Contact Analysis - Thermally Preloaded Ubolt and tube 1

[cspkumar]

Hello,

I have a convergence problem with my contact model.

I have a Ubolt (Solid185) which is wrapped around a tube (Shell 181) (modeled such as the bottom inner node of the Ubolt has almost no penetration/gap with the bottom node on the tube).

No separation contact is used because the bolt may slide with applied preload. Tube is target (Targ170) & Ubolt is contact (Conta173).

Even though I have a fine mesh on my Ubolt, I still have a 1e-2 penetration at a location away from the bottom, maybe due to the facets. I used Keyopt(9)=1, exclude penetration/gap.

Preload: I keep applying a thermal load to the Ubolt
(E=0.288e8,alpha=0.45e-4) until I obtain the desired contact force (46000 lbs)at the flange. Bolt/Flange is bonded contact.

The model converges if the thermal load is small but does not at large loads (-1200). The max stress point is at the node which had the max penetration of 1e-2.

My questions---
1) Which keyopt should I use in this case so that I don't have a penetration due to the facets?
2) Any other tips or suggestions that will help the model converge?


Regards,
cspkumar

 

[meshparts]

I have done contact simulations about 2 years ago. What I can remember is, that if too many nodes have initial contact, then convergence is difficult. So you have to choose at the beginning of the simulation very, very small time steps, or else the contact force will vary to rapidly.
Second, I would try to use both methods: Lagrangian and penalty.
If you use the penalty method, vary the penalty stiffness ore use automatic computation of it (Ansys can do this for, but it get slower)

Hope it helps!
Regards,
Alex

 

[cspkumar]

Thanks for your reply. I tried nsubst,100,1000,20 but the model converges only until 10% of load. I get a warning saying that 2 contact points have too much penetration. Also tried standard contact instead of no separation and I get the same message. Currently I am running the model by slowly increasing the load (-10 in the 1st loadstep, -100 in the second, -1000 in the 3rd). Hope it works. Any other suggestions?

Regards,
cspkumar

 

[meshparts]

If the nodes have too much penetration, then I would set a bigger contact stiffness (if you are using the penalty method).

Regards,
Alex

 

[cspkumar]

I am using the Augmented Lagrangian method & tried normal contact stiffnes, FKN of 0.1 (default is 1, I think) & the model did not run past 2% of total load. I have not run the model with penalty method yet.

Thanks

 

[doatis]

If you want to reduce/eliminate the penetration, then you should set your contact settings to be Normal Lagrange, with contact detection at the nodes (rather than by default at the gauss points).

From what you describe, it sounds like there is in reality a line-on-surface contact (since you have a u-bolt going around a tube). In this case, I would split the surface of the u-bolt so I had a line at the initial contact point. I would then setup face-to-face contact AND line-to-surface contact. You'll run into this problem whenever you have two curved surfaces running into each other.

You can play with the interference option, using the automated close gap/reduce penetration, or by specifying a manual CNOF, where you offset the contact surface into (positive value) or away from the target (negative).

As a final step, set all your contact to be bonded and make sure that the model runs, and the convergence is actually a factor of the contact, not because of an unconstrained model.

Good Luck