regionCoupledPressureFlux

Overview

regionCoupledPressureFlux is the Neumann (flux) half of the partitioned pressure coupling across a sharp, mesh-tracked fluid-fluid interface. It acts on a volScalarField (p or pKin) and derives from genericRegionCoupledFlux<scalar>, i.e. from fixedGradient. Although it is built on the generic flux-matching scheme, its fluxJump() cancels the neighbour flux. The normal pressure gradient therefore depends only on the local normal acceleration $\mathbf{n}\cdot\partial\mathbf{U}/\partial t$. The partner condition on the other side is regionCoupledPressureValue (or regionCoupledMassTransferPressureValue, inferred: there is no mass-transfer pressure-flux BC). It is used with capillaryInterface.

Mathematical Formulation

The BC sits on side $B$ in all tutorials. $\mathbf{n}_B$ is the outward patch normal and $\tilde F = \mathcal{I}_{A\to B}(F_A)$ the interpolated neighbour flux snGrad(p_A)*k_A. The generic flux BC sets $k_B\,\partial p_B/\partial n = -\tilde F + \text{fluxJump}$ with

so that

This is the normal momentum balance at the interface without the convective and viscous terms (the code that included them is commented out). The gradient is relaxed by the acceleration model, $g^{k} = g^{k-1} + \omega\,(g^{*} - g^{k-1})$, and the patch value is reconstructed as $p_B = p_P + \mathbf{k}\cdot\nabla p_P + g/\Delta_f$ (first order) or $p_P + \mathbf{k}\cdot\nabla p_P + (g + \mathbf{n}\cdot\nabla p_P)/(2\Delta_f)$ (secondOrder yes); the $\mathbf{k}$ term only with nonOrthCorr yes.

The diffusivity $k_B$ comes from diffCoeff() with the hardcoded name v:

For p the imposed gradient is therefore $-\mathbf{n}_B\cdot\partial_t\mathbf{U}_B/\rho_B$ instead of $-\rho_B\,\mathbf{n}_B\cdot\partial_t\mathbf{U}_B$ (see Known Limitations).

Implementation

updateCoeffs() is the generic one of genericRegionCoupledFlux:

1. Return if updated or coupled no (gradient frozen).
2. Call update() on the first interfaceType.
3. Look up the neighbour field by the local field name and refCast its patch field to genericRegionCoupledJump<scalar>; interpolate its flux() and negate it.
4. Add fluxJump(), divide by diffCoeff(), relax, call fixedGradient::updateCoeffs().

fluxJump() repeats step 3 to get $\tilde F$ and returns $\tilde F - \mathbf{n}_B\cdot(\partial_t\mathbf{U})_b$. It also reads rho and mu from the local transportProperties (required to exist), but does not use them. Unlike the other capillary BCs it never calls capInterface(), so it does not check the interface type.

The p flux residual of the pUPimple DNA loop comes from this BC, because the side-A pressure patch carries a jump BC. The neighbour flux cancels in it as well:

normalised as described in genericRegionCoupledFlux.

Dictionary Entries

write() does not write gradient.

Usage

tutorials/multiphaseFlow/2dRisingBubble/0/fluidB/orig/partitioned/p (side B):

interfaceShadow
{
    type                    regionCoupledPressureFlux;
    diffusivity             "v";                    // ignored, always v
    interfaceType           (capillaryInterface);
    secondOrder             false;
    nonOrthCorr             false;
    value                   uniform 0;              // not read
}

Partner on side A, 0/fluidA/orig/partitioned/p:

interface
{
    type                    regionCoupledPressureValue;
    interfaceType           (capillaryInterface);
    value                   uniform 0;
}

The interface and DNA entries are shown on the regionCoupledVelocityValue page and in capillaryInterface.

Known Limitations

• Wrong diffusivity for p (bug). diffCoeff() renames v to rho before it checks for v, so the reciprocal is never taken and $k_B = \rho_B$. For a field named p the imposed gradient is off by a factor $\rho_B^2$ and has the wrong units. pKin is not affected. The tutorials use p.
• Simplified normal momentum balance. Convective and viscous contributions to the normal pressure gradient are not included.
• Neighbour flux has no effect. The interpolated neighbour flux cancels. It is still computed, and the neighbour patch field must derive from genericRegionCoupledJump<scalar>, otherwise the refCast aborts.
• No interface-type check. Any interface type listed first is accepted; it is only update()d.
• diffusivity and neighbourFieldName are ignored; gradient is not written to the time directories.
• No runnable tutorial. The tutorials use the disabled interTrackFluid.

Tutorials

The BC is set in the 0/fluidB/orig/partitioned/p variant of each tutorial.

References

• 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