Error in ANSYS Contact modeling.

[rwangope]

Hey,

I am doing a contact modeling for pipe in pipe structure. Basically, my 3D pipe model has two annulus pipes,i.e. a small OD pipe is sitting in the middle of a large OD pipe. In ANSYS GUI 'Contact Manger', I defined the following contact pair: Pick Target-> large pipe inner wall, Pick Contact->small pipe outer wall. The problem is after the analysis is done, the small pipe penetrated through the large pipe. I didn't see any clear surface contact between the two pipes. I did increase the normal penalty stiffness, but same thing happened. Can any expert here give me some hint to correct this problem? Thank you in advance.

BTW, I already set the displacement ratio to 1:1.

Rick

 

[rwangope]

BTW, there is 1/4 inch gap between the two pipes? Thanks.

Rick

 

[Transient1]

I'm not sure if I can help you with your problem because I don't have a lot of experience with contact elements in the classic interface, but I have the following questions:

What elements are you using to model the pipes? (Pipe elements or solid elements?)

What contact/target elements are you using? Are you specifying any particular keyoptions/options?

After using the contact wizard did you see the contact elements on the inner/outer surface?

 

[rwangope]

Thanks Transient1.

I have solved the problem by giving more sub-steps to the solution process. In my model, I am using solid contact element (contact170 and contact174). After the contact is set-up, I can see them.

From your post, it seems pipe element can also be used to model contact. If it's true, could you give some details? It can make my model much more simpler. Thanks.

Rick

 

[cbrn]

Hi,
back to the original problem: if there is gap between the pipes, then the contact is initially "open". If you don't set "update contact stiffness -> each equilibrium iteration", the program will most likely "miss" the contact.
You can avoid this by setting a pinball which is bigger than the gap, so that the program will "see" the contact as "closed" (with a very low if not null initial contact stiffness, but "closed" and active from the start).
If you managed to solve your problem with more substeps, then it is likely that the "stiffness update" was already ON, but refered to "each substep".
Instead of increasing the stiffness, you can specify a maximum allowed contact penetration. Don't exaggerate, however, 'cause it could take "forever" to solve!!!
Another thing to try is the "predict for impact" option.
Regards

 

[rwangope]

Thanks cbrn. Your comments are really valuable. I will try the different things you mentioned coz my model is still have some problems when there are multiple contact pairs even with much more substeps.

Regards.

Rick