Mesh Convergence 3

[agdyp]

Dear Friends,

I am trying to find out if the mesh refinement in the area of interest is good enough to give me good results.

This is what I tried initially. I ran the model with a reasonably refined mesh in region of interest. I noted 1) max equivalent stress and 2) the average stress in that area (by exporting result in excel). Then I refined the mesh in the area of interest and again ran the solution. Again I made a note of the above 2 results. I repeated this for 3 times, each time refining more and more in area of interest.

I observed that the max equivalent stress keeps on rising (RAPIDLY). The contact region where that max equivalent stress occurs is a line contact.

I have also tried using mesh convergence scoped to area of interest but due to a huge % change in stress this did not help.

Could you please advice how I could verify my mesh convergence?

Thank you.

BR,

agdyp

 

[Stringmaker]

Agdyp,
If your contact surface is a line then it only makes sense that your constact stress continues to rise as the mesh is refined. By definition a line is not a two dimensional quantity however your output of the analysis, stress, is. In real life everything has nonzero length; be it in your case very small. You have two options as I see it:

a) You can model the exact geometry (i.e. the line must be translated into an area having length and width) and use a suitable mesh.

b) Use a closed form solution an applicable is one available.

Just my thoughts...perhaps a little better explanation of what you're trying to do exactly is in order.

 

[agdyp]

Thanks for your response. The contact is between a concave surface and a convex surface. So, it is a line contact. I agree that the theoretical stresses will be infinite due to this. But then, is there any other way to analyze this except by creating an area contact.
I am not aware of the closed form solution that you mentioned. Could you please elaborte on this?
Thanks again.

Agdyp

 

[Stringmaker]

This is not a case of line contact. The contact area, while small, does exist. The stress present at the contact is called Hertzian stress and does contain a closed form solution. I would either look in a copy of Roark's or get a good machine design book (Shigley?) and you should have no problems finding the proper formulas for your case in there. Or try searching the web. Analysis should not be necessary from the description you've provided here.

 

[cbrn]

Hi,
100% agree w/ Stringmaker. Your case is indeed a surface-to-surface contact, it doesn't matter if ideally you can think of it as being "concentrated" on a line.
Roark-Young has a very good section about Hertzian contacts. Anyway, you shouldn't have any problem in setting up a surf-surf contact pair in Ansys.

Regards

 

[agdyp]

Dear Friends,

Thank you for your responses. I am still trying to find out if my mesh is refined enough to give good results. I am also trying to use the mesh convergence in the area of interest, which is a fillet. I'm seeing that as the mesh is refined more and more the % error increases. At fairly coarse mesh I get 10% error, whereas with finer mesh I get 40% error. Why is there such a big difference? This fillet is not even in direct contact with the other mating part. Am I dealing with singularity issues even while working with fillet? Could you please give me some feedback?

Another relatively easy question I have is how to update the mesh, once mesh convergence has been achieved using the convergence tool. In other words, when I look at the convergence table in the results, I see different number of elements and nodes AS compared with what I see by clicking on 'Mesh' and looking into the details.

Thanks.

 

[gurmeet2003]

agdyp,
Antoher possibility is to use non-linear material properties and include the effect of yielding. I am guessing that with a line contact your sresses must by exceeding yielding. If so when you include the effect of yielding, the contact area will automatically enlarge and stresses will reduce to reasonable values. Then if you try mesh convergence it will give you better results.

Of course the run time will increase when you go non-linear.

Gurmeeet

 

[cbrn]

Hi,
possibly the solution time won't increase at all because the solution is set to non-linear by default when contacts are involved (of any kind), because as you can understand contact phenomena are non-linear by definition.
There are also a few things to control in the contact's properties:
- make sure "update stiffness" is set to "each equilibrium iteration": especially in cases of very "concentrated" contacts, this can increase the accuracy by incredible amounts!
- make sure that the contact stiffness is not "forced" to be too high because of a manual choice of Normal Stiffness
- if the solution is achieved with too high a max Penetration, that means that this solution is equilibrated but "unphysical": at the expense of some more risk of mis-convergence, set the "Penetration Tolerance" to a sensible "manual" value.

Regards