# k-omega SST cylinder with no wall Functions

 Register Blogs Members List Search Today's Posts Mark Forums Read

 July 24, 2012, 15:03 k-omega SST cylinder with no wall Functions #1 Senior Member   Awais Ali Join Date: Feb 2010 Location: Germany Posts: 128 Rep Power: 9 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 Last edited by owayz; July 25, 2012 at 10:37.

July 25, 2012, 02:39
#2
Senior Member

Roman Thiele
Join Date: Aug 2009
Location: London, UK
Posts: 368
Rep Power: 13
Quote:
 Originally Posted by owayz Hallo All, I am running an in-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 (y+ and u+ values with low-Re RANS turbulence models: utility + testcase).
__________________
~roman

 July 25, 2012, 08:38 #3 Senior Member   Awais Ali Join Date: Feb 2010 Location: Germany Posts: 128 Rep Power: 9 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

July 25, 2012, 09:13
#4
Senior Member

Roman Thiele
Join Date: Aug 2009
Location: London, UK
Posts: 368
Rep Power: 13
Quote:
 Originally Posted by owayz 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.
I meant only the first cell needs to be in y+<1.

Quote:
 Originally Posted by owayz 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. Ali
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.
__________________
~roman

July 25, 2012, 10:37
#5
Senior Member

Awais Ali
Join Date: Feb 2010
Location: Germany
Posts: 128
Rep Power: 9
Quote:
 Originally Posted by romant 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.
Regards,
Awais

July 26, 2012, 11:13
#6
Senior Member

Awais Ali
Join Date: Feb 2010
Location: Germany
Posts: 128
Rep Power: 9
@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
Attached Files
 compressiblePlusPostRANS.zip (6.4 KB, 10 views)

 July 26, 2012, 11:26 #7 Senior Member     Roman Thiele Join Date: Aug 2009 Location: London, UK Posts: 368 Rep Power: 13 Hej Awais, as far as I know this should be the cell center, since OpenFOAM uses cell centered data storage. __________________ ~roman

 July 30, 2012, 08:36 #8 Senior Member   Awais Ali Join Date: Feb 2010 Location: Germany Posts: 128 Rep Power: 9 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

July 30, 2012, 15:09
Compressible?
#9
New Member

Johannes N Theron
Join Date: Feb 2010
Location: Hamburg
Posts: 21
Rep Power: 8
owayz

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

Jan Theron

Quote:
 Originally Posted by owayz 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

 July 31, 2012, 14:59 #10 Senior Member   Awais Ali Join Date: Feb 2010 Location: Germany Posts: 128 Rep Power: 9 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

 July 31, 2012, 16:57 #11 New Member   Johannes N Theron Join Date: Feb 2010 Location: Hamburg Posts: 21 Rep Power: 8 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

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Arnoldinho OpenFOAM Running, Solving & CFD 37 June 9, 2015 09:35 Attesz CFX 7 January 5, 2013 04:32 kd55 Main CFD Forum 2 April 13, 2012 04:37 cristobal OpenFOAM 2 May 6, 2011 04:10 HFLUENT Fluent UDF and Scheme Programming 0 April 27, 2011 12:03

All times are GMT -4. The time now is 23:21.