k-omega SST cylinder with no wall Functions
 

Hallo All,
I am running a compressible simulation of flow over a cylinder, using k-OmegaSST as turbulence model and rhoPimpleFoam as solver. The Reynolds number is 10000.
I read in some other threads that k-Omega is a high Re Turbulence model. But considering the cylinder case the Re didn't seem to be that high. So I tried using the k-OmegaSST without wall functions. Tried to resolve the y+ in first cell < 1. I haven't checked the y+ yet, but here are some observations:
1- The coefficient of drag on cylinder Cd ~ 1
2- I am able to see the vortex shedding phenomena that is typical for a cylinder flow at this Re.
3- I calculated the Strouhal Number to be St ~ 0.22, which looks pretty good.

My questions:
1-Seeing the results can I conclude that k-OmegaSST can be used without wall functions for low Re flows?
2-I am pretty satisfied with the case setup, (i.e boundary conditions, solver set up, thermophysical properties) can I really rely on this setup or do I need to conduct some other checks as well, before putting my confidence in this setup (for similar problems)?

Regards,
Ali

Hej,

the term high-Reynolds number turbulence model results from the fact that one uses wall functions and does not resolve the parts close to the wall (low Reynolds number locally, due to the velocity tending to 0 at the wall). Low Reynolds number turbulence models on the other hand do resolve those parts and then the y+ has to be lower than one as you pointed out. the has nothing to do with high and low Reynolds number in the sense of high and low velocity over a cylinder or inside a pipe.

k-omega-SST is a special case. k-omega based models do not need special treatment for the low-Reynolds effects and can therefore always be used without wall functions, as long as the boundary layer is well resolved, e.g. the first node should be y+<1 and there needs to be a smooth transition in cell size within the boundary layer. therefore, answer 1: k-omega-sst can be used without wall functions for all flows, as long as the mesh permits it.

to gain more confidence in your simulation, also check if when you change your mesh resolution that your check values (Strouhal number, Cd, etc.) don't change too much. You should also check that your y+ is below 1 everywhere. In case you use wall functions, run the normal yPlus utility and if there are parts where y+ is larger than expected (and above the log law region y+>150-300), check in paraview where this occurs and refine the mesh accordingly. In case you want to use the model in low Reynolds number mode with y+<1 and the boundary layer resolved, check the forum for a tool called yPlusPostRANS (http://www.cfd-online.com/Forums/ope...estcase-2.html).

Hallo Roman,
Thanks for your kind reply. It really helped me. Now I have a few more questions.When you say that "You should also check that your y+ is below 1 everywhere" Do you mean on the wall in first cells or everywhere around the cylinder, like first 3 cells should lie below y+ < 1 or any other number. (If you could explain it a little. :) )
Also I tried using yPlusPostRANS utility but it just works for incompressible cases. I guess I will have to make changes to make it work. Which I am not really sure about, and I have posted a question regarding this on the forum.
Thanks again for your kind reply.
Regards,
Ali

I meant only the first cell needs to be in y+<1.

In your first post you said that you simulate incompressible flow? If not I guess you will have to modify the yPlusPostRANS utility a little bit.

My mistake it was late in the night I was a bit dizzy. Ya I would look for the changes I need to do.
Thanks for your help.
Regards,
Awais

@romant
Hello Roman,
Sorry to trouble you again. I changed the utility accordingly to work with compressible problems. I am not sure whether its right or not. But I have one question:
The y distance which this utility is using is cell center distance or the height of the cell?
Regards,
Awais

Hej Awais,

as far as I know this should be the cell center, since OpenFOAM uses cell centered data storage.

Thanks for the reply. It would really help me if someone else could test this utility and tell me if its calculation is right.
Regards,
Awais Ali

Compressible?
 

owayz

What are your flow conditions and cylinder diameter to give you compressible flow at Re=10,000?

Jan Theron

Well I have a very slow flow velocity (hence the Mach number is also low).
Uinf = 9.4 m/s
Diameter = 16 mm
But I am considering a compressible flow because ultimately I will be taking my simulation towards heated walls. And my aim is to study the vortex shedding frequency and fluctuations in pressure effected by heating of the cylinder walls.
That is why I am considering a compressible flow.
What do you thin about it?
Regards,
Awais

I must admit I have no experience with nonisothermal flows, but I would think that a compressible solver such as rhoPimpleFoam coupled with a proper wall heat transfer BC would work.

You might want to browse around a bit and contact the authors of http://virtual.vtt.fi/virtual/safir2..._SAFIR2010.pdf
to see what they did to get such nice plots of forced convective heat transfer over a cylinder depicted on page 10 of their paper.

Jan