Discussion Forum

Hi

that depends on your model, if you have a stress concentration point you can get such increase of maximum value with the mesh density. This typically appears at corners or with point or edge loads in 3D.
try to use only domain and boundary loads, and implement small fillets to all edges, normally you should then not get any of these stress concetration locations (somewhat model dependnet though)

Anyhow, stress concentration does not mean, necessarily, that the rest of the model is wrong, it could be limited to a small region

This is the FEM world one must know/learn and master (and it's version independent !)

--
Good luck
Ivar

Hi everybody,

I have the same issue regarding the von mises stress and the mesh sensitivity.

Thanks for your answer, Ivar, but it is a bit frustrating... It would mean that the maximal von mises stress has no interest (because it depends on the mesh).

However, it is usually used as a failure criterium. (if the VM stress is larger than XXX, we have failure), so what is the solution?

Kind regards,

Patrick

Hi

You should not really be too frustrated for solid and von Mises stres:s you get to a saturation if you have a "smooth" shape

take a look ;)

It's different (worse) for ACDC and sharp corners ...
--
Good luck
Ivar

Hi Ivar,

thanks for your kind answer and your example. May we conclude that the maximal von mises stress cannot be properly evaluated, when there is an right (or sharp) angle?

I have to make a sensitivity analysis. The objective function is the max. of the von mises stress, and the parameters that can change are geometrical ones. The max. is located in edge that cannot be transformed into fillet (please, see the mph file to see why)

I have tried the following options, but without success:
-) recover
-) plot at the Gauss point

Does it make sense to make such a study? Would it be another mechanical criterion (principal stress for example?) which would be less sensitive to the mesh?

thanks a lot,

Kind regards,

Patrick

When it comes to a singularity all stress and strain measures should blow-up. You should either check away from the singularity, smooth the geometry, or allow some local plasticity (which will lower your stresses).

Keep in mind however that not all sharp corners are singularities. Some singularities are a result of modeling errors/assumptions. In your model for example the highest stress region is a singularity only because you fix the bottom surface of the plate in all directions. If the plate is fixed elsewhere or the face that you fixed is only constrained in the Z-direction then you should have no singularity there.

Nagi Elabbasi
Veryst Engineering

Dear Nagi,

thanks for your precious answer.

I totally agree with you when you say that the plasticity would lower the mecahnical stress. In fact, I only want to know if the structure would enter locally into plasticity or not. Therefoire, I do not need to consider the plasticity during the computation. I only need to check the maximal von mises stress, and to compare it (in postprocessing) to the yield stress...

Thanks for your remark about the importance of the modeling assumption. When I change the Z_constraint from a boundary constraint to a point constraint, it changes the location of the maximum of the VM stress, but it is still in a sharp angle, so the problem is only ''translated''.

Do you see any way to know the correct value of the VM stress in this point? As you can see in the .mph file, we can not unfortunately smooth the geometry there..

Thanks for your help!
Kind regards,

Patrick

Hi

you could make your stem round and not square, or at least with filleted angles. That will help somewhat.

Then play with the mesh density in the critical region, try a 1:2:4 ratio and see how the max vM value changes (based on the plot and colour ruler not on the absolute "max" value.

You should also check the plot with "Quality: No refinement, Smoothing: None" it gives you a better view of the mesh and related stress values

But even FEM is no "absolute science, absolute precision" some good engineering guesses are required here too ;)

--
Good luck
Ivar

Thanks everyone for your participation.

As you recommanded, I have only plotted the area where solid.mises were larger than the yield stress, and I decided to check if this quantity appears only near the singularities (in 2D) or in a volume (in 3D)

The resulting estimator is not mesh dependent anymore!

kind regards,

Patrick

Hi,

Wow, it post had a great dicussion on mesh convergence which I gain a lot of benefit and knowledge.
Thanks for sharing.

At the initial stage, I used 2-D Free Mesh Parameter to solve for the von Mises stress, It end up no convergence result as the stress value getting bigger and bigger. Things goes better when I used Mapped mesh parameter, by increase the edge element, the stress value seem not so mesh dependent anymore.

Any comment toward this? May I know what method does Patrick used for solving?

Thanks.

Regards,
PS

Hi Xsu,

I am glad you took benefit from our previous conversation!

Regarding the convergence when refining the mesh, I had no convergence when I look at the maximum value of the von Mises stress, even if I used Mapped or structured meshes (prism/tetra/quad..). That is the reason why I had decided to have a "volume approach" instead of having a "maximum approach". But your result is very good for you!

You ask me the method I used to solve.. Could you be more precise? Do you want to know the linear solver (PARDISO is the best, ever, on a workstation)? the damping parameter? ...

Send me your model if you want me to have a look!

Kind regards,

Patrick

Hi,

Thanks and very appreciate Patrick for your time and your kind offer in model visualizing.
My value converge when I use cross section plot parameter to visualise my von Mises stress value.
I previously observe my Max von Mises stress value from plot parameter>>max/min, the stress value is getting bigger and bigger (Initial stage).

I only deal with simple 2-D model to visualise the contact force exerted to the membrane deflection,by utilsing SPOOLS for my system solver. Thanks for your information that PARDISO is a very nice solver for workstation.
I am going to have a try on PARDISO to check the result whether it varies for both solver. Actually my intention is to know your method in getting the stress converging, where you had mention with volume approach idea.

Warmest Regards,
PS

Hi all,

I need a guidance on the following problem. It is a pressurized spherical vessel (of radius Rv) with nozzle attachment of radius Rn. I need to use two approaches (the shell and solid element in comsol) to get variation of stresses (inner and outer hoop and axial/meridional). The shell solution works perfectly for me, having used 3D model (see attachment (a)). However, results of the stress variations along the indicated edges (in color) of the vessel and nozzle show singularity problem at the juncture when a 2D axisymmetric solid model (attachment (b)) is used. I used fillets to get away with this problem but it doesn't work well; different results (Fig. c) are obtained from those of the shell model (Fig. d). I'm using version 4.3a in my work. I would appreciate your kind help on this.

Thanks