[pvpnrao]

Dear Alberto

http://www.cfd-online.com/Forums/members/alberto.html

I was wondering the reason for selecting the ce value in you dynamic Smagorinsky library.

I am new to OpenFOAM, what is ce and what is the reason for specifying that particular value to it?

[syavash]

Originally Posted by huangxianbei

Hi,alberto:
I have a question about the MM definition in volScalarField dynamicSmagorinsky::cD
As Lily stated, MM=filter(delta)^2*filter(S_bar)*filter(D)-(delta)^2*filter(S_bar*D)
D=symm(grad(U))=Sij
in the dynamicSmagorinsky.C
MM=sqr(delta())*(filter_(mag(D)*(D)) - 4*mag(filter_(D))*filter_(D))
So filter(delta)/delta=2 is used
However, mag(D) returns (SijSij)^1/2 instead of (2SijSij)^1/2=S_bar
as a result,
MM=MM_exact/(2^1/2)
Thus
cD=cD_exact*2^1/2
Above, _exact represents the exact value in Lily's method
If it's my misunderstanding, please correct me.
Best reguards
Xianbei

Dear Xianbei or anyone else,

Would you please point out that where "D" is defined in the code?!

Thanks

Syavash

[moh-farmani]

Dear Alberto,

i want to use dynamicsmagorinsky code that you have generously contributed, but as i use your instructions (wmake libso) in openFoam3.01 the error is appeared:

wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file dynamicSmagorinsky.C
could not open file Smagorinsky.H for source file dynamicSmagorinsky.C due to No such file or directory
could not open file LESfilter.H for source file dynamicSmagorinsky.C due to No such file or directory
g++ -m64 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam30/src/turbulenceModels -I/opt/openfoam30/src/turbulenceModels/LES/LESdeltas/lnInclude -I/opt/openfoam30/src/turbulenceModels/LES/LESfilters/lnInclude -I/opt/openfoam30/src/turbulenceModels/incompressible/LES/lnInclude -I/opt/openfoam30/src/transportModels -I/opt/openfoam30/src/finiteVolume/lnInclude -I/opt/openfoam30/src/meshTools/lnInclude -IlnInclude -I. -I/opt/openfoam30/src/OpenFOAM/lnInclude -I/opt/openfoam30/src/OSspecific/POSIX/lnInclude -fPIC -c dynamicSmagorinsky.C -o Make/linux64GccDPInt32Opt/dynamicSmagorinsky.o
In file included from dynamicSmagorinsky.C:25:0:
dynamicSmagorinsky.H:85:25: fatal error: Smagorinsky.H: No such file or directory
compilation terminated.
/opt/openfoam30/wmake/rules/General/transform:8: recipe for target 'Make/linux64GccDPInt32Opt/dynamicSmagorinsky.o' failed
make: *** [Make/linux64GccDPInt32Opt/dynamicSmagorinsky.o] Error 1
could you please help me to use the model properly?

Regards
Mohammad

[Lorenzo92]

Originally Posted by syavash

Dear Xianbei or anyone else,

Would you please point out that where "D" is defined in the code?!

Thanks

Syavash

have a look in Member functions of dynamicSmagorinsky.C. There is a line:

const volSymmTensorField D(dev(symm(gradU)));

Hope be helpful

Lorenzo

[huangfei]

Has anyone compiled this code in version 4.0 and shared for me? I fail to do this .
Yours,
Bo Kong

[Lorenzo92]

Originally Posted by huangfei

Has anyone compiled this code in version 4.0 and shared for me? I fail to do this .
Yours,
Bo Kong

Compiling procedure between OF 4.0 and previous versions are quite different. Try switching back to OF 2.4.0 for instance. I compiled Alberto's model with success on such this version

[shang]

Hi Alberto,Thank you very much for sharing the model.

I just read your code and compared with homogeneousDynSmagorinsky in OF230. I got some questions hope to get answer from you:
1. Do you achieve the locally averaging by adding the class "fvc" in front of the function, if yes, can you explain a little bit more why is that?
2. In the code "nuSgs_ = max(cD(D)*sqr(delta())*sqrt(magSqr(D)), -nu());", why you use "-nu()" rather than 0? If cD(D)*sqr(delta())*sqrt(magSqr(D)) < -nu() and -nu() should be a negative value anywhere, this will produce a negative nuSgs value. Am I right?

Kind regards,
Yeru

[syavash]

For All those who miss dynamicSmagorinsky model on new versions of OpenFOAM,


I have developed and compiled the code for version 4.1. You can find the code at the following link:


https://github.com/syavash20/TurbLab...magorinsky_4.1


Also, a channel395 example has been provided to test the implementation.


Enjoy,


Syavash

[nimasam]

Originally Posted by syavash

For All those who miss dynamicSmagorinsky model on new versions of OpenFOAM,


I have developed and compiled the code for version 4.1. You can find the code at the following link:


https://github.com/syavash20/TurbLab...magorinsky_4.1


Also, a channel395 example has been provided to test the implementation.


Enjoy,


Syavash

Thanks , i modified it for OpenFOAM 3

[cyss38]

For info the 4.1 version can be used with the versions 5.0 and 1806

[KingKraut]

I am a bit confused that the during a simulation no output about bounding k is written to the log, as it was done in previous versions of this turbulence model (OF231).
Can anybody confirm this? Or am I doing something plainly wrong?
Or was this taken out of the code?


I am doing a pimpleFoam simulation with a custom solver with the setup of turbulenceProperties as suggested by the creators,

https://github.com/syavash20/TurbLab...magorinsky_4.1


Thanks a lot in advance to anybody clarifying this for me.
Best wishes






Edit: I am using OF1812+

[syavash]

Originally Posted by KingKraut

I am a bit confused that the during a simulation no output about bounding k is written to the log, as it was done in previous versions of this turbulence model (OF231).
Can anybody confirm this? Or am I doing something plainly wrong?
Or was this taken out of the code?


I am doing a pimpleFoam simulation with a custom solver with the setup of turbulenceProperties as suggested by the creators,

https://github.com/syavash20/TurbLab...magorinsky_4.1


Thanks a lot in advance to anybody clarifying this for me.
Best wishes






Edit: I am using OF1812+

Dear Johannes,

AFAIK, k is bounded only when its value is smaller than SMALL=1e-20, otherwise its minimum value would be read from the field.

But in general, bounding k to a minimum value should not affect the solution procedure as k is an independent quantity. It is considered in the SGS stress tensor only. It will become more noticeable if you would like to calculate the ratio of resolved to total turbulent kinetic energy.

Regards,
Syavash

[KingKraut]

Dear syavash,


thanks a lot for the fast reply.
So I understand correctly that no output from bounding k is written since this is simply not applicable?


By the way thanks again for this implementation of dynamic smagorinsky for the versions OF4 and upwards. The results are practically identical to my previous simulations with OF231.


Best wishes
Johannes

[Santiago]

Originally Posted by syavash

Dear Johannes,

AFAIK, k is bounded only when its value is smaller than SMALL=1e-20, otherwise its minimum value would be read from the field.

But in general, bounding k to a minimum value should not affect the solution procedure as k is an independent quantity. It is considered in the SGS stress tensor only. It will become more noticeable if you would like to calculate the ratio of resolved to total turbulent kinetic energy.

Regards,
Syavash

It is true that k is not being used for any further calculation, but the sole fact that k is being bounded it means that something is going wrong on the way your algorithm is calculating things. It is simply not possible to have k<0 by using a purely dissipative smagorinsky model. In the case where deconvolution (eg, bardina) are used for reconstructing L, k<0 MIGHT occur, but rarely, and should be clipped away.

[syavash]

Originally Posted by KingKraut

Dear syavash,


thanks a lot for the fast reply.
So I understand correctly that no output from bounding k is written since this is simply not applicable?


By the way thanks again for this implementation of dynamic smagorinsky for the versions OF4 and upwards. The results are practically identical to my previous simulations with OF231.


Best wishes
Johannes

Dear Johannes,

You're welcome.
You don't see the output since the function "bound" is not used anymore.

Best Regards,
Syavash

[boundary93]

Could somebody please explain what I have to change if I want to use it with a compressible solver. I tried to compare the Smagorinsky model to see what to change but if I start it still tells me the dynamic model is not available.

I want to use the version of syavash: https://github.com/syavash20/TurbLab



Thanks in advance

[boundary93]

Originally Posted by boundary93

Could somebody please explain what I have to change if I want to use it with a compressible solver. I tried to compare the Smagorinsky model to see what to change but if I start it still tells me the dynamic model is not available.

I want to use the version of syavash: https://github.com/syavash20/TurbLab



Thanks in advance

I had to change the makeTurbulence.C to this

// Copyright held by original authors

#include "CompressibleTurbulenceModel.H"
#include "compressibleTransportModel.H"
#include "fluidThermo.H"
#include "addToRunTimeSelectionTable.H"
#include "makeTurbulenceModel.H"

#include "ThermalDiffusivity.H"
#include "EddyDiffusivity.H"

#include "LESModel.H"

#define makeLESModel(Type)                                                     \
    makeTemplatedTurbulenceModel                                               \
    (fluidThermoCompressibleTurbulenceModel, LES, Type)
    
namespace Foam
{
    typedef ThermalDiffusivity<CompressibleTurbulenceModel<fluidThermo> >  fluidThermoCompressibleTurbulenceModel;    

    typedef LESModel<EddyDiffusivity<fluidThermoCompressibleTurbulenceModel> >  LESfluidThermoCompressibleTurbulenceModel;       
}

#include "dynamicSmagorinsky.H"
makeLESModel(dynamicSmagorinsky);

and the Make file to this

EXE_INC = \
    -I$(LIB_SRC)/TurbulenceModels/compressible/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \
    -I$(LIB_SRC)/transportModels/compressible/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/solidThermo/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/solidSpecie/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude \

LIB_LIBS = \
    -lcompressibleTransportModels \
    -lfluidThermophysicalModels \
    -lsolidThermo \
    -lsolidSpecie \
    -lturbulenceModels \
    -lspecie \
    -lfiniteVolume \
    -lmeshTools

my mistake was a missing LIB but with this changes it works

[Tian Jin]

Hello.

I want to employ the dynamic procedure on the scalar flux, but I don't know if we can get dynamic diffusivity or Schmidt number in the dynamic Smagorinsky model.

Is there anyone doing this before?

For now, I use the dynamic Smagorinsky model for the flow, but for the scalar transport, I use the function scalartransport in OpenFOAM, they need alpha_t and alpha, and this is the constant value, I want to use dynamic diffusivity/Schmidt number in the scalar transport equation. Does anyone have the good idea?

[Santiago]

Originally Posted by Tian Jin

Hello.

I want to employ the dynamic procedure on the scalar flux, but I don't know if we can get dynamic diffusivity or Schmidt number in the dynamic Smagorinsky model.

Is there anyone doing this before?

For now, I use the dynamic Smagorinsky model for the flow, but for the scalar transport, I use the function scalartransport in OpenFOAM, they need alpha_t and alpha, and this is the constant value, I want to use dynamic diffusivity/Schmidt number in the scalar transport equation. Does anyone have the good idea?

If you mean whether someone has done it, yes. Check Armenio & Piomelli (2000). If what you mean is whether such a model has been implemented in OpenFOAM, then also yes, check this article:

https://www.mdpi.com/2311-5521/4/3/171

[Tian Jin]

Originally Posted by Santiago

If you mean whether someone has done it, yes. Check Armenio & Piomelli (2000). If what you mean is whether such a model has been implemented in OpenFOAM, then also yes, check this article:

https://www.mdpi.com/2311-5521/4/3/171

Thanks very much, Santiago.

I am a beginner and I don't know how to translate your formula to OpenFOAM code. Would you be kind enough to share with me your OpenFOAM code about the dynamic scalar flux?