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 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 steady-state, SIMPLE algorithm
- overSimpleFoam extension of simpleFoam with Overset
- SRFSimpleFoam variant of simpleFoam resolved in SRF
Incompressible, Transient - Main Solvers
- pimpleFoam transient, PIMPLE algorithm, DyM
- overPimpleDyMFoam extension of pimpleFoam with Overset, DyM
- SRFPimpleFoam variant of pimpleFoam resolved in SRF
Incompressible, Transient - Simplified Solvers*
- * 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 steady-state, pressure-based, small density changes
- overRhoSimpleFoam extension of rhoSimpleFoam with Overset
Subsonic / Transonic, Transient, Ma < 1
- rhoPimpleFoam transient, pressure-based, small density changes, DyM
- overRhoPimpleDyMFoam extension of rhoPimpleFoam with Overset, DyM
Transonic / Supersonic, Pressure-Based, Ma > 1
- sonicFoam transient, pressure-based, shock waves
- sonicDyMFoam extension of sonicFoam with DyM
Transonic / Supersonic, Density-Based, Ma > 1
- rhoCentralFoam transient, density-based, shock waves
- rhoCentralDyMFoam 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 steady-state, compressible, buoyancy-driven flow
- buoyantPimpleFoam transient, compressible, buoyancy-driven flow
Heat Transfer, Single Fluid - Boussinesq
- buoyantBoussinesqSimpleFoam steady-state, incompressible, buoyancy using Boussinesq approximation
- buoyantBoussinesqPimpleFoam transient, incompressible, buoyancy using Boussinesq approximation
Heat Transfer, Single Solid
- laplacianFoam steady-state and transient, thermal conduction in solid
- overLaplacianDyMFoam extension of laplacianFoam with Overset
CHT, Multiple Fluids / Solids
- chtMultiRegionSimpleFoam steady-state, compressible, arbitrary fluid and solid regions
- chtMultiRegionFoam 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 2 immiscible fluids, DyM
- multiphaseInterFoam multiple immiscible fluids, DyM
- interIsoFoam* 2 immiscible fluids, isoAdvector* method, DyM
- overInterDyMFoam extension of interFoam with Overset, DyM
- compressibleInterFoam compressible version of interFoam with heat transfer
- compressibleInterDyMFoam compressible version of interFoam with heat transfer and DyM
Free Surface (VoF) - Miscible
- interMixingFoam 3 fluids (2 miscible and 1 immiscible), DyM
- twoLiquidMixingFoam** 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 2 immiscible fluids, dedicated to cavitation, Homogeneous Equilibrium Model (HEM)
- interPhaseChangeFoam 2 immiscible fluids, dedicated to cavitation, VoF, Phase Change Models: Schnerr-Sauer, Merkle, Kunz
- cavitatingDyMFoam extension of cavitatingFoam with DyM
- interPhaseChangeDyMFoam extension of interPhaseChangeFoam with DyM
- overInterPhaseChangeDyMFoam extension of interPhaseChangeFoam with Overset, DyM
Phase Change - Condensation / Evaporation
- interCondensatingEvaporatingFoam 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 multiple miscible fluids, Euler-Euler approach
Dispersed - Lagrangian
- DPMFoam 1 fluid and particles, particle-particle interactions resolved explicitly (direct approach)
- MPPICFoam 1 fluid and particles, dense particle cloud using particle-particle interactions model (simplified approach, MP-PIC method)
- MPPICInterFoam 2 immiscible fluids and particles, dense particle cloud using particle-particle interactions model (simplified approach, MP-PIC method)
- DPMDyMFoam extension of DPMFoam with DyM
- MPPICDyMFoam extension of MPPICFoam with DyM
Dispersed - Drift-Flux
- driftFluxFoam 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 steady-state, multiphase particle clouds
- reactingParcelFoam transient, multiphase particle clouds
Spray
- sprayFoam transient, liquid particles only, dedicated to fuel spray combustion
- sprayDyMFoam extension of sprayFoam with DyM
Coal
- simpleCoalParcelFoam steady-state, coal particles only
- coalChemistryFoam transient, coal particles only
Gas*
- reactingFoam fluids with minor density fluctuations (caused by pressure variance), no buoyancy
- rhoReactingFoam fluids with density variations due to reactions, no buoyancy
- rhoReactingBuoyantFoam extension of rhoReactingFoam with buoyancy forces
- * All solvers in this group are transient
- DyM - Dynamic Mesh