zeroGradientCorrected

Zero-gradient condition whose patch value includes a non-orthogonal correction evaluated on a patch sub-mesh; foam-extend interface-tracking legacy, compiled into libinterfaceTrackingFvMesh.

Overview

zeroGradientCorrected is a zero-gradient condition for fields of any type (scalar, vector, sphericalTensor, symmTensor, tensor). Instead of copying the near-wall cell value, it sets the patch value to the cell value plus a non-orthogonal correction $\mathbf{c}\cdot\nabla\phi_P$, evaluated on a small sub-mesh around the patch. The same correction enters the matrix 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

$$ \left.\frac{\partial\phi}{\partial n}\right|_b = 0 \quad \text{on } \partial\Omega, \qquad \phi_b = \phi_P + \phi_c, \qquad \phi_c = \mathbf{c}\cdot(\nabla\phi)_P, \quad \mathbf{c} = \boldsymbol{\Delta} - \mathbf{n}\,(\mathbf{n}\cdot\boldsymbol{\Delta}) $$

Matrix coefficients:

Coefficient	Value
`valueInternalCoeffs`	$1$
`valueBoundaryCoeffs`	$\phi_c$
`gradientInternalCoeffs`	$0$
`gradientBoundaryCoeffs`	$0$
`snGrad()`	$0$

Symbol	Description	Unit
$\phi$	Patch field	field unit
$\mathbf{n}$	Patch unit normal	–
$\boldsymbol{\Delta}$	Patch delta vector (`patch().delta()`)	m
$\mathbf{c}$	Correction vector	m
$\phi_c$	Stored correction (`corrVecGrad`), updated in `updateCoeffs()`	field unit

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 zeroGradient.

Implementation

Construction: the base class reads volFieldName (required) and the optional corrVecGrad. The patch value is set to $\phi_P + \phi_c$. value is not read.
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 uses the current $\phi_c$.
evaluate(): declared without the Pstream::commsTypes argument. It does not override fvPatchField::evaluate(const Pstream::commsTypes), which correctBoundaryConditions() calls. The base version runs, and it only resets the updated flag. The patch value is not recomputed after a solve. It stays at the construction value $\phi_P + \phi_c$ of the initial field, so it does not behave like a zero-gradient value at all.
Mapping: autoMap/rmap map the value only.
Sub-mesh motion: interfaceTrackingFvMesh::update() moves the sub-mesh only for U and p.
write(): type, volFieldName, corrVecGrad. No value is written.

Dictionary Entries

Keyword	Description	Required	Default
`type`	`zeroGradientCorrected`	yes	–
`volFieldName`	Name of the volume field this patch field belongs to	yes	– (no default)
`corrVecGrad`	Initial stored correction $\phi_c$	no	zero

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

Usage

outlet
{
    type            zeroGradientCorrected;
    volFieldName    U;
}

Known Limitations

Patch value frozen at its initial value, because the evaluate() signature does not match (see Implementation). Explicit operators that use patch values (fvc::grad, fvc::interpolate, face fluxes) see the initial 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 zeroGradient instead.

Tutorials

No tutorial uses zeroGradientCorrected.

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