Contact Pressure diverges when mesh on slave surface is refined

[coolFL]

Hello everyone,

I am trying to solve one contact problem of two axisymmetric geometries. The (zipped) .cae file of the model is attached. Issue is: stresses in the direction normal to applied load are under-predicted in the subsurface region just below the contact. Also, the contact pressure values diverge from true analytical solution as mesh on slave surface is refined. Can somebody please guide me on where am I going wrong? Any suggestions would be highly appreciated.
Thanks in advance,

Nik

 

[StefCon]

Hello,
I don't have CAE installed so I cannot look at the model.

Do you have surface smoothing active? It could help.

If you haven't seen this document yet, have a look. It might give you some ideas.
[URL unfurl="true"]http://marketing.intrinsys.co.uk/CONTACT_SEMINAR.pdf[/url]

 

[coolFL]

Yes, surface smoothening is active.

 

[StefCon]

Hmmm,
What elements are you using? If you send an input file I can maybe have a look.

/S

 

[kukogoba]

Linear elements please, don´t use quadratic elements with contacts.

 

[kukogoba]

In order to improve the convergence, you can active the contact control.
But then you must make sure that the energy disipated is under 5% more or less. ALLIE vs ALLSE

 

[coolFL]

.inp file of the model is attached. Theory predicts contact Pressure is 1081 MPa for this model. In FEA closest that I could get was 1121 MPa, with 2nd order quad elements. This means error of 3.7%. All other elements predict CPRESS with higher error. Also, as per Abaqus manual 2nd order elements are fine with surface to surface (Finite Sliding) discretization hence I am using them. This error of 3.7% keeps on increasing as the applied load on the model is increased. I couldn't figure out its source. Hope you guys can help me to fix this!
Also, I tried contact controls approach (with very little damping factor so as not to alter the Physics of the model) it was of very little help.
Any guidance on this issue would be highly appreciated,
Thank you in advance,

Nik

 

[IceBreakerSours]

a) Second order elements are NOT recommended to be used when contact is in the picture. In addition to some modeling tricks, there are *modified* quadratic elements that allow you to model contact reasonably well in some situations but, in general, you want to use linear elements anytime there is an interaction.

b) Increasing the load for a certain spatial discretization is changing the problem at hand. You might want to read about mesh convergence.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[kukogoba]

Hey CoolFL, i´ve seen the .cae you uploaded, i´m quite new doing FEM analysis but, so... if you want you can take my advice, or wait to another answer.
Some recomendations i have learned working hard xDDD:
Change initial incremet size to 0,01 and maximun to 0,1.
I don´t know which units are you using, but i thing that you have chosen distance in milimeters and force in N. So... the mass would be in Tons and the pressure in MPa. Corect me if i´m wrong.
The density of the steel is 7,8E-9, not 7,8 E-6, put for the static analysis i think that it is useless and the energy is mJ.
I have achieved the convergence very easily with those changes. I think that your problem is nummerical, due to a very big time increment.

 

[coolFL]

Hey kukogoba,
can you please tell how much contact pressure did you achieve? In the analysis that I am doing accuracy is more important.
Thanks again,

 

[kukogoba]

For which model?

 

[coolFL]

for the .inp file that I uploaded above. If you have simulated above .inp file with initial increment of 0.01 and maximum increment of 0.1, then I am curious to know how much maximum contact pressure did you obtain?

 

[kukogoba]

yes, but you have 7 models.

 

[StefCon]

Making mesh equally dense on both contact surfaces might help.
Also improving element quality at the contact boundary (close to perfect squares).
Contact adjustment might remove some numerical problems (initial overclosure), or even better, separate contacts at analysis start and then move them into contact.

Please report back if you find the answer!

 

[coolFL]

Dear StefCon,
Thanks for your suggestions!
I tried equally dense mesh on both contact surfaces and close to perfect square elements. I also automatically adjusted slave surface for initial over closures. But I am not familiar with the last approach that is to separate contact at analysis start and then move them into contact. Is there any specific control/option for this? Please let me know.

Dear kukogoba,
I am referring to Model with the name: 2mm_Q=4500_Run_57

Thanks to both for your assistance in this matter,

Cheers!

 

[StefCon]

Hello again,
I was just thinking that you could move the part in the assembly and then use a boundary condition to move them into contact. Overclosure adjustment might change the shape a little. It was just a suggestion.

This is an interesting topic. Let me/us know of your findings. A certain error is to be expected. Your results aren't that bad imo.

Just a thought: Were you using a symmetry boundary condition? I know contact pressures are strange at the symmetry boundary. I tried once and I got really confused and started doing an averaging of a small area instead. Are you looking at the contour plot or nodal values? In CAE you can change the results averaging (default 75%). Anyway, good luck!