overInterDyMFoam求解器报错

stergopilot

我在openfoam-v1702版本中使用求解器overInterDyMFoam模拟一个两相流问题，添加了一个温度方程，网格用ICEM和starccm+分别做了一遍，导入openfoam后，求解过程中报错。结果如下：请问是什么问题？大概从哪方面入手解决。谢谢。

Create time

Create mesh for time = 0

Selecting dynamicFvMesh dynamicOversetFvMesh
Selecting motion solver: multiSolidBodyMotionSolver
Selecting solid-body motion function linearMotion
Applying solid body motion linearMotion to 8709 points of cellZone movingZone

PIMPLE: no residual control data found. Calculations will employ 2 corrector loops

Reading field p_rgh

Reading field U

Reading/calculating face flux field phi

Creating cellMask field to block out hole cells

inverseDistance : detected 1 mesh regions
    zone:0 nCells:294994  voxels:(66 66 66) bb:(-0.500003 -0.200003 -0.600003) (2.5 0.800003 0.600003)
Overset analysis : nCells : 294994
    calculated   : 288000
    interpolated : 0 (interpolated from local:0  mixed local/remote:0  remote:0)
    hole         : 6994

Creating interpolatedCells field 

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Reading field T

Selecting turbulence model type laminar
Selecting laminar stress model Stokes

Reading g

Reading hRef
Calculating field g.h

No MRF models present

No finite volume options present

DICPCG:  Solving for pcorr, Initial residual = 1, Final residual = 5.02939e+06, No Iterations 1001
Reading/calculating face velocity Uf

Courant Number mean: 0 max: 0

Starting time loop

Courant Number mean: 0 max: 0
Interface Courant Number mean: 0 max: 0
deltaT = 0.0120482
Time = 0.0120482

PIMPLE: iteration 1
inverseDistance : detected 1 mesh regions
    zone:0 nCells:294994  voxels:(66 66 66) bb:(-0.500003 -0.200003 -0.600003) (2.5 0.800003 0.600003)
Overset analysis : nCells : 294994
    calculated   : 288000
    interpolated : 0 (interpolated from local:0  mixed local/remote:0  remote:0)
    hole         : 6994

Execution time for mesh.update() = 3.08 s
smoothSolver:  Solving for alpha.water, Initial residual = 0, Final residual = 0, No Iterations 0
Phase-1 volume fraction = 1  Min(alpha.water) = 1  Max(alpha.water) = 1
MULES: Correcting alpha.water
MULES: Correcting alpha.water
Phase-1 volume fraction = 1  Min(alpha.water) = 1  Max(alpha.water) = 1
DILUPBiCG:  Solving for T, Initial residual = 0.449627, Final residual = 1.05799e-09, No Iterations 4
Begin change rhok
End change rhok


--> FOAM FATAL ERROR: 

    request for volScalarField none from objectRegistry region0 failed
    available objects of type volScalarField are

20
(
rhok
alpha.water_0
interfaceProperties:K
alpha.water
rho
rAU
cellMask
p_rgh
interpolatedCells
nu
gh
nu1
p
rho_0
nu2
T
T_0
alpha.air
((alpha.water*Cp)+(alpha.air*Cp))
div(phiHbyA)
)


    From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&, bool) const [with Type = Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>]
    in file /home/tan/OpenFOAM/OpenFOAM-v1706/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 239.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&, bool) const at ??:?
#3  ? at totalPressureFvPatchScalarField.C:?
#4  Foam::totalPressureFvPatchScalarField::updateCoeffs(Foam::Field<double> const&, Foam::Field<Foam::Vector<double> > const&) at ??:?
#5  Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) at ??:?
#6  Foam::fv::gaussLaplacianScheme<double, Foam::SymmTensor<double> >::fvmLaplacianUncorrected(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#7  Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#8  ? at ??:?
#9  ? at ??:?
#10  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#11  ? at ??:?
已放弃 (核心已转储)

之后只用overInterDyMFoam求解，还是相同的问题 request for volScalarField none from objectRegistry region0 failed。请问是什么问题？大概从哪方面入手解决。谢谢。

Jacobian

某个边界的压力边条用了totalPressure吧？你的代码里面是不是没有psi这个变量？

stergopilot

是的，我设置的水池顶部的边界条件是totalPressure，代码里也没有psi变量。

Jacobian

把压力的边界条件贴出了看看吧

stergopilot

top
    {
        type            totalPressure;
        p0              uniform 0;
        U               U;
        phi             phi;
        rho             none;
        psi             none;
        gamma           1;
        value           uniform 0;

    }

改成top

    {
        type            totalPressure;
        p0              uniform 0;
    }

就不报错了，不知道是什么原因。

Jacobian

举个相关的例子，比如我们要给a赋值，公式是a等于b乘以c，那么有两种方式：
第一种，最普通的：

a = b*c;

还有第二种，调用lookUpObject：

a = b*b.db().lookUpObject("c");

这样，lookUpObject可以从已经注册的变量中去寻找需要的那一个，如果找不到就会报你看到的那种错误。
可想而知，如果用的是第一种方式，没有定义变量c就会导致编译时提示错误。而如果用的是第二种方式，就算没有定义变量c，编译时也不会报错，但计算时就会出错。
totalPressureFvPatchScalarField.C 中虽然调用的是lookupPatchField<surfaceScalarField, scalar>("xxxxxx")，但情况是类似的

stergopilot

明白了，谢谢！

CFD中文网

overInterDyMFoam求解器报错