Docs: rhoPimpleFluid

Mon, 01 Jan 0001 00:00:00 +0000

Overview

rhoPimpleFluid solves the transient, compressible Navier-Stokes equations for a Newtonian single-phase fluid with the PIMPLE (merged PISO–SIMPLE) pressure-velocity coupling algorithm. It is a port of OpenFOAM’s rhoPimpleFoam: density follows from a run-time selectable thermophysical model (fluidThermo), and an energy equation for sensible enthalpy or internal energy is solved alongside momentum. It supports compressible turbulence modelling (laminar, RANS, LES), a transonic pressure formulation, local time stepping (LTS), moving meshes, MRF and fvOptions. It is suitable for subsonic to supersonic gas flows, standalone or as the fluid side of a multi-region problem.

Governing Equations

Continuity

$$ \frac{\partial \rho}{\partial t} + \nabla \cdot \left(\rho\mathbf{U}\right) = S_\rho $$

Momentum

$$ \frac{\partial \left(\rho\mathbf{U}\right)}{\partial t} + \nabla \cdot \left(\rho\mathbf{U}\mathbf{U}\right) - \nabla \cdot \mathbf{R} = -\nabla p + \mathbf{S}_U $$

The effective stress divergence is provided by the turbulence model via compressible::turbulenceModel::divDevRhoReff(U).

Energy

The energy variable $e$ is either sensible enthalpy $h$ or sensible internal energy $e$, selected by the energy keyword in thermophysicalProperties. With $K = \tfrac{1}{2}|\mathbf{U}|^2$:

$$ \frac{\partial \left(\rho h\right)}{\partial t} + \nabla \cdot \left(\rho\mathbf{U}h\right) + \frac{\partial \left(\rho K\right)}{\partial t} + \nabla \cdot \left(\rho\mathbf{U}K\right) - \frac{\partial p}{\partial t} - \nabla \cdot \left(\alpha_\text{eff}\nabla h\right) = S_h $$

For internal energy the pressure-work term $-\partial p/\partial t$ is replaced by $\nabla \cdot \left(p\,\mathbf{U}\right)$ (div(phiv,p)). The $\partial p/\partial t$ term is only included if dpdt is enabled in the thermophysical model (default yes). With active MRF zones the term $\nabla \cdot (\phi_\text{MRF}\,p)$ is added.

Equation of state

Density is closed by the thermophysical model, $\rho = \rho(p, T)$, with compressibility $\psi = \partial\rho/\partial p$ used in the pressure equation.

Symbol	Description	Unit
$\rho$	Density	kg/m³
$\mathbf{U}$	Velocity	m/s
$p$	(Static) pressure	Pa
$T$	Temperature	K
$h$, $e$	Sensible enthalpy / internal energy	J/kg
$K$	Specific kinetic energy	m²/s²
$\psi$	Compressibility	s²/m²
$\mathbf{R}$	Effective stress tensor (viscous + turbulent)	Pa
$\alpha_\text{eff}$	Effective thermal diffusivity (laminar + turbulent)	kg/(m·s)
$S_\rho$, $\mathbf{S}_U$, $S_h$	Sources (from `fvOptions`)	—

Stress tensor (for FSI coupling)

After each pressure-correction stage the Cauchy stress tensor is updated:

$$ \boldsymbol{\sigma} = -p\,\mathbf{I} - \mathbf{R}^\text{dev} $$

where $\mathbf{R}^\text{dev}$ is turbulence::devRhoReff(). Since $p$ is the static pressure in Pa, no density scaling is applied (unlike pimpleFluid).

Numerical Algorithm

The region implements the regionType PIMPLE interface (usesPIMPLE() = true), so the outer PIMPLE loop is driven by multiRegionSystem. Per time step:

correct() — reset the outer-iteration counter; if correctPhi is active, snapshot $\nabla\cdot(\rho\mathbf{U})$ for flux correction; if LTS is active, recompute the local time-step field rDeltaT (see below).
Pre-predictor — on the first outer iteration of the step (or every iteration with moveMeshOuterCorrectors yes): mesh.controlledUpdate(); if the mesh changed, update MRF, rebuild the flux from rhoUf, apply CorrectPhi, make the flux relative and correct rhoUf; optionally print the mesh Courant number.
Momentum predictor —
- on the first outer iteration and unless SIMPLErho is set, solve the density transport equation;
- assemble the momentum matrix (cached for the pressure corrector), relax, and solve it with $-\nabla p$ if momentumPredictor yes; update $K$;
- assemble and solve the energy equation, then thermo.correct().
Pressure corrector (PISO loop, nCorrectors) — for each corrector: update $\rho$ from thermo (unless SIMPLErho), build $\mathbf{H}/A$ and $\phi_{HbyA}$ (with ddtCorr, MRF and mesh-motion corrections, optional consistent SIMPLEC treatment), constrain pressure BCs, and solve the compressible pressure equation inside the non-orthogonal loop:

$$ \frac{\partial \rho}{\partial t} + \psi\,\frac{\partial p'}{\partial t} + \nabla\cdot\phi_{HbyA} - \nabla\cdot\left(\rho\, r_{AU}\,\nabla p\right) = S_p $$

With transonic yes the flux is split into a convective part $\phi_d = (\psi_f/\rho_f)\,\phi_{HbyA}$ treated implicitly ($\nabla\cdot(\phi_d\,p)$) and the pressure equation is relaxed for diagonal dominance. Afterwards: explicit pressure relaxation, velocity correction $\mathbf{U} = \mathbf{H}/A - r_{AU}\nabla p$, pressure limiting (pressureControl), thermo.correctRho with rhoMin/rhoMax, a second density solve, continuity-error report, $\rho$ reset to thermo, rhoUf correction and $\partial p/\partial t$ update. 5. Turbulence correction — turbulence->correct() if pimple.turbCorr() (see turbOnFinalIterOnly), then update of sigma.

Steps 2–5 are repeated for nOuterCorrectors outer iterations; step 4 for nCorrectors inner iterations.

Mesh motion corrector (meshMotionCorrector(), called by multiRegionSystem::preSolve and in the FSI coupling loop) performs controlledUpdate, MRF update, flux reconstruction from rhoUf + CorrectPhi, and rhoUf correction.

Time-step control

Global time stepping — getMinDeltaT() returns $\Delta t_\text{max} = \text{maxCo}/\text{Co}\;\Delta t$, where the Courant number is evaluated from the mass flux, $\text{Co} = \tfrac{1}{2}\max\left(\sum_f|\phi|/(\rho V)\right)\Delta t$. maxCo is read from controlDict (default 1.0).
Local time stepping (LTS) — enabled automatically when fvSchemes selects ddtSchemes { default localEuler; }. getMinDeltaT() then returns GREAT (the global step is left untouched) and rDeltaT is computed per cell from the Courant number (plus an acoustic estimate with transonic), then smoothed and damped, as in stock rhoPimpleFoam.

Sub-Models

Sub-model	Selection mechanism	Notes
Thermophysical model	`constant/thermophysicalProperties`	`fluidThermo::New`; `hePsiThermo` or `heRhoThermo`; energy must be `h` or `e` variant
Turbulence (laminar / RANS / LES)	`constant/turbulenceProperties`	`compressible::turbulenceModel`
Moving Reference Frame (MRF)	`constant/MRFProperties`	`IOMRFZoneList`
`fvOptions`	`system/fvOptions` (or `constant/fvOptions`)	Sources/constraints on $\rho$, $\mathbf{U}$, $h$/$e$, $p$ (e.g. `limitTemperature`)
Dynamic mesh	`constant/dynamicMeshDict`	Any `dynamicFvMesh`; enables `rhoUf` and `correctPhi`

Required Fields

Field	Type	Description	Unit
`p`	`volScalarField`	Pressure (read by thermo)	Pa
`T`	`volScalarField`	Temperature (read by thermo)	K
`U`	`volVectorField`	Velocity	m/s
Turbulence fields	—	As required by selected model (e.g. `k`, `omega`, `nut`, `alphat`)	—

Additionally created at runtime:

Field	Type	Description	Condition
`rho`	`volScalarField`	Density (read if present, else from thermo)	always
`phi`	`surfaceScalarField`	Mass flux $\rho\mathbf{U}\cdot\mathbf{S}_f$ (read if present)	always
`K`	`volScalarField`	Kinetic energy $\tfrac12	\mathbf{U}
`dpdt`	`volScalarField`	$\partial p/\partial t$	always (zero if `dpdt no`; written only on dynamic meshes)
`kappa`	`volScalarField`	Effective thermal conductivity `kappaEff`	always (heat-transfer coupling)
`sigma`	`volSymmTensorField`	Cauchy stress tensor	always (FSI)
`rhoUf`	`surfaceVectorField`	Face momentum	dynamic mesh only
`rDeltaT`	`volScalarField`	Reciprocal local time step	LTS only
`uniform/cumulativeContErr`	`uniformDimensionedScalarField`	Cumulative continuity error	always

Case Setup

Required dictionaries

constant/thermophysicalProperties – thermo type, mixture properties
constant/turbulenceProperties – turbulence model selection
system/fvSolution – PIMPLE sub-dict and linear solver settings
system/fvSchemes – discretisation schemes (localEuler → LTS)

`multiRegionProperties` entry

regions
(
 ( gas (rhoPimpleFluid) )
);

`controlDict` (singleRegionMode)

application multiPhysicsFoam;
singleRegionMode yes;
regionType rhoPimpleFluid;

`thermophysicalProperties` (from `aerofoilNACA0012`)

thermoType
{
 type hePsiThermo;
 mixture pureMixture;
 transport const;
 thermo hConst;
 equationOfState perfectGas;
 specie specie;
 energy sensibleInternalEnergy; // or sensibleEnthalpy
}

mixture
{
 specie { molWeight 28.9; }
 thermodynamics { Cp 1005; Hf 0; }
 transport { mu 1.82e-05; Pr 0.71; }
}

Key `fvSolution` settings

PIMPLE
{
 momentumPredictor yes;
 nOuterCorrectors 1;
 nCorrectors 2;
 nNonOrthogonalCorrectors 1;

 transonic no; // implicit convective pressure term
 consistent no; // SIMPLEC-like correction
 SIMPLErho no; // skip rho transport, take rho from thermo
 turbOnFinalIterOnly true;

 // Pressure limits (pressureControl): pMin/pMax or pMinFactor/pMaxFactor
 pMinFactor 0.1;
 pMaxFactor 2;

 // Density bounds for thermo.correctRho
 rhoMin 0; // default 0
 rhoMax 1e5; // default GREAT

 // Moving mesh
 correctPhi yes; // defaults to yes if mesh is dynamic
 checkMeshCourantNo no;
 moveMeshOuterCorrectors no;

 // LTS only (ddtSchemes default localEuler)
 maxCo 0.5; // default 0.8
 rDeltaTSmoothingCoeff 0.1; // default 0.02
 rDeltaTDampingCoeff 0.9; // default 1.0 (no damping)
 maxDeltaT 1; // default GREAT
}

Adjustable time stepping (`controlDict`)

adjustTimeStep yes;
maxCo 0.5; // default 1.0
maxDeltaT 1e-4;

Coupling

Interface type	Exchanged fields	Coupling modes
`heatTransferInterface`	Temperature `T`, heat flux via `kappa`	partitioned (DNA)
`fsiInterface`	Displacement `D`, traction from `sigma`	partitioned (DNA)
`defaultInterface`	Any scalar (generic `regionCoupledScalarJump`/`Flux` BCs)	partitioned (DNA)

For partitioned heat transfer, setCoupledEqns assembles a separate temperature equation (independent of the fieldName argument):

$$ \frac{\partial \left(\rho c_{pv} T\right)}{\partial t} + \nabla\cdot\left(c_{pv,f}\,\phi\,T\right) = \nabla\cdot\left(\kappa_\text{eff}\nabla T\right) $$

with $c_{pv} = $ thermo.Cpv() and kappa refreshed from turbulence->kappaEff() on each call. The matrix is registered as T<region>MeshrhoPimpleFluidTypeEqn. The regionCoupledTemperatureJump / regionCoupledHeatFlux BCs read the diffusivity field kappa by default. selfCoupledFieldNames() is not overridden (empty list).

Known Limitations

Coupled temperature equation is decoupled from the energy equation — the DNA T equation in setCoupledEqns contains no pressure-work, kinetic-energy, MRF or fvOptions terms, and postSolve() is a no-op, so thermo.correct() is not called after the coupled T solve and he is not updated from the new T.
Heat-transfer and FSI coupling are untested — no multi-region tutorial uses rhoPimpleFluid; only single-region cases exist.
Monolithic coupling not implemented — setCoupledEqns only provides the partitioned T matrix; monolithic coupling is disabled in multiRegionSystem.
solveRegion() and postSolve() are no-ops — all work happens inside the PIMPLE hooks.
maxDeltaT not applied in getMinDeltaT() — maxDeltaT from controlDict is read but the returned value is only Courant-based.
Mesh motion corrector does not make the flux relative — unlike prePredictor, meshMotionCorrector() does not call fvc::makeRelative after CorrectPhi.
Single phase, single species — reacting or multi-species mixtures and buoyancy (gravity, p_rgh) are not handled; use buoyantPimpleFluid for buoyancy-driven flows.

Tutorials

Tutorial path	Description
`tutorials/singleRegion/rhoPimpleFluid/aerofoilNACA0012`	Compressible RANS (kOmegaSST) flow around a NACA0012 aerofoil, internal energy, `limitTemperature` fvOption
`tutorials/singleRegion/rhoPimpleFluid/obliqueShock`	Laminar supersonic oblique shock with `transonic` formulation and LTS (`localEuler`)

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

multiPhysicsFoam – Compressible