potentialFluid

Overview

potentialFluid solves for potential flow: an inviscid, irrotational, incompressible idealisation in which the velocity field is the gradient of a scalar velocity potential $\Phi$, reducing the flow problem to a single Laplace equation. It is the multiPhysicsFoam port of OpenFOAM’s potentialFoam.

Its primary use is initialisation: it produces a smooth, discretely divergence-free velocity and flux field consistent with the boundary conditions, from which a full Navier-Stokes region such as pimpleFluid can start without a violent initial transient. It is also a cheap mesh-quality diagnostic. Because the model contains no viscosity, it resolves no boundary layers, separation, wakes, or drag, and is not intended as a final-answer solver.

The region re-solves on every time step. For the usual one-shot initialiser workflow, limit the run to a single step via controlDict (endTime 1, deltaT 1), as both tutorials do.

Governing Equations

Continuity and irrotationality

Velocity potential

Irrotationality permits $\mathbf{U} = \nabla \Phi$, which with continuity gives Laplace’s equation:

Discretely this is solved in projection form. From the flux field $\phi^{*}$ implied by the boundary conditions,

so that $\nabla \cdot \phi = 0$ to solver tolerance on the actual mesh. The cell velocity is recovered by fvc::reconstruct(phi).

Euler pressure (optional)

Enabled by writep. Taking the divergence of the steady Euler equation, with the source filtered along the flow direction by $\mathbf{F} = \hat{\mathbf{U}} \otimes \hat{\mathbf{U}}$ to suppress spurious cross-stream pressure variation:

Numerical Algorithm

There is no PIMPLE loop and no time integration: usesPIMPLE() returns false and the whole algorithm runs in solveRegion(), which the orchestrator calls before any PIMPLE stage. Per run:

1. Make the flux relative to any MRF zones.
2. Balance the global flux (adjustPhi). Applied only when $p_\text{kin}$ needs a reference, i.e. no fixed-value pressure boundary exists; total inflow is then forced to equal total outflow.
3. Non-orthogonal corrector loop — assemble and solve $\nabla^2\Phi = \nabla\cdot\phi$ with setReference applied. On the final iteration only, correct the flux: phi -= PhiEqn.flux().
4. Restore the absolute flux.
5. Report the continuity error $\overline{|\nabla \cdot \phi|}$, volume-weighted.
6. Reconstruct U from phi and correct its boundary conditions.
7. Report the interpolated velocity error — the drift between fvc::flux(U) and phi; a mesh-quality diagnostic.
8. Solve the Euler pressure in its own non-orthogonal loop, if writep.
9. Update the dimensional pressure $p = p_\text{kin}\rho$.

A reference cell is required because an all-Neumann Laplacian is singular ($\Phi$ and $\Phi + C$ are both solutions). setReference derives its keywords from the field name, so the case dictionary uses PhiRefCell/PhiRefValue and pKinRefCell/pKinRefValue.

Steps 1–9 execute on every time step; the solve is not latched. Since the solution is fully determined by the boundary conditions, additional steps recompute the same answer unless a sibling region has perturbed U or phi in the meantime — so restrict the run to one step unless you want that re-establishment.

Sub-Models

Required Fields

Additionally created at runtime:

Where pKin and Phi are not supplied, their boundary types are inferred by inverting Dirichlet and Neumann at each step: pKin is zeroGradient wherever U fixes value and fixedValue elsewhere; Phi inverts that again. Supplying 0/U alone is therefore sufficient.

Case Setup

Required dictionaries

constant/transportProperties   – density (rho); required, read MUST_READ
system/fvSolution              – Phi/pKin linear solvers, potentialFlow sub-dict
system/fvSchemes               – discretisation schemes

Unlike stock potentialFoam, constant/transportProperties is mandatory:

rho             1000;

multiRegionProperties entry

regions
(
    ( fluid (potentialFluid) )
);

To initialise a field that another region then solves, list potentialFluid first so that it owns and constructs the shared fields:

regions
(
    ( fluid (potentialFluid pimpleFluid) )
);

controlDict (singleRegionMode)

singleRegionMode    yes;
regionType          potentialFluid;

endTime             1;      // one step == one potential flow solve
deltaT              1;
adjustTimeStep      no;     // getMinDeltaT() returns GREAT

Key fvSolution settings

solvers
{
    Phi
    {
        solver          GAMG;
        smoother        DIC;
        tolerance       1e-06;
        relTol          0.01;
    }

    pKin
    {
        $Phi;
    }
}

potentialFlow
{
    nNonOrthogonalCorrectors 3;

    writePhi        true;
    writep          true;

    // Reference cells (closed domains)
    PhiRefCell      0;
    PhiRefValue     0;
    pKinRefCell     0;
    pKinRefValue    0;
}

potentialFlow dictionary entries

potentialFoam’s command-line flags become optional dictionary entries, all read as Foam::Switch and defaulting to false:

Being Switch-valued, each accepts any of true/false, yes/no, on/off or none/any; the tutorials use true/false.

Dropped: -pName (the field is always pKin), -withFunctionObjects (function objects run automatically), and -writephi (phi is always written).

Coupling

potentialFluid implements no interface-specific behaviour: setCoupledEqns() is a no-op, it declares no selfCoupledFieldNames(), and it takes no part in DNA partitioned coupling.

Coupling is implicit, through the object registry: the fields it constructs (U, phi, pKin, p) are visible by name to sibling regions on the same mesh, which is what enables the initialiser role.

Known Limitations

• Re-solves every time step — the solve is not latched, but the solution is fully determined by the boundary conditions, so a long endTime repeats the same computation. Limit the run to a single step in controlDict.
• writep false writes a zero pKin and p — the Euler pressure is never calculated, but both fields are AUTO_WRITE regardless.

Tutorials

Both reproduce the corresponding $FOAM_TUTORIALS/basic/potentialFoam/ case field-for-field, with 0/p renamed to 0/pKin, the command-line flags moved into the potentialFlow dict, and constant/transportProperties added.

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
• Batchelor, G.K., An Introduction to Fluid Dynamics, CUP, 1967 — Ch. 6, irrotational flow theory.
• Upstream source: $FOAM_APP/solvers/basic/potentialFoam/