|
[Sponsors] |
March 18, 2010, 08:22 |
|
#41 | |
Senior Member
Sandy Lee
Join Date: Mar 2009
Posts: 213
Rep Power: 18 |
Quote:
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: 530
Rep Power: 20 |
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<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so" #4 Foam::operator/(Foam::tmp<Foam::Field<double> > const&, Foam::UList<double> 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<double>::evaluate(Foam::Pstream::commsTypes) in "/opt/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/simpleFoam" #8 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/opt/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/simpleFoam" #9 Foam::incompressible::RASModels::kEpsilon::kEpsilon(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&) in "/opt/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so" #10 Foam::incompressible::RASModel::adddictionaryConstructorToTable<Foam::incompressible::RASModels::kEpsilon>::New(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&) in "/opt/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so" #11 Foam::incompressible::RASModel::New(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> 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 |
|
March 29, 2010, 05:25 |
|
#43 |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
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, 05:32 |
|
#44 |
Member
Axel Söhngen
Join Date: Jan 2010
Location: Germany, Trier
Posts: 31
Rep Power: 16 |
I get the same failure when I use "nutSpalartAllmarasWallFunction"! How can I eliminate this crash?
|
|
April 21, 2010, 10:23 |
|
#45 |
Senior Member
Join Date: Feb 2010
Posts: 213
Rep Power: 17 |
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 ***; } Thanks for your help. |
|
April 28, 2010, 15:13 |
|
#46 | |
Senior Member
|
Quote:
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, 20:45 |
|
#47 |
Senior Member
Sandy Lee
Join Date: Mar 2009
Posts: 213
Rep Power: 18 |
Quote:
|
|
April 29, 2010, 07:13 |
|
#48 |
Senior Member
Join Date: Feb 2010
Posts: 213
Rep Power: 17 |
||
April 29, 2010, 08:17 |
|
#49 |
Senior Member
Sandy Lee
Join Date: Mar 2009
Posts: 213
Rep Power: 18 |
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, 12:24 |
|
#50 |
Senior Member
Join Date: Feb 2010
Posts: 213
Rep Power: 17 |
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, 18:48 |
|
#51 | |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
Quote:
I could not find a nutUSpaldingWallFunction in 1.7? However, nutSpalartAllmarasWallFunction still exists(?) and the release notes tell me:
Regards Bastian |
||
July 3, 2010, 19:18 |
|
#52 |
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 22 |
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, 10:10 |
|
#53 | ||
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Thus:
Quote:
Quote:
mad |
|||
July 5, 2010, 10:12 |
|
#54 |
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 22 |
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, 10:19 |
|
#55 | |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Quote:
mad |
||
July 5, 2010, 10:53 |
|
#56 |
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 22 |
nutLowReWallFunction is to be used with low-Re models on walls for which y+>1.
H |
|
July 5, 2010, 11:01 |
|
#57 |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
||
July 6, 2010, 04:52 |
|
#58 |
Senior Member
|
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, 05:34 |
|
#59 |
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 22 |
nutLowReWallFunction is for low-Re models, k-Omega SST isn't. You need the continuous wall-function currently called nutSpalartAllmarasWallFunction, see previous posts.
H |
|
September 19, 2010, 09:24 |
|
#60 |
New Member
Peter
Join Date: Aug 2010
Posts: 16
Rep Power: 16 |
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 | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Nearwall treatment for the kOmegaSST turbulence model | johnb | OpenFOAM Running, Solving & CFD | 3 | January 22, 2009 03:52 |
ChtMultiRegionFoam kOmegaSST solidDisplacementFoam | marico | OpenFOAM Running, Solving & CFD | 4 | January 16, 2009 03:51 |
How can run MRFSimpleFoam with KOmegaSST turbulence model | waynezw0618 | OpenFOAM Running, Solving & CFD | 0 | April 21, 2008 05:40 |
Question on new implemented komegaSST model in OF 14 | peterh | OpenFOAM Running, Solving & CFD | 7 | February 7, 2008 03:09 |
compressible | John | Main CFD Forum | 1 | April 6, 2003 13:35 |