[Table of Contents] [Index] [ **Version 9** | Version 8 | Version 7 | Version 6 | Version 5 | Version 4 ]

## 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 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 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)

### 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

© 2011-2021 OpenFOAM Foundation

OpenFOAM v9 User Guide: 3.5 Standard solvers