Discrepancy between plate/shell/thin 3D solid

Please login with a confirmed email address before reporting spam

Hello, I am trying to do a very simple eigenfrequency analysis on a 17cm.17cm.25um plate. My material has E=4.95GPa, rho=1.38g/cm^3, nu=0.4. I tried using three different physics modules: - 2D plate (physics defined mesh, finer) - 3D shell (physics defined mesh, finer) - 3D solid mechanics (swept triangular mesh, finer, 10 elements in the thickness)

The two first models give very similar results, but the third one give different eigenfrequencies (11.49Hz insteads of 2.95Hz for the fundamental) Is this discrepancy commonly observed, due to the approximations made in the plate and shell modules or is it more likely due to an error in my model?

Thank you for any help!


3 Replies Last Post Mar 26, 2020, 5:09 PM EDT
Jeff Hiller COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 2 weeks ago Mar 25, 2020, 4:43 PM EDT
Updated: 2 weeks ago Mar 26, 2020, 8:55 AM EDT

Hi Juliette,

In addition to the approximations made by the shell and plate models, you should look at boundary conditions as a possible source of the difference. It's easy to make a model much stiffer/softer via BCs when you move from shell/plate to fully 3D. For instance, a shell BC of zero displacement and zero rotation is softer than zero displacement on the entire corresponding face in 3D.

Best,

Jeff

-------------------
Jeff Hiller
Hi Juliette, In addition to the approximations made by the shell and plate models, you should look at boundary conditions as a possible source of the difference. It's easy to make a model much stiffer/softer via BCs when you move from shell/plate to fully 3D. For instance, a shell BC of zero displacement and zero rotation is softer than zero displacement on the entire corresponding face in 3D. Best, Jeff

Henrik Sönnerlind COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 2 weeks ago Mar 26, 2020, 4:03 PM EDT

It may also be so that the solid model is ill-conditioned.

Given the size proportions, the solid elements will have a very bad aspect ratio unless you are running on a very big computer. If you want 10 elements in the thickness direction, I guess you would need something like 1 billion degrees of freedom in a solid model with acceptable mesh quality.

For an eigenfrequency analysis, it would however be sufficient with 1 element in the thickness direction, and then you could get through with 1 million degrees of freedom.

-------------------
Henrik Sönnerlind
COMSOL
It may also be so that the solid model is ill-conditioned. Given the size proportions, the solid elements will have a very bad aspect ratio unless you are running on a *very* big computer. If you want 10 elements in the thickness direction, I guess you would need something like 1 billion degrees of freedom in a solid model with acceptable mesh quality. For an eigenfrequency analysis, it would however be sufficient with 1 element in the thickness direction, and then you could get through with 1 million degrees of freedom.

Jeff Hiller COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 2 weeks ago Mar 26, 2020, 5:09 PM EDT
Updated: 2 weeks ago Mar 27, 2020, 8:34 AM EDT

Henrik is right on the money about ill-conditioning. I am attaching two models (shell and 3D solid) where I guessed that your BCs are all Fixed Constraints on the edges. Both models give around 2.96Hz for the first mode, as long as the 3D solid model is meshed finely enough in the plane before sweeping.

Best,

Jean-Francois (X94!)

-------------------
Jeff Hiller
Henrik is right on the money about ill-conditioning. I am attaching two models (shell and 3D solid) where I guessed that your BCs are all Fixed Constraints on the edges. Both models give around 2.96Hz for the first mode, as long as the 3D solid model is meshed finely enough in the plane before sweeping. Best, Jean-Francois (X94!)

Reply

Please read the discussion forum rules before posting.

Please log in to post a reply.

Note that while COMSOL employees may participate in the discussion forum, COMSOL® software users who are on-subscription should submit their questions via the Support Center for a more comprehensive response from the Technical Support team.