"No penetration" error 1

[xhbg]

Hi,

I have a question. There are 2 metal parts in my model separated by a layer of elastic. Even thought I set "no penetration" (surface to surface) between each surface of the metal parts with each surface at both sides of the elastic part, and also between the two surfaces of the metal parts, the result still shows the two metal parts even go through the elastic layer and penetrating into each other. Why does this happen and is there anyway to solve this problem? Is it because of the setting or this is a software issue?

I am using CosmosWorks Professional 2006, Service Pack 4.1.

Your help would be greatly appreciated. Thank you so much in advance.

xhbg

 

[cbrn]

Hi,
I don't know exactly how the "contact" settings are in CW 2006, because I stopped using it when it was v. 2004, but here's some general consideration:
1- "No penetration" refers to the algorithmic behaviour of the surf-surf contact; it doesn't mean that the solver will not calculate ANY mutual penetration: in fact, this depends upon the parameters of the materials and of the contact itself. In v.2004 there was no way to properly control the behaviour of a contact, you had to rely on the software. I believe it used some kind of pure-penalty calculation method, where the intrinsic contact stiffness was evaluated once at the solution start, and then never updated (thus leading to a linear analysis). If it is still the case, then the stiffness calculated in undeformed position will lead to very bad results in case of strongly non-linear materials, as in your case; the best you could do would be to shift to a non-linear analysis where contact params would be updated at every iteration (if possible with CW 2006)
2- If the penetration you see is merely "visual", be careful to the displacement magnification scale!!! It may make you see enormous penetrations where in reality the software calculated only microns or fractions of micron.
3- Bear in mind that a small amount of penetration is perfectly admissible: it only should be one order of magnitude smaller than the calculated deformation or the calculated contact gap (if any). Forcing the contact parameters in order to approach "zero-penetration" will lead to more and more realistic simulations but at the expense of numerical instability problems (slow convergence, chattering, etc...). It's up to you to find the correct balance between speed of the simulation and "realism".

Hope this helps...

Regards

 

[xhbg]

Thanks, cbrn!
1) So you meant because I run the model in linear range that could cause the problem? But I did try to activate the large displacement flag to enable non-linear analysis, the analysis fails at about 28%. I save the result up to that point but the result image I get is not much better....How to solve it without activating large displacement?
2)I did change it to the scale of 1, but it stil shows penetration.
3)How small of penetration is allowed? How can we calculate the percentage?
I do appreciate your help. Once again, thank you.

 

[cbrn]

Hi Xhbg,

2) OK, so you're not misled by false visualization. I don't know if in CW 2006 you can plot contact penetration: if so, you'd better plot that instead of deformation / displacement, in order to have a better understanding of the real values of the computed algorithmic penetration

1) No, no, penetration will occur anyway, be it in linear or non-linear analysis. As I previously tried to explain (but perhaps I wasn't very clear... This matter is a bit complicated and I don't know if the CW manual explains it very well), it's due to the algorithmic computation of the contact parameters. At a certain point, there is a balance between convergence rate and surface stiffness: an infinite surface stiffness would lead to zero penetration even with infinite contact pressure, but at the expense of very slow convergence (or even mis-convergence). To be more complex, you might choose to evaluate the surface stiffness only at the beginning of the analysis (thus remaining in a linear analysis), or have the solver update it at every equilibrium iteration (most precise but most resource-expensive) or at least at each timestep. But the "sine qua non" condition is that the program must offer you this setting: in v.2004, it was not possible.
In your case, the non-linearity doesn't come from not respecting the small displacement hypothesis, but from the material behaviour. You have to define a non-linear material. Then, in v.2004 you had to shift to Cosmos-M (it was automatic: the Cosmos-M interface and solver would be called each time a non-linear analysis would be needed); I don't know if in newer versions the full non-linear capability has been embedded inside CW or not.

3- You can consider that as long as contact penetration is one order of magnitude smaller than the deformations or the gaps, you can consider it acceptable. But in order to be sure of it, you have to output the penetration values, if you can. Otherwise, you have to "visually" estimate the max penetration value and compare it to the deformation or the gap. Or, otherwise, completely ignore the problem... No, no, I'm joking !!!

Hope this helps...

Regards