regionCoupledPressureValue

Overview

regionCoupledPressureValue is the Dirichlet (jump) half of the partitioned pressure coupling across a sharp, mesh-tracked fluid-fluid interface. It acts on a volScalarField (p, or the kinematic pressure pKin) and derives from genericRegionCoupledJump<scalar>, i.e. from fixedValue. The patch value is the interpolated neighbour pressure plus the normal-stress jump: capillary pressure $\sigma\kappa$, the viscous normal-stress jump and a hydrostatic correction. The partner condition on the other side is regionCoupledPressureFlux. Both belong to capillaryInterface, and this BC aborts if the first entry of its interfaceType list is not capillaryInterface. The variant with phase change is regionCoupledMassTransferPressureValue.

Mathematical Formulation

Region $A$ is the first entry of coupledPatchPair and carries the faMesh of the capillaryInterface. This BC sits on side $A$ (see Known Limitations). $\mathcal{I}_{B\to A}$ is the patch-to-patch interpolation.

For a field named p:

For a field named pKin the same jump is applied in kinematic form:

The viscous term is the jump of $2\mu\,\partial u_n/\partial n$ with $\partial u_n/\partial n = -\nabla_s\cdot\mathbf{u}_s$. The gravity term implies that p excludes the hydrostatic part $\rho\,\mathbf{g}\cdot(\mathbf{x}-\mathbf{x}_\text{ref})$ (inferred from the formula). The value is then relaxed: $p_A^{k} = p_A^{k-1} + \omega\,(p_A^{*} - p_A^{k-1})$.

Implementation

updateCoeffs() is the generic one of genericRegionCoupledJump: return if updated or coupled no; call update() on the first interfaceType (curvature and $\mathbf{u}_s$); interpolate the neighbour field (looked up by the local field name) onto this patch; add valueJump(); relax; call fixedValue::updateCoeffs().

valueJump():

• takes $\sigma$, $\kappa$ and $\mathbf{u}_s$ from the capillaryInterface and computes $\nabla_s\cdot\mathbf{u}_s$ with fac::div;
• reads pRefPoint from the PISO sub-dictionary of region A’s fvSolution and looks up g in region A (both required);
• reads mu and rho of both regions from their registered transportProperties dictionaries;
• for pKin returns the bracket above divided by $\rho_A$, minus the interpolated neighbour value, so that the base class sum gives the kinematic formula.

It also computes the mesh flux and the patch normals, but does not use them.

The jump residual for p in the pUPimple DNA loop is taken from this BC, because side A is checked first: $\lVert p_A - \mathcal{I}_{B\to A}(p_B) - \text{valueJump}\rVert_2$, normalised as described in genericRegionCoupledJump.

flux() (inherited) returns snGrad()*k with $k$ from diffCoeff() and the hardcoded diffusivity name v. diffCoeff() maps v to rho, but the step that should take the reciprocal is never reached, so $k = \rho_A$ instead of $1/\rho_A$ ($k = 1$ for pKin). The partner regionCoupledPressureFlux cancels this flux, so the error does not reach the solution.

Dictionary Entries

Entries read from other files:

Usage

tutorials/multiphaseFlow/2dRisingBubble/0/fluidA/orig/partitioned/p (side A):

interface
{
    type                    regionCoupledPressureValue;
    diffusivity             "v";                    // ignored, always v
    interfaceType           (capillaryInterface);
    secondOrder             false;
    nonOrthCorr             false;
    value                   uniform 0;
}

Partner on side B, 0/fluidB/orig/partitioned/p:

interfaceShadow
{
    type                    regionCoupledPressureFlux;
    diffusivity             "v";
    interfaceType           (capillaryInterface);
    secondOrder             false;
    nonOrthCorr             false;
    value                   uniform 0;
}

system/fluidA/fvSolution must contain PISO { ... pRefPoint (0 0 0); }. The interface and DNA entries are shown on the regionCoupledVelocityValue page and in capillaryInterface.

Known Limitations

• capillaryInterface only. capInterface() aborts unless the first interfaceType entry is capillaryInterface.
• Must sit on side A (inferred). $\sigma$, $\kappa$ and $\nabla_s\cdot\mathbf{u}_s$ are taken from the side-A faMesh index by index, without interpolation.
• Constant properties. $\mu$ and $\rho$ are single scalars from transportProperties; registered mu or rho fields are not used.
• PISO.pRefPoint is required, even if the region solver uses a PIMPLE dictionary.
• diffCoeff() returns $\rho$ instead of $1/\rho$ for the diffusivity v. Without consequence for this BC (see Implementation).
• diffusivity and neighbourFieldName are ignored.
• The header example omits interfaceType, which is required.
• No runnable tutorial. The tutorials use the disabled interTrackFluid.

Tutorials

The BC is set in the 0/fluidA/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