twoPhaseEulerFoam中的ITAE模型

upc_ngh

各位前辈，想要在twoPhaseEulerFoam中的ITAE模型中，添加一个温度传输方程，准备求解液固流沉积后的管内温度场，在ITAE.C中添加完成T的求解方程后，出现了两个问题：
（1）这里的phase_.phi()只是单纯的离散相的通量，而这个求解温度场需要的是离散相和连续相的通量和即fluid.phi()，这个fluid.phi()应该怎么去表示？
（2）当植入求解方程T后，报错如下，希望各位老师指点一下，不胜感激

diameterModels/IATE/IATE.C: In member function ‘virtual void Foam::diameterModels::IATE::correct()’:
diameterModels/IATE/IATE.C:220:19: error: ‘laplacian’ is not a member of ‘Foam::fvm’
                  -fvm::laplacian(niandu,Tcell_)
                   ^
/opt/openfoam4/wmake/rules/General/transform:8: recipe for target '/opt/openfoam4/platforms/linux64GccDPInt32Opt/applications/solvers/multiphase/twoPhaseEulerFoam/twoPhaseSystem/diameterModels/IATE/IATE.o' failed

更改后的ITAE.C代码如下

Foam::diameterModels::IATE::IATE
(
    const dictionary& diameterProperties,
    const phaseModel& phase
)
:
    diameterModel(diameterProperties, phase),
    kappai_
    (
        IOobject
        (
            IOobject::groupName("kappai", phase.name()),
            phase_.U().time().timeName(),
            phase_.U().mesh(),
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        phase_.U().mesh()
    ),
    
    Tcell_
    (
    IOobject
    (
      //  "Tcell",
        IOobject::groupName("Tcell", phase.name()),
          phase_.U().time().timeName(),
            phase_.U().mesh(),
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
    ),
   phase_.U().mesh()//T
    ),
    
    rho1_("rho1", dimensionSet(1,0,-3,0,0), diameterProperties_),//properties
    rho2_("rho2", dimensionSet(1,0,-3,0,0), diameterProperties_),
    Khydrate_("Khydrate", dimensionSet(1,1,-3,1,0), diameterProperties_),
    Kwater_("Kwater", dimensionSet(1,1,-3,1,0), diameterProperties_),
    Cpwater_("Cpwater", dimensionSet(0,2,-2,1,0), diameterProperties_),
    Cphydrate_("Cphydrate", dimensionSet(0,2,-2,1,0), diameterProperties_),
    dMax_("dMax", dimLength, diameterProperties_),
    dMin_("dMin", dimLength, diameterProperties_),
    
    residualAlpha_
    (
        "residualAlpha",
        dimless,
        diameterProperties_
    ),
    d_
    (
        IOobject
        (
            IOobject::groupName("d", phase.name()),
            phase_.U().time().timeName(),
            phase_.U().mesh(),
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        dsm()
    ),
    sources_
    (
        diameterProperties_.lookup("sources"),
        IATEsource::iNew(*this)
    )
//Tcellnow(phase.TTT)
   
{}


// * * * * * * * * * * * * * * * * Destructor  * * * * * * * * * * * * * * * //

Foam::diameterModels::IATE::~IATE()
{}


// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
  /* const volScalarField& Tcelliate() const
        {
            return phase.fluid().Tcell();
        }
*/

Foam::tmp<Foam::volScalarField> Foam::diameterModels::IATE::dsm() const
{
    return max(6/max(kappai_, 6/dMax_), dMin_);
}

// Placeholder for the nucleation/condensation model
// Foam::tmp<Foam::volScalarField> Foam::diameterModels::IATE::Rph() const
// {
//     const volScalarField& T = phase_.thermo().T();
//     const volScalarField& p = phase_.thermo().p();
//
//     scalar A, B, C, sigma, vm, Rph;
//
//     volScalarField ps(1e5*pow(10, A - B/(T + C)));
//     volScalarField Dbc
//     (
//         4*sigma*vm/(constant::physicoChemical::k*T*log(p/ps))
//     );
//
//     return constant::mathematical::pi*sqr(Dbc)*Rph;
// }

void Foam::diameterModels::IATE::correct()
{
    // Initialise the accumulated source term to the dilatation effect
    volScalarField R
    (
        (
            (1.0/3.0)
           /max
            (
                fvc::average(phase_ + phase_.oldTime()),
                residualAlpha_
            )
        )
       *(fvc::ddt(phase_) + fvc::div(phase_.alphaPhi()))
    );


    volScalarField niandu
    (
       Khydrate_*phase_/Cphydrate_/rho1_+Kwater_*(1-phase_)/Cpwater_/rho2_
    );//niandu



    // Accumulate the run-time selectable sources
    forAll(sources_, j)
    {
        R -= sources_[j].R();
    }

    fv::options& fvOptions(fv::options::New(phase_.mesh()));

    // Construct the interfacial curvature equation
    fvScalarMatrix kappaiEqn
    (
        fvm::ddt(kappai_) + fvm::div(phase_.phi(), kappai_)
      - fvm::Sp(fvc::div(phase_.phi()), kappai_)
     ==
      - fvm::SuSp(R, kappai_)
  //  - Rph() // Omit the nucleation/condensation term
      + fvOptions(kappai_)
    );

    kappaiEqn.relax();

    fvOptions.constrain(kappaiEqn);

    kappaiEqn.solve();

    // surfaceScalarField& phiphi = phase_.phi();
     fvScalarMatrix TEqn//qiu jie T
              (
                  fvm::ddt(Tcell_)
                 +fvm::div(phase_.phi(),Tcell_)
                 -fvm::laplacian(niandu,Tcell_)
              );
             TEqn.solve(); 
    // Update the Sauter-mean diameter
    d_ = dsm();
}

李东岳

添加T方程为什么要去ITAE库中去做？

另外，你用reactingTwoPhaseEulerFoam里面就有T了

upc_ngh

@东岳我这里求解的是壁面冷却，内部是流体的管内温度分布，不涉及两种流体之间的温度场求解；使用ITAE是因为要把求解出来的温度场传递到ITAE中的Rph中，作为流体相变的驱动力。之前把温度方程直接放到twoPhaseEulerFoam.C中，可以顺利的求解，现在卡了好久也不知道怎么把求解出的温度场再传回ITAE中去，希望东岳老师和各位前辈多指点一下

upc_ngh

各位老师，经过测试发现问题好像是fvm::laplacian(A,B)中的AB两个的数据类型不正确，对于第一个mesh注册的Tcell是没有问题的，对于第二个注册在phase_.U().mesh()内的Tcell就不可以进行计算。现在主要问题是怎么在ITAE.C中将T注册到mesh中，或者有什么办法能够在ITAE库中进行fvm::laplacian(A,B)，标量传输方程正常计算，希望各位老师点拨一下，添加一个标量传输方程咋这么难，哎

volScalarField Tcell
(
    IOobject
    (
        "Tcell",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
    ),
    mesh
);

volScalarField Tcell
    (
    IOobject
    (
        "Tcell",
       // IOobject::groupName("Tcell", phase.name()),
          phase_.U().time().timeName(),
            phase_.U().mesh(),
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
    ),
   phase_.U().mesh()//T
    );

李东岳

使用ITAE是因为要把求解出来的温度场传递到ITAE中的Rph中

你在求解器.C层面，将T植入，这个你会的吧。

然后在ITAE中，通过

const volScalarField& T = mesh.lookupObject<volScalarField>("T"):

传入，这样不可以么

upc_ngh

@东岳谢谢东岳老师，好的我按照这个思路试一下

upc_ngh

@东岳东岳老师现在出现这个问题，麻烦老师有时间再给看看，谢谢谢谢

diameterModels/IATE/IATEsources/randomCoalescence/randomCoalescence.C: In member function ‘virtual Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::diameterModels::IATEsources::randomCoalescence::R() const’:
diameterModels/IATE/IATEsources/randomCoalescence/randomCoalescence.C:94:40: error: ‘mesh’ was not declared in this scope
     const volScalarField& TcellnowLX = mesh.lookupObject<volScalarField>("Tcell");
                                        ^
diameterModels/IATE/IATEsources/randomCoalescence/randomCoalescence.C:94:72: error: expected primary-expression before ‘>’ token
     const volScalarField& TcellnowLX = mesh.lookupObject<volScalarField>("Tcell");

李东岳

const volScalarField& T = phase_.U().mesh().lookupObject<volScalarField>("T"):

upc_ngh

@东岳东岳老师，现在植入进去也能编译成功了，但是开始计算就发散，错误代码如下，看了论坛上和网上的也没找到啥相关的资料，希望东岳老师再给点指导，谢谢

Starting jisuan kappai

smoothSolver:  Solving for kappai.air, Initial residual = 0.164043, Final residual = 3.33679e-07, No Iterations 2
Constructing momentum equations
GAMG:  Solving for p_rgh, Initial residual = 0.0861362, Final residual = 8.71808e-09, No Iterations 55
GAMG:  Solving for p_rgh, Initial residual = 0.00100705, Final residual = 9.19158e-09, No Iterations 42
GAMG:  Solving for p_rgh, Initial residual = 9.49796e-06, Final residual = 9.7128e-09, No Iterations 18
new cannot satisfy memory request.
This does not necessarily mean you have run out of virtual memory.
It could be due to a stack violation caused by e.g. bad use of pointers or an out of date shared library
已放弃 (核心已转储)

植入代码如下：
ITAE.C中

Foam::tmp<Foam::volScalarField> Foam::diameterModels::IATE::Rph() const
 {
     //const volScalarField& T = phase_.thermo().T();
     //const volScalarField& p = phase_.thermo().p();
const volScalarField& Tcellnow = phase_.U().mesh().lookupObject<volScalarField>("Tcell");
   // scalar Teq = 275;
    //scalar rhohydrate = 850;
   // scalar phaseh = 50;
    //scalar qianre = 43500;
dimensionedScalar Teq("Teq", dimensionSet(0,0,0,1,0), 275);
dimensionedScalar rhohydrate("rhohydrate", dimensionSet(1,-3,0,0,0), 850);
dimensionedScalar phaseh("phaseh", dimensionSet(1,1,-3,-1,0), 50);
dimensionedScalar qianre("qianre", dimensionSet(0,2,-2,0,0), 43500);

    volScalarField delt(Tcellnow - Teq);
    volScalarField Rph(0.0085*phaseh*delt*phase_*pow(kappai_,5)/rhohydrate/qianre);
    volScalarField Dsm(max(6/max(kappai_, 6/dMax_), dMin_));

   // volScalarField Dbc
 //  (
        // 4*sigma*vm/(constant::physicoChemical::k*T*log(p/ps))
   //);

     return constant::mathematical::pi*sqr(Dsm)*Rph;
 }

李东岳

编译完库之后，重新编译一下求解器，然后再计算

李东岳

Um...这个应该是IATE，不是ITAE

upc_ngh

@东岳哈哈谢谢东岳老师，一直打错了。。。
重新编译库还是不行，将

const volScalarField& Tcellnow = phase_.U().mesh().lookupObject<volScalarField>("Tcell");

更改为

volScalarField Tcellnow = phase_.U().mesh().lookupObject<volScalarField>("Tcell");

还是不行，增加虚拟机内存还是不行，但是把湍流改成层流就能顺利计算了，这是怎么回事？？？

upc_ngh

晚上又测试了一下，在linux系统下是可以顺利的进行计算，谢谢东岳老师的帮助