# SimFlow CFD Solvers Source: https://help.sim-flow.com/solvers Last updated: 2026-10-14 ## What is a solver A solver is the part of SimFlow that does the actual calculation. It takes your mesh, material properties and boundary conditions, and computes how the flow behaves: velocity, pressure, temperature and other results. ## Why there are many solvers Different physical problems need different equations. Air flowing slowly around a building, a supersonic jet, water filling a tank and fuel burning in an engine are all described in different ways from a calculation point of view. That is why there is no single solver that fits every case. Each solver is built for one type of problem. ## How you choose a solver in SimFlow In SimFlow you usually do not pick an OpenFOAM solver by name. You define a [Simulation Type](https://help.sim-flow.com/documentation/panels/setup) that matches your problem. That choice selects one solver for the case. The groups below follow the same idea as the Simulation Types: incompressible flow, compressible flow, heat transfer, multiphase flow, and species and reactions. Some solvers could fit more than one group. In that case the docs list the solver under its main feature, so a compressible solver for heat transfer is in the Heat Transfer group. ## Steady-state and transient Most groups have both steady-state and transient solvers. A steady-state solver looks for the final, settled flow, for example air in a ventilation duct that does not change over time. A transient solver follows how the flow changes in time, for example a breaking wave. ## How solvers are named Solver names usually tell you what the solver does. Some are named after the algorithm they use, like simpleFoam (SIMPLE algorithm) or pimpleFoam (PIMPLE algorithm). Others are named after the physics, like cavitatingFoam or twoLiquidMixingFoam. You mainly need these names when you look at the lists below or at OpenFOAM materials. Below you will find a comparison of the solvers in each group. ## Incompressible Solvers Incompressible Solvers In this group, we have included single-phase, pressure-based solvers for **low-speed flows** with negligible variations in density, applicable for **external** and **internal aerodynamics** (**Ma < 0.3**) and **hydrodynamics**. These solvers use incompressibility features for stability and robustness. **Incompressible, Steady-State - Main Solvers** - [simpleFoam](https://help.sim-flow.com/solvers/simple-foam) steady-state, SIMPLE algorithm - [overSimpleFoam](https://help.sim-flow.com/solvers/over-simple-foam) extension of simpleFoam with Overset - [SRFSimpleFoam](https://help.sim-flow.com/solvers/srf-simple-foam) variant of simpleFoam resolved in SRF **Incompressible, Transient - Main Solvers** - [pimpleFoam](https://help.sim-flow.com/solvers/pimple-foam) transient, PIMPLE algorithm, DyM - [overPimpleDyMFoam](https://help.sim-flow.com/solvers/over-pimple-dym-foam) extension of pimpleFoam with Overset, DyM - [SRFPimpleFoam](https://help.sim-flow.com/solvers/srf-pimple-foam) variant of pimpleFoam resolved in SRF **Incompressible, Transient - Simplified Solvers*** - [pisoFoam](https://help.sim-flow.com/solvers/piso-foam) transient, PISO** algorithm - [icoFoam](https://help.sim-flow.com/solvers/ico-foam) transient, PISO** algorithm, laminar flows only (no turbulence), Newtonian fluids only - * Dedicated solvers for simplified scenarios, improve stability and computational efficiency - ** The PISO algorithm is used for cases with a small Courant number Co < 1 - DyM - Dynamic Mesh - MRF - Multiple Reference Frame - SRF - Single Reference Frame - Overset - also known as Chimera Grid (Method) - SIMPLE - Semi-Implicit Method for Pressure-Linked Equations - PIMPLE - merged PISO and SIMPLE - PISO - Pressure-Implicit Split-Operator ## Compressible Solvers Compressible Solvers In this group, we have included single-phase, pressure and density-based solvers that can handle flows with significant variations in density, mostly applicable for **high-speed aerodynamics** (**Ma > 0.3**). **Subsonic / Transonic, Steady-State, Ma < 1** - [rhoSimpleFoam](https://help.sim-flow.com/solvers/rho-simple-foam) steady-state, pressure-based, small density changes - [overRhoSimpleFoam](https://help.sim-flow.com/solvers/over-rho-simple-foam) extension of rhoSimpleFoam with Overset **Subsonic / Transonic, Transient, Ma < 1** - [rhoPimpleFoam](https://help.sim-flow.com/solvers/pimple-foam) transient, pressure-based, small density changes, DyM - [overRhoPimpleDyMFoam](https://help.sim-flow.com/solvers/over-rho-pimple-dym-foam) extension of rhoPimpleFoam with Overset, DyM **Transonic / Supersonic, Pressure-Based, Ma > 1** - [sonicFoam](https://help.sim-flow.com/solvers/sonic-foam) transient, pressure-based, shock waves - [sonicDyMFoam](https://help.sim-flow.com/solvers/sonic-dym-foam) extension of sonicFoam with DyM **Transonic / Supersonic, Density-Based, Ma > 1** - [rhoCentralFoam](https://help.sim-flow.com/solvers/rho-central-foam) transient, density-based, shock waves - [rhoCentralDyMFoam](https://help.sim-flow.com/solvers/rho-central-dym-foam) extension of rhoCentralFoam with DyM - Ma - Mach Number - DyM - Dynamic Mesh - Overset - also known as Chimera Grid (Method) ## Heat Transfer Solvers Heat Transfer Solvers In this group, we have included solvers that are designed to model: **Heat Transfer**, **Radiation**, **Natural** and **Forced Convection**, **Conjugate Heat Transfer (CHT)**. **Heat Transfer, Single Fluid** - [buoyantSimpleFoam](https://help.sim-flow.com/solvers/buoyant-simple-foam) steady-state, compressible, buoyancy-driven flow - [buoyantPimpleFoam](https://help.sim-flow.com/solvers/buoyant-pimple-foam) transient, compressible, buoyancy-driven flow **Heat Transfer, Single Fluid - Boussinesq** - [buoyantBoussinesqSimpleFoam](https://help.sim-flow.com/solvers/buoyant-boussinesq-simple-foam) steady-state, incompressible, buoyancy using Boussinesq approximation - [buoyantBoussinesqPimpleFoam](https://help.sim-flow.com/solvers/buoyant-boussinesq-pimple-foam) transient, incompressible, buoyancy using Boussinesq approximation **Heat Transfer, Single Solid** - [laplacianFoam](https://help.sim-flow.com/solvers/laplacian-foam) steady-state and transient, thermal conduction in solid - [overLaplacianDyMFoam](https://help.sim-flow.com/solvers/over-laplacian-dym-foam) extension of laplacianFoam with Overset **CHT, Multiple Fluids / Solids** - [chtMultiRegionSimpleFoam](https://help.sim-flow.com/solvers/cht-multi-region-simple-foam) steady-state, compressible, arbitrary fluid and solid regions - [chtMultiRegionFoam](https://help.sim-flow.com/solvers/cht-multi-region-foam) transient, compressible, arbitrary fluid and solid regions - CHT - Conjugate Heat Transfer - MRF - Multiple Reference Frame - Overset - also known as Chimera Grid (Method) ## Multiphase - Free Surface (VoF) Solvers Free Surface (VoF) Solvers In this group, we have included solvers implementing the **Volume of Fluid (VoF)** approach to handle multiple immiscible and miscible fluids and interactions between them. **Free Surface (VoF) - Immiscible** - [interFoam](https://help.sim-flow.com/solvers/inter-foam) 2 immiscible fluids, DyM - [multiphaseInterFoam](https://help.sim-flow.com/solvers/multiphase-inter-foam) multiple immiscible fluids, DyM - [interIsoFoam*](https://help.sim-flow.com/solvers/inter-iso-foam) 2 immiscible fluids, isoAdvector* method, DyM - [overInterDyMFoam](https://help.sim-flow.com/solvers/over-inter-dym-foam) extension of interFoam with Overset, DyM - [compressibleInterFoam](https://help.sim-flow.com/solvers/compressible-inter-foam) compressible version of interFoam with heat transfer - [compressibleInterDyMFoam](https://help.sim-flow.com/solvers/compressible-inter-dym-foam) compressible version of interFoam with heat transfer and DyM **Free Surface (VoF) - Miscible** - [interMixingFoam](https://help.sim-flow.com/solvers/inter-mixing-foam) 3 fluids (2 miscible and 1 immiscible), DyM - [twoLiquidMixingFoam**](https://help.sim-flow.com/solvers/two-liquid-mixing-foam) 2 miscible fluids - * isoAdvector - an alternative approach for interface capturing, MULES method used in other VoF solvers - ** Solver designed to handle mixtures consisting of multiple fluids within the same phase, such as two gases or two liquids - VoF - Volume of Fluid - DyM - Dynamic Mesh - Overset - also known as Chimera Grid (Method) ## Multiphase - Phase Change Solvers Phase Change Solvers In this group, we have included solvers implementing **Phase Change** models to handle cavitation and surface evaporation/condensation (liquid and its vapor phases). **Phase Change - Cavitation** - [cavitatingFoam](https://help.sim-flow.com/solvers/cavitating-foam) 2 immiscible fluids, dedicated to cavitation, Homogeneous Equilibrium Model (HEM) - [interPhaseChangeFoam](https://help.sim-flow.com/solvers/inter-phase-change-foam) 2 immiscible fluids, dedicated to cavitation, VoF, Phase Change Models: Schnerr-Sauer, Merkle, Kunz - [cavitatingDyMFoam](https://help.sim-flow.com/solvers/cavitating-dym-foam) extension of cavitatingFoam with DyM - [interPhaseChangeDyMFoam](https://help.sim-flow.com/solvers/inter-phase-change-dym-foam) extension of interPhaseChangeFoam with DyM - [overInterPhaseChangeDyMFoam](https://help.sim-flow.com/solvers/over-inter-phase-change-dym-foam) extension of interPhaseChangeFoam with Overset, DyM **Phase Change - Condensation / Evaporation** - [interCondensatingEvaporatingFoam](https://help.sim-flow.com/solvers/inter-condensating-evaporating-foam) 2 immiscible fluids, phase changes (evaporation and condensation) between a fluid and its vapor phase - VoF - Volume of Fluid - DyM - Dynamic Mesh - Overset - also known as Chimera Grid (Method) ## Multiphase - Dispersed Solvers Dispersed Solvers In this group, we have included solvers implementing the **Eulerian** or **Lagrangian** approach to handle multiple fluids and particle clouds considering **Dispersed Phases** or **Fluid-Particle interactions**. **Dispersed - Euler** - [multiphaseEulerFoam](https://help.sim-flow.com/solvers/multiphase-euler-foam) multiple miscible fluids, Euler-Euler approach **Dispersed - Lagrangian** - [DPMFoam](https://help.sim-flow.com/solvers/dpm-foam) 1 fluid and particles, particle-particle interactions resolved explicitly (direct approach) - [MPPICFoam](https://help.sim-flow.com/solvers/mppic-foam) 1 fluid and particles, dense particle cloud using particle-particle interactions model (simplified approach, MP-PIC method) - [MPPICInterFoam](https://help.sim-flow.com/solvers/mppic-inter-foam) 2 immiscible fluids and particles, dense particle cloud using particle-particle interactions model (simplified approach, MP-PIC method) - [DPMDyMFoam](https://help.sim-flow.com/solvers/dpm-dym-foam) extension of DPMFoam with DyM - [MPPICDyMFoam](https://help.sim-flow.com/solvers/mppic-dym-foam) extension of MPPICFoam with DyM **Dispersed - Drift-Flux** - [driftFluxFoam](https://help.sim-flow.com/solvers/drift-flux-foam) 1 fluid and slurry or plastic dispersed phase, drift flux approximation for relative phase motion - DPM - Discrete Phase Model - MP-PIC - multiphase particle-in-cell method - DyM - Dynamic Mesh ## Species & Reactions Solvers Species & Reactions Solvers In this group, we have included compressible (pressure-based) solvers that can be used to simulate: **Species Transport**, **Multicomponent Gas Mixtures**, **Chemical Reactions**, **Combustion**. **Multicomponent** - [simpleReactingParcelFoam](https://help.sim-flow.com/solvers/simple-reacting-parcel-foam) steady-state, multiphase particle clouds - [reactingParcelFoam](https://help.sim-flow.com/solvers/simple-reacting-parcel-foam) transient, multiphase particle clouds **Spray** - [sprayFoam](https://help.sim-flow.com/solvers/spray-foam) transient, liquid particles only, dedicated to fuel spray combustion - [sprayDyMFoam](https://help.sim-flow.com/solvers/spray-dym-foam) extension of sprayFoam with DyM **Coal** - [simpleCoalParcelFoam](https://help.sim-flow.com/solvers/simple-coal-parcel-foam) steady-state, coal particles only - [coalChemistryFoam](https://help.sim-flow.com/solvers/coal-chemistry-foam) transient, coal particles only **Gas*** - [reactingFoam](https://help.sim-flow.com/solvers/reacting-foam) fluids with minor density fluctuations (caused by pressure variance), no buoyancy - [rhoReactingFoam](https://help.sim-flow.com/solvers/rho-reacting-foam) fluids with density variations due to reactions, no buoyancy - [rhoReactingBuoyantFoam](https://help.sim-flow.com/solvers/rho-reacting-buoyant-foam) extension of rhoReactingFoam with buoyancy forces - * All solvers in this group are transient - DyM - Dynamic Mesh