dynamicMeshDict设置问题

[sungda]

计算过程中显示：

--> FOAM Warning : 
    From function Foam::autoPtr<Foam::mapPolyMesh> Foam::dynamicRefineFvMesh::unrefine(const labelList&)
    in file dynamicRefineFvMesh/dynamicRefineFvMesh.C at line 546
    Cannot find surfaceScalarField ((interpolate(grad(psi))|(mag(interpolate(grad(psi)))+(1e-06|dimChange)))&S) in user-provided flux mapping table 
7
(
phi none
rhoPhi none
rhoPhiH none
nHatf none
alphaPhi10 none
ghf none
alphaPhi none
)
    The flux mapping table is used to recreate the flux on newly created faces.
    Either add the entry if it is a flux or use (((interpolate(grad(psi))|(mag(interpolate(grad(psi)))+(1e-06|dimChange)))&S) none) to suppress this warning.

我在correctFluxes中加入

 (((interpolate(grad(psi))|(mag(interpolate(grad(psi)))+(1e-06|dimChange)))&S) none) 

但是结果显示格式不正确，有大佬遇到过相类似的情况吗？目前针对这块还不是很熟悉，请大家多多指教

[李东岳]

@sungda 这样可以吗

((interpolate(grad(psi))|(mag(interpolate(grad(psi)))+(1e-06|dimChange)))&S) none

你为什么会存在这个通量，自己写的求解器么

[sungda]

@李东岳 李老师，这是我自己的求解器，但是这个通量我也不知道为什么会出来
我在dynamicMeshDict加了您说的这个，结果报错，可能是代码的问题。

correctFluxes
(
    (phi none)
    (rhoPhiH none)
    (nHatf none)
    (rhoPhi none)
    (alphaPhi none)
    (ghf none)
    (alphaPhi10 none)
    (phi_0 none)
    (((interpolate(grad(psi))|(mag(interpolate(grad(psi)))+(1e-06|dimChange)))&S) none)
);

[0] --> FOAM FATAL IO ERROR: 
[0] wrong token type - expected word, found on line 56 the punctuation token '('
[0] 
[0] file: /home/oufool/OpenFOAM/oufool-5.0/run/bubblecol/bubblecol9/constant/dynamicMeshDict.correctFluxes at line 56.
[0] 
[0]     From function Foam::Istream& Foam::operator>>(Foam::Istream&, Foam::word&)
[0]     in file primitives/strings/word/wordIO.C at line 74.
[0] 
FOAM parallel run exiting

[李东岳]

@sungda

('((interpolate(grad(psi))|(mag(interpolate(grad(psi)))+(1e-06|dimChange)))&S)' none)

这样行么

[sungda]

@李东岳 李老师，这样是可以的，

("((interpolate(grad(psi))|(mag(interpolate(grad(psi)))+(1e-06|dimChange)))&S)" none)