OpenFOAM v9 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

adjointShapeOptimisationFoam: 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.
pisoFoam: Transient solver for incompressible, turbulent ﬂow, using the PISO algorithm.
porousSimpleFoam: Steady-state solver for incompressible, turbulent ﬂow with implicit or explicit porosity treatment and support for multiple reference frames (MRF).
shallowWaterFoam: Transient solver for inviscid shallow-water equations with rotation.
simpleFoam: Steady-state solver for incompressible, turbulent ﬂow, using the SIMPLE algorithm.
SRFPimpleFoam: Large time-step transient solver for incompressible, turbulent ﬂow in a single rotating frame.
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.
rhoPorousSimpleFoam: Steady-state solver for turbulent ﬂow of compressible ﬂuids, with implicit or explicit porosity treatment and optional sources.
rhoSimpleFoam: Steady-state solver for turbulent ﬂow of compressible ﬂuids.

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.
compressibleMultiphaseInterFoam: Solver for $\text{[math]}$ 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.
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 $\text{[math]}$ 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.

3.5.5 Direct numerical simulation (DNS)

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

3.5.6 Combustion

buoyantReactingFoam: Solver for combustion with chemical reactions using a density based thermodynamics package with enhanced buoyancy treatment.
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.
PDRFoam: Solver for compressible premixed/partially-premixed combustion with turbulence modelling.
reactingFoam: Solver for combustion with chemical reactions.
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

denseParticleFoam: Transient solver for the coupled transport of particle clouds including the eﬀect of the volume fraction of particles on the continuous phase, 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.
rhoParticleFoam: 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.

OpenFOAM v9 User Guide - 3.5 Standard solvers