OFtutorial08_customBC
OFtutorial08_customBC
用户自定义边界条件
注：
本文是对Github上openfoam开发教程的中文解析。
总的来说这个系列的教程，边界条件这块做的不是很易懂，我回头会结合其他资料自己写一个易懂的
类：Foam::prescribedPipeInletFvPatchVectorField
组：grpInletBoundaryConditions grpWallBoundaryConditions
描述：对圆形管道的入口设置边界条件。流动方向通过面的法方向自动获得，只需要指定速度的大小。
| Property | Description | Required | Default value |
|---|---|---|---|
| R | pipe radius | yes | |
| flowSpeed | magnitude of flow velocity | yes | |
| deltaByR | wall function thickness as a fraction of pipe radius | yes | |
| approximationType | name of approximation profile | no | exponential |
| centrePoint | point on the centreline of the pipe | no | (0 0 0) |
| lambda | pressure gradient coefficient | no | 0 |
指定边界条件的例子：
inlet
{
// prescribes a parabolic inlet profile
type prescribedPipeInlet;
// (optional, default exponential) type of profile used for approximation
approximationType exponential;
// pipe radius
R $Rpipe;
// magnitude of flow velocity into the pipe
flowSpeed $flowVelocity;
// (optional, defaults at origin) centrepoint of the pipe used to determine the radius of each face
centrepoint (0 0 0);
// inlet as a function of radius
deltaByR $deltaByR;
// (optional, default 0) pressure gradient coefficient (see Polhausen profile literature for explanation)
lambda 0.;
// dummy value overwritten by the BC, used for initialisation only
value $internalField;
}
参考Foam::fixedValueFvPatchField类
代码：
#ifndef prescribedPipeInletFvPatchVectorField_H
#define prescribedPipeInletFvPatchVectorField_H
//your code
#endif
作用：
养成良好的代码习惯，在所有的头文件中加上这种结构防止头文件被重复包含。
代码：
class prescribedPipeInletFvPatchVectorField
:
public fixedValueFvPatchVectorField
{
private:
public:
}
作用：
以公有继承的方式继承现有的fixedValueFvPatchVectorField类。fixedValueFvPatchVectorField类在边界上指定固定的值，但是在新建的prescribedPipeInletFvPatchVectorField实现了在边界上指定不均匀的值。
代码：
private:
// Private data
// NOTE: these class fields are used to determine the inlet profile
// denotes the type of the profile used to perform the approximation
// (optional, defaults to exponential)
word approximationType_;
// flow velocity magnitude
scalar flowSpeed_;
// bl thickness
scalar deltaByR_;
// centre of the pipe (optional, defaults to the origin)
vector centrepoint_;
// radius of the pipe
scalar R_;
// pressure gradient coefficient (optional, default to 0, not used by all approximations)
scalar lambda_;
作用：
私有变量
这些量决定了入口处的信息。
word approximationType_：近似的方式，可选，默认是指数型
scalar flowSpeed_：入口处的速度的大小
scalar deltaByR_：bl thickness（我也不知道啥意思）
vector centrepoint_：管道中心的位置（可选，默认值为原点）
scalar R_：管道的半径
scalar lambda_：压力梯度系数（可选，默认值为0，并不是在所有的近似中都使用）
代码：
以下均为public
TypeName("prescribedPipeInlet");
作用：
Runtime类型信息
定义边界条件的名称。通过RuntimeSelector使用。openfoam通过这个名称知道用户使用的边界类型。
代码：
// Constructors
//- Construct from patch and internal field
prescribedPipeInletFvPatchVectorField
(
const fvPatch&,
const DimensionedField<vector, volMesh>&
);
//- Construct as copy setting internal field reference
prescribedPipeInletFvPatchVectorField
(
const prescribedPipeInletFvPatchVectorField&,
const DimensionedField<vector, volMesh>&
);
作用：
类的构造器。此处为函数重载，两个同名函数有不同的输入。编译器会根据输入的类型决定调用哪一个函数。
- 根据patch和internal field构造
- 从internal field中拷贝构造
代码：
//- Construct and return a clone setting internal field reference
virtual tmp<fvPatchVectorField> clone
(
const DimensionedField<vector, volMesh>& iF
) const
{
return tmp<fvPatchVectorField>
(
new prescribedPipeInletFvPatchVectorField(*this, iF)
);
}
作用：
构造并返回内部流场引用的克隆
代码：
//- Construct from patch, internal field and dictionary
prescribedPipeInletFvPatchVectorField
(
const fvPatch&,
const DimensionedField<vector, volMesh>&,
const dictionary&,
const bool valueRequired=true
);
作用：
另一个构造器，从patch，内部场以及dictionary中构造
代码：
//- Construct by mapping given prescribedPipeInletFvPatchVectorField
// onto a new patch
prescribedPipeInletFvPatchVectorField
(
const prescribedPipeInletFvPatchVectorField&,
const fvPatch&,
const DimensionedField<vector, volMesh>&,
const fvPatchFieldMapper&,
const bool mappingRequired=true
);
作用：
通过映射prescribedPipeInletFvPatchVectorField到一个新的patch构造
代码：
//- Disallow copy without setting internal field reference
prescribedPipeInletFvPatchVectorField(const prescribedPipeInletFvPatchVectorField&) = delete;
作用：
在未设置内部场的时候不允许复制。
代码：
成员函数
// Evaluation functions
//- Update the coefficients associated with the patch field
virtual void updateCoeffs();
作用：
更新与patch相关的系数
代码：
//- Write
virtual void write(Ostream&) const;
作用：
IO，写数据
代码：
Foam::prescribedPipeInletFvPatchVectorField::prescribedPipeInletFvPatchVectorField
(
const fvPatch& p,
const DimensionedField<vector, volMesh>& iF
)
:
// NOTE: call the default constructor to make sure everything gets initialised properly
fixedValueFvPatchVectorField(p, iF),
// NOTE: assign default values to the members using an initialiser list
approximationType_("exponential"),
flowSpeed_(0.),
deltaByR_(0.),
centrepoint_(vector::zero),
R_(0.),
lambda_(0.)
{}
作用：
调用默认的构造器以确保类中的数据会被初始化。把默认值赋给成员变量。
代码：
Foam::prescribedPipeInletFvPatchVectorField::prescribedPipeInletFvPatchVectorField
(
const fvPatch& p,
const DimensionedField<vector, volMesh>& iF,
const dictionary& dict,
const bool valueRequired
)
:
// NOTE: this constructor reads all of the control parameters from the boundary
// condition definition specified in the time folder U file, imported here
// as a dictionary reference.
fixedValueFvPatchVectorField(p, iF),
approximationType_("exponential"),
flowSpeed_(0.),
deltaByR_(0.),
centrepoint_(vector::zero),
R_(0.),
lambda_(0.)
{
// NOTE: calls the = operator to assign the value to the faces held by this BC
fvPatchVectorField::operator=(vectorField("value", dict, p.size()));
// NOTE: looks up the necessary paramters
approximationType_ = dict.lookupOrDefault<word>("approximationType","exponential");
dict.lookup("flowSpeed") >> flowSpeed_;
dict.lookup("deltaByR") >> deltaByR_;
centrepoint_ = dict.lookupOrDefault<vector>("centrepoint",vector::zero);
dict.lookup("R") >> R_;
lambda_ = dict.lookupOrDefault<scalar>("lambda",0.);
// NOTE: calls the .updateCoeffs() method to calculate the inlet profile in
// accordance with the controls which have just been read.
updateCoeffs();
}
作用：
这个构造函数在指定的文件夹下的U文件中读取边界条件的控制参数，然后输出到这里作为边界条件的参考值。
fvPatchVectorField::operator=(vectorField("value", dict, p.size()))：调用=操作符给
lookup读取必要的数据
调用updateCoeffs()方法根据刚刚读到的参数计算入口的profile
代码：
Foam::prescribedPipeInletFvPatchVectorField::prescribedPipeInletFvPatchVectorField
(
const prescribedPipeInletFvPatchVectorField& ptf,
const fvPatch& p,
const DimensionedField<vector, volMesh>& iF,
const fvPatchFieldMapper& mapper,
const bool mappingRequired
)
:
// NOTE: this constructor, and the two subsequent ones, transfer data to the
// instance being created from another one.
fixedValueFvPatchVectorField(ptf, p, iF, mapper),
approximationType_(ptf.approximationType_),
flowSpeed_(ptf.flowSpeed_),
deltaByR_(ptf.deltaByR_),
centrepoint_(ptf.centrepoint_),
R_(ptf.R_),
lambda_(ptf.lambda_)
{}
Foam::prescribedPipeInletFvPatchVectorField::prescribedPipeInletFvPatchVectorField
(
const prescribedPipeInletFvPatchVectorField& rifvpvf,
const DimensionedField<vector, volMesh>& iF
)
:
fixedValueFvPatchVectorField(rifvpvf, iF),
approximationType_(rifvpvf.approximationType_),
flowSpeed_(rifvpvf.flowSpeed_),
deltaByR_(rifvpvf.deltaByR_),
centrepoint_(rifvpvf.centrepoint_),
R_(rifvpvf.R_),
lambda_(rifvpvf.lambda_)
{}
作用：
这；两个构造器，把数据传输给另一个构造器创建的实例中。
代码：
以下为成员函数
void Foam::prescribedPipeInletFvPatchVectorField::updateCoeffs()
{
if (updated())
{
return;
}
// assign inlet velocity normal to the patch
// by convention, patch faces point outside of the domain
vectorField Uin = (-1.)*(patch().Sf()/patch().magSf()) * flowSpeed_;
// go over each face and add the BL profile for faces close to the wall
forAll(patch().Cf(), faceI)
{
// non-dimensional distance away from the wall
scalar yOverDelta ( (1.-mag(centrepoint_ - patch().Cf()[faceI])/R_)/deltaByR_ );
if (approximationType_.compare("parabolic") == 0)
{
if (yOverDelta < 1.0)
Uin[faceI] *= (2*yOverDelta-pow(yOverDelta,2.0));
}
else if (approximationType_.compare("Polhausen") == 0)
{
if (yOverDelta < 1.0)
Uin[faceI] *= 1.-(1.+yOverDelta)*pow(1.-yOverDelta,3.) + lambda_/6.*yOverDelta*pow(1.-yOverDelta,3.);
}
else if (approximationType_.compare("exponential") == 0)
{
if (yOverDelta < 1.0)
Uin[faceI] *= pow(yOverDelta,1./7.);
}
else
{
FatalErrorIn
(
"prescribedPipeInletFvPatchVectorField::updateCoeffs()"
) << "Unknown boundary layer profile approximation type " << approximationType_ << nl << nl
<< "Valid types are :" << nl
<< tab << "parabolic" << nl
<< tab << "Polhausen" << nl
<< tab << "exponential" << nl
<< exit(FatalError);
}
}
// set the value_ of this patch to the newly computed flow speed
this->operator==(Uin);
// call the base class method to make sure all the other bits and pieces get updated
fixedValueFvPatchVectorField::updateCoeffs();
}
作用：
这个是这个类中的主要的方法，在这个方法里面计算入口条件。
vectorField Uin = (-1.)*(patch().Sf()/patch().magSf()) * flowSpeed_：把总的流速分解为x,y,z三个方向的值，得到的向量与面垂直。patch().Sf()这个函数得到面的法向量。patch().magSf()得到面的法向量的模。两个相除，得到单位法向量。边界上的面的法向量指向外侧，所以需要乘以-1。
代码：
void Foam::prescribedPipeInletFvPatchVectorField::write(Ostream& os) const
{
fvPatchVectorField::write(os);
os.writeKeyword("approximationType") << approximationType_ << token::END_STATEMENT << nl;
os.writeKeyword("flowSpeed") << flowSpeed_ << token::END_STATEMENT << nl;
os.writeKeyword("deltaByR") << deltaByR_ << token::END_STATEMENT << nl;
os.writeKeyword("centrepoint") << centrepoint_ << token::END_STATEMENT << nl;
os.writeKeyword("R") << R_ << token::END_STATEMENT << nl;
os.writeKeyword("lambda") << lambda_ << token::END_STATEMENT << nl;
writeEntry(os, "value", *this);
}
作用：
写文件
编译：
options文件：
EXE_INC = \
-I$(LIB_SRC)/finiteVolume/lnInclude
LIB_LIBS = \
-lfiniteVolume
files文件：
prescribedPipeInletFvPatchVectorField.C
LIB = $(FOAM_USER_LIBBIN)/libprescribedPipeInlet
说明：
边界条件属于生成一个C++的库，makes文件和files文件的书写与教程7中的类似。
使用：
在controlDict文件的末尾要按照以下方式包含进去这个库，不然运行的时候会找不到
// include the custom inlet library
libs ("libprescribedPipeInlet.so");
总体代码：
prescribedPipeInletFvPatchVectorField.H：
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2011-2013 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::prescribedPipeInletFvPatchVectorField
Group
grpInletBoundaryConditions grpWallBoundaryConditions
Description
Prescribes an inlet profile for a circular pipe inlet patch. Flow direction is determined
automatically from face normals, only velocity magnitude needs to be provided.
\heading Patch usage
\table
Property | Description | Required | Default value
R | pipe radius | yes |
flowSpeed | magnitude of flow velocity | yes |
deltaByR | wall function thickness as a fraction of pipe radius | yes |
approximationType | name of approximation profile | no | exponential
centrePoint | point on the centreline of the pipe | no | (0 0 0)
lambda | pressure gradient coefficient | no | 0
\endtable
Example of the boundary condition specification:
\verbatim
inlet
{
// prescribes a parabolic inlet profile
type prescribedPipeInlet;
// (optional, default exponential) type of profile used for approximation
approximationType exponential;
// pipe radius
R $Rpipe;
// magnitude of flow velocity into the pipe
flowSpeed $flowVelocity;
// (optional, defaults at origin) centrepoint of the pipe used to determine the radius of each face
centrepoint (0 0 0);
// inlet BL thickness as a function of radius
deltaByR $deltaByR;
// (optional, default 0) pressure gradient coefficient (see Polhausen profile literature for explanation)
lambda 0.;
// dummy value overwritten by the BC, used for initialisation only
value $internalField;
}
\endverbatim
SeeAlso
Foam::fixedValueFvPatchField
SourceFiles
prescribedPipeInletFvPatchVectorField.C
\*---------------------------------------------------------------------------*/
#ifndef prescribedPipeInletFvPatchVectorField_H
#define prescribedPipeInletFvPatchVectorField_H
#include "fvPatchFields.H"
#include "fixedValueFvPatchFields.H"
#include "Switch.H"
#include "addToRunTimeSelectionTable.H"
#include "volFields.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
/*---------------------------------------------------------------------------*\
Class prescribedPipeInletFvPatchVectorField Declaration
\*---------------------------------------------------------------------------*/
// NOTE: the patch is derived from a fixedValue BC since it does prescribe
// a fixed value, although non-uniform across all of the faces, unlike the base
// class does.
class prescribedPipeInletFvPatchVectorField
:
public fixedValueFvPatchVectorField
{
private:
// Private data
// NOTE: these class fields are used to determine the inlet profile
// denotes the type of the profile used to perform the approximation
// (optional, defaults to exponential)
word approximationType_;
// flow velocity magnitude
scalar flowSpeed_;
// bl thickness
scalar deltaByR_;
// centre of the pipe (optional, defaults to the origin)
vector centrepoint_;
// radius of the pipe
scalar R_;
// pressure gradient coefficient (optional, default to 0, not used by all approximations)
scalar lambda_;
public:
//- Runtime type information
// NOTE: this gets used by the runtimeSelector. In other words, this is the
// name under which OpenFOAM knows this BC.
TypeName("prescribedPipeInlet");
// Constructors
//- Construct from patch and internal field
prescribedPipeInletFvPatchVectorField
(
const fvPatch&,
const DimensionedField<vector, volMesh>&
);
//- Construct as copy setting internal field reference
prescribedPipeInletFvPatchVectorField
(
const prescribedPipeInletFvPatchVectorField&,
const DimensionedField<vector, volMesh>&
);
//- Construct and return a clone setting internal field reference
virtual tmp<fvPatchVectorField> clone
(
const DimensionedField<vector, volMesh>& iF
) const
{
return tmp<fvPatchVectorField>
(
new prescribedPipeInletFvPatchVectorField(*this, iF)
);
}
//- Construct from patch, internal field and dictionary
prescribedPipeInletFvPatchVectorField
(
const fvPatch&,
const DimensionedField<vector, volMesh>&,
const dictionary&,
const bool valueRequired=true
);
//- Construct by mapping given prescribedPipeInletFvPatchVectorField
// onto a new patch
prescribedPipeInletFvPatchVectorField
(
const prescribedPipeInletFvPatchVectorField&,
const fvPatch&,
const DimensionedField<vector, volMesh>&,
const fvPatchFieldMapper&,
const bool mappingRequired=true
);
//- Disallow copy without setting internal field reference
prescribedPipeInletFvPatchVectorField(const prescribedPipeInletFvPatchVectorField&) = delete;
// Member functions
// Evaluation functions
//- Update the coefficients associated with the patch field
virtual void updateCoeffs();
// I-O
//- Write
virtual void write(Ostream&) const;
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif
// ************************************************************************* //
prescribedPipeInletFvPatchVectorField.H：
/*---------------------------------------------------------------------------* \
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2011 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 "prescribedPipeInletFvPatchVectorField.H"
// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
Foam::prescribedPipeInletFvPatchVectorField::prescribedPipeInletFvPatchVectorField
(
const fvPatch& p,
const DimensionedField<vector, volMesh>& iF
)
:
// NOTE: call the default constructor to make sure everything gets initialised properly
fixedValueFvPatchVectorField(p, iF),
// NOTE: assign default values to the members using an initialiser list
approximationType_("exponential"),
flowSpeed_(0.),
deltaByR_(0.),
centrepoint_(vector::zero),
R_(0.),
lambda_(0.)
{}
Foam::prescribedPipeInletFvPatchVectorField::prescribedPipeInletFvPatchVectorField
(
const fvPatch& p,
const DimensionedField<vector, volMesh>& iF,
const dictionary& dict,
const bool valueRequired
)
:
// NOTE: this constructor reads all of the control parameters from the boundary
// condition definition specified in the time folder U file, imported here
// as a dictionary reference.
fixedValueFvPatchVectorField(p, iF),
approximationType_("exponential"),
flowSpeed_(0.),
deltaByR_(0.),
centrepoint_(vector::zero),
R_(0.),
lambda_(0.)
{
// NOTE: calls the = operator to assign the value to the faces held by this BC
fvPatchVectorField::operator=(vectorField("value", dict, p.size()));
// NOTE: looks up the necessary paramters
approximationType_ = dict.lookupOrDefault<word>("approximationType","exponential");
dict.lookup("flowSpeed") >> flowSpeed_;
dict.lookup("deltaByR") >> deltaByR_;
centrepoint_ = dict.lookupOrDefault<vector>("centrepoint",vector::zero);
dict.lookup("R") >> R_;
lambda_ = dict.lookupOrDefault<scalar>("lambda",0.);
// NOTE: calls the .updateCoeffs() method to calculate the inlet profile in
// accordance with the controls which have just been read.
updateCoeffs();
}
Foam::prescribedPipeInletFvPatchVectorField::prescribedPipeInletFvPatchVectorField
(
const prescribedPipeInletFvPatchVectorField& ptf,
const fvPatch& p,
const DimensionedField<vector, volMesh>& iF,
const fvPatchFieldMapper& mapper,
const bool mappingRequired
)
:
// NOTE: this constructor, and the two subsequent ones, transfer data to the
// instance being created from another one.
fixedValueFvPatchVectorField(ptf, p, iF, mapper),
approximationType_(ptf.approximationType_),
flowSpeed_(ptf.flowSpeed_),
deltaByR_(ptf.deltaByR_),
centrepoint_(ptf.centrepoint_),
R_(ptf.R_),
lambda_(ptf.lambda_)
{}
Foam::prescribedPipeInletFvPatchVectorField::prescribedPipeInletFvPatchVectorField
(
const prescribedPipeInletFvPatchVectorField& rifvpvf,
const DimensionedField<vector, volMesh>& iF
)
:
fixedValueFvPatchVectorField(rifvpvf, iF),
approximationType_(rifvpvf.approximationType_),
flowSpeed_(rifvpvf.flowSpeed_),
deltaByR_(rifvpvf.deltaByR_),
centrepoint_(rifvpvf.centrepoint_),
R_(rifvpvf.R_),
lambda_(rifvpvf.lambda_)
{}
// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
// NOTE: this is the key method which implements the actual maths for calculating
// the inlet profiles.
void Foam::prescribedPipeInletFvPatchVectorField::updateCoeffs()
{
if (updated())
{
return;
}
// assign inlet velocity normal to the patch
// by convention, patch faces point outside of the domain
vectorField Uin = (-1.)*(patch().Sf()/patch().magSf()) * flowSpeed_;
// go over each face and add the BL profile for faces close to the wall
forAll(patch().Cf(), faceI)
{
// non-dimensional distance away from the wall
scalar yOverDelta ( (1.-mag(centrepoint_ - patch().Cf()[faceI])/R_)/deltaByR_ );
if (approximationType_.compare("parabolic") == 0)
{
if (yOverDelta < 1.0)
Uin[faceI] *= (2*yOverDelta-pow(yOverDelta,2.0));
}
else if (approximationType_.compare("Polhausen") == 0)
{
if (yOverDelta < 1.0)
Uin[faceI] *= 1.-(1.+yOverDelta)*pow(1.-yOverDelta,3.) + lambda_/6.*yOverDelta*pow(1.-yOverDelta,3.);
}
else if (approximationType_.compare("exponential") == 0)
{
if (yOverDelta < 1.0)
Uin[faceI] *= pow(yOverDelta,1./7.);
}
else
{
FatalErrorIn
(
"prescribedPipeInletFvPatchVectorField::updateCoeffs()"
) << "Unknown boundary layer profile approximation type " << approximationType_ << nl << nl
<< "Valid types are :" << nl
<< tab << "parabolic" << nl
<< tab << "Polhausen" << nl
<< tab << "exponential" << nl
<< exit(FatalError);
}
}
// set the value_ of this patch to the newly computed flow speed
this->operator==(Uin);
// call the base class method to make sure all the other bits and pieces get updated
fixedValueFvPatchVectorField::updateCoeffs();
}
void Foam::prescribedPipeInletFvPatchVectorField::write(Ostream& os) const
{
fvPatchVectorField::write(os);
os.writeKeyword("approximationType") << approximationType_ << token::END_STATEMENT << nl;
os.writeKeyword("flowSpeed") << flowSpeed_ << token::END_STATEMENT << nl;
os.writeKeyword("deltaByR") << deltaByR_ << token::END_STATEMENT << nl;
os.writeKeyword("centrepoint") << centrepoint_ << token::END_STATEMENT << nl;
os.writeKeyword("R") << R_ << token::END_STATEMENT << nl;
os.writeKeyword("lambda") << lambda_ << token::END_STATEMENT << nl;
writeEntry(os, "value", *this);
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
makePatchTypeField
(
fvPatchVectorField,
prescribedPipeInletFvPatchVectorField
);
}
// ************************************************************************* //
浙公网安备 33010602011771号