[Kosdalak]

Hey,

I'm currently trying to implement my own RSM Model in OF.
For that I just copied the SSG Files in a new directory with the goal to change them later.

Before that I tried to compile them after changing their names and all appearances in the files. No Errors so far (nothing really changed, so why should be there erros?). I was using the "makeTemplatedTurbulenceModel" macro. That's the way you should implement your own model, right?

Now, I started a test run with the "new" model. Not found... I got a small warning directly at the start (loading my own, new library with the model):

--> FOAM Warning : 
    From function void* Foam::dlOpen(const Foam::fileName&, bool)
    in file POSIX.C at line 1251
    dlopen error : /home/xxx/OpenFOAM/xxx-X/platforms/linux64GccDPInt32Opt/lib/libmySSGLRR.so: undefined symbol: _ZN4Foam8RASModelINS_29IncompressibleTurbulenceModelINS_15turbulenceModelEEEE8typeNameE
--> FOAM Warning : 
    From function bool Foam::dlLibraryTable::open(const Foam::fileName&, bool)
    in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 105
    could not load "libmySSGLRR.so"

Obviously, the library was not load because of a undefined symbol. I figured out it could help to load an extra library with this symbol within it.
BUT there is no library with this symbol in it (at least not in the normal directory...)


I using OF Version 7 on Ubuntu 20.04.1 LTS.

Does anybody have an idea how I can solve this problem?
Thanks in advance!

Jan

[agustinvo]

Hi,


as far as I know, it's better if you replicate the existing files structure in your OF user directory, instead of generating your own library like this. It can also help to implement more models in the future. At least, this is what I do and I had no problems until now.


PS: I'm curious about the RSM model you want to implement. ¿Which one is it?

[Kosdalak]

I have to admit thats a good idea. You mean just copy the whole installation of OF and than change the "original" models?

I want to try the SSG-LRR omega model proposed by Eisfeld. The basic idea is to combine the SSG and the LRR with a omega equation and to create a low Re model (like Menters SST).

The (I believe original paper) is:
"REYNOLDS STRESS MODELLING FOR COMPLEX AERODYNAMIC
FLOWS" from Bernhard Eisfeld.
You can also check the NASA website:
https://turbmodels.larc.nasa.gov/rsm-ssglrr.html

[agustinvo]

The idea is to replicate the folders structure. Then, on the wmake files tou just link these libraries to the ones of the installation if needed (e.g. when compiling a new turbulence model just link it to the turbulence model).

[clapointe]

To add to the discussion, for OF7 specifically, what I've done in the past is :

Like was suggested make folders in e.g. your project directory for src/TurbulenceModels/turbulenceModels/RAS and src/TurbulenceModels/compressible (or incompressible)

Then just add new code, without replicating native code, in each folder respectively. An example for compressible LES models can be found here : https://github.com/clapointe2011/public/tree/master/of7. The resulting library can be loaded at runtime to use your custom model.

Caelan

[nainavinod]

Hey Jan!

This might be late, but I have succesfully implemented the SSG/LRR-omega fully turbulent model by Eisfeld et al., (that you're referring to) on OpenFOAM-v2006. You can find the code here:
https://github.com/nainapisharoti/SSG-LRR-omega-gamma

You can find the complete code for the SSG/LRR-omega model in the "Base folder". The "RAS" folder also has the makeTurbulenceModel.C script which you just have to compile using "wmake" and you should be good to go.

I had implemented the fully turbulent model to formulate my transition model SSG/LRR-omega-gamma. If you're interested, you can find the code for that as well in the same repository.

Good luck!
Naina.

[sr786]

Hi,

I know this is an old thread but I am also looking into implementing changes with the Reynolds Stress models using OpenFOAM. All I am looking to do is simplify the DREff() term in the .C file. I am using OpenFOAM-v9.

Prior to introducing any changes to the source code I am first sorting out compiling a new turbulence model.

I have found that I am really struggling to compile either the LRR or SSG model in the OpenFOAM environment as compared to compiling a eddy viscosity model.

Here are my Make files

Options

  EXE_INC = \
    -I$(LIB_SRC)/MomentumTransportModels/momentumTransportModels/lnInclude \
    -I$(LIB_SRC)/MomentumTransportModels/incompressible/lnInclude \
    -I$(LIB_SRC)/transportModels/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude \

LIB_LIBS = \
    -ltransportModels \
    -lmomentumTransportModels \
    -lfiniteVolume \
    -lmeshTools

Files

mykinematicMomentumTransportModels.C


LIB = $(FOAM_USER_LIBBIN)/mykinematicMomentumTransportModels

I am getting the following error message

  wmake libso .
wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file mykinematicMomentumTransportModels.C
g++ -std=c++14 -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 -Wno-attributes -O3  -DNoRepository -ftemplate-depth-100 -I/home/cfd/OpenFOAM/OpenFOAM-9/src/MomentumTransportModels/momentumTransportModels/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/MomentumTransportModels/incompressible/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/transportModels/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/finiteVolume/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/meshTools/lnInclude  -IlnInclude -I. -I/home/cfd/OpenFOAM/OpenFOAM-9/src/OpenFOAM/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/OSspecific/POSIX/lnInclude   -fPIC -c mykinematicMomentumTransportModels.C -o Make/linux64GccDPInt32Opt/mykinematicMomentumTransportModels.o
In file included from myLRR.H:219:0,
                 from mykinematicMomentumTransportModels.C:49:
myLRR.C: In instantiation of ‘Foam::RASModels::myLRR<BasicMomentumTransportModel>::myLRR(const alphaField&, const rhoField&, const volVectorField&, const surfaceScalarField&, const surfaceScalarField&, const transportModel&, const Foam::word&) [with BasicMomentumTransportModel = Foam::IncompressibleMomentumTransportModel<Foam::kinematicTransportModel>; Foam::RASModels::myLRR<BasicMomentumTransportModel>::alphaField = Foam::geometricOneField; Foam::RASModels::myLRR<BasicMomentumTransportModel>::rhoField = Foam::geometricOneField; Foam::volVectorField = Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>; Foam::surfaceScalarField = Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>; Foam::RASModels::myLRR<BasicMomentumTransportModel>::transportModel = Foam::kinematicTransportModel]’:
/home/cfd/OpenFOAM/OpenFOAM-9/src/MomentumTransportModels/momentumTransportModels/lnInclude/RASModel.H:100:9:   required from ‘static Foam::autoPtr<Foam::RASModel<BasicMomentumTransportModel> > Foam::RASModel<BasicMomentumTransportModel>::adddictionaryConstructorToTable<RASModelType>::New(const alphaField&, const rhoField&, const volVectorField&, const surfaceScalarField&, const surfaceScalarField&, const transportModel&) [with RASModelType = Foam::RASModels::myLRR<Foam::IncompressibleMomentumTransportModel<Foam::kinematicTransportModel> >; BasicMomentumTransportModel = Foam::IncompressibleMomentumTransportModel<Foam::kinematicTransportModel>; Foam::RASModel<BasicMomentumTransportModel>::alphaField = Foam::geometricOneField; Foam::RASModel<BasicMomentumTransportModel>::rhoField = Foam::geometricOneField; Foam::volVectorField = Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>; Foam::surfaceScalarField = Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>; Foam::RASModel<BasicMomentumTransportModel>::transportModel = Foam::kinematicTransportModel]’
/home/cfd/OpenFOAM/OpenFOAM-9/src/MomentumTransportModels/momentumTransportModels/lnInclude/RASModel.H:100:9:   required from ‘Foam::RASModel<BasicMomentumTransportModel>::adddictionaryConstructorToTable<RASModelType>::adddictionaryConstructorToTable(const Foam::word&) [with RASModelType = Foam::RASModels::myLRR<Foam::IncompressibleMomentumTransportModel<Foam::kinematicTransportModel> >; BasicMomentumTransportModel = Foam::IncompressibleMomentumTransportModel<Foam::kinematicTransportModel>]’
mykinematicMomentumTransportModels.C:50:1:   required from here
myLRR.C:219:14: error: ‘bound’ was not declared in this scope
         bound(epsilon_, this->epsilonMin_);
         ~~~~~^~~~~~~~~~~~~~~~~~~~~~~~~~~~~
myLRR.C:219:14: note: suggested alternative: ‘found’
         bound(epsilon_, this->epsilonMin_);
         ~~~~~^~~~~~~~~~~~~~~~~~~~~~~~~~~~~
         found
myLRR.C: In instantiation of ‘void Foam::RASModels::myLRR<BasicMomentumTransportModel>::correct() [with BasicMomentumTransportModel = Foam::IncompressibleMomentumTransportModel<Foam::kinematicTransportModel>]’:
mykinematicMomentumTransportModels.C:50:20:   required from here
myLRR.C:325:10: error: ‘bound’ was not declared in this scope
     bound(epsilon_, this->epsilonMin_);
     ~~~~~^~~~~~~~~~~~~~~~~~~~~~~~~~~~~
myLRR.C:325:10: note: suggested alternative: ‘found’
     bound(epsilon_, this->epsilonMin_);
     ~~~~~^~~~~~~~~~~~~~~~~~~~~~~~~~~~~
     found
make: *** [/home/cfd/OpenFOAM/OpenFOAM-9/wmake/rules/General/transform:26: Make/linux64GccDPInt32Opt/mykinematicMomentumTransportModels.o] Error 1

I have no clue as to why this has happened. As you guys have managed to successfully implement a new RSM could I please have some guidance on why I can't compile LRR?

A link to the thread I originally published is provided OpenFOAM - Implement Change To Modelled Term Reynolds Stress Models (LRR & SSG)

[nainavinod]

Hey! It seems like you might be missing some header file declarations. Have you made sure you have included the following lines in your header file?

#include "RASModel.H"
#include "ReynoldsStress.H"

Can you also share the way you have declared your model class at the beginning of your header file?
Maybe you're missin some step there.

Regards,
Naina.

[sr786]

Hi,

For myLRR.H, both RASModel.H and ReynoldsStress.H have been declared as I have not made any changes to the files barring changing LRR to myLRR

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Copyright (C) 2011-2021 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.

    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.

    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.

    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.

Class
    Foam::RASModels::myLRR

Description
    Launder, Reece and Rodi Reynolds-stress turbulence model for
    incompressible and compressible flows.

    Reference:
    \verbatim
        Launder, B. E., Reece, G. J., & Rodi, W. (1975).
        Progress in the development of a Reynolds-stress turbulence closure.
        Journal of fluid mechanics, 68(03), 537-566.
    \endverbatim

    Including the recommended generalised gradient diffusion model of
    Daly and Harlow:
    \verbatim
        Daly, B. J., & Harlow, F. H. (1970).
        Transport equations in turbulence.
        Physics of Fluids (1958-1988), 13(11), 2634-2649.
    \endverbatim

    Optional Gibson-Launder wall-reflection is also provided:
    \verbatim
        Gibson, M. M., & Launder, B. E. (1978).
        Ground effects on pressure fluctuations in the
        atmospheric boundary layer.
        Journal of Fluid Mechanics, 86(03), 491-511.
    \endverbatim

    The default model coefficients are:
    \verbatim
        myLRRCoeffs
        {
            Cmu             0.09;
            C1              1.8;
            C2              0.6;
            Ceps1           1.44;
            Ceps2           1.92;
            Cs              0.25;
            Ceps            0.15;

            wallReflection  yes;
            kappa           0.41
            Cref1           0.5;
            Cref2           0.3;

            couplingFactor  0.0;
        }
    \endverbatim

SourceFiles
    myLRR.C

\*---------------------------------------------------------------------------*/

#ifndef myLRR_H
#define myLRR_H

#include "RASModel.H"
#include "ReynoldsStress.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

I've been really stuck on why its failing to compile. If I can get it to compile successfully then the change I want to implement should be very straightforward

[dlahaye]

Pls. share here the output of the linux command

nm -g myLRR.o

[sr786]

Hi,

Here is the output of the command

 cfd@UOL-PC-301943:~/OF_cases/myLRR> nm -g myLRR.o
nm: 'myLRR.o': No such file

[sr786]

I think that command might be redundant in OF9. As I typed the same thing for a compiled mykOmega and it gave the same output message:

 cfd@UOL-PC-301943:~/OF_cases/mykOmega> wmake libso
wmake libso .
wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file mykinematicMomentumTransportModels.C
g++ -std=c++14 -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 -Wno-attributes -O3  -DNoRepository -ftemplate-depth-100 -I/home/cfd/OpenFOAM/OpenFOAM-9/src/MomentumTransportModels/momentumTransportModels/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/MomentumTransportModels/incompressible/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/transportModels/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/finiteVolume/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/meshTools/lnInclude  -IlnInclude -I. -I/home/cfd/OpenFOAM/OpenFOAM-9/src/OpenFOAM/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/OSspecific/POSIX/lnInclude   -fPIC -c mykinematicMomentumTransportModels.C -o Make/linux64GccDPInt32Opt/mykinematicMomentumTransportModels.o
g++ -std=c++14 -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 -Wno-attributes -O3  -DNoRepository -ftemplate-depth-100 -I/home/cfd/OpenFOAM/OpenFOAM-9/src/MomentumTransportModels/momentumTransportModels/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/MomentumTransportModels/incompressible/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/transportModels/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/finiteVolume/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/meshTools/lnInclude  -IlnInclude -I. -I/home/cfd/OpenFOAM/OpenFOAM-9/src/OpenFOAM/lnInclude -I/home/cfd/OpenFOAM/OpenFOAM-9/src/OSspecific/POSIX/lnInclude   -fPIC -fuse-ld=bfd -shared -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPInt32Opt/mykinematicMomentumTransportModels.o -L/home/cfd/OpenFOAM/OpenFOAM-9/platforms/linux64GccDPInt32Opt/lib \
    -ltransportModels -lmomentumTransportModels -lfiniteVolume -lmeshTools  -o /home/cfd/OpenFOAM/cfd-9/platforms/linux64GccDPInt32Opt/lib/mykinematicMomentumTransportModels.so
cfd@UOL-PC-301943:~/OF_cases/mykOmega> nm -g mykOmega.o
nm: 'mykOmega.o': No such file

[dlahaye]

Apologies, my bad.

In case that the compilation of myLRR.C fails, the file myLRR.o is indeed not created.

Pls. share output of

nm -g LRR.o

Observe the use of the original LRR.o here.

[sr786]

Hi,

I've inputted the same command but for LRR.o, same result

 cfd@UOL-PC-301943:~/OF_cases> nm -g LRR.o
nm: 'LRR.o': No such file

[dlahaye]

In the compilation of kEpsilon.C, kOmega.C and LRR.C does succeed (as you claim above), the files kEpsilon.o, kOmega.o and LRR.o should most obviously be created and written somewhere.

[sr786]

When I compile mykOmega I get a .o file for mykinematicMomentumTransportModels.o

 cfd@UOL-PC-301943:~/OF_cases/mykOmega/Make/linux64GccDPInt32Opt> ls
files  mykinematicMomentumTransportModels.C.dep  mykinematicMomentumTransportModels.o
cfd@UOL-PC-301943:~/OF_cases/mykOmega/Make/linux64GccDPInt32Opt>

[sr786]

When I attempt to compile myLRR, the .o file is missing for mykinematicMomentumTransportModels.o

 cfd@UOL-PC-301943:~/OF_cases/myLRR/Make/linux64GccDPInt32Opt> ls
files  mykinematicMomentumTransportModels.C.dep
cfd@UOL-PC-301943:~/OF_cases/myLRR/Make/linux64GccDPInt32Opt>

[sr786]

Okay, I spoke to someone with experience in modifying source code for OpenFOAM. He went through my test case and found that in the myLRR.C file, you have to include the following term:

#include "simpleLRR.H"
#include "fvModels.H"
#include "fvConstraints.H"
#include "wallDist.H"
#include "bound.C"

Which for some reason was omitted in the LRR file originally. This allowed me to successfully compile a new turbulence model and test it worked.

SIMPLE: Convergence criteria found
        U: tolerance 1e-05
        p: tolerance 1e-05
        k: tolerance 1e-05
        epsilon: tolerance 1e-05
        R: tolerance 1e-05
        omega: tolerance 1e-05

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model myLRR
RAS
{
    model           myLRR;
    turbulence      on;
    printCoeffs     on;
    couplingFactor  0;
    Cmu             0.09;
    C1              1.8;
    C2              0.6;
    Ceps1           1.44;
    Ceps2           1.92;
    Cs              0.25;
    Ceps            0.15;
    wallReflection  true;
    kappa           0.41;
    Cref1           0.5;
    Cref2           0.3;
}

Creating MRF zone list from MRFProperties
    creating MRF zone: SRF
No fvModels present
No fvConstraints present

Starting time loop

[sr786]

I've now managed to implement my changes and I can successfully compile and run a simulation


The simulation can run in serial or parallel. The only thing I am noticing is for a parallel run some warning symbols appear when decomposing:

--> FOAM Warning : 
    From function void* Foam::dlOpen(const Foam::fileName&, bool)
    in file POSIX.C at line 1247
    dlopen error : /home/cfd/OpenFOAM/cfd-9/platforms/linux64GccDPInt32Opt/lib/libsimpleLRRMomentumTransportModels.so: undefined symbol: _ZTIN4Foam36incompressibleMomentumTransportModelE
--> FOAM Warning : 
    From function bool Foam::dlLibraryTable::open(const Foam::fileName&, bool)
    in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 106
    could not load "libsimpleLRRMomentumTransportModels.so" 

FOAM Warning : 
    From function void* Foam::dlOpen(const Foam::fileName&, bool)
    in file POSIX.C at line 1247
    dlopen error : /home/cfd/OpenFOAM/cfd-9/platforms/linux64GccDPInt32Opt/lib/libsimpleLRRMomentumTransportModels.so: undefined symbol: _ZTIN4Foam36incompressibleMomentumTransportModelE
--> FOAM Warning : 
    From function bool Foam::dlLibraryTable::open(const Foam::fileName&, bool)
    in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 106
    could not load "libsimpleLRRMomentumTransportModels.so"

Is this just a bug as the simulation still runs regardless of the warning sign. Someone else has also made a similar observation before too in reddit https://www.reddit.com/r/OpenFOAM/co...ryso_warnings/ and he suggested the warning signs didn't make any difference as he could still run his simulations.

[lpz456]

Have you solve this problem? I also met the issue. I want to create a base model like kOmegaSSTBase model, and derive other models. Ths same issue happened.