# Compressible kOmegaSST

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

March 18, 2010, 08:22
#41
Senior Member

Sandy Lee
Join Date: Mar 2009
Posts: 213
Rep Power: 10
Quote:
 Originally Posted by henry Provides a wall function boundary condition/constraint on omega Computed value is: omega = sqrt(omega_vis^2 + omega_log^2) where omega_vis = omega in viscous region omega_log = omega in logarithmic region Model described by Eq.(15) of: @verbatim Menter, F., Esch, T. "Elements of Industrial Heat Transfer Prediction" 16th Brazilian Congress of Mechanical Engineering (COBEM), Nov. 2001 @endverbatim H

Hi Henry, I still don't know how to give the boundary on omega, because I can not get the paper. Could you send me a copy about the paper or the detailed formulum about the boundary? Thanks.

Sandy
sandy.lee37@gmail.com

 March 26, 2010, 13:09 #42 Senior Member   BastiL Join Date: Mar 2009 Posts: 488 Rep Power: 12 I get segfaults when using nutSpalartAllmarasWallFunction in combination with k-omega SST (and also with kEpsilon): Reading/calculating face flux field phi Code:  Selecting incompressible transport model Newtonian Selecting RAS turbulence model kEpsilon #0 Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so" #2 ?? in "/lib64/libc.so.6" #3 Foam::divide(Foam::Field&, Foam::UList const&, Foam::UList const&) in "/opt/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so" #4 Foam::operator/(Foam::tmp > const&, Foam::UList const&) in "/opt/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so" #5 Foam::incompressible::RASModels::nutSpalartAllmarasWallFunctionFvPatchScalarField::calcNut() const in "/opt/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so" #6 Foam::incompressible::RASModels::nutWallFunctionFvPatchScalarField::updateCoeffs() in "/opt/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so" #7 Foam::fvPatchField::evaluate(Foam::Pstream::commsTypes) in "/opt/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/simpleFoam" #8 Foam::GeometricField::GeometricBoundaryField::evaluate() in "/opt/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/simpleFoam" #9 Foam::incompressible::RASModels::kEpsilon::kEpsilon(Foam::GeometricField, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField const&, Foam::transportModel&) in "/opt/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so" #10 Foam::incompressible::RASModel::adddictionaryConstructorToTable::New(Foam::GeometricField, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField const&, Foam::transportModel&) in "/opt/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so" #11 Foam::incompressible::RASModel::New(Foam::GeometricField, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField const&, Foam::transportModel&) in "/opt/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so" #12 main in "/opt/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/simpleFoam" #13 __libc_start_main in "/lib64/libc.so.6" #14 __gxx_personality_v0 in "/opt/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/simpleFoam" Floating point exception I have no idea what is going wrong there. Maybe my setup is wrong....

 March 29, 2010, 04:25 #43 Senior Member   BastiL Join Date: Mar 2009 Posts: 488 Rep Power: 12 I can reproduce this behaviour for the boundaryFoam Tutorial: replace nutWallFunction with nutSpalartAllmarasWallFunction in boundaryFoam/boundaryWallFunctions/0/nut and you will geht this crash... I guess there is something wrong with my setup? Are there further changes needed? Thanks Bastian

 April 21, 2010, 04:32 #44 Member   Axel Söhngen Join Date: Jan 2010 Location: Germany, Trier Posts: 31 Rep Power: 8 I get the same failure when I use "nutSpalartAllmarasWallFunction"! How can I eliminate this crash?

 April 21, 2010, 09:23 #45 Senior Member   Join Date: Feb 2010 Posts: 213 Rep Power: 9 Please, I have some questions about implementation of SST turbulent model and wall functions. I hope Mr Weller can answer to me. 1. In most papers or threads of this forum I read that, when a wall function is used, y+ must be greater than 30, if possible closed to 30, so wall-adjacent first cells centroid is located within the log-law layer. But someone, with SST, sets y+ above 11. Is it correct? Why? I can't find theoretical support for that. 2. Must I set initial condition for nut, as in motorBike tutorial? Even if I do not, my case works and or values seem good. Anyway, after the code running I find a nut file in my time folders, so I think it's calculated. 3. I'm in trouble with inlet boundary conditions for . In FLUENT manual and other papers I read but I find also In other words, my question is: or ? 4. I set Code: wall { type omegaWallFunction; value uniform ***; } with *** as internalField value. Is it wrong? Is there a better way to evaluate initial wall value for ? Thanks for your help.

April 28, 2010, 14:13
#46
Senior Member

Ivan Flaminio Cozza
Join Date: Mar 2009
Location: Torino, Piemonte, Italia
Posts: 207
Rep Power: 10
Quote:
 Originally Posted by henry I am referring to nutSpalartAllmarasWallFunction for incompressible flow and mutSpalartAllmarasWallFunction for compressible flow. Even though these were created for use with the Spalart-Allmaras model they are not dependent on this particular model in any way being generic implementations of the Spalding continuous wall-function using U rather than k as the controlling variable and can be used with other turbulence models. We tested the kOmegaSST model with the nutSpalartAllmarasWallFunction wall-function and obtained good results, as good as others have obtained with adaptive/continuous wall-functions. H
A question on using mutSpalartAllmarasWallFunction:
When I use it in a adaptive fashon (let's say, my y+ is in between 1 and 15), I have to set k to fixedValue 1e-12, or I can set it to wallFunction as well?

Thanks,
Ivan

April 28, 2010, 19:45
#47
Senior Member

Sandy Lee
Join Date: Mar 2009
Posts: 213
Rep Power: 10
Quote:
 Originally Posted by vaina74 Please, I have some questions about implementation of SST turbulent model and wall functions. I hope Mr Weller can answer to me. 1. In most papers or threads of this forum I read that, when a wall function is used, y+ must be greater than 30, if possible closed to 30, so wall-adjacent first cells centroid is located within the log-law layer. But someone, with SST, sets y+ above 11. Is it correct? Why? I can't find theoretical support for that. 2. Must I set initial condition for nut, as in motorBike tutorial? Even if I do not, my case works and or values seem good. Anyway, after the code running I find a nut file in my time folders, so I think it's calculated. 3. I'm in trouble with inlet boundary conditions for . In FLUENT manual and other papers I read but I find also In other words, my question is: or ? 4. I set Code: wall { type omegaWallFunction; value uniform ***; } with *** as internalField value. Is it wrong? Is there a better way to evaluate initial wall value for ? Thanks for your help.
Hi vaina74, I think you should use a smaller Beta = nu_t / nu (about 0.1 ~0.2). I guess, by analyzing the physics mechanics, you can explain why, right?

 April 29, 2010, 06:13 #48 Senior Member   Join Date: Feb 2010 Posts: 213 Rep Power: 9 I'm not sure but in FLUENT guidelines and other papers is 1-10 for and turbulence models (external flow). Maybe it doesn't matter, if boundaries are far away. I think SST has a approach far from the wall, so the turbulent model is not so sensitive to the inlet turbulent quantities.

 April 29, 2010, 07:17 #49 Senior Member   Sandy Lee Join Date: Mar 2009 Posts: 213 Rep Power: 10 But, in my case about an external flow, I could not get convergent solutions to Beta equal 1~10 ... If Beta = 1~10, it means the turbulence nu_t > nu. Is it really reasonable to turbulence flows?

 April 29, 2010, 11:24 #50 Senior Member   Join Date: Feb 2010 Posts: 213 Rep Power: 9 Sorry, I'm a beginner and maybe I can't help you. What turbulence model do you apply? Which are your boundary condition? Is your mesh a bad or good one, what's your y+? I got in troubles with model, perhaps problems as yours. But now I'm focusing on SST model and it seems to work fine (I need it for a later propeller simulation), so I gave up with other turbulence models.

July 3, 2010, 17:48
#51
Senior Member

BastiL
Join Date: Mar 2009
Posts: 488
Rep Power: 12
Quote:
 Originally Posted by henry In the next release we will rename nutSpalartAllmarasWallFunction to nutUSpaldingWallFunction to make it clear that it is a general purpose continuous wall-function using U as the defining variable. H
Henry,

I could not find a nutUSpaldingWallFunction in 1.7?
However, nutSpalartAllmarasWallFunction still exists(?) and the release notes tell me:
• New nutWallFunction continuous wall function,
• New nutLowReWallFunction continuous wall function,
So both are continuous where is the difference? Which to use for a mesh with y+>30 everywhere, y+<1 everywhere and a all y+ mesh? Thanks.

Regards Bastian

 July 3, 2010, 18:18 #52 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 14 nutSpalartAllmarasWallFunction has not been renamed yet but it will be. For this release we decided to maintain backward-compatibility with 1.6.x on this and a few other issues. > New nutWallFunction continuous wall function Sorry this is a mistake in the release notes I will correct it. nutWallFunction is the high-Re wall-function based on k. The nutLowReWallFunction is the missing wall-function implementation for the low-Re models, it is not "continuous", again I will correct the release notes. If having a "continuous" wall-function for the low-Re models would be useful it could easily be created in the same manner as the nutLowReWallFunction H

July 5, 2010, 09:10
#53
Senior Member

Join Date: Mar 2009
Posts: 436
Rep Power: 14
Thus:
Quote:
 Originally Posted by henry nutWallFunction is the continuous ... high-Re wall-function based on k. nutLowReWallFunction is the missing wall-function implementation for the low-Re models, it is not "continuous"
In that case, does the usual y+ rule apply? 30<y+<100 for nutWallFunction and y+<1 for nutLowReWallFunction I mean... Or:

Quote:
 Originally Posted by bastil Which to use for a mesh with y+>30 everywhere, y+<1 everywhere and a all y+ mesh?
Thanks,

 July 5, 2010, 09:12 #54 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 14 If your near-wall y+<1 everywhere you can use a low-Re model; you don't need wall-functions at all. H

July 5, 2010, 09:19
#55
Senior Member

Join Date: Mar 2009
Posts: 436
Rep Power: 14
Quote:
 Originally Posted by henry If your near-wall y+<1 everywhere you can use a low-Re model; you don't need wall-functions at all. H
That sounds good. So when am I going to use a nutLowReWallFunction?
• High-Re: nutWallFunction + highRe turbulence model -> 30<y+<100
• Low-Re: no wall function + low Re turbulence model -> y+<1
• ???: nutLowReWallFunction + lowRe turbulence model --> ???
Sorry if I insist, but this new nutLowReWallFunction is a bit confusing for me...

 July 5, 2010, 09:53 #56 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 14 nutLowReWallFunction is to be used with low-Re models on walls for which y+>1. H kiddmax, crossley90, Aerospace and 1 others like this.

July 5, 2010, 10:01
#57
Senior Member

Join Date: Mar 2009
Posts: 436
Rep Power: 14
Quote:
 Originally Posted by henry nutLowReWallFunction is to be used with low-Re models on walls for which y+>1. H
Perfect! Thank you!

 July 6, 2010, 03:52 #58 Senior Member   Ivan Flaminio Cozza Join Date: Mar 2009 Location: Torino, Piemonte, Italia Posts: 207 Rep Power: 10 Just to clear my mind, is nutLowReWallFunction ok if I use the k-Omega SST model on a wall that somewhere has a resolution of y+ O(1) and somewhere else O(10)? That's something similar to what starccm+ do with its "all y+" wall treatment... Thanks, Ivan

 July 6, 2010, 04:34 #59 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 14 nutLowReWallFunction is for low-Re models, k-Omega SST isn't. You need the continuous wall-function currently called nutSpalartAllmarasWallFunction, see previous posts. H Aerospace likes this.

 September 19, 2010, 08:24 #60 New Member   Peter Join Date: Aug 2010 Posts: 16 Rep Power: 8 Hey @ all! This all is a little bit confusing to me: I have to simulate a case(turbulent, compressible, rhosimple solver) using the k-omega-sst model. Now, If i have a mesh with y+>30, I need to use wall functions, thats clear. But, If I have a mehs y+<1(low-re), and I'd like to use the k-omega-sst modell, what boundary conditions for the walls do I have to take? Zerogradient for omega and k with very low values (10^-8), and calculated for alphat and mut (or other values?)? Or do I have to take a wall function (like mutlowrewallfunction) for one of those? I tried several approaches (y+30 mesh with wall functions => not very good results, probably because of the coarse mesh; y+1 mesh with wall functions: almost good results, but not good enough, I guess because the mesh is for low-re models, so I get trouble in this region; y+1 mesh with omega and k set to zero gradient, value 10^-8, completely wrong results) I'm a new user of OpenFoam, and I also never did CFD-Simulations before, so I only have little experience and not much knowledge about those equations, please excuse this. I hope somebody is able to help me. Thank you very much!

 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 johnb OpenFOAM Running, Solving & CFD 3 January 22, 2009 03:52 marico OpenFOAM Running, Solving & CFD 4 January 16, 2009 03:51 waynezw0618 OpenFOAM Running, Solving & CFD 0 April 21, 2008 04:40 peterh OpenFOAM Running, Solving & CFD 7 February 7, 2008 03:09 John Main CFD Forum 1 April 6, 2003 12:35

All times are GMT -4. The time now is 18:54.