OpenFOAM v8 User Guide

[version 12][version 11][version 10][version 9][version 8][version 7][version 6]

[chapter contents][previous topic][next topic][index]

3.5 Standard solvers

The solvers with the OpenFOAM distribution are in the $FOAM_SOLVERS directory, reached quickly by typing sol at the command line. This directory is further subdivided into several directories by category of continuum mechanics, e.g. incompressible flow, combustion and solid body stress analysis. Each solver is given a name that is reasonably descriptive, e.g.icoFoam solves incompressible, laminar flow. The current list of solvers distributed with OpenFOAM is given in the following Sections.

3.5.1 ‘Basic’ CFD codes

laplacianFoam: Solves a simple Laplace equation, e.g. for thermal diffusion in a solid.
potentialFoam: Potential flow solver which solves for the velocity potential, to calculate the flux-field, from which the velocity field is obtained by reconstructing the flux.
scalarTransportFoam: Solves the steady or transient transport equation for a passive scalar.

3.5.2 Incompressible flow

adjointShapeOptimizationFoam: Steady-state solver for incompressible, turbulent flow of non-Newtonian fluids with optimisation of duct shape by applying ”blockage” in regions causing pressure loss as estimated using an adjoint formulation.
boundaryFoam: Steady-state solver for incompressible, 1D turbulent flow, typically to generate boundary layer conditions at an inlet, for use in a simulation.
icoFoam: Transient solver for incompressible, laminar flow of Newtonian fluids.
nonNewtonianIcoFoam: Transient solver for incompressible, laminar flow of non-Newtonian fluids.
pimpleFoam: Transient solver for incompressible, turbulent flow of Newtonian fluids, with optional mesh motion and mesh topology changes.
SRFPimpleFoam: Large time-step transient solver for incompressible, turbulent flow in a single rotating frame.
pisoFoam: Transient solver for incompressible, turbulent flow, using the PISO algorithm.
shallowWaterFoam: Transient solver for inviscid shallow-water equations with rotation.
simpleFoam: Steady-state solver for incompressible, turbulent flow, using the SIMPLE algorithm.
porousSimpleFoam: Steady-state solver for incompressible, turbulent flow with implicit or explicit porosity treatment and support for multiple reference frames (MRF).
SRFSimpleFoam: Steady-state solver for incompressible, turbulent flow of non-Newtonian fluids in a single rotating frame.

3.5.3 Compressible flow

rhoCentralFoam: Density-based compressible flow solver based on central-upwind schemes of Kurganov and Tadmor with support for mesh-motion and topology changes.
rhoPimpleFoam: Transient solver for turbulent flow of compressible fluids for HVAC and similar applications, with optional mesh motion and mesh topology changes.
rhoSimpleFoam: Steady-state solver for turbulent flow of compressible fluids.
rhoPorousSimpleFoam: Steady-state solver for turbulent flow of compressible fluids, with implicit or explicit porosity treatment and optional sources.

3.5.4 Multiphase flow

cavitatingFoam: Transient cavitation code based on the homogeneous equilibrium model from which the compressibility of the liquid/vapour ”mixture” is obtained, with optional mesh motion and mesh topology changes.
compressibleInterFoam: Solver for 2 compressible, non-isothermal immiscible fluids using a VOF (volume of fluid) phase-fraction based interface capturing approach, with optional mesh motion and mesh topology changes including adaptive re-meshing.
compressibleInterFilmFoam: Solver for 2 compressible, non-isothermal immiscible fluids using a VOF (volume of fluid) phase-fraction based interface capturing approach and surface film modelling.
compressibleMultiphaseInterFoam: Solver for $n \relax \special {t4ht=$ compressible, non-isothermal immiscible fluids using a VOF (volume of fluid) phase-fraction based interface capturing approach.
driftFluxFoam: Solver for 2 incompressible fluids using the mixture approach with the drift-flux approximation for relative motion of the phases.
interFoam: Solver for 2 incompressible, isothermal immiscible fluids using a VOF (volume of fluid) phase-fraction based interface capturing approach, with optional mesh motion and mesh topology changes including adaptive re-meshing.
interMixingFoam: Solver for 3 incompressible fluids, two of which are miscible, using a VOF method to capture the interface, with optional mesh motion and mesh topology changes including adaptive re-meshing.
interPhaseChangeFoam: Solver for 2 incompressible, isothermal immiscible fluids with phase-change (e.g. cavitation). Uses a VOF (volume of fluid) phase-fraction based interface capturing approach, with optional mesh motion and mesh topology changes including adaptive re-meshing.
multiphaseEulerFoam: Solver for a system of any number of compressible fluid phases with a common pressure, but otherwise separate properties. The type of phase model is run time selectable and can optionally represent multiple species and in-phase reactions. The phase system is also run time selectable and can optionally represent different types of momentun, heat and mass transfer.
multiphaseInterFoam: Solver for $n \relax \special {t4ht=$ incompressible fluids which captures the interfaces and includes surface-tension and contact-angle effects for each phase, with optional mesh motion and mesh topology changes.
potentialFreeSurfaceFoam: Incompressible Navier-Stokes solver with inclusion of a wave height field to enable single-phase free-surface approximations, with optional mesh motion and mesh topology changes.
twoLiquidMixingFoam: Solver for mixing 2 incompressible fluids.
twoPhaseEulerFoam: Solver for a system of 2 compressible fluid phases with one phase dispersed, e.g. gas bubbles in a liquid including heat-transfer.

3.5.5 Direct numerical simulation (DNS)

dnsFoam: Direct numerical simulation solver for boxes of isotropic turbulence.

3.5.6 Combustion

chemFoam: Solver for chemistry problems, designed for use on single cell cases to provide comparison against other chemistry solvers, that uses a single cell mesh, and fields created from the initial conditions.
coldEngineFoam: Solver for cold-flow in internal combustion engines.
engineFoam: Transient solver for compressible, turbulent engine flow with a spray particle cloud.
fireFoam: Transient solver for fires and turbulent diffusion flames with reacting particle clouds, surface film and pyrolysis modelling.
PDRFoam: Solver for compressible premixed/partially-premixed combustion with turbulence modelling.
reactingFoam: Solver for combustion with chemical reactions.
rhoReactingBuoyantFoam: Solver for combustion with chemical reactions using a density based thermodynamics package with enhanced buoyancy treatment.
rhoReactingFoam: Solver for combustion with chemical reactions using density based thermodynamics package.
XiEngineFoam: Solver for internal combustion engines.
XiFoam: Solver for compressible premixed/partially-premixed combustion with turbulence modelling.

3.5.7 Heat transfer and buoyancy-driven flows

buoyantPimpleFoam: Transient solver for buoyant, turbulent flow of compressible fluids for ventilation and heat-transfer.
buoyantSimpleFoam: Steady-state solver for buoyant, turbulent flow of compressible fluids, including radiation, for ventilation and heat-transfer.
chtMultiRegionFoam: Solver for steady or transient fluid flow and solid heat conduction, with conjugate heat transfer between regions, buoyancy effects, turbulence, reactions and radiation modelling.
thermoFoam: Solver for energy transport and thermodynamics on a frozen flow field.

3.5.8 Particle-tracking flows

coalChemistryFoam: Transient solver for compressible, turbulent flow, with coal and limestone particle clouds, an energy source, and combustion.
DPMFoam: Transient solver for the coupled transport of a single kinematic particle cloud including the effect of the volume fraction of particles on the continuous phase, with optional mesh motion and mesh topology changes.
MPPICFoam: Transient solver for the coupled transport of a single kinematic particle cloud including the effect of the volume fraction of particles on the continuous phase. Multi-Phase Particle In Cell (MPPIC) modeling is used to represent collisions without resolving particle-particle interactions, with optional mesh motion and mesh topology changes.
particleFoam: Transient solver for the passive transport of a single kinematic particle cloud, with optional mesh motion and mesh topology changes.
reactingParcelFoam: Transient solver for compressible, turbulent flow with a reacting, multiphase particle cloud, and surface film modelling.
rhoParticleFoam: Transient solver for the passive transport of a particle cloud.
simpleReactingParcelFoam: Steady state solver for compressible, turbulent flow with reacting, multiphase particle clouds and optional sources/constraints.
sprayFoam: Transient solver for compressible, turbulent flow with a spray particle cloud, with optional mesh motion and mesh topology changes.

3.5.9 Discrete methods

dsmcFoam: Direct simulation Monte Carlo (DSMC) solver for, transient, multi-species flows.
mdEquilibrationFoam: Solver to equilibrate and/or precondition molecular dynamics systems.
mdFoam: Molecular dynamics solver for fluid dynamics.

3.5.10 Electromagnetics

electrostaticFoam: Solver for electrostatics.
magneticFoam: Solver for the magnetic field generated by permanent magnets.
mhdFoam: Solver for magnetohydrodynamics (MHD): incompressible, laminar flow of a conducting fluid under the influence of a magnetic field.

3.5.11 Stress analysis of solids

solidDisplacementFoam: Transient segregated finite-volume solver of linear-elastic, small-strain deformation of a solid body, with optional thermal diffusion and thermal stresses.
solidEquilibriumDisplacementFoam: Steady-state segregated finite-volume solver of linear-elastic, small-strain deformation of a solid body, with optional thermal diffusion and thermal stresses.

3.5.12 Finance

financialFoam: Solves the Black-Scholes equation to price commodities.

OpenFOAM v8 User Guide - 3.5 Standard solvers