[Rubel Ahammed]

Dear Experts,

Here I have done my geometry by using space claim. Actually I want to do a sinusoidal motion of a piston inside a cylinder. Cylinder is occupied by a magneto-rheological fluid.

Inside of piston have two passage for passing fluid one side to another. During reciprocating motion fluid will pass from one side to another.

I have attached picture here for my geometry and mesh. When i run my simulation an error occur after completing 1-2 iterations.

| ERROR #002100004 has occurred in subroutine Out_Scales_Flu. |
| Message: |
| The Reynolds number is outside of the range expected based on the |
| Option selected for the TURBULENCE MODEL. Check this setting, |
| the values of the properties, mesh scale, consistency of units |
| and solution values in the input file. Execution will proceed.

>> Shear stress transport model.
Piston Displacement: 20[mm]*sin(2*3.1416*t/1.0[s])
Velocity: 50[mm/s]*sin(2*3.1416*t/1.0[s])

How can I solve this problem.

Thanks in advance


With Regards
Rubel

[karachun]

This is not your problem message. This is a warning, not an actual error. This message does not need a user response - CFX calculates Re based on some representative length scale (something like cubic root from domain volume) and this scale is wrong for most cases.


True error messages are hidden somewhere in solver output. You should post whole .out file so other users can observe it and find actual error code.

[Rubel Ahammed]

Dear Alexander Karachun

I Think this problem occur due to inappropriate mesh.

I have attached here solver manager status. After running 1-2 iteration it shows abnormal completion.

Could you please suggest me how can I fix this problem.


With Regards
Rubel

[ghorrocks]

You need to look in the output file to see the detailed error messages. So please post the output file on the forum if you want us to look at it.

But from the screen dump you attach it has an error about a distorted element in the boundary layer. This would appear to be the problem. Your issue is likely to be related to this FAQ: https://www.cfd-online.com/Wiki/Ansy..._went_wrong.3F

[Rubel Ahammed]

Dear Glenn

I have attached out file here. I would like to request to you look at my out file.


Thanks
Rubel

[ghorrocks]

You have not specified the wall boundaries correctly for them to move without folding the mesh. Save a full results file every time step and rerun your simulation and look at the way you mesh moves. You should be able to work it out from there. Here's a hint: the side walls need to be "unspecified", and a second hint: if you start the simulation at top dead centre and expand the mesh out from there you will find this MUCH easier than starting at bottom dead centre and compressing the mesh.

Also, your time step is way too big. It is not converging in the first time step.

You have a non-Newtonian fluid specified. You should debug this simulation with a standard Newtonian fluid (maybe use air or water) until you get the mesh motion working. Only when everything else is working should you change to a non-Newtonian fluid.