CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

k-omega SST cylinder with no wall Functions

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

Like Tree4Likes
  • 4 Post By romant

Reply
 
LinkBack Thread Tools Display Modes
Old   July 24, 2012, 15:03
Default k-omega SST cylinder with no wall Functions
  #1
Senior Member
 
Awais Ali
Join Date: Feb 2010
Location: Germany
Posts: 128
Rep Power: 8
owayz is on a distinguished road
Send a message via MSN to 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

Last edited by owayz; July 25, 2012 at 10:37.
owayz is offline   Reply With Quote

Old   July 25, 2012, 02:39
Default
  #2
Senior Member
 
romant's Avatar
 
Roman Thiele
Join Date: Aug 2009
Location: Stockholm, Sweden
Posts: 366
Rep Power: 12
romant is on a distinguished road
Quote:
Originally Posted by owayz View Post
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).
owayz, Jonathan, fumiya and 1 others like this.
__________________
~roman
romant is offline   Reply With Quote

Old   July 25, 2012, 08:38
Default
  #3
Senior Member
 
Awais Ali
Join Date: Feb 2010
Location: Germany
Posts: 128
Rep Power: 8
owayz is on a distinguished road
Send a message via MSN to owayz
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
owayz is offline   Reply With Quote

Old   July 25, 2012, 09:13
Default
  #4
Senior Member
 
romant's Avatar
 
Roman Thiele
Join Date: Aug 2009
Location: Stockholm, Sweden
Posts: 366
Rep Power: 12
romant is on a distinguished road
Quote:
Originally Posted by owayz View Post
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 View Post
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
romant is offline   Reply With Quote

Old   July 25, 2012, 10:37
Default
  #5
Senior Member
 
Awais Ali
Join Date: Feb 2010
Location: Germany
Posts: 128
Rep Power: 8
owayz is on a distinguished road
Send a message via MSN to owayz
Quote:
Originally Posted by romant View Post
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
owayz is offline   Reply With Quote

Old   July 26, 2012, 11:13
Default
  #6
Senior Member
 
Awais Ali
Join Date: Feb 2010
Location: Germany
Posts: 128
Rep Power: 8
owayz is on a distinguished road
Send a message via MSN to owayz
@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
File Type: zip compressiblePlusPostRANS.zip (6.4 KB, 10 views)
owayz is offline   Reply With Quote

Old   July 26, 2012, 11:26
Default
  #7
Senior Member
 
romant's Avatar
 
Roman Thiele
Join Date: Aug 2009
Location: Stockholm, Sweden
Posts: 366
Rep Power: 12
romant is on a distinguished road
Hej Awais,

as far as I know this should be the cell center, since OpenFOAM uses cell centered data storage.
__________________
~roman
romant is offline   Reply With Quote

Old   July 30, 2012, 08:36
Default
  #8
Senior Member
 
Awais Ali
Join Date: Feb 2010
Location: Germany
Posts: 128
Rep Power: 8
owayz is on a distinguished road
Send a message via MSN to owayz
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
owayz is offline   Reply With Quote

Old   July 30, 2012, 15:09
Default Compressible?
  #9
New Member
 
Johannes N Theron
Join Date: Feb 2010
Location: Hamburg
Posts: 21
Rep Power: 8
jantheron is on a distinguished road
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 View Post
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
jantheron is offline   Reply With Quote

Old   July 31, 2012, 14:59
Default
  #10
Senior Member
 
Awais Ali
Join Date: Feb 2010
Location: Germany
Posts: 128
Rep Power: 8
owayz is on a distinguished road
Send a message via MSN to owayz
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
owayz is offline   Reply With Quote

Old   July 31, 2012, 16:57
Default
  #11
New Member
 
Johannes N Theron
Join Date: Feb 2010
Location: Hamburg
Posts: 21
Rep Power: 8
jantheron is on a distinguished road
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
jantheron is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Near wall treatment in k-omega SST Arnoldinho OpenFOAM Running, Solving & CFD 37 June 9, 2015 09:35
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
wall functions kd55 Main CFD Forum 2 April 13, 2012 04:37
wall functions and boundary conditions in OF 1.7.1 cristobal OpenFOAM 2 May 6, 2011 04:10
UDF for wall slipping HFLUENT Fluent UDF and Scheme Programming 0 April 27, 2011 12:03


All times are GMT -4. The time now is 07:06.