Setup Guide: Incompressible Flows

Draft. These settings are drawn from SU2 source, tutorials and regression cases. Recommendations marked (to be reviewed) still need an experienced user’s review.

Use this guide to choose settings and understand their consequences. Follow the linked Tutorials for worked examples and consult V&V for numerical and physical comparisons. Example settings are starting points, not evidence that a case is converged or validated.

The documentation guide explains the source tags used below: (code), (test case), (tutorial), (docs), (advice) and (to be reviewed).

When to use this guide

Use this guide for a flow where the density does not depend on the pressure. This covers liquids and low-speed gas flows, also with heat transfer, where density may depend on temperature and composition while remaining independent of the hydrodynamic pressure. As a rule of thumb, the Mach number is below about 0.3 (advice).

This guide covers the solvers INC_EULER, INC_NAVIER_STOKES and INC_RANS. For mixing gases and flames, continue with Setup Guide: Species Transport and Combustion. For coupled heat transfer between fluid and solid, continue with Setup Guide: Heat Transfer and Conjugate Heat Transfer.

Every option is listed in the option reference. Every output field is listed in the output fields reference.

Start from

This config is a laminar flow through a pipe bend. It has a velocity inlet, a pressure outlet, adiabatic walls and a symmetry plane. It is the test case incomp_navierstokes/bend/lam_bend.cfg with fewer options. Changes to the test case: ITER is raised from 11 to 2000, and MARKER_ANALYZE and HISTORY_OUTPUT are added to check the mass flow. The mesh mesh_bend_coarse.cgns is in the folder incomp_navierstokes/bend of the TestCases repository.

% ------------- Problem -------------%
SOLVER= INC_NAVIER_STOKES
KIND_TURB_MODEL= NONE
MATH_PROBLEM= DIRECT
RESTART_SOL= NO
%
% ------------- Fluid and initial state -------------%
INC_DENSITY_MODEL= CONSTANT
INC_ENERGY_EQUATION= NO
INC_DENSITY_INIT= 1.2886
INC_VELOCITY_INIT= ( 0.1, 0.0, 0.0 )
INC_TEMPERATURE_INIT= 288.15
INC_NONDIM= INITIAL_VALUES
VISCOSITY_MODEL= CONSTANT_VISCOSITY
MU_CONSTANT= 1.716E-5
%
% ------------- Boundary conditions -------------%
INC_INLET_TYPE= VELOCITY_INLET
MARKER_INLET= ( INLET, 288.15, 0.1, 1.0, 0.0, 0.0 )
INC_OUTLET_TYPE= PRESSURE_OUTLET
MARKER_OUTLET= ( OUTLET, 0.0 )
MARKER_HEATFLUX= ( WALL1, 0.0, WALL2, 0.0 )
MARKER_SYM= ( SYMMETRY )
MARKER_MONITORING= ( WALL1, WALL2 )
MARKER_ANALYZE= ( INLET, OUTLET )
%
% ------------- Numerics -------------%
NUM_METHOD_GRAD= GREEN_GAUSS
CONV_NUM_METHOD_FLOW= FDS
MUSCL_FLOW= YES
SLOPE_LIMITER_FLOW= NONE
TIME_DISCRE_FLOW= EULER_IMPLICIT
CFL_NUMBER= 1e2
LINEAR_SOLVER= FGMRES
LINEAR_SOLVER_PREC= ILU
LINEAR_SOLVER_ERROR= 1E-15
LINEAR_SOLVER_ITER= 5
%
% ------------- Convergence and output -------------%
ITER= 2000
CONV_FIELD= RMS_PRESSURE
CONV_RESIDUAL_MINVAL= -8
CONV_STARTITER= 10
MESH_FILENAME= mesh_bend_coarse.cgns
MESH_FORMAT= CGNS
SCREEN_OUTPUT= (INNER_ITER, RMS_PRESSURE, RMS_VELOCITY-X, SURFACE_MASSFLOW)
HISTORY_OUTPUT= (ITER, RMS_RES, FLOW_COEFF, FLOW_COEFF_SURF)

Settings that matter

Solver

Choose the solver with SOLVER:

  • INC_EULER: no viscosity. Use it for quick checks of pressure fields, for example on a hydrofoil. SU2 stops if you combine it with a density model other than CONSTANT, or with INC_ENERGY_EQUATION= YES (code).
  • INC_NAVIER_STOKES: laminar flow.
  • INC_RANS: turbulent flow. Choose the turbulence model with KIND_TURB_MODEL (SA or SST).

For INC_RANS with SST, the free-stream turbulence comes from FREESTREAM_TURBULENCEINTENSITY (default 0.05, a fraction) and FREESTREAM_TURB2LAMVISCRATIO (default 10, the eddy-to-laminar viscosity ratio). With SA, FREESTREAM_NU_FACTOR (default 3.0) sets nu-tilde divided by the kinematic viscosity (code). Inlets use these settings unless overridden with MARKER_INLET_TURBULENT: two values per marker for SST (intensity, viscosity ratio), or one for SA (nu-tilde divided by the local kinematic viscosity). The SA factor is not the eddy-to-laminar viscosity ratio. With SA_OPTIONS= BCM, SU2 also multiplies nu-tilde by 0.005 (code). See Turbulence Models.

Density-based or pressure-based solver

KIND_INCOMP_SYSTEM selects how SU2 couples pressure and velocity (code):

  • DENSITY_BASED (default): SU2 adds a pseudo-time derivative of the pressure to the continuity equation. This is called artificial compressibility, a form of preconditioning. SU2 solves pressure and velocity together, with enthalpy in the coupled system when the energy equation is enabled; temperature is recovered from the fluid model. All tutorials on this page use it.
  • PRESSURE_BASED: a segregated method of the SIMPLE type, which solves the equations one after the other. Choose SIMPLE (default) or SIMPLEC with KIND_PB_ITER. It uses CONV_NUM_METHOD_FLOW= UDS (upwind) or CDS (centered).

With PRESSURE_BASED, SU2 stops if you use multigrid (MGLEVEL above 0), an adjoint, MARKER_PERIODIC, streamwise periodic flow, or TIME_MARCHING= TIME_STEPPING (code). If you need the pressure-based solver, start from the test case incomp_navierstokes/bend/pb_lam_bend.cfg. The rest of this page is about the density-based solver.

Density model and energy equation

INC_DENSITY_MODEL decides how the density can change. INC_ENERGY_EQUATION switches the temperature equation on or off. The table shows what the code does (code):

INC_DENSITY_MODEL Density Energy equation FLUID_MODEL
CONSTANT (default) constant your choice SU2 sets CONSTANT_DENSITY
BOUSSINESQ constant, plus a buoyancy force from temperature always on SU2 sets CONSTANT_DENSITY
VARIABLE from the ideal gas law, changes with temperature always on without species INC_IDEAL_GAS, INC_IDEAL_GAS_POLY, FLUID_MIXTURE or FLUID_FLAMELET
FLAMELET read from a flamelet table handled by the flamelet solver FLUID_FLAMELET

How to choose:

  • No heat transfer, or temperature as a passive quantity. Use CONSTANT. With INC_ENERGY_EQUATION= YES, SU2 solves the energy equation for enthalpy and recovers temperature. Temperature is passive only when properties affecting momentum, notably viscosity, are independent of temperature and no thermal buoyancy is present. Constant density alone does not ensure one-way coupling: POLYNOMIAL_VISCOSITY can still make viscosity temperature-dependent (code). Constant-property one-way coupling is used in the laminar flat plate tutorial (tutorial). Set SPECIFIC_HEAT_CP (default 1004.703 J/(kg K)).
  • Small temperature differences with buoyancy. Use BOUSSINESQ. The buoyancy force uses THERMAL_EXPANSION_COEFF (default 0.00347 1/K) and the difference to INC_TEMPERATURE_INIT. Gravity is fixed at 9.81 m/s², along the negative y axis in 2D and the negative z axis in 3D. You cannot add BODY_FORCE= YES: SU2 stops (code).
  • Large temperature differences in a gas. Use VARIABLE with FLUID_MODEL= INC_IDEAL_GAS (constant specific heat) or INC_IDEAL_GAS_POLY (specific heat as a polynomial of temperature, set with CP_POLYCOEFFS, five coefficients). Set MOLECULAR_WEIGHT in g/mol (default 28.96) and SPECIFIC_HEAT_CP.
  • Mixtures of gases. Use VARIABLE with FLUID_MODEL= FLUID_MIXTURE. See the species guide.

When you set INC_DENSITY_MODEL to CONSTANT or BOUSSINESQ, SU2 replaces your FLUID_MODEL with CONSTANT_DENSITY. Other fluid models only take effect with VARIABLE or FLAMELET (code).

Operating pressure of an ideal gas

With VARIABLE density, SU2 computes the density from an operating pressure, the molecular weight and the temperature. The operating (thermodynamic) pressure is constant in space. The flow pressure in SU2 is a gauge pressure on top of it (Theory).

INIT_OPTION_INC decides which of the two you prescribe (code):

  • DENSITY_INIT: SU2 scales THERMODYNAMIC_PRESSURE so that the density at INC_TEMPERATURE_INIT equals INC_DENSITY_INIT. This is the default for INC_IDEAL_GAS and INC_IDEAL_GAS_POLY.
  • OPERATING_PRESSURE: SU2 uses THERMODYNAMIC_PRESSURE (default 101325 Pa) and computes the density. This is the default for FLUID_MIXTURE and FLUID_FLAMELET.

The buoyancy cavity test case uses DENSITY_INIT with a very small INC_DENSITY_INIT to reach a chosen Rayleigh number (test case).

Gravity for variable density

For natural convection with VARIABLE density, set BODY_FORCE= YES and BODY_FORCE_VECTOR= ( 0.0, -9.81, 0.0 ) (an acceleration in m/s²), as in the buoyancy cavity tutorial. With variable density, the force is (ρ − ρ₀)·g, where ρ₀ is the initial density. So the computed pressure does not contain the hydrostatic pressure of the initial density (code).

Viscosity and conductivity

  • VISCOSITY_MODEL: the default is SUTHERLAND. SU2 stops if you use it with constant density, so set VISCOSITY_MODEL= CONSTANT_VISCOSITY and MU_CONSTANT (default 1.716e-5 kg/(m s)) (code). Sutherland’s law is allowed with INC_IDEAL_GAS, INC_IDEAL_GAS_POLY and FLUID_MIXTURE. POLYNOMIAL_VISCOSITY uses MU_POLYCOEFFS.
  • CONDUCTIVITY_MODEL: the default CONSTANT_PRANDTL computes the conductivity from viscosity, specific heat and PRANDTL_LAM (default 0.72). CONSTANT_CONDUCTIVITY uses THERMAL_CONDUCTIVITY_CONSTANT (default 0.0257 W/(m K)). POLYNOMIAL_CONDUCTIVITY uses KT_POLYCOEFFS.
  • TURBULENT_CONDUCTIVITY_MODEL: CONSTANT_PRANDTL_TURB (default) uses PRANDTL_TURB (default 0.9). NONE switches the turbulent heat transport off.

The defaults are values for air. For water or another liquid, set all of them (advice).

Initial state and non-dimensionalization

INC_DENSITY_INIT, INC_VELOCITY_INIT and INC_TEMPERATURE_INIT set the initial field. The initial pressure is always zero. They also set the free-stream state used at MARKER_FAR markers, the Reynolds number printed on screen, and the free-stream turbulence level (code).

INC_NONDIM chooses the reference values that SU2 divides by internally (code):

  • INITIAL_VALUES (default): the reference density, velocity and temperature are the initial values. The reference velocity is the magnitude of INC_VELOCITY_INIT.
  • REFERENCE_VALUES: you set INC_DENSITY_REF, INC_VELOCITY_REF and INC_TEMPERATURE_REF (all default to 1.0).
  • DIMENSIONAL: all reference values are 1, so SU2 works in SI units.

The reference pressure is the reference density times the reference velocity squared. The inputs in the config file are always in SI units (NACA 0012 tutorial). The flow energy solution field is ENTHALPY in SOLUTION; TEMPERATURE is a recovered field in PRIMITIVE. The separate weakly coupled heat solver instead uses TEMPERATURE as its solution variable (CFlowIncOutput, code). Output and restart fields depend on the requested groups; do not read an enthalpy column as temperature. Pressure, velocity and recovered temperature are divided by their respective reference values unless you use DIMENSIONAL (code). SU2 prints the reference values and the non-dimensional values at the start of the run. Use them to convert results back to SI units.

Advice:

  • Use DIMENSIONAL if you want SI values in the output files. Almost all CHT, species, flamelet and streamwise periodic test cases use it (test case). The choice should not change the converged solution (advice, to be reviewed).
  • Do not use INITIAL_VALUES with a zero INC_VELOCITY_INIT, for example in a closed cavity: the reference velocity becomes zero. Set a small non-zero velocity (the buoyancy cavity test uses 1 m/s), or use DIMENSIONAL (code).
  • Streamwise periodic flow needs INC_NONDIM= DIMENSIONAL (code).

Inlets

MARKER_INLET sets the inlet markers. INC_INLET_TYPE gives one type per inlet marker, in the same order (code):

  • VELOCITY_INLET: MARKER_INLET= ( marker, temperature [K], velocity magnitude [m/s], nx, ny, nz ). SU2 normalizes the nonzero direction vector, so it does not need unit length (code). The temperature is needed even without the energy equation, but then SU2 does not use it (Markers and BC).
  • PRESSURE_INLET: MARKER_INLET= ( marker, temperature [K], total gauge pressure [Pa], nx, ny, nz ). SU2 adjusts the inlet velocity to reach the total pressure. INC_INLET_DAMPING (default 0.1) damps these updates.

The incompressible solver has no mass flow inlet (code). To prescribe a mass flow, use a velocity inlet (velocity = mass flow / (density × area)) or a mass flow outlet.

For a measured or computed inlet profile, set SPECIFIED_INLET_PROFILE= YES and INLET_FILENAME, as in the laminar step tutorial.

Outlets

MARKER_OUTLET sets the outlet markers. INC_OUTLET_TYPE gives one type per outlet marker (code):

  • PRESSURE_OUTLET: MARKER_OUTLET= ( marker, gauge pressure [Pa] ). This is the usual choice. Zero is a good value, because the pressure level is arbitrary in incompressible flow (advice).
  • MASS_FLOW_OUTLET: MARKER_OUTLET= ( marker, mass flow [kg/s] ). In a planar 2D case, this is the rate for a unit out-of-plane depth. SU2 adjusts the outlet pressure to reach the target. INC_OUTLET_DAMPING (default 0.1) damps these updates.

Put the outlet far enough downstream that no recirculation crosses it (advice, to be reviewed).

Walls and far field

  • MARKER_HEATFLUX= ( marker, heat flux [W/m²] ): no-slip wall. Zero means adiabatic.
  • MARKER_ISOTHERMAL= ( marker, temperature [K] ): no-slip wall at a fixed temperature.
  • MARKER_HEATTRANSFER= ( marker, h [W/(m² K)], T_inf [K] ): wall with a heat transfer coefficient.
  • MARKER_EULER: slip wall, for INC_EULER.
  • MARKER_SYM: symmetry plane.
  • MARKER_FAR: far field. It uses INC_VELOCITY_INIT, zero gauge pressure and INC_TEMPERATURE_INIT (code).

The heat transfer guide explains the thermal wall conditions.

Convective scheme and gradients

For the density-based solver, CONV_NUM_METHOD_FLOW accepts these schemes (code):

  • FDS (flux difference splitting, an upwind scheme). Almost all incompressible test cases use it. It has no tuning parameters (Convective Schemes).
  • JST and LAX-FRIEDRICH (centered schemes with artificial dissipation).

MUSCL_FLOW= YES (default) enables second-order reconstruction for the upwind FDS scheme; it does not change the centered schemes. The default limiter is VENKATAKRISHNAN, but most incompressible test cases use SLOPE_LIMITER_FLOW= NONE (code, test case). Add a limiter only if the solution shows wiggles, or if the run diverges near sharp gradients (advice, to be reviewed).

For INC_RANS, the test cases use CONV_NUM_METHOD_TURB= SCALAR_UPWIND. BOUNDED_SCALAR is also available for incompressible flow. It corrects for a non-zero velocity divergence during convergence (Convective Schemes).

Artificial compressibility factor

The density-based solver scales its pseudo-time pressure term with β² = max(4.1, BETA_FACTOR) × (maximum velocity)². So BETA_FACTOR (default 4.1) changes the result only when you set it above 4.1 (code). A larger value can make the pressure-velocity coupling more robust, but slower (advice, to be reviewed). Most users keep the default.

Streamwise periodic flow

Use streamwise periodic flow for one module of a repeating geometry, such as a channel with a row of pins. Read Streamwise Periodicity and the tutorial.

  • Join the periodic faces with MARKER_PERIODIC= ( periodic, donor, rotation center (3), rotation angles (3), translation (3) ).
  • Use KIND_STREAMWISE_PERIODIC= PRESSURE_DROP with STREAMWISE_PERIODIC_PRESSURE_DROP [Pa] (default 1.0), or MASSFLOW with STREAMWISE_PERIODIC_MASSFLOW [kg/s]. With MASSFLOW, SU2 adapts the pressure drop and damps the update with INC_OUTLET_DAMPING (code).
  • With the energy equation, STREAMWISE_PERIODIC_TEMPERATURE= YES makes the temperature periodic too. It allows only MARKER_HEATFLUX and MARKER_SYM, no MARKER_ISOTHERMAL (code). With NO, SU2 removes heat at the outlet; set the amount with STREAMWISE_PERIODIC_OUTLET_HEAT [W].
  • SU2 stops unless INC_NONDIM= DIMENSIONAL. INC_EULER and AXISYMMETRIC= YES are not supported (code).

Iterations and CFL number

  • Steady runs: set ITER (default 1000) or INNER_ITER. CFL_NUMBER sets the pseudo-time step (default 1.25) (code). The incompressible test cases use CFL numbers from 10 to 1000, and up to 50000 in a streamwise periodic case, all with TIME_DISCRE_FLOW= EULER_IMPLICIT (test case).
  • CFL_ADAPT= YES with CFL_ADAPT_PARAM lets SU2 raise the CFL number while the residuals fall, as in the NACA 0012 RANS test case (test case).
  • Unsteady runs: set TIME_DOMAIN= YES, TIME_MARCHING= DUAL_TIME_STEPPING-2ND_ORDER, TIME_STEP, TIME_ITER and INNER_ITER. See the von Karman tutorial and Solver Setup.
  • MGLEVEL (default 0) adds multigrid levels. Some inviscid and laminar test cases use 3 levels (test case).

Check convergence and results

  • Residuals. The default convergence field is RMS_PRESSURE for the density-based solver and RMS_VELOCITY-X for the pressure-based solver (code). Set CONV_FIELD and CONV_RESIDUAL_MINVAL (log10 of the residual, default −14). A drop of 4 to 6 orders is a common target for steady engineering cases (advice, to be reviewed).
  • Field names. SU2 ignores unknown names in CONV_FIELD and prints Ignoring Convergence Field(s) at the start. If all names are unknown, the convergence check is off and the run goes on to ITER (code).
  • Integrated values. Monitor a value you care about, for example DRAG on MARKER_MONITORING markers, or SURFACE_PRESSURE_DROP on MARKER_ANALYZE markers. A stop based on a coefficient uses CONV_CAUCHY_ELEMS and CONV_CAUCHY_EPS (Solver Setup).
  • Mass balance. Add the inlets and outlets to MARKER_ANALYZE, and FLOW_COEFF_SURF to HISTORY_OUTPUT. The history file then has the mass flow of each marker. Inlet and outlet mass flows should agree to a small fraction of a percent at convergence (advice, to be reviewed).
  • Reference values. Read the table of reference and non-dimensional values printed at the start of the run. Check that density, viscosity and Reynolds number are what you intended.
  • Energy equation. With the energy equation, RMS_ENTHALPY is the residual of the energy equation (code). TOTAL_HEATFLUX gives the heat flux through the MARKER_MONITORING markers.

Common problems

Symptom Likely cause What to try
SU2 stops: “Sutherland’s law only valid for ideal gases in incompressible flows”. The default VISCOSITY_MODEL is SUTHERLAND (code). Set VISCOSITY_MODEL= CONSTANT_VISCOSITY and MU_CONSTANT.
SU2 stops: “Inlet types for incompressible problem improperly specified”. INC_INLET_TYPE has fewer entries than MARKER_INLET has markers (code). Give one type per inlet marker, for example INC_INLET_TYPE= VELOCITY_INLET, PRESSURE_INLET. The same applies to INC_OUTLET_TYPE.
SU2 stops: “Variable density incompressible solver limited to ideal gases”. INC_DENSITY_MODEL= VARIABLE with the default FLUID_MODEL= STANDARD_AIR (code). Set FLUID_MODEL= INC_IDEAL_GAS or INC_IDEAL_GAS_POLY.
SU2 stops: “Inviscid incompressible problems must be constant density”. INC_EULER with variable density or with the energy equation (code). Use INC_NAVIER_STOKES, or INC_DENSITY_MODEL= CONSTANT and INC_ENERGY_EQUATION= NO.
The density does not follow THERMODYNAMIC_PRESSURE. With INC_IDEAL_GAS, the default INIT_OPTION_INC= DENSITY_INIT rescales the operating pressure to match INC_DENSITY_INIT (code). Set INIT_OPTION_INC= OPERATING_PRESSURE, or choose an INC_DENSITY_INIT that matches your pressure.
FLUID_MODEL seems to have no effect. INC_DENSITY_MODEL is CONSTANT or BOUSSINESQ, so SU2 uses CONSTANT_DENSITY (code). Use INC_DENSITY_MODEL= VARIABLE.
Non-physical values or a division by zero at the start of a closed-cavity case. INC_VELOCITY_INIT is zero with INC_NONDIM= INITIAL_VALUES (code). Set a small non-zero initial velocity, or use INC_NONDIM= DIMENSIONAL.
The temperature hits a limit; SU2 reports non-physical points. The temperature left TEMPERATURE_LIMITS (default 0 K to 5000 K), so SU2 rejects the update in those points (code). Lower the CFL number and check the thermal boundary values. Widen TEMPERATURE_LIMITS only if the range is physical.
The residuals stall or oscillate. The CFL number is too high, or the flow is really unsteady (advice). Lower CFL_NUMBER or use CFL_ADAPT. If the flow sheds vortices, run it unsteady (to be reviewed).
A pressure inlet case converges slowly. INC_INLET_DAMPING slows down the update of the inlet velocity (code). Try a larger INC_INLET_DAMPING (to be reviewed).
A streamwise periodic case stops at the start. INC_NONDIM is not DIMENSIONAL, or an isothermal wall is used with STREAMWISE_PERIODIC_TEMPERATURE= YES (code). Set INC_NONDIM= DIMENSIONAL. Use MARKER_HEATFLUX, or set STREAMWISE_PERIODIC_TEMPERATURE= NO.
The flow from a pressure inlet or a far field goes the wrong way. The direction vector or INC_VELOCITY_INIT points the wrong way (advice). Check the signs of the direction components against the mesh axes.

Tutorials:

Test cases (density-based unless noted):

User guide pages: Physical Definition, Markers and BC, Theory, Convective Schemes, Solver Setup, Custom Output.

Source review: 22 October 2026, against SU2 docs_site at 41ea6a219a. See the review scope and outstanding validation. Setup recommendations remain draft where indicated.


Improve this page