|Subject:||Re: [Getfem-users] Problem with Hertzian contact|
|Date:||Fri, 6 May 2022 12:53:29 +0200|
ah ok, I think I know what the issue is here. The Lagrange multiplier for imposing the contact condition corresponds to a 1st Piola Kirchhoff stress, while the analytical solution gives you the Cauchy stress. You can use Nanson's formula to convert between the two. In your model the Lagrange multiplier is like q in the upper left case of the following table:to convert this q to the equivalent one for the upper right case you need to postprocess your Lagrange multiplier and export the following quantity instead:"contact_mult/(Det(F)*Norm(Inv(F)'*Normal))"I hope it works.It is actually a good observation. I don't recall accounting for this difference in the presentation of the results in our paper from 2015, but maybe our meshes were too coarse to notice the difference, compared to your simulations.BRKostasOn Fri, May 6, 2022 at 11:52 AM David Danan <email@example.com> wrote:Dear Kostas,first, thank a lot for the feedback, the convergence is much cleaner now!Thanks also for sharing this script here, it contains several features i had never use so far, it's quite interesting/intriguing.However, i am afraid i did not properly explained what my issue was.Somehow, i was able to make the solver converge even without enabling some options for the solve and the result was qualitatively correct, as far as i could tell.But it turned out there is a large difference between the pressure predicted by the Hertz theory and the result i get and i was wondering whether i am doing something wrong. I tried to list the potential suspects in the first emailRegarding your remarks:-Yes,using a punctual load bother me a lot, which is why i wonder if i am supposed to do that to reproduce Hertz analytical case.-Regarding the unit, i wanted to stay in the small deformation assumption as i was not sure the analytical solution is supposed to hold for large deformation. Therefore, here, the Saint Venant Kirchhoff "becomes" a mere Hooke's law.Do you have any idea how to reproduce the analytical results?Thanks to your help regarding the parameters fiddling, i was at least able to reproduce a different case where there is no ponctual force (surfacic load instead) with a half-disk and a different analytical formula and...It worked (see the results enclosed for the pressure comparison on the contact boundary)!Before, it failed to converge. However, this formula is not really well documented at all, i would rather have a comparison with the classical formula.Thanks in advance for your help,David.PS: sorry for the duplicate, i forgot to put the mailing list in copy previouslyLe ven. 6 mai 2022 à 09:23, Konstantinos Poulios <firstname.lastname@example.org> a écrit :Dear David,With the attached script you should also be able to reproduce the results for the first example of our paper
https://www.sciencedirect.com/science/article/pii/S0045794915000656(the script is only slightly modified compared to the original one, so that it can run on python3 and the current version of GetFEM).Best regardsKonstantinosOn Fri, May 6, 2022 at 8:45 AM Konstantinos Poulios <email@example.com> wrote:Hi,Your script looks very nice and clean. It just needs a bit of fiddling with the augmentation parameter and the solver. The attached version produces this resultJust some general comments:- Point constraints/loads make almost never sense (unless you know beforehand the reaction force at a constrained point will be zero)- Maybe there is some issue with your units, I needed to increase the load to a very large value to get some visible deformations- The Saint-Venant Kirchhoff material law, that we often use for demonstrations, is a "toy" material law. If you do anything with moderate/large strains, use some proper hyperelastic law- The augmentation parameter should be in the same order of magnitude like the modulus of elasticity, from 1-2 orders of magnitude below to 1-2 orders of magnitude above.Best regardsKostasOn Thu, May 5, 2022 at 8:04 PM David Danan <firstname.lastname@example.org> wrote:Dear Getfem-users,My issue might be utterly simple, but i cannot find what i am doing wrong...I am trying to compare the solution provided by Getfem to the analytical solution of an Hertzian contact in 2D (namely, a deformable ball against a perfectly rigid plane) but, so far, i do not get correct results.Please, find enclosed my script. I use gmsh python api to generate the mesh but, if you do not want to use it, you can comment the line to generate the mesh in the script and juste use the mesh also enclosed.Here are some of my concerns:-Are the formula used in the script for the analytical contact pressure/contact surface area etc... correct in 2D?-Is it correct to use a punctual nodal force in such a case? Does it make sense in this context?-Is it correct to compare the analytical pressure to the lagrange multipliers?I have also tried to use a testcase provided in Code_Aster documentation and i got much better results, although not perfect but within the tolerance given in the documentation below.
https://www.code-aster.org/doc/default/en/man_v/v1/v1.01.246.pdfIt might be because these formula are for 3D only but i am not sure yet.Thanks in advance for your help,kind regards,David.
|[Prev in Thread]||Current Thread||[Next in Thread]|