OpenFOAM提取等职面并计算面积

OpenFOAM中的等值面类

OpenFOAMV9中的isoSurface类可以用来提取等值面。
该类的实例化方式为：

sampledSurfaces::isoSurface isosurf = sampledSurfaces::isoSurface(
            "isoSurface",
            mesh,
            isoSurfaceDict);

"isoSurface"是一个自定义的名字（一般取对象名），mesh是所研究问题的网格，isoSurfaceDict是一个数据字典，该数据字典的内容如下

/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 9 \\/ M anipulation | ------------------------------------------------------------------------------- Description Writes out iso-surface files with interpolated field data in VTK format. \*---------------------------------------------------------------------------*/
FoamFile
{
    
    format      ascii;
    class       dictionary;
    location    "system";
    object      isoSurfaceDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

type        isoSurface;
isoField    p;		//需要提取等值线的场，这里是压力场
isoValue    10;	//等值线的数值，这里三10Pa
filter      full;
interpolate yes;

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

有了isosurf这个对象之后，可以用以下一行代码完成等值面提取的工作

isosurf.sample(p);

提取完成等值面后，可以获得等值面的面单元向量和等值面的顶点坐标

//等值面的面单元向量
faceList faces = isosurf.faces();
//等值面的顶点坐标
pointField points = isosurf.points();

points描述了该等值面是由哪些点构成的，提供了这些点的坐标信息。faces描述了这些点的连接关系。如果要访问第faceI个单元面的面积，可以使用以下代码:

mag(faces[faceI].area(points))

为了方便可视化，还可以将得到的等值面输出为VTK文件

vtkSurfaceWriter vtkWriter = vtkSurfaceWriter(IOstream::streamFormat::ASCII);
vtkWriter.write("postProcess",
                "someContours",
                points,
                faces);

代码

教程案例

以教程案例pitzDaily为例子，将其复制到自己的文件夹。使用simpleFoam求解器完成求解，结果如下：

修改求解器

在simpleFoam求解器源代码的基础上添加有关等值面的内容，改进后的求解器main函数如下

/*---------------------------------------------------------------------------*\ ========= | \\ / 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/>. Application isoSimpleFoam Description Steady-state solver for incompressible, turbulent flow, using the SIMPLE algorithm. \*---------------------------------------------------------------------------*/

#include "fvCFD.H"
#include "singlePhaseTransportModel.H"
#include "kinematicMomentumTransportModel.H"
#include "simpleControl.H"
#include "pressureReference.H"
#include "fvModels.H"
#include "fvConstraints.H"
//有关等值面的头文件
#include "sampledIsoSurface.H"
#include "vtkSurfaceWriter.H"

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

int main(int argc, char *argv[])
{
    
#include "postProcess.H"

#include "setRootCaseLists.H"
#include "createTime.H"
#include "createMesh.H"
#include "createControl.H"
#include "createFields.H"
#include "initContinuityErrs.H"

    //读取等值线字典
    dictionary isoSurfaceDict = IOdictionary(IOobject(
        "isoSurfaceDict",
        mesh.time().system(),
        mesh,
        IOobject::MUST_READ,
        IOobject::NO_WRITE));

    turbulence->validate();

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

    Info << "\nStarting time loop\n"
         << endl;

    while (simple.loop(runTime))
    {
    
        Info << "Time = " << runTime.timeName() << nl << endl;

        fvModels.correct();

        // --- Pressure-velocity SIMPLE corrector
        {
    
#include "UEqn.H"
#include "pEqn.H"
        }

        laminarTransport.correct();
        turbulence->correct();

        //修改等值线字典中的isoValue数值
        isoSurfaceDict.set("isoValue", 7);
        //实例化isoSurface对象
        sampledSurfaces::isoSurface isosurf = sampledSurfaces::isoSurface(
            "isoSurface",
            mesh,
            isoSurfaceDict);
        //提取等值面
        isosurf.sample(p);
        //等值面的面单元向量
        faceList faces = isosurf.faces();
        //等值面的顶点坐标
        pointField points = isosurf.points();
        //计算等值面的面积
        scalar area = 0;
        forAll(faces, faceI)
        {
    
            area += mag(faces[faceI].area(points));
        }
        Info << "面积:" << area << endl;
        //将等值面输出为VTK文件
        vtkSurfaceWriter vtkWriter = vtkSurfaceWriter(IOstream::streamFormat::ASCII);
        vtkWriter.write("postProcess",
                        "someContours",
                        points,
                        faces);

        runTime.write();

        Info << "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
             << " ClockTime = " << runTime.elapsedClockTime() << " s"
             << nl << endl;
    }

    Info << "End\n"
         << endl;

    return 0;
}

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

编译的过程见OpenFOAM用户手册，这里仅介绍基本步骤。
新建Make文件夹，在Make文件夹中新建files文件，写入编译信息

isoSimpleFoam.C

EXE = $(FOAM_USER_APPBIN)/isoSimpleFoam

在Make文件夹中新建options文件，写入依赖信息

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$(LIB_SRC)/meshTools/lnInclude \
    -I$(LIB_SRC)/sampling/lnInclude \
    -I$(LIB_SRC)/surfMesh/lnInclude

EXE_LIBS = \
    -lmomentumTransportModels \
    -lincompressibleMomentumTransportModels \
    -ltransportModels \
    -lfiniteVolume \
    -lmeshTools \
    -lfvModels \
    -lfvConstraints \
    -lsampling\
    -lsurfMesh

使用wmake命令完成编译，得到isoSimpleFoam求解器。该求解器将计算pitzDaily案例中压力为7Pa的等值面面积，并输出为VTK文件。

7Pa等值面

计算完成后，使用paraview读取postProcess文件夹下的someContours.vtk文件，可得到下图

这就是提取得到的等值面，其面积为9.043e-05