[Jiricbeng]

Hi there,

I encountered the following issue:
I am simulating a radial bearing. The geometry is simple: cylindrical region with radially shifted inner wall to obtain eccentricity. This region includes inlet pipe. All meshed together in ICEM as hexa mesh.

Based on theory for given shaft speed and lubrication gap, the radial force is independent on density, because pressure force and viscous force are dominant, thus density goes away.

This behaviour was confirmed in Fluent, I computed density 1000 kg/m3, 1 kg/m3 and 0.0001 kg/m3, and the force (Fx^2 + Fy^2)^0.5 is almost same, the results deviate negligibly.
But when computing this in CFX, I have different results for density 1000 and 1. The difference is more than 200%-300%.. !! The results however get closer for density 1 and 0.0001.

I verified the influence of reference pressure and others.... no idea yet.

Computations run in CFX and Fluent are as follows: double precision, laminar, incompressible, isothermal, isoviscous...

Thanks a lot..

[evcelica]

Just checking, you are not including buoyancy/gravity in either case?

[ghorrocks]

There are many, many details you need to get correct for you to get the correct results. So something is likely to be wrong in your CFX setup. You will have to do a close comparison between the CFX and Fluent models, including looking at the documentation about understanding exactly what all the options mean.

[Jiricbeng]

Well, I think I get it.
Velocity - pressure coupling solver is the culprit. It is very surprising to me. Both cases are converged, but to a different result. It again opens the question regarding the local minima of N-S equations system. Different solvers - different results, although both converged.

See the attachment.

To evelica: no I do not consider gravity.

[ghorrocks]

Make sure you know what you are dealing with here. The option you changed is the Rhie-Chow pressure to velocity coupling. You did not change the CFX coupled solver for the linear equations (which is what most people think of when they think solver coupling).

You should have a close read of the documentation regarding Rhie-Chow and P-V coupling and work out which approach is most suitable for your case. As you have an unusual case (likely low Re number, highly rotational flow) a non-default Rhie-Chow may be more suitable.