Contact Analysis - Thermally Preloaded Ubolt and tube
Contact Analysis - Thermally Preloaded Ubolt and tube
(OP)
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
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





RE: Contact Analysis - Thermally Preloaded Ubolt and tube
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
RE: Contact Analysis - Thermally Preloaded Ubolt and tube
Regards,
cspkumar
RE: Contact Analysis - Thermally Preloaded Ubolt and tube
Regards,
Alex
RE: Contact Analysis - Thermally Preloaded Ubolt and tube
Thanks
RE: Contact Analysis - Thermally Preloaded Ubolt and tube
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