twoPhaseEulerFoam中的ITAE模型

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It could be due to a stack violation caused by e.g. bad use of pointers or an out of date shared library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

CFD中文网

twoPhaseEulerFoam中的ITAE模型