Discussion Closed This discussion was created more than 6 months ago and has been closed. To start a new discussion with a link back to this one, click here.
Discrepancy between plate/shell/thin 3D solid
Posted 25.03.2020, 16:07 GMT-4 Acoustics & Vibrations Version 5.4 5 Replies
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!
Please login with a confirmed email address before reporting spam
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
Please login with a confirmed email address before reporting spam
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
Please login with a confirmed email address before reporting spam
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
Attachments:
Please login with a confirmed email address before reporting spam
Thanks a lot to both of you! Problem solved indeed. I was not aware that the aspect ratio of the elements matters. Out of curiosity, why do we need elements with a not too high aspect ratio?
Best,
Juliette (X13!)
Please login with a confirmed email address before reporting spam
Hi Juliette,
For this particular analysis, COMSOL used the finite element method. With your material being isotropic, the stiffness matrix for an element with a very high aspect ratio will have some terms that are several orders of magnitude bigger than others. In layman's terms, this is similar to a sheet of paper: it's much stiffer in two directions than in the third. When the global stiffness matrix is assembled from all the elemenal stiffness matrix, you'll again have some terms that are much much larger than others, resulting in eigenvalues that span many orders of magnitude. Such matrices are referred to as ill-conditioned and, linear systems involving ill-conditioned matrices are very challenging to invert numerically, see for instance this page for a more in-depth discussion of ill-conditioning, and this blog post.
Best,
JF
-------------------Jeff Hiller