Big Difference in Eigenfreq calculated by COMSOL and Elmer

[lennart0901]

Hello everybody,
we are trying to simulate AFM-Cantilevers using Elmer.
A colleague created the attached net using COMSOL and
we calculated the smallest 5 Eigenfreqencies with it
in COMSOL and Elmer with the following Parameters

Young's modulus: 131E9[Pa]
Density: 2330[kg/m^3]
Poisson's ratio: 0.27

Boundary 1: fixed

in COMSOL we got as frequencies:
145.91304727792047
851.6402470717361
905.067362125763
1447.0501932487887
2494.210141372177

in Elmer:
164.533047139
856.891973312
1047.94320206
1766.8530061
2894.73324964

The mphtxt,sif and the mph can be found in my dropbox:

mphtxt: http://dl.dropbox.com/u/14298064/simple ... esh.mphtxt
sif: http://dl.dropbox.com/u/14298064/case.sif
mph: http://dl.dropbox.com/u/14298064/simplereed.mph

I have no idea where those big differences can come from perhaps you can help me

regards Lennart Fricke

[raback]

Hi

Wild guess: Comsol uses sometimes internally second order elements but the .mphtxt file only includes the definition of linear ones. Therefore the lower order elements in Elmer result to 'locking' which gives higher eigenfreqs.

-Peter

[lennart0901]

You seem to be right. When I select linear elements in COMSOL I get exactly the same results as in Elmer.
Is there a way to tell Elmer that the default element type is quadratic?

[raback]

Hi

Elmer supports p-elements that might be specified on the command file. However, normal nodal elements need to be defined on the mesh already. You could do like this

Code: Select all

ElmerGrid 2 2 mesh_linear -increase -out mesh_quadratic

and change in the sif file the directory correspondingly. Note that the GUI sets the directory to be just "." so you might have to make the directory and place the mesh.* files in there.

A second alterbative might be to give the "-increase" directly when reading in the file in ElmerGrid or in ElmerGUI (ElmerGrid option line).

Note that when nodes are added this way the possible curved boundaries of the initial geometry cannot be honored. The "-increase" flag might also not work for some elementtypes.

-Peter

[lennart0901]

Hello,

thank you very much. So I believe the best way is to generate the mesh by myself as comsol's export does not differ when I export a mesh with linear or quadratic elements.

Regards Lennart