetshell solver, its results match with comercial software.

Do you know how can use the facet shell for harmonic analysis? I used the attached sif file trying to analysis an plate under harmonic forces (applied through loads), but the results are all zero.

There exists an old and undocumented facet shell solver (FacetShellSolve) which utilizes drilling DOFs. While it's known that the facet shell elements may generally be unreliable (no convergence to solutions which a proper shell theory predicts, which gave a motivation to write a new shell solver), in the case of geometries consisting of just planar patches good results might however be possible (convergence failure needs a curved mid-surface).

I checked the first eigenvalues of a beam which has an L-shaped cross section and which is fixed at one end by using a facet shell model

facet-L.png

and a 3D solid model

solid-L.png

The solid model gives

EigenSolve: Computed 10 Eigen Values
EigenSolve: --------------------------------
EigenSolve: 1: 1.319919E+03 0.000000E+00
EigenSolve: 2: 4.496784E+03 0.000000E+00
EigenSolve: 3: 5.081996E+04 0.000000E+00
EigenSolve: 4: 5.499638E+04 0.000000E+00
EigenSolve: 5: 1.509114E+05 0.000000E+00
EigenSolve: 6: 3.854250E+05 0.000000E+00
EigenSolve: 7: 5.035877E+05 0.000000E+00
EigenSolve: 8: 8.492267E+05 0.000000E+00
EigenSolve: 9: 1.406722E+06 0.000000E+00
EigenSolve: 10: 1.531419E+06 0.000000E+00
EigenSolve: --------------------------------

while the facet shell solver outputs

EigenSolve: Computed 10 Eigen Values
EigenSolve: --------------------------------
EigenSolve: 1: 1.216743E+03 0.000000E+00
EigenSolve: 2: 4.464833E+03 0.000000E+00
EigenSolve: 3: 4.679074E+04 0.000000E+00
EigenSolve: 4: 5.240912E+04 0.000000E+00
EigenSolve: 5: 1.466158E+05 0.000000E+00
EigenSolve: 6: 3.541928E+05 0.000000E+00
EigenSolve: 7: 4.769901E+05 0.000000E+00
EigenSolve: 8: 8.113645E+05 0.000000E+00
EigenSolve: 9: 1.278976E+06 0.000000E+00
EigenSolve: 10: 1.411605E+06 0.000000E+00
EigenSolve: --------------------------------

There seems to be quite good agreement of the eigenvalues, so perhaps you could try a facet model for a box. For an example case in the tests directory see the test FacetShell2.

-- Mika

[mika]

I think the limitation is again the inability to define an imaginary part of the load (to have this possible some structural solvers would need simple modifications which still wait). Otherwise the facet shell solver might work. I started from the test case PlatesHarmonic and modified it as in the attachment in order to use the facet shell solver with a real-valued point load. This gives a non-zero solution at least.

[alexbrown]

Hi Mika,

This can give a non-zero results, but the displacement is the same under all frequencies. I assume the harmonic analysis is not carried out, is that correct?

Do we have a verified shell solver examples that can carry out harmonic analysis? it seems the solver is not very stable.

I think the limitation is again the inability to define an imaginary part of the load (to have this possible some structural solvers would need simple modifications which still wait). Otherwise the facet shell solver might work. I started from the test case PlatesHarmonic and modified it as in the attachment in order to use the facet shell solver with a real-valued point load. This gives a non-zero solution at least.

[mika]

I see, with the "Harmonic Mode" keyword the frequency must be given in the solver section, so change the place of "Frequency" command. "Harmonic Mode" is not a very old option and hasn't probably been tested in all possible settings in a thorough manner. Some test problems have been solved to verify the eigenanalysis results of shells. The harmonic analysis is built on the same ingredients as eigenanalysis, so if there are nevertheless mistakes they are hopefully relatively easy to correct.

-- Mika

[alexbrown]

Thanks, Mika. Another question, for shell with beam analysis, can the FacetShell also be used or only shell solver is supported?

I see, with the "Harmonic Mode" keyword the frequency must be given in the solver section, so change the place of "Frequency" command. "Harmonic Mode" is not a very old option and hasn't probably been tested in all possible settings in a thorough manner. Some test problems have been solved to verify the eigenanalysis results of shells. The harmonic analysis is built on the same ingredients as eigenanalysis, so if there are nevertheless mistakes they are hopefully relatively easy to correct.

-- Mika

[mika]

The assembly of beam sections was added into the shell solver only, so the facet shell solver doesn't understand beam sections.

-- Mika

[alexbrown]

Hi Mika,

I updated the sif file as attached (moved the frequency command to the solver section), but it seems the results is still not changing under different frequencies.

Do you know what the reason may be?

The assembly of beam sections was added into the shell solver only, so the facet shell solver doesn't understand beam sections.

-- Mika

[mika]

You are right. The facet shell solver wasn't updated to assemble the mass matrix when "Harmonic Mode" = True. This is now fixed in the devel repository. At the minimum FacetShellSolve.F90 has to be recompiled in order to try again.

-- Mika

[alexbrown]

I recompiled the FacetShellSolve.F90 file, the result is at least changing under different frequencies.

As the shell solver doens't seems to give correct results for eigen analysis and harmonic anlaysis, will you consider to update the facet shell solver to make it can couple with beam section and solid elements?

Another question, how to set the damping value of the harmonic analysis?

You are right. The facet shell solver wasn't updated to assemble the mass matrix when "Harmonic Mode" = True. This is now fixed in the devel repository. At the minimum FacetShellSolve.F90 has to be recompiled in order to try again.

-- Mika

[mika]

Another question, how to set the damping value of the harmonic analysis?

I just updated the source codes of both shell solvers in order to enable mass-proportional damping. If the material section has the command

Rayleigh Damping Alpha = Real ...

the solver should now create a damping matrix D = alpha * M, with M being the mass matrix. I didn't have time to run any shell case with damping, but in principle this should work after recompilation.

I nevertheless hesitate over how much time I'm willing to spend developing the facet shell solver, since the analysis presented in the article

Bernadou, M, Trouve, P. Approximation of general shell problems by flat plate elements. Part 2: Addition of a drilling degree of freedom. Comput. Mech., 6 , 359–378 (1990)

gives a good reason to think that for general shells the facet finite element approach gives curvature-dependent errors which cannot be reduced by refining the mesh. The article proposes a perturbation term and a way to estimate the shell curvatures to get rid of this error, but the facet shell solver of Elmer doesn't try to add such a modification. Moreover, the plate formulation used in Elmer is different from that used in the article, so one should perhaps do some maths to find an appropriate perturbation term for the Reissner-Mindlin model. I believe there are better approaches to general shell problems.

As the shell solver doens't seems to give correct results for eigen analysis

What makes you think that switching to eigenanalysis makes the solution obtained with the shell solver incorrect? There are some verification cases where the results of shell eigenanalysis has been compared with results given in literature, obtained with commercial software or given by other models of the same problem

https://github.com/ElmerCSC/elmerfem/tr ... s_Cylinder
https://github.com/ElmerCSC/elmerfem/tr ... _Spherical
https://github.com/ElmerCSC/elmerfem/tr ... enanalysis

If wrong results are obtained, I doubt the root reason may not be that the solution type is selected to be eigenanalysis, but something else.

A non-traditional feature of the (newer) shell solver of Elmer is that it models the straining in the normal direction. Unfortunately the normal strain is a difficult concept when the director data makes large jumps. It has now become known that the discontinuities in the director data would need some special treatment to get the equations right. Hopefully we can improve this somehow in future, so that this wouldn't be a cause for opting for the otherwise doubtful facet shell model.

On the other hand, the ability of the shell solver to model normal strain makes the coupling with solid elements more straightforward and we have recently developed some functionality related to such coupling. In addition to the test Shell_with_Solid_Eigenanalysis, other tests related to this option are

https://github.com/ElmerCSC/elmerfem/tr ... hmarkCase1
https://github.com/ElmerCSC/elmerfem/tr ... hmarkCase2
https://github.com/ElmerCSC/elmerfem/tr ... Solid_Beam
https://github.com/ElmerCSC/elmerfem/tr ... Beam_Eigen

I'm afraid trying to repeat these coupling tests with the facet shell solver would require more than a quick modification of the code. Adding beam sections would be an easier task by making some additional modularization. Nevertheless, with very limited resources it would be ideal to put efforts to developing one shell solver rather than sharing the work between two solvers. Perhaps this is an ideal thought as in some cases it might be nice to have an option to use solid shell elements (very special 3-D finite elements) and this would be a third approach.

-- Mika