How to add a turbulence model in OpenFOAM-3.0.0

Hassan Kassem

Comments

Source

/images/template.png

In OpenFOAM-3.0.0 [1], the turbulence models library had major facelift. Actually, it had major operation not just a facelift. Now, all models are based on one base template class including RANS, LES, incompressible and compressible. Therefore, if you followed most of the available tutorials on how to modify/implement turbulence model, it will not work. You will face many compiler errors from the first step. This post shows how to overcome this problem step-by-step. Moreover, it discusses briefly the reasons causing these errors.

What is the problem?

Back in January 2015, a new commit [2] was pushed to OpenFOAM-dev repository on gitHub [3]. This update was relased in November 2015 with OpenFOAM-3.0.0 [4]. The new implementation is based on multilayer template class [5]. If you normally consider a class as a blueprint of an object, then you can consider template class as a blueprint of a blueprint of an object. An object of class is usually initialised in the main program and the compiler does not have to know anything about it during the compilation process of the class. Unlike a template which is written by the compiler.

First let's compare how add a turbulence model in the old versions and what will happen if we followed the same process in OpenFOAM-3.0.0.

Previous versions

As you may read in many available tutorials online about how to create a new turbulence model in OpenFOAM, you just have to follow the these steps to create incompressible turbulence model based on realizableKE

# copy to run directory
$ cp -r $FOAM_SRC/turbulenceModels/incompressible/RAS/realizableKE/ .
# rename all files
$ mv realizableKE myrealizableKE
$ mv myrealizableKE/realizableKE.H myrealizableKE/myrealizableKE.H
$ mv myrealizableKE/realizableKE.C myrealizableKE/myrealizableKE.C
# rename all instances of realizableKE to myrealizableKE
# you can use replace all in your text editor
$ find myrealizableKE -type f -exec sed -i 's/realizableKE/myrealizableKE/g' {} \;

Then a Make directory is needed to compile the new mode,

Make/files

myrealizableKE.C

LIB = $(FOAM_USER_LIBBIN)/libmyrealizableKE

Make/options (you can copy it from $FOAM_SRC/turbulenceModels/incompressible/RAS/Make/options and link it to RASModels library)

EXE_INC = \
    -I$(LIB_SRC)/turbulenceModels/incompressible/RAS/lnInclude \
    -I$(LIB_SRC)/turbulenceModels \
    -I$(LIB_SRC)/transportModels \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude

LIB_LIBS = \
    -lincompressibleRASModels \
    -lincompressibleTurbulenceModel \
    -lfiniteVolume \
    -lmeshTools

For compressible flow, it is the same process with minor modifications to Make. That is all you need, just add the new library to controlDict libs and you are ready to go.

New version

let's try to apply the same steps using any OpenFOAM version starting from v-3.0.0

# note: Diffrent path.
$ cp -r $FOAM_SRC/TurbulenceModels/turbulenceModels/RAS/realizableKE .

Then follow the same steps as Previous versions. If you still not sure how to update your case files to v-3.0.0, check this post [6]

First error

If you followed these steps you will get a very long error but actually it is just one repeated error like this one,

myrealizableKE.C:###:##: error: redefinition of 'function name'
myrealizableKE.C:###:##: note: 'function name' previously declared here

Probably you are familiar with such error. It basically means that the member functions of class myrealizableKE are defined more than once. Indeed the compiler never lies unless it has a bug. The first idea could be tried to over come this error is removing the following three lines in the myrealizableKE.H (comment them out we will need them later). You maybe do not understand these lines but .C file included in .H file in C++ looks weird!!

// #ifdef NoRepository
// #   include "myrealizableKE.C"
// #endif

Now recompile the code, surprisingly no errors!!

Second error

However this code was compiled without any errors, it will not work. That could be confirmed by linking the library to any case and select the new turbulence model myrealizableKE. Simply the solver will not recognise the new model. Now, uncomment the three lines and save all files and let's solve this problem.

Solution

Definitely copy and rename strategy does not work here. There are two reasons causing this problem and you may face if you tried to modify any of the core template libraries in OpenFOAM. The first reason is the fact that myrealizableKE is a template class. The second reason, it is not included in the run time table [7].

RANS incompressible models

Follow the same steps as described in New version section but an extra file is needed which you can copy from OpenFOAM source

$ cp $FOAM_SRC/TurbulenceModels/incompressible/turbulentTransportModels/turbulentTransportModels.C makeTurModel.C

In simple words, this file has two tasks. The first task this file will do is inislize the template class [8] [9]. The second task is adding the new model to the run time selection table.

Edit makeTurModel.C (Please note this file is based on turbulentTransportModels.C and makeTurbulenceModel.H)

 #include "IncompressibleTurbulenceModel.H"
 #include "transportModel.H"
 #include "addToRunTimeSelectionTable.H"
 #include "makeTurbulenceModel.H"

 #include "laminar.H"
 #include "RASModel.H"
 #include "LESModel.H"

 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 #define createBaseTurbulenceModel(Alpha, Rho, baseModel, BaseModel, Transport) \
                                                                                \
     namespace Foam                                                             \
     {                                                                          \
         typedef BaseModel<Transport> Transport##BaseModel;                     \
         typedef RASModel<Transport##BaseModel> RAS##Transport##BaseModel;      \
         typedef LESModel<Transport##BaseModel> LES##Transport##BaseModel;      \
     }

 createBaseTurbulenceModel
 (
     geometricOneField,
     geometricOneField,
     incompressibleTurbulenceModel,
     IncompressibleTurbulenceModel,
     transportModel
 );

 #define makeRASModel(Type)                                                     \
     makeTemplatedTurbulenceModel                                               \
     (transportModelIncompressibleTurbulenceModel, RAS, Type)

 #define makeLESModel(Type)                                                     \
     makeTemplatedTurbulenceModel                                               \
     (transportModelIncompressibleTurbulenceModel, LES, Type)

#include "myrealizableKE.H"
makeRASModel(myrealizableKE);

Also modify files to compile makeTurModel.C

makeTurModel.C

LIB = $(FOAM_USER_LIBBIN)/libmyrealizableKE

Finally options

EXE_INC = \
    -I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/incompressible/lnInclude \
    -I$(LIB_SRC)/transportModels/incompressible/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude

LIB_LIBS = \
    -lturbulenceModels \
    -lincompressibleTurbulenceModels \
    -lincompressibleTransportModels \
    -lfiniteVolume \
    -lmeshTools

RANS compressible models

Here you can see a glimpse of the beauty of template classes in C++ (You do not have to agree with me on this!). The same source files myrealizableKE.H and myrealizableKE.C can be used to compile the same model but for compressible flow. Only makeTurModel.C and Make need to be modified as follows, (Please note this file is based on turbulentFluidThermoModels.C and compressible/makeTurbulenceModel.H)

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

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

#include "laminar.H"
#include "RASModel.H"
#include "LESModel.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#define createBaseTurbulenceModel(                                             \
    Alpha, Rho, baseModel, BaseModel, TDModel, Transport)                      \
                                                                               \
    namespace Foam                                                             \
    {                                                                          \
        typedef TDModel<BaseModel<Transport>>                                  \
            Transport##BaseModel;                                              \
        typedef RASModel<EddyDiffusivity<Transport##BaseModel>>                \
            RAS##Transport##BaseModel;                                         \
        typedef LESModel<EddyDiffusivity<Transport##BaseModel>>                \
            LES##Transport##BaseModel;                                         \
    }

createBaseTurbulenceModel
(
    geometricOneField,
    volScalarField,
    compressibleTurbulenceModel,
    CompressibleTurbulenceModel,
    ThermalDiffusivity,
    fluidThermo
);

#define makeRASModel(Type)                                                     \
    makeTemplatedTurbulenceModel                                               \
    (fluidThermoCompressibleTurbulenceModel, RAS, Type)

#define makeLESModel(Type)                                                     \
    makeTemplatedTurbulenceModel                                               \
    (fluidThermoCompressibleTurbulenceModel, LES, Type)

#include "myrealizableKE.H"
makeRASModel(myrealizableKE);

In files just change the name of the compiled dynamic library and change options to

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

The order of first two links in EXE_INC is essential.

Final Remarks

The introduced createBaseTurbulenceModel macro is based on makeBaseTurbulenceModel which is included in OpenFOAM source code. It can be used with LES models as well, but with using makeLESModel instead of makeRASModel. Hopefully in the near future, I will explain this solution in more details. If you interested in adding new phaseCompressible turbulence model, please check my post on CFD-online [10].

Please feel free to comment below. Your feedback will be highly appreciated.

[1] OpenFOAM® and OpenCFD® are registered trademarks of OpenCFD Limited, the producer OpenFOAM software. All registered trademarks are property of their respective owners. This offering is not approved or endorsed by OpenCFD Limited, the producer of the OpenFOAM software and owner of the OPENFOAM® and OpenCFD® trade marks. Hassan Kassem is not associated to OpenCFD.
[2] commit 93732c8af4a545c617399600ee810081fdb42b07
[3] OpenFOAM-dev
[4] OpenFOAM 3.0.0 relase notes 2015
[5] Templates and Template Classes in C++
[6] Updating OpenFOAM case files for 3.0.x
[7] Run-Time Type Selection Series, sourceflux blog
[8] Compiling Template Classes
[9] How To Organize Template Source Code
[10] Adding New phaseCompressible Turbulence Model

Comments

Comments powered by Disqus