Moment and Friction problem

[Yunus9696]

Dear coleagues
Hope you're fine.

I have two cylinders. The outer surface of the smaller cylinder (lets call it Pin) is in contact to the inner surface of the larger one(lets call it Box).
The contact type is surface-to-surface and by a friction coeficient of 0.8 (tangentioal behavior>>penalty = 0.8).
I apply a moment of 0.2 N.m along the axis of the Pin to a reference point that is coupled to Pin's top surface.
I have constrained the bottom of Box in all directions.
I'm using two static general steps, first one to increase the firction coeficient from "frictionless" to "penalty = o.8"
and the next one to apply the torque.
I run the simulation and expect the Pin rotates along its own axis and produce a stress fiels in both Pin and the Box, the first step gets done by 1 increment but in the 2nd step what I get is only a "too many attempts" error and it doesn't even work for an increment.

Here I attached the picture of a cross section of the assembly, BCs and moment load.

I would highly appreciate it if you could help me out.

Regards,
Yunus.

 

[FEA way]

What exactly happens in the first step - is there some prescribed rotation ? It’s good to establish contact with displacement control in the first step.

 

[Yunus9696]

Dear FEA way
Thanks for your reply

In the initial step, I defined the contact with frictionless behavior and encastre boundary condition for the box bottom.

In the first step, I hold the boundary conditions and change the contact behavior to penalty=0.8

In the second step, which doesn't works, I just apply the moment of 0.2 N.m .

I don't know why this doesn't work? (I can attach the cae and inp files if needed)
Could you please let me know how to establish contact with prescribed displacement control?

Best regards,
Yunus.

 

[FEA way]

It might be difficult to get converged results in such static analysis involving contact and force control. I would try applying non-zero rotational displacement first. If it doesn't help, check if there are any significant gaps between the parts and try enabling automatic stabilization.

 

[Yunus9696]

About the gaps I'm sure that there isn't since the inner diameter of the box is exactly equal to the outer diameter of the pin, and it can be checked visually.

But if I don't use force control (ie. the 0.2 N.m moment), then how can I apply the exact 0.2 N.m torque on the pin?

I'd also appreciate it if you could refer me to a reference or kindly tell me why force control and contact don't work together.


Thanks again and Best regards.

 

[FEA way]

Displacement control might be necessary only in the first step to establish contact. And then you could apply torque in the second step. Another way is to use automatic stabilization (on the step or contact level) or a dynamic quasi-static step. Or discrete dashpots but as a last resort.

Generally speaking, displacement control is better in nonlinear analysis, it makes it much easier to achieve convergence. In the case of simulations involving contact, displacement control (unlike force control) eliminates rigid body motions.

 

[Yunus9696]

Thanks dear FEA way for your complete response and various methods to tackle this problem :
1. Displacement control load to establish contact
2. Automatic stabilization
3. Dynamic quasi-static step
4. Discrete dashpots

I should do a search about last three ones, but about the first one, you kindly mean to apply a small rotation (eg. 0.01 radian) in the first step just to establish the contact and then apply the moment in the next step, did I get it right?

Best regards.

PS: I'll explore the other options too and share the results for future reference.

 

[FEA way]

Yes, exactly. Some small rotation just to make contact work. Check its status (mainly CSTATUS, COPEN, CPRESS and CSLIP output variables) once it solves.

 

[Yunus9696]

Hello again
I tried the 1rst and 2nd method and I found the root of convergence problem.
As you kindly mentioned, there is a gap between two parts,however not at the beginnig of the step but once the moment is applied.
The moment along Pin's axis seems to shrink it in radial direction and there produces a gap between the Pin and the Box (I kindly attached the picture).
Friction coeficient between Pin and Box is 0.8 .

Regarding this issue, how can I properly exert the torque on the Pin and see the resuling stress field in the box?


PS1: I applied Automatic stabilization factor 0.01 and 1 percent of the load (0.001 N.m) in the forst step.
Maximum UR (Rotations) is about 0.6 (I guess in radians).

 

[FEA way]

Does the same happen in the model with 2 steps (first one with displacement control) ? Can you share the .cae file ? I would try to resolve the problem with one of the standard approaches.

 

[Yunus9696]

Yes, this model seems to be beneficial for future reference for who wants to model a screw in 2 or 3D.
Here I kindly attached the model files.

can't wait for your great tips,
Regards,
Yunus.

 

[FEA way]

It’s hard to get this model to converge when torque is applied, even with the help of stabilization, dynamic implicit procedure or dashpots. Strain-free resolution of initial gaps caused by discretization also doesn’t help because even if the analysis goes through the initial increments (with a very low increment size), which is not so hard to achieve here, it fails at some point later. Of course, dynamic explicit analysis with proper settings (to make it quasi-static) would help because non-convergence is not an issue there. However, it makes more sense to apply rotational displacement and measure the torque at the reference point. You may just have to change the value of the rotational displacement until you get the desired torque as output.