[Table of Contents][Index][Version 4 | Version 3]

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
Large time-step transient solver for incompressible, turbulent flow, using the PIMPLE (merged PISO-SIMPLE) algorithm.
pimpleDyMFoam
Transient solver for incompressible, turbulent flow of Newtonian fluids on a moving mesh.
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.
rhoCentralDyMFoam
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.
rhoPimpleDyMFoam
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.
sonicFoam
Transient solver for trans-sonic/supersonic, turbulent flow of a compressible gas.
sonicDyMFoam
Transient solver for trans-sonic/supersonic, turbulent flow of a compressible gas, with optional mesh motion and mesh topology changes.
sonicLiquidFoam
Transient solver for trans-sonic/supersonic, laminar flow of a compressible liquid.


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.
cavitatingDyMFoam
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.
compressibleInterDyMFoam
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.
compressibleMultiphaseInterFoam
Solver for n 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.
interDyMFoam
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.
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.
interPhaseChangeDyMFoam
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 many compressible fluid phases including heat-transfer.
multiphaseInterFoam
Solver for n incompressible fluids which captures the interfaces and includes surface-tension and contact-angle effects for each phase.
multiphaseInterDyMFoam
Solver for n 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
potentialFreeSurfaceDyMFoam
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.
reactingMultiphaseEulerFoam
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.
reactingTwoPhaseEulerFoam
Solver for a system of 2 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.
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
Solver for internal combustion engines.
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.
XiFoam
Solver for compressible premixed/partially-premixed combustion with turbulence modelling.


3.5.7 Heat transfer and buoyancy-driven flows

buoyantBoussinesqPimpleFoam
Transient solver for buoyant, turbulent flow of incompressible fluids.
buoyantBoussinesqSimpleFoam
Steady-state solver for buoyant, turbulent flow of incompressible fluids.
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
Transient solver for buoyant, turbulent fluid flow and solid heat conduction with conjugate heat transfer between solid and fluid regions.
chtMultiRegionSimpleFoam
Steady-state solver for buoyant, turbulent fluid flow and solid heat conduction with conjugate heat transfer between solid and fluid regions.
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.
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.
icoUncoupledKinematicParcelFoam
Transient solver for the passive transport of a single kinematic particle cloud.
icoUncoupledKinematicParcelDyMFoam
Transient solver for the passive transport of a single kinematic particle cloud, with optional mesh motion and mesh topology changes.
reactingParcelFilmFoam
Transient solver for compressible, turbulent flow with a reacting, multiphase particle cloud, and surface film modelling.
reactingParcelFoam
Transient solver for compressible, turbulent flow with a reacting, multiphase particle cloud, and optional sources/constraints.
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.
sprayDyMFoam
Transient solver for compressible, turbulent flow with a spray particle cloud, with optional mesh motion and mesh topology changes.
sprayEngineFoam
Transient solver for compressible, turbulent engine flow with a spray particle cloud.
uncoupledKinematicParcelFoam
Transient solver for the passive transport of a particle cloud.


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.

© 2011-2016 OpenFOAM Foundation
CC-NC-ND 3.0