CONTACT STRESSES 1

[meher634]

Dear FEA gurus,
I am performing contact stress analysis on an assmebly that has male and female mating parts (similar to dovetail joint). I made sure that mesh is good (most of the elements that are part of the contact area has aspect ratio close to 1 and meshed with brick elements).High contact stresses are always shown in one or two node locations. The adjacent elements have very low contact stresses. Thus there is local stress error at the highest stress location. Everytime i refine the mesh the contact stresses increases also the local stress errror increases very high with mesh refinement, I am not sure what the highest stress magnitude is ? should that be the highest stress node location or the location where the stresses are almost average. Please let me know.
many Thanks.
meher

 

[prost]

My guess is that you have a singularity, as the stresses at this point around which you are refining the mesh show a continuously increasing stress--this observed behavior is normally symptomatic of a stress singularity. Is this node fixed in space, perhaps? Or is the node on one body collocated with a node on the other body, and the boundary conditions are set up so that one node follows the other? This would be a problem if one body wants to deform so that those two collocated nodes should be sliding tangentially relative to each other.

 

[GregLocock]

Does your contact model use an exponential stiffness? if so have you set that to a sensible value?

Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[corus]

It sounds like point contact is being made and so a load through zero area gives infinite stress. In practice this point would yield and the contact stresses would be spread about more.

corus

 

[prost]

This is very interesting concept--what is an 'exponential stiffness'?

 

[Kwan]

do you have all bricks? Check in the location of the problem for tets. I suspect you have irregular stiffness due to the mesh.

 

[GregLocock]

I haven't used a contact model in FEA, so I'm not sure how they cope, but basically there is a dynamic instability as the two surfaces contact, if you use a linear elasticity model. So, to get around that, most lumped contact algorithms use an exponential (Hertzian) stiffness model.



Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[corus]

I think exponential stiffness in contact provides a 'soft' contact rather than 'hard' contact. Some algorithms also use soft springs to help with any instability that you might get from 'chattering' at the contact faces.

corus

 

[sr11]

Maybe you just using a wrong software, incapable of performing contact stress analysis.
Some time ago I have had a similar problem in calculating contact (Hertz) stress in Algor. It simply did not support contact stress calculations.
Ansys, on the other hand gave me good correlation between FEA results of Contact Stress and expected theoretical values (for typical cases). It uses special target and node-to-surface contact elements.
Check out “Disks in Point Contact “ example from Cornell University:

http://instruct1.cit.cornell.edu/courses/ansys/contact/index.htm.

 

[gio1]

You say "most of the elements that are part of the contact area has aspect ratio close to 1 and meshed with brick elements". Are they ALL brick elements (on the whole surface of both sides)? If so, are they 8 or 20 nodes brick?

The element formulation is crucial when it comes to stress recovery in contact analyses. Try looking at the manuals of your software (what are you using?) to find out whether the elements you use are recommended for contact analyses.

As Greg mentioned, there are chances that your contact model is using an exponential pressure-closure curve. If this is the case I would revert to a standard "hard contact" model (although this will make convergence harder).

Finally, stresses are more accurate if a surface to surface algorithm is used. Use it if you can.

Cheers

Gio1

 

[alberto78]

Hello guys, I'm a new member of this forum and I'm trying to give an answer to this question:
what is the maximum allowable Hertz contact stress for a steel with 520MPa of yield strength?
Thanks to all.

Alberto

 

[gio1]

Alberto,

Please remember to start a new thread if you want to discuss a different topic.

As for your question, the maximum allowable contact stress is not so related to yield strength as much as to surface hardness, which in turn depends on the treatment/coating process that the metal has undergone.

Cheers
Gio1

 

[cbrn]

Hi,
the contact problem of the O.P. is in fact very common even with the most sophisticated FE programs. Let's first suppose that it's a numerical overshoot and not a "real" structural contact stress hot-spot: it may be encountered if the position of a gaussian node on the target almost exactly coincides with (and follows) the position of a gaussian node on the contact: despite surface/surface formulation, if this happens, locally the contact will become like point-to-point and the stiffness will have a singularity.
Let's suppose now that it's not a numerical overshoot: if the calculation is made in the linear field, contact stiffness is estimated at the start of the calc and then never updated. This can lead to very bad results in many cases, especially when the contact involves a small contact area on a large target surface. Unfortunately, some FE programs have no other way to calculate contact stiffness. As an example, instead, in Ansys you can choose to update the contact stiffness at each equilibrium iteration inside the same time-step.
As regards algorithms to determine this stiffness, yes, there are several and the choice is not really simple, involving in most cases a "good balance" btw convergence rate and precision (dealing with inter-element compenetration which of course is absolutely not physical!): pure-penalty based algorythms are simple to set up but give (very) unprecise results when the contact is not purely-normal (i.e. has a considerable "tilting" tendency); augmented-Lagrange algorithms instead are far more controllable but require to specify tolerances for the compenetration and the normal stiffness.
As far as I knew, "exponential transition" is refered to the way in which the tangential static friction is transitioned to the dynamic friction, as soon as the two surfaces that are in contact begin to slide. But GregLocock and others use it with another meaning, i.e. "exponential" seems to be refered to the law "contact load - vs - closure". Is it right? I personally wouldn't know how to correctly set the params for a contact law like that, since in the FE I use the contact stiffness is elaborated from the constitutional laws of the elements, where the reactions of the contact-elems and of the target-elems mutually influence each other.

Regards

 

[alberto78]

First of all thanks for the answers, I made a check to verify the steel hardness:
it is 192 HB (207 HV), having a tensile strength of 655MPa.
The Hertzian stresses I've found in the F.E.A. are very high,
but considering that I used a very fine mesh, I think that results could be realistic, (and quite supported by the Hertzian theory).
Are 1850MPa of contact pressure too much for my steel?

Best regards

 

[cbrn]

Hi,
as surface stress, generally it is accepted to consider a maximum resistance equal to the average btw yield stress and ultimate strength, unless you have stricter specifications or other requirements (e.g. if you have to turn an hex-nut over a surface, you can not overcome yield or you won't be able to turn any more).
Perhaps, but not sure, on MaterialScience or somewhere like that you can find this kind of info, which unfortunately is not very common.