Static structural analysis of two overlapping tubes kept together by pins-ANSYS Mech.
on Ansys Workbench (Static structural) I'm trying to simulate two tubes, the minimum radius of one of them is equal to the maximum radius of the other one. They overlap on the extremities and they are kept together by 6 pins normal to the tubes surface. Boundary conditions are as follows: the larger tube has its non overlapping extremity fixed not to move longitudinally, on the non overlapping extremity of the smaller tube a pulling pressure is applied, and the same internal pressure in both tubes is applied.
The tubes simulate the wall of an artery and a prosthesis, so I set appropriate materials properties for them, the pins are made of steel instead.
I have to allow sliding betwen the tubes and I set a 0.05 Friction coefficient in the Contact tab, but I can't find a way to set the contacts between the tubes and the pins that leads to convergence.
I'd like to ask if anyone has any suggestions for my problem.
Thank you in advance for your help.
Can you post an image of the geometry?
first of all I want to say that I´m starting myself learning Ansys both CFX, Fluent and mechanical. I´m not sure my suggestions will be of any help, but I´ll try.
Pins, big tube and small tube are 3 different non united bodies?
Are all the materials well defined? sometimes for nonlinear problems, material definitions give lot of trouble for convergence, if I´m not wrong.
Try, before to apply contact, start appling movement restrictions everywhere. Also very small pressures/forces, much more than the ones you are willing to use. Mesh very coarse for fast try and error learning method. Then run the solver, analisis, etc. It works? If no, check your geometry. If it works, then start to increse a litle more your forces or pressures to see if it works, until you have applied all your pressure values. The same with movement restrictions, start to "untie" your bodies, and check if it works. At the very end if still works, refine a litle your mesh. Then start setting your contacts. Check ansys help about contacts (it´s very tricky) symmetry, and asymetric contact situation, bonded or friction, frictionless settings, and "PLAY" with all the contact seetings. Do try and error, don´t change everything at the same time. Sometimes is good to slice or split your geometry faces where contact ocurs, also to increase the normal stiffness and sett it to 1. I had myself lots of proplems with bonded, friction, etc settings my self. Hopefully smarter people than me will start to use this mechanical subforum and give us some clues/help .
thank you very much for your reply.
First of all yes, smaller tube, bigger tube and pins are all separate bodies.
I tried and I'm still trying to follow your suggestions step by step.
I obtained a converged solution (the only warning message is that weak springs were automatically added) applying 100 times smaller forces then the desired ones and setting the contacts between tubes and pins as "Rough", which is plausible, as tubes can deform because of pins but they can't separate.
If I increase the forces up to still 10 times smaller than the required ones, the solver fails to converge and it says that contact status has experienced an abrupt change. Anyway, I think adding more movement restrictions would mean to get further from the real case.
I have done some analyses with contacts. Here are some recommendations that you should take into account:
- first, if all parts are separated, you should define contacts between each 2 of them; that includes the pin-tube contact too;
- in the case of pins you should add a constraint as they will move radially and the solver will interpret this as a rigid movement and crash;
- you should use a higher friction ratio; the friction coefficient must be between 0 and 1; 0 is transforms the contact in frictionless and 1 transforms it in bonded; from my experience, a value between 0.2 and 0.4 works fine;
- the info "contact status has experienced an abrupt change" is due to the nonlinear nature of your problem; if you define frictional contacts, the problem becomes nonlinear and the solver will determine the solution iteratively; therefore you have to be sure that the loads are inputted in small steps; this is done in Analysis Settings by setting:
- Auto Time Stepping: ON
- Defined by: Substeps
- Initial Substeps: 5
- Minimum Substeps: 3
- Maximum Substeps: 15
- Large Deflections: ON
- when you run the analysis you can keep track of the convergence by clicking Solution information>Force convergence.
I hope this will solve your problem.
|All times are GMT -4. The time now is 03:05.|