OpenFoam-6 导入并编译一个新湍流模型

本文参考了以下链接
http://hassankassem.me/posts/newturbulencemodel/#new-version
https://pingpong.chalmers.se/public/courseId/7056/lang-en/publicPage.do?item=3256524
https://www.cfd-online.com/Forums/openfoam-programming-development/181508-addition-new-turbulence-models-giviing-errors.html#post660305
https://www.cfd-online.com/Forums/openfoam/199105-error-during-add-turbulence-model-openfoam-5-0-a.html
https://www.cfd-online.com/Forums/openfoam-programming-development/191446-symbol-lookup-error-simplefoam.html

一准备原始模型

首先,在终端在定位到你的工作目录,然后执行以下操作(如果你不熟悉命令行操作,也可以按注释进行图形界面的操作)

#从$FOAM_SRC/TurbulenceModels/turbulenceModels/RAS/ 中复制kOmegaSST文件夹并改名为newkOmegaSST
cp  -r $FOAM_SRC/TurbulenceModels/turbulenceModels/RAS/kOmegaSST $FOAM_RUN/newkOmegaSST
# 进入你新建的文件夹
cd newkOmegaSST
# 将文件夹中的kOmegaSST.H命名为newkOmegaSST.H
mv kOmegaSST.H newkOmegaSST.H
# 将文件夹中的kOmegaSST.C命名为newkOmegaSST.C
mv kOmegaSST.C newkOmegaSST.C
# 复制 $FOAM_SRC/TurbulenceModels/incompressible中的Make文件夹到你的工作目录
cp -r $FOAM_SRC/TurbulenceModels/incompressible/Make/ .
cp -r $FOAM_SRC/TurbulenceModels/incompressible/turbulentTransportModels/turbulentTransportModels.C maketurbulentTransportModels.C

二修改编译配置

在前述操作中,你从OpenFOAM的源文件中复制了一个名为turbulentTransportModels.C的文件,并将其命名为maketurbulentTransportModels.C
现在打开该文件,仅保留第一个#include声明及第一个宏命令,其余内容全部删除,并添加下述内容:

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

修改完成后的文件如下所示

接着你应当修改Make文件夹下的files文件
首先打开这个文件,并清空里面的内容,并加入如下代码,最后保存退出
这段代码表示了.so文件的生成路径，也可以生成在当前目录下，需要调用的时候指定.so文件所在目录就行

maketurbulentTransportModels.C
LIB = $(FOAM_USER_LIBBIN)/libmyincompressibleTurbulenceModels

如下图所示

对Make文件夹下的options作如下操作
清空该文件原始内容,并添加如下代码,保存退出.

EXE_INC = \-I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \-I$(LIB_SRC)/TurbulenceModels/incompressible/lnInclude \-I$(LIB_SRC)/transportModels \-I$(LIB_SRC)/finiteVolume/lnInclude \-I$(LIB_SRC)/meshTools/lnInclude \LIB_LIBS = \-lincompressibleTransportModels \-lturbulenceModels \-lfiniteVolume \-lmeshTools

如下图所示

三修改.H 和.C 文件

采用gedit命令分别打开newkOmegaSST.H和newkOmegaSST.C文件，将原有出现kOmegaSST的地方使用newkOmegaSST进行替换，但使用sed命令进行替换时需要注意不要将基类替换，这里需要替换的地方较少我采用手动替换，以便清楚展示。
newkOmegaSST.H

/*---------------------------------------------------------------------------*\=========                 |\\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox\\    /   O peration     | Website:  https://openfoam.org\\  /    A nd           | Copyright (C) 2016-2018 OpenFOAM Foundation\\/     M anipulation  |
-------------------------------------------------------------------------------
LicenseThis file is part of OpenFOAM.OpenFOAM is free software: you can redistribute it and/or modify itunder the terms of the GNU General Public License as published bythe 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 WITHOUTANY WARRANTY; without even the implied warranty of MERCHANTABILITY orFITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public Licensefor more details.You should have received a copy of the GNU General Public Licensealong with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.\*---------------------------------------------------------------------------*/#include "newkOmegaSST.H"// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //namespace Foam
{
namespace RASModels
{// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //template<class BasicTurbulenceModel>
newkOmegaSST<BasicTurbulenceModel>::newkOmegaSST
(const alphaField& alpha,const rhoField& rho,const volVectorField& U,const surfaceScalarField& alphaRhoPhi,const surfaceScalarField& phi,const transportModel& transport,const word& propertiesName,const word& type
)
:Foam::kOmegaSST<eddyViscosity<RASModel<BasicTurbulenceModel>>,BasicTurbulenceModel>(type,alpha,rho,U,alphaRhoPhi,phi,transport,propertiesName)
{if (type == typeName){this->printCoeffs(type);}
}// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //} // End namespace RASModels
} // End namespace Foam// ************************************************************************* //

newkOmegaSST.H

/*---------------------------------------------------------------------------*\=========                 |\\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox\\    /   O peration     | Website:  https://openfoam.org\\  /    A nd           | Copyright (C) 2016-2018 OpenFOAM Foundation\\/     M anipulation  |
-------------------------------------------------------------------------------
LicenseThis file is part of OpenFOAM.OpenFOAM is free software: you can redistribute it and/or modify itunder the terms of the GNU General Public License as published bythe 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 WITHOUTANY WARRANTY; without even the implied warranty of MERCHANTABILITY orFITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public Licensefor more details.You should have received a copy of the GNU General Public Licensealong with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.ClassFoam::RASModels::kOmegaSSTDescriptionSpecialisation for RAS of the generic kOmegaSSTBase base class.For more information, see Description of kOmegaSSTBase.HSee alsoFoam::kOmegaSSTSourceFileskOmegaSST.C\*---------------------------------------------------------------------------*/#ifndef newkOmegaSST_H
#define newkOmegaSST_H#include "kOmegaSSTBase.H"
#include "RASModel.H"
#include "eddyViscosity.H"// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //namespace Foam
{
namespace RASModels
{/*---------------------------------------------------------------------------*\Class kOmegaSST Declaration
\*---------------------------------------------------------------------------*/template<class BasicTurbulenceModel>
class newkOmegaSST
:public Foam::kOmegaSST<eddyViscosity<RASModel<BasicTurbulenceModel>>,BasicTurbulenceModel>
{public:typedef typename BasicTurbulenceModel::alphaField alphaField;typedef typename BasicTurbulenceModel::rhoField rhoField;typedef typename BasicTurbulenceModel::transportModel transportModel;//- Runtime type informationTypeName("newkOmegaSST");// Constructors//- Construct from componentsnewkOmegaSST(const alphaField& alpha,const rhoField& rho,const volVectorField& U,const surfaceScalarField& alphaRhoPhi,const surfaceScalarField& phi,const transportModel& transport,const word& propertiesName = turbulenceModel::propertiesName,const word& type = typeName);//- Destructorvirtual ~newkOmegaSST(){}
};// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //} // End namespace RASModels
} // End namespace Foam// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#ifdef NoRepository#include "newkOmegaSST.C"
#endif// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif// ************************************************************************* //

四编译

定位到newkOmegaSST文件夹，wclean,wmake进行编译
如图所示

五调用新模型计算

复制simpleFoam中的pitzDaily算例至$FOAM_RUN文件夹，在system文件夹中的controlDict文件中添加以下语句

libs ("libmyincompressibleTurbulenceModels.so");

如图所示

如果之前自定义了生成的.so文件路径，则需要加上路径。

接下来打开constant文件夹中的turbulenceProperties替换湍流模型为newkOmegaSST

定位到pitzDaily文件夹，在终端执行计算命令，成功出现结果。