1. Home
  2. OpenFOAM
  3. 如何从字典读入一串系数

如何从字典读入一串系数

  • Y
    OpenFOAM讲师

    各位大佬好，我最近在写一个流体的热物性参数，计算Cp和he等需要使用多项式，需要读入一串的scalar，我采用的scalarList，但是编译时出现了类型错误，我想请问一下，需要读入一串scalar的时候，大家采用的是什么方法？
    LiquidThermo.C

    class LiquidThermo
{
    private:
        //constructor
        LiquidThermo();
        //constructor 
        LiquidThermo(const fvMesh & mesh,const dictionary & dict);    
        protected:
        //rho
        scalarList Coerho_[8];
        scalarList Coepsi_[7];
        // NSRDfunc
        scalarList Coemu_[5];
        //cp
        scalarList CoeCp_[8];
        //kappa
        scalarList Coekappa_[6];
        //he
        scalarList Coehe_[8];
    public:
        //inline functions used for constructor and correct function 
        //rho
        inline scalar rho(const scalar p,const scalar T) const;
        inline scalar psi(const scalar p,const scalar T) const;
        inline scalar mu(const scalar p,const scalar T) const;
        inline scalar Cp(const scalar p,const scalar T) const;
        inline scalar kappa(const scalar p,const scalar T) const;
        inline scalar alpha(const scalar p,const scalar T) const;
        inline scalar he(const scalar p,const scalar T) const;
...

    LiquidThermo.H
    //constructor and member fucntion

    //constructor 
Foam::LiquidThermo::LiquidThermo
(
    const fvMesh & mesh,
    const dictionary& dict
):
    name_(dict.dictName()),
    mesh_(mesh),
    p_(mesh.thisDb().lookupObject<volScalarField>(dict.lookup("p"))),
    T_(mesh.thisDb().lookupObject<volScalarField>(dict.lookup("T"))),
    rho_
    (
	IOobject
	(
	    IOobject::groupName("rho", name_),
	    mesh.time().timeName(),
	    mesh,
	    IOobject::NO_READ,
	    IOobject::NO_WRITE
	),
    ...
{
    //read scalar
    Coerho_ = dict.lookup("Coerho");
    Coepsi_ = dict.lookup("Coepsi");
    Coemu_ = dict.lookup("Coemu");
    CoeCp_ = dict.lookup("CoeCp");
    Coekappa_ = dict.lookup("Coekappa");
    Coehe_ = dict.lookup("Coehe");
    R_   = readScalar(dict.lookup("R"));
    ...
}
//inline function 
inline Foam::scalar Foam::LiquidThermo::rho
(
    const scalar p,
    const scalar T
) const
{
    //Coerho_[6]=pref ,Coerho_[7]=Tref
    return Coerho_[0]+Coerho_[1]*(p-Coerho_[6])+Coerho_[2]*(T-Coerho_[7])
    +Coerho_[3]*Foam::pow(p-Coerho_[6],2.0)+Coerho_[4]*Foam::pow(T-Coerho_[7],2.0)+Coerho_[5]*(p-Coerho_[6])*(T-Coerho_[7]);
}

    基于OpenFoam2.4,编译错误为：

    LiquidThermo.C: In member function ‘Foam::scalar Foam::LiquidThermo::rho(Foam::scalar, Foam::scalar) const’:
LiquidThermo.C:20:123: error: cannot convert ‘Foam::tmp<Foam::Field<double> >’ to ‘Foam::scalar {aka double}’ in return
     +Coerho_[3]*Foam::pow(p-Coerho_[6],2.0)+Coerho_[4]*Foam::pow(T-Coerho_[7],2.0)+Coerho_[5]*(p-Coerho_[6])*(T-Coerho_[7]);
                                                                                                                           ^
  • Y
    OpenFOAM讲师

    在http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2017/DavidSegersson/report_David_Segersson.pdf找到了相关的例子。

    定义变量： scalarList Coerho_;//8
初始化：从字典读取 
 dict.lookup("Coerho")>>Coerho_;
在字典中书写：
Coerho   （1.0 2.0 3.0）;

    以上为例子调用如下代码不会出错：

    Info<<Coerho_[0]+Coerho_[6];

    Coerho_[6]会被默认为0.

  • 李东岳

    感谢分享！:xiexie:

  • W
    OpenFOAM教授

    OpenFOAM 中提供了专门描述多项式的类：Polynomial

    用法可以参考：src/thermophysicalModels/specie/transport/polynomial/polynomialTransport.H

  • 范准

    我是这样做的：
    在求解器中，添加这样的代码：

            IOdictionary meshProperties
        (
            IOobject
            (
                "meshProperties",
                runTime.constant(),
                mesh,
                IOobject::MUST_READ,
                IOobject::NO_WRITE
            )
        );
	scalar xnumber(int(readScalar(meshProperties.lookup("xnumber"))));
	scalar ynumber(int(readScalar(meshProperties.lookup("ynumber"))));

    在算例文件夹的constant文件夹中，创建一个名为meshProperties的文件，内容为

    /*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      meshProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

xnumber                       20;
ynumber                       10;

    这样一来，参数xnumber和参数ynumber的值，就是通过算例文件夹里面的参数设定文件读取的了

    李东岳 1 Reply
  • 李东岳

    @范准 非常好，感谢分享 :xiexie:

Log in to reply