Contact issue with paper transport (NX nastran SOL 601 129 )

[vandongenp]

Hello,

I'm trying to perform a simulation whereby i transport a paper sheet between two pair of pressure rollers.

- The lower rollers are fixed in the translation directions.
- The upper rollers are performing a transient movement towards the lower rollers,
so there will be a contact force between the sheet and the roller pairs.
When the pressure rollers are finished with the downwards movement i perform a transient rotation of the lower rollers of 45 degrees.

I use solution 601 129, the simulation is working oké, but i get some slip between the two contact surfaces.

I expect a paper transport approximately of 13.75 (diameter roller 35mm with a rotation of 45 degrees)

The result that i get is around 8 mm.

I try to adjust a lot of parameters like contact/ time step size / damping /etc, they all have influence on the end result, but i cannot manage to get a realistic result.

I added the FEM and SIM file.

Hopefully somebody can help me to understand this problem.

The simulation and fem file

http://files.engineering.com/getfil...a-4003-b208-2e898bfecbc3&file=DoubleWheel.zip

Kind regards Peter

 

[hokhay]

Hi vandongenp,

Have you tried refine the mesh? From the result, I can see the X displacement vary from 4 to 7mm. Does this imply any error in the boundary condition? Should they be roughly the same if the problem is set correctly?

Jason

 

[janFEA]

Hello vandongenp,

I rerun your analysis in NX 10.0.3.5 - the version can be relevant.
I noticed the task was not finished to the defined final time, it stopped in 9,6s - I recommend you to check .log or/and .f06 file.

Yes, although it stopped 0.4s before finish I understand your expectation, it is still small displacement.
Good indicators can be in both mentioned text files:
*** *ATS*,no convergence,new time step= 4.3750E-02 new solution time= 9.6687E+00
*** Step number = 49 step size = 4.3750000E-02 time = 9.6687500E+00
*** Element distorted, Jacobian DET= -1.213125E-02 GROUP= 2 EL= 28220

etc. etc.
You can see these element belongs to the model of rubber cylinder.
The rubber is in your case defined as non-hyperelastic material with Poisson ratio almost 0.5 - this can be issue, you can consider mixed configuration.
But before this I would recommend to invest effort to check the entire model - f.e. paper sheet. Is it modeled as midsurface, or have you used only one layer from 0.1mm thickness (top or bottom?). I don't have .prt so it is hard to measure the distance f.e. the paper from cylinders, I think you should check if there is something missing - in case midsurface you should define OFFTYPE: Half the shell thickness in contact parameters. If you use some layer, then you should define corresponding OFFSET etc.
This is probably the most important, after you can continue with the rest.

Let me ask you the question:
1. You are doing transient analysis. Why not steady-state? Do you assume that inertia effect plays a big role, in respect to defined sliding velocity?
Or you would like simulate some stick-slip effect?
2. I see you used contact damping. The value was chosen by you? I just want to express that the damping can be pretty tricky - sometimes helps, sometimes the results are inaccurate.

Good luck and let us know,

Jan

Dr. Jan Vojna
Lead Engineer Development
Siemens, s.r.o.