记录一些自己用过的代码

李东岳

const fvPatchList& patches = mesh.boundary();

forAll(patches, patch)
{
	Info << patches[patch].name() << nl;
        const fvPatch& currPatch = patches[patch];
        forAll(currPatch, face)
        {
		Info << abs_[0].boundaryField()[patch][face] << nl;
	}
}

李东岳

OpenFOAM-4.x以前？反正是老的：

const scalarField& psi = U.internalField(); 
scalarField& psi = U.internalField();

OpenFOAM-5.x, 4.x：

const scalarField& psi = U.primitiveField(); 
scalarField& psi = U.primitiveFieldRef();

tmp旧式风格：

tmp<volScalarField> tField = ... 
volScalarField& non_const_field = tField(); 
const volScalarField& const_field = tField();

新式风格：

tmp<volScalarField> tField = ... 
volScalarField& non_const_field = tField().ref(); 
const volScalarField& const_field = tField();

旧式：

const volScalarField::GeometricBoundaryField& bsf = field.boundaryField(); 
volScalarField::GeometricBoundaryField& bsf = field.boundaryField();

新式：

const volScalarField::Boundary& bsf = field.boundaryField(); 
volScalarField::Boundary& bsf = field.boundaryFieldRef();

dimensionedInternalField已经被volScalarField::Internal替换
https://www.openfoam.com/documentation/developer-upgrade-guide.php

李东岳

    const labelUList& owner = mesh_.owner();
    const labelUList& neighbour = mesh_.neighbour();

    forAll(weis_, kth)
    {
        forAll(sumWeisF[kth], cellI)
        {

            Info << "Current cell index is " << cellI << nl;

            //- Loop the faces of cellI
            forAll(mesh_.cells()[cellI], faceI)
            {
                //- Check if it is an internal face
                if (mesh_.isInternalFace(mesh_.cells()[cellI][faceI]))   
                {
                    label faceIndex = mesh_.cells()[cellI][faceI];
                    Info << " its faceIndex is " << faceIndex;
                    Info << ", and this face's owner is "
                        << owner[faceIndex] << ", its neighbour is "
                        << neighbour[faceIndex] << nl;
                }
            }
            
            Info << nl;
        } 
    }

输出如下：

Current cell index is 851
 its faceIndex is 1684, and this face's owner is 851, its neighbour is 852
 its faceIndex is 1685, and this face's owner is 851, its neighbour is 896
 its faceIndex is 1596, and this face's owner is 806, its neighbour is 851
 its faceIndex is 1682, and this face's owner is 850, its neighbour is 851

Current cell index is 852
 its faceIndex is 1686, and this face's owner is 852, its neighbour is 853
 its faceIndex is 1687, and this face's owner is 852, its neighbour is 897
 its faceIndex is 1598, and this face's owner is 807, its neighbour is 852
 its faceIndex is 1684, and this face's owner is 851, its neighbour is 852

希望有用 :confused:

李东岳

const labelList& inletCells = mesh.boundary()["inlet"].faceCells();

template<class Type>
void zeroCells
(
    GeometricField<Type, fvPatchField, volMesh>& vf,
    const labelList& cells
)
{
    forAll(cells, i)
    {
        vf[cells[i]] = Zero;
    }
}

zeroCells(alpha, inletCells);

李东岳

输出边界条件类型：

Info << alpha.boundaryField().types()[patch] << nl;

同学博

亲测实用

CFD中文网

记录一些自己用过的代码