关于用lookupObject引用变量报错，求大佬们指点。

Chen_hao

错误如下：

lnInclude/linearViscousStress.C: In constructor ‘Foam::linearViscousStress<BasicTurbulenceModel>::linearViscousStress(const Foam::word&, const alphaField&, const rhoField&, const volVectorField&, const surfaceScalarField&, const surfaceScalarField&, const transportModel&, const Foam::word&)’:
lnInclude/linearViscousStress.C:81:75: error: expected primary-expression before ‘>’ token
   81 |     const volScalarField& omega_ = this->mesh_.lookupObject<volScalarField>("omega_");
      |                                                                           ^
make: *** [/home/dyfluid/OpenFOAM/OpenFOAM-7/wmake/rules/General/transform:26: /home/dyfluid/OpenFOAM/OpenFOAM-7/platforms/linux64GccDPInt32Opt/src/TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/fWallFunctions/fWallFunction/fWallFunctionFvPatchScalarField.o] Error 1

代码如下：

#include "linearViscousStress.H"
#include "fvc.H"
#include "fvm.H"

// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //

template<class BasicTurbulenceModel>
Foam::linearViscousStress<BasicTurbulenceModel>::linearViscousStress
(
    const word& modelName,
    const alphaField& alpha,
    const rhoField& rho,
    const volVectorField& U,
    const surfaceScalarField& alphaRhoPhi,
    const surfaceScalarField& phi,
    const transportModel& transport,
    const word& propertiesName
)
:
    BasicTurbulenceModel
    (
        modelName,
        alpha,
        rho,
        U,
        alphaRhoPhi,
        phi,
        transport,
        propertiesName
    ),
    

    
    nonlinearStress_ 
    (
        IOobject
        (
            IOobject::groupName("nonlinearStress", alphaRhoPhi.group()),
            this->runTime_.timeName(),
            this->mesh_
        ),
        this->mesh_,
        dimensionedSymmTensor
        (
            "nonlinearStress",
            sqr(dimVelocity), 
            Zero 
        )
           
    )   
    {

    tensor I(1,0,0,0,1,0,0,0,1);  
    volSymmTensorField S(twoSymm(fvc::grad(this->U_)));
    volTensorField W(twoSkew(fvc::grad(this->U_)));
    const volScalarField& omega_ = this->mesh_.lookupObject<volScalarField>("omega_");
    
    nonlinearStress_ =
     1.0/omega_                            
     *(
       S&S 
       - (1.0/3.0)*magSqr(W)*I 
       + twoSymm(S&W) 
       + (2.5)*(W&W - (1.0/3.0)*magSqr(W)*I));
    }


// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //

template<class BasicTurbulenceModel>
bool Foam::linearViscousStress<BasicTurbulenceModel>::read()
{
    return BasicTurbulenceModel::read();
}


template<class BasicTurbulenceModel>
Foam::tmp<Foam::volSymmTensorField>
Foam::linearViscousStress<BasicTurbulenceModel>::devRhoReff() const
{
    return volSymmTensorField::New
    (
        IOobject::groupName("devRhoReff", this->alphaRhoPhi_.group()),
        (-(this->alpha_*this->rho_*this->nuEff()))
       *dev(twoSymm(fvc::grad(this->U_)))
    );
}


template<class BasicTurbulenceModel>
Foam::tmp<Foam::fvVectorMatrix>
Foam::linearViscousStress<BasicTurbulenceModel>::divDevRhoReff
(
    volVectorField& U
) const
{
    return
    (
      - fvc::div((this->alpha_*this->rho_*this->nuEff())*dev2(T(fvc::grad(U))))
      - fvc::div((this->alpha_*this->rho_*this->nuEff())*nonlinearStress_ )
      - fvm::laplacian(this->alpha_*this->rho_*this->nuEff(), U)
    );
}


template<class BasicTurbulenceModel>
Foam::tmp<Foam::fvVectorMatrix>
Foam::linearViscousStress<BasicTurbulenceModel>::divDevRhoReff //
(
    const volScalarField& rho,
    volVectorField& U
) const
{
    return
    (
      - fvc::div((this->alpha_*rho*this->nuEff())*dev2(T(fvc::grad(U))))
      - fvc::div((this->alpha_*rho*this->nuEff())*nonlinearStress_ )
      - fvm::laplacian(this->alpha_*rho*this->nuEff(), U)
    );
}


template<class BasicTurbulenceModel>
void Foam::linearViscousStress<BasicTurbulenceModel>::correct()
{
    BasicTurbulenceModel::correct();
}


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

在线性项里加入一个非线性部分，引用omega_出问题（omega_未在linearViscousStress文件中定义），这个引用方式是按照论坛其他帖子写的，需要怎么改正~

bestucan

编译器认为volScalarField不是一个类型。所以要把定义 volScalarfield 类型的头文件包含进来

Chen_hao

@bestucan
谢谢老师的指点，编译已通过！顺着老师的思路，我找到问题的解决办法：

  const volScalarField& omega_ = 
  (
    this->mesh_.objectRegistry::template
    lookupObject<volScalarField>("omega_")
   );

原文地址：链接文本
最后想问一下：我直接修改了komegaSSTbase.C原文件，在~/OpenFOAM/OpenFOAM-7/src/TurbulenceModels/turbulenceModels中wmake，是不是就可以了？

bestucan

@chen_hao 应该跑到最外面wmake all（会把文件都过一遍，速度不说多快，也不慢）。这样依赖komegaSSTbase的文件也会重新编译。

或者 wmake update： https://openfoam.org/download/source/compiling-openfoam/
我猜这样也可以

Chen_hao

@bestucan
谢谢，刚才的wmake通过的太轻松了哈哈哈，还好问了一下，
果然很多错才是该有的样子。我先自己改改，有问题可能还会麻烦老师~

Chen_hao

@bestucan @李东岳
虽然上面编译通过了，可兴致勃勃开始运行算例提示错误如下

--> FOAM FATAL ERROR: 

    request for volScalarField omega_ from objectRegistry region0 failed
    available objects of type volScalarField are

15
(
sigmaMag
alphas
nu.pos
muMag_0
rho
nu.molten
p_rgh
nu
alpha.molten
nu.neg
muMag
rho_0
alpha.neg
alpha.pos
sigmaMag_0
)


    From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>]
    in file /home/dyfluid/OpenFOAM/OpenFOAM-7/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 193.

还是关于omega_的引用问题，我在想是不是因为linearVicousStress.C是父类，而omega是在SSTbase.C中定义的（类似于子类），所以找不到？难道我要在linearVicousStress.C中重新IObject？
还是说这个引用方式有问题...但我用

const volScalarField& omega_ = this->mesh_.lookupObject<volScalarField>("omega_");

会编译不通过......不知道老师们有没有想法，十分需要帮助，再次感谢老师们

Chen_hao

@wwzhao
老师，可以帮忙解答一下吗~

Chen_hao

@chen_hao 在关于用lookupObject引用变量报错，求大佬们指点。中说：

@bestucan @李东岳
虽然上面编译通过了，可兴致勃勃开始运行算例提示错误如下
--> FOAM FATAL ERROR: 

    request for volScalarField omega_ from objectRegistry region0 failed
    available objects of type volScalarField are

15
(
sigmaMag
alphas
nu.pos
muMag_0
rho
nu.molten
p_rgh
nu
alpha.molten
nu.neg
muMag
rho_0
alpha.neg
alpha.pos
sigmaMag_0
)


    From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>]
    in file /home/dyfluid/OpenFOAM/OpenFOAM-7/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 193.
还是关于omega_的引用问题，我在想是不是因为linearVicousStress.C是父类，而omega是在SSTbase.C中定义的（类似于子类），所以找不到？难道我要在linearVicousStress.C中重新IObject？
还是说这个引用方式有问题...但我用
const volScalarField& omega_ = this->mesh_.lookupObject<volScalarField>("omega_");
会编译不通过......不知道老师们有没有想法，十分需要帮助，再次感谢老师们

我的分析原因是：执行求解器的时候linearStress.C先执行，所以此时omega还没注册进表里，显示找不到它，我现在在linearStress.C中加入一个omega的IOobject可不可行，毕竟在SST.C中还会IOobject一次，一个变量可以注册多次吗，会不会影响计算结果?

李东岳

你看一下其他的雷诺数 ShihQuadrat模型怎么调用的k epsilon？

Chen_hao

@李东岳
针对 ncompressible::turbulenceModel 模板特化后的 ShihQuadraticKE 模型，仔细研究了一下其怎么实现非线性项的实现，发现其是在 NonlinearEddyViscosity.H 中定义 nonlinearStress_ 项，然后用 ShihQuadraticKE 作为子类继承父类 NonlinearEddyViscosity 以便在 ShihQuadraticKE.C 中直接引用omega_。

但由于我修改的是SSTkomegabase.H( 继承于TurbulenceModel类 )与 linearViscousStrss.H ( 继承于BasicturbulenceModel原则类 ) 没有特例化，不能简单类似上面的ShihQuadraticKE 模型。需要从新仿造框架，是一项大工程！

我的策略是：在现有的文件上直接硬植入，简单很多，毕竟涉及到湍流模型的类错综复杂，针对找不到omega，按照我的分析应该是对的，运行求解器时linearViscousStrss.C先运行此时并未运行SSTkomegabase.C 所以没有omega场注册，找不到他，所以我在creatfield.H中IOobject一下omega场，目前可以算了，结果还未检查，不知道我的理解有没有问题。

CFD中文网

关于用lookupObject引用变量报错，求大佬们指点。