OFtutorial03_understandingTheMesh
第三讲：理解网格
代码：
#include "setRootCase.H"
#include "createTime.H"
#include "createMesh.H"
作用：
检查算例结构是否完整，创建时间系统（实例名为：runTime）和fvmesh（实例名为：mesh）
代码：
Info << "Hello there, the most recent time folder found is " << runTime.timeName() << nl
<< "The mesh has " << mesh.C().size() << " cells and " << mesh.Cf().size()
<< " internal faces in it. Wubalubadubdub!" << nl << endl;
作用：
runTime和mesh是对象（或者类）的实例。
要调用的子函数 .timeName(), .C(), .Cf()在这些类中部署。
很重要的一点是：mesh.C()以及mesh.Cf()返回一个向量场，代表了每个网格或者面的中心。
调用mesh.C().size()方法也可以返回mesh的大小。
注意：mesh.Cf()指internal face（内部网格）
代码：
for (label cellI = 0; cellI < mesh.C().size(); cellI++)
if (cellI%20 == 0) // only show every twentieth cell not to spam the screen too much
Info << "Cell " << cellI << " with centre at " << mesh.C()[cellI] << endl;
Info << endl; // spacer
作用：
可以通过C++标准for循环来遍历每一个网格。
代码：
for (label faceI = 0; faceI < mesh.owner().size(); faceI++)
if (faceI%40 == 0)
Info << "Internal face " << faceI << " with centre at " << mesh.Cf()[faceI]
<< " with owner cell " << mesh.owner()[faceI]
<< " and neighbour " << mesh.neighbour()[faceI] << endl;
Info << endl;
作用：
每个cell都是由面组成的。这些面可能是OpenFOAM中的内部面，边界面或者patch。内部面有一个主网格还有一个邻居网格。
代码：
forAll(mesh.boundaryMesh(), patchI)
Info << "Patch " << patchI << ": " << mesh.boundary()[patchI].name() << " with "
<< mesh.boundary()[patchI].Cf().size() << " faces. Starts at total face "
<< mesh.boundary()[patchI].start() << endl;
Info << endl;
作用：
边界条件可以通过boundaryMesh对象获取。
实际上，每个边界面的描述都包含在了constant/polyMesh/faces文件中。但是，在这个文件中，内部面被首先定义。
此外，在constant/polyMesh/boundary文件中定义了起始面的ID，表明边界文件的起始位置。OpenFOAM也为循环提供宏定义，这可以减少很多代码量。
代码：
label patchFaceI(0);
forAll(mesh.boundaryMesh(), patchI)
Info << "Patch " << patchI << " has its face " << patchFaceI << " adjacent to cell "
<< mesh.boundary()[patchI].patch().faceCells()[patchFaceI]
<< ". It has normal vector " << mesh.boundary()[patchI].Sf()[patchFaceI]
<< " and surface area " << mag(mesh.boundary()[patchI].Sf()[patchFaceI])
<< endl;
Info << endl;
作用：
可以用上述方式获取紧邻边界的面。
一个很有用的事情是如何知道面的法向量和面积。
代码：
const faceList& fcs = mesh.faces();
const List<point>& pts = mesh.points();
const List<point>& cents = mesh.faceCentres();
forAll(fcs,faceI)
if (faceI%80==0)
{
if (faceI<mesh.Cf().size())
Info << "Internal face ";
else
{
forAll(mesh.boundary(),patchI)
if ((mesh.boundary()[patchI].start()<= faceI) &&
(faceI < mesh.boundary()[patchI].start()+mesh.boundary()[patchI].Cf().size()))
{
Info << "Face on patch " << patchI << ", faceI ";
break; // exit the forAll loop prematurely
}
}
Info << faceI << " with centre at " << cents[faceI]
<< " has " << fcs[faceI].size() << " vertices:";
forAll(fcs[faceI],vertexI)
// Note how fcs[faceI] holds the indices of points whose coordinates
// are stored in the pts list.
Info << " " << pts[fcs[faceI][vertexI]];
Info << endl;
}
Info << endl;
作用：
对于内部的面来说，.Sf()方法可直接被mesh实例调用。
在计算面的面积的时候有一个更简短的方法.magSf()，这个方法返回面积的数量值。
对于内部面，法向量从owner指向neighbor，且owner的索引比neighbor小。对于边界面，面的法向量指向计算域的外侧。
也可以查看定义面的点。
首先定义面中各种对象的引用。这些变量被定义为常量，因为我们不想去更改他们。
注意：
这些lists代表了面物理上的定义，所以包含了变截面。用户可以通过mesh.boundary()[patchI].Cf().size()和mesh.boundary()[patchI].start()方法来判断面试边界面还是内部面。
代码：
label patchID(0);
const polyPatch& pp = mesh.boundaryMesh()[patchID];
if (isA<emptyPolyPatch>(pp))
{
// patch patchID is of type "empty".
Info << "You will not see this." << endl;
}
作用：
在原始的cavity教程中，frontAndBack边界被定义为“empty”类型。这是一种很特殊的边界条件，会引起很多意料之外的问题。比如说.Cf()会尺寸为0.
可能需要检测patch的类型以避免类似的问题。
代码：
word patchName("movingWall");
patchID = mesh.boundaryMesh().findPatchID(patchName);
Info << "Retrieved patch " << patchName << " at index " << patchID << " using its name only." << nl << endl;
作用：
patches也可以通过他们的名称访问。当用户想从dictionary中引用特定的patch时，这可能会被用到。（比如：计算特定的patch的受力）
总体代码：
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2011-2015 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/>.
\*---------------------------------------------------------------------------*/
#include "fvCFD.H"
int main(int argc, char *argv[])
{
#include "setRootCase.H"
// These two create the time system (instance called runTime) and fvMesh (instance called mesh).
#include "createTime.H"
#include "createMesh.H"
// runTime and mesh are instances of objects (or classes).
// If you are not familiar with what a class or object is, it is HIGHLY RECOMMENDED you visit this
// website and only come back once you've read everything about classes, inheritance and polymorphism:
// http://www.cplusplus.com/doc/tutorial/classes/
// Note how the next lines call functions .timeName(), .C() and .Cf() implemented in the objects.
// It is also important to realise that mesh.C() and .Cf() return vector fields denoting centres of each
// cell and internal face.
// Calling the mesh.C().size() method therefore yields the total size of the mesh.
Info << "Hello there, the most recent time folder found is " << runTime.timeName() << nl
<< "The mesh has " << mesh.C().size() << " cells and " << mesh.Cf().size()
<< " internal faces in it. Wubalubadubdub!" << nl << endl;
// It's possible to iterate over every cell in a standard C++ for loop
for (label cellI = 0; cellI < mesh.C().size(); cellI++)
if (cellI%20 == 0) // only show every twentieth cell not to spam the screen too much
Info << "Cell " << cellI << " with centre at " << mesh.C()[cellI] << endl;
Info << endl; // spacer
// Each cell is constructed of faces - these may either be internal or constitute a
// boundary, or a patch in OpenFOAM terms; internal faces have an owner cell
// and a neighbour.
for (label faceI = 0; faceI < mesh.owner().size(); faceI++)
if (faceI%40 == 0)
Info << "Internal face " << faceI << " with centre at " << mesh.Cf()[faceI]
<< " with owner cell " << mesh.owner()[faceI]
<< " and neighbour " << mesh.neighbour()[faceI] << endl;
Info << endl;
// Boundary conditions may be accessed through the boundaryMesh object.
// In reality, each boundary face is also included in the constant/polyMesh/faces
// description. But, in that file, the internal faces are defined first.
// In addition, the constant/polyMesh/boundary file defines the starting faceI
// indices from which boundary face definitions start.
// OpenFOAM also provides a macro definition for for loops over all entries
// in a field or a list, which saves up on the amount of typing.
forAll(mesh.boundaryMesh(), patchI)
Info << "Patch " << patchI << ": " << mesh.boundary()[patchI].name() << " with "
<< mesh.boundary()[patchI].Cf().size() << " faces. Starts at total face "
<< mesh.boundary()[patchI].start() << endl;
Info << endl;
// Faces adjacent to boundaries may be accessed as follows.
// Also, a useful thing to know about a face is its normal vector and face area.
label patchFaceI(0);
forAll(mesh.boundaryMesh(), patchI)
Info << "Patch " << patchI << " has its face " << patchFaceI << " adjacent to cell "
<< mesh.boundary()[patchI].patch().faceCells()[patchFaceI]
<< ". It has normal vector " << mesh.boundary()[patchI].Sf()[patchFaceI]
<< " and surface area " << mag(mesh.boundary()[patchI].Sf()[patchFaceI])
<< endl;
Info << endl;
// For internal faces, method .Sf() can be called directly on the mesh instance.
// Moreover, there is a shorthand method .magSf() which returns the surface area
// as a scalar.
// For internal faces, the normal vector points from the owner to the neighbour
// and the owner has a smaller cellI index than the neighbour. For boundary faces,
// the normals always point outside of the domain (they have "imaginary" neighbours
// which do not exist).
// It is possible to look at the points making up each face in more detail.
// First, we define a few shorthands by getting references to the respective
// objects in the mesh. These are defined as constants since we do not aim to
// alter the mesh in any way.
// NOTE: these lists refer to the physical definition of the mesh and thus
// include boundary faces. Use can be made of the mesh.boundary()[patchI].Cf().size()
// and mesh.boundary()[patchI].start() methods to check whether the face is internal
// or lies on a boundary.
const faceList& fcs = mesh.faces();
const List<point>& pts = mesh.points();
const List<point>& cents = mesh.faceCentres();
forAll(fcs,faceI)
if (faceI%80==0)
{
if (faceI<mesh.Cf().size())
Info << "Internal face ";
else
{
forAll(mesh.boundary(),patchI)
if ((mesh.boundary()[patchI].start()<= faceI) &&
(faceI < mesh.boundary()[patchI].start()+mesh.boundary()[patchI].Cf().size()))
{
Info << "Face on patch " << patchI << ", faceI ";
break; // exit the forAll loop prematurely
}
}
Info << faceI << " with centre at " << cents[faceI]
<< " has " << fcs[faceI].size() << " vertices:";
forAll(fcs[faceI],vertexI)
// Note how fcs[faceI] holds the indices of points whose coordinates
// are stored in the pts list.
Info << " " << pts[fcs[faceI][vertexI]];
Info << endl;
}
Info << endl;
// In the original cavity tutorial, on which the test case is based,
// the frontAndBack boundary is defined as and "empty" type. This is a special
// BC case which may cause unexpected behaviour as its .Cf() field has size of 0.
// Type of a patch may be checked to avoid running into this problem if there
// is a substantial risk that an empty patch type will appear
label patchID(0);
const polyPatch& pp = mesh.boundaryMesh()[patchID];
if (isA<emptyPolyPatch>(pp))
{
// patch patchID is of type "empty".
Info << "You will not see this." << endl;
}
// Patches may also be retrieved from the mesh using their name. This could be
// useful if the user were to refer to a particular patch from a dictionary
// (like when you do when calculating forces on a particular patch).
word patchName("movingWall");
patchID = mesh.boundaryMesh().findPatchID(patchName);
Info << "Retrieved patch " << patchName << " at index " << patchID << " using its name only." << nl << endl;
Info<< "End\n" << endl;
return 0;
}
// ************************************************************************* //