fixedGradientCorrected

Overview

fixedGradientCorrected is a Neumann condition for fields of any type (scalar, vector, sphericalTensor, symmTensor, tensor). It prescribes the patch-normal gradient. Its patch value and value coefficients include a non-orthogonal correction $\mathbf{c}\cdot\nabla\phi_P$, evaluated on a small sub-mesh around the patch. Unlike fixedValueCorrected, the correction enters the matrix directly, through valueBoundaryCoeffs. It comes from the foam-extend interface-tracking solver (interTrackFoam, Tuković). The BC is compiled into libinterfaceTrackingFvMesh. It derives from the common base correctedFvPatchField (type corrected). The base class, the sub-mesh machinery, the corrected type and the porting status (interTrackFluid disabled, patchCorrected snGrad not ported) are described on the fixedValueCorrected page.

Mathematical Formulation

with the correction from the base class

Matrix coefficients:

Note on OpenFOAM.com. fvPatch::delta() is patch-normal for every non-coupled patch in OpenFOAM.com, so $\mathbf{c} \equiv \mathbf{0}$ and $\phi_c \equiv 0$. The coefficients reduce to those of stock fixedGradient.

Implementation

• Construction: the base class reads volFieldName (required) and the optional corrVecGrad. This class then reads gradient (required). If value is given, it is used as the initial patch value. Otherwise $\phi_P + \delta g + \phi_c$ is used, with $\phi_c = 0$ at that point unless corrVecGrad was given. nGradInternal is set to $g$.
• updateCoeffs() (base class): recomputes $\mathbf{c}$ if the mesh moves, rebuilds $\phi_c$ on the patch sub-mesh (gradient scheme snGradCorr(<volFieldName>)). It is called whenever an fvMatrix for the field is constructed, so valueBoundaryCoeffs always uses the current $\phi_c$.
• evaluate(): the class declares evaluate() without the Pstream::commsTypes argument. It therefore does not override fvPatchField::evaluate(const Pstream::commsTypes), which correctBoundaryConditions() calls. In practice the base evaluate runs, and that only resets the updated flag. The patch value is not recomputed from $\phi_P + \phi_c + \delta g$ after a solve. It keeps its initial value unless code assigns it explicitly. Only the matrix coefficients follow the formula above.
• Mapping: autoMap/rmap map the value and gradient.
• Sub-mesh motion: interfaceTrackingFvMesh::update() moves the sub-mesh only for U and p.
• write(): type, volFieldName, corrVecGrad, gradient, value.

Dictionary Entries

The library must be loaded with libs ("libinterfaceTrackingFvMesh.so"); in system/controlDict.

Usage

outlet
{
    type            fixedGradientCorrected;
    volFieldName    p;
    gradient        uniform 0;
    value           uniform 0;
}

Known Limitations

• Patch value not updated by correctBoundaryConditions() because the evaluate() signature does not match (see Implementation). Explicit operators that use patch values (fvc::grad, fvc::interpolate, face fluxes) see a stale value.
• No correction in OpenFOAM.com (patch-normal delta()). The cost of the sub-mesh gradient remains on every updateCoeffs().
• Interface-tracking context not available: interTrackFluid is disabled and patchCorrected is not ported (see fixedValueCorrected).
• volFieldName has no default and must match the field name.
• Sub-mesh motion only for U and p.

In practice, use the stock fixedGradient instead.

Tutorials

No tutorial uses fixedGradientCorrected.

References

• Tuković, Ž., Jasak, H., A moving mesh finite volume interface tracking method for surface tension dominated interfacial fluid flow, Computers & Fluids 55, 2012. DOI: 10.1016/j.compfluid.2011.11.003
• Alkfri, A., Habes, C., Marschall, H., multiRegionFoam: A Unified Multiphysics Framework for Multi-Region Coupled Continuum-Physical Problems, Engineering with Computers, 2023. DOI: 10.1007/s00366-024-01974-4