Setup Guide: Heat Transfer and Conjugate Heat Transfer

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 when temperature matters in your simulation:

  • a fluid with heated or cooled walls,
  • heat conduction in a solid alone,
  • conjugate heat transfer (CHT): heat flows between a fluid zone and one or more solid zones, and SU2 solves all zones together.

The examples use the incompressible solver. CHT also works with the compressible NAVIER_STOKES solver; see the test case coupled_cht/comp_2d. For the fluid settings, read Setup Guide: Incompressible Flows first. For the general multizone setup, read Basics of Multi-Zone Computations.

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

Start from

This setup is a 2D laminar air flow around three cylinders. Each cylinder is a solid zone with a hot core at 350 K. It is the test case coupled_cht/incomp_2d with fewer options. The steady CHT tutorial uses the same case. Changes to the test case: OUTER_ITER is raised from 11 to 2000, and HISTORY_OUTPUT and OUTPUT_FILES are added to the main file. The mesh mesh_cht_3cyl.su2 holds all four zones. It is in the folder coupled_cht/incomp_2d of the TestCases repository.

Main config file cht_2d_3cylinders.cfg:

SOLVER= MULTIPHYSICS
CONFIG_LIST= (flow_cylinder.cfg, solid_cylinder1.cfg, solid_cylinder2.cfg, solid_cylinder3.cfg)
%
% Pairs of markers that touch: fluid side, solid side
MARKER_ZONE_INTERFACE= (cylinder_outer1, cylinder_inner1, cylinder_outer2, cylinder_inner2, cylinder_outer3, cylinder_inner3)
MARKER_CHT_INTERFACE= (cylinder_outer1, cylinder_inner1, cylinder_outer2, cylinder_inner2, cylinder_outer3, cylinder_inner3)
CHT_COUPLING_METHOD= DIRECT_TEMPERATURE_ROBIN_HEATFLUX
%
TIME_DOMAIN= NO
OUTER_ITER= 2000
%
MESH_FILENAME= mesh_cht_3cyl.su2
MESH_FORMAT= SU2
HISTORY_OUTPUT= (ITER, BGS_RES[0], BGS_RES[1], HEAT[0])
OUTPUT_FILES= (RESTART, PARAVIEW_MULTIBLOCK)

Fluid zone flow_cylinder.cfg:

SOLVER= INC_NAVIER_STOKES
KIND_TURB_MODEL= NONE
%
INC_DENSITY_MODEL= VARIABLE
INC_ENERGY_EQUATION= YES
INC_DENSITY_INIT= 0.000210322
INC_VELOCITY_INIT= ( 3.40297, 0.0, 0.0 )
INC_TEMPERATURE_INIT= 288.15
INC_NONDIM= DIMENSIONAL
FLUID_MODEL= INC_IDEAL_GAS
SPECIFIC_HEAT_CP= 1004.703
MOLECULAR_WEIGHT= 28.96
VISCOSITY_MODEL= CONSTANT_VISCOSITY
MU_CONSTANT= 1.7893e-05
CONDUCTIVITY_MODEL= CONSTANT_PRANDTL
PRANDTL_LAM= 0.72
%
MARKER_FAR= ( farfield )
MARKER_MONITORING= ( cylinder_outer1, cylinder_outer2, cylinder_outer3 )
%
NUM_METHOD_GRAD= GREEN_GAUSS
CONV_NUM_METHOD_FLOW= FDS
MUSCL_FLOW= YES
SLOPE_LIMITER_FLOW= NONE
TIME_DISCRE_FLOW= EULER_IMPLICIT
CFL_NUMBER= 10.0
LINEAR_SOLVER= FGMRES
LINEAR_SOLVER_PREC= ILU
LINEAR_SOLVER_ERROR= 1E-15
LINEAR_SOLVER_ITER= 5

Solid zone solid_cylinder1.cfg (zones 2 and 3 are the same, with core2 and core3):

SOLVER= HEAT_EQUATION
INC_NONDIM= DIMENSIONAL
FREESTREAM_TEMPERATURE= 350.0
%
MATERIAL_DENSITY= 0.000210322
SPECIFIC_HEAT_CP= 1004.703
THERMAL_CONDUCTIVITY_CONSTANT= 0.1028
%
MARKER_ISOTHERMAL= ( core1, 350.0 )
%
NUM_METHOD_GRAD= GREEN_GAUSS
TIME_DISCRE_HEAT= EULER_IMPLICIT
CFL_NUMBER= 10.0
LINEAR_SOLVER= FGMRES
LINEAR_SOLVER_PREC= ILU
LINEAR_SOLVER_ERROR= 1E-15
LINEAR_SOLVER_ITER= 5

The zone files do not list the interface markers as boundary conditions. MARKER_CHT_INTERFACE in the main file sets them, and the zone files inherit every option of the main file (Multizone).

Settings that matter

Thermal wall conditions in the fluid

These conditions need the energy equation in the fluid: INC_ENERGY_EQUATION= YES for the incompressible solver.

  • MARKER_ISOTHERMAL= ( marker, T [K] ): fixed wall temperature. Use it when you know the wall temperature.
  • MARKER_HEATFLUX= ( marker, q [W/m²] ): fixed heat flux. Zero gives an adiabatic wall. With INTEGRATED_HEATFLUX= YES, the value is a total heat rate in W, spread over the marker area (Markers and BC). In these finite-volume thermal boundary conditions, a positive value adds heat to the domain (code). For a planar 2D case, integrated heat rates represent a unit out-of-plane depth.
  • MARKER_HEATTRANSFER= ( marker, h [W/(m² K)], T_inf [K] ): the wall heat flux is h·(T_inf − T_wall). Use it to model a wall that you do not mesh, such as a thin wall to an outside fluid. h = 0 gives an adiabatic wall; a very large h gives a wall at T_inf (Markers and BC).

Only the flow solvers implement MARKER_HEATTRANSFER. The heat equation solver for solids does not (code).

Temperature without coupling to the flow

If the temperature does not change the flow (constant density and constant properties), you have two options:

  • INC_DENSITY_MODEL= CONSTANT with INC_ENERGY_EQUATION= YES: the flow solver solves for enthalpy and recovers temperature from the fluid model (laminar flat plate tutorial).
  • WEAKLY_COUPLED_HEAT_EQUATION= YES with INC_ENERGY_EQUATION= NO: SU2 solves the temperature with the separate heat solver, using the flow velocity (code). Its numerics use CONV_NUM_METHOD_HEAT, MUSCL_HEAT, TIME_DISCRE_HEAT and TIMESTEP_HEAT. Example: disc_adj_heat/primal.cfg.

For incompressible CHT, SU2 stops unless the fluid zone has INC_ENERGY_EQUATION= YES (code). So in CHT, use the energy equation, not the weakly coupled heat equation.

Heat conduction in a solid

Set SOLVER= HEAT_EQUATION in the solid zone. This solver solves for temperature only.

  • THERMAL_CONDUCTIVITY_CONSTANT [W/(m K)], MATERIAL_DENSITY [kg/m³] and SPECIFIC_HEAT_CP [J/(kg K)] define the material.
  • The defaults are meant for other uses: 0.0257 W/(m K) for air, 7854 kg/m³ for steel, 1004.703 J/(kg K) for air (code). So always set all three.
  • FREESTREAM_TEMPERATURE (default 288.15 K) is the initial solid temperature (code).
  • Boundary conditions: MARKER_ISOTHERMAL, MARKER_HEATFLUX, MARKER_PERIODIC, and the CHT interface.
  • All solid test cases use INC_NONDIM= DIMENSIONAL (test case).

For steady conduction with prescribed thermal boundary data, density and specific heat drop out of the physical heat equation; they still affect the numerical convergence. Conductivity sets the heat flux and, with flux or Robin data, the temperature gradients. A uniform conductivity cancels from a source-free, purely prescribed-temperature problem. Density and specific heat set the thermal response time in an unsteady run.

A solid alone runs as a normal single-zone case, for example solid_heat_conduction/periodic_pins/configSolid.cfg.

Zones and config files

A CHT case is a multiphysics case (Multizone):

  1. Write one config file per zone. Each one sets SOLVER, and the boundary conditions and numerics of the zone.
  2. Write a main config file with SOLVER= MULTIPHYSICS and CONFIG_LIST, the list of zone files. The order in CONFIG_LIST gives the zone number, starting at 0.
  3. Options that are the same in all zones can go in the main file. The zone files inherit them (Multizone).

The mesh:

  • One file for all zones: MULTIZONE_MESH= YES (default). This works with the SU2 mesh format, with NZONE= and IZONE= in the mesh file (Multizone).
  • One file per zone: MULTIZONE_MESH= NO, and MESH_FILENAME in each zone file. The contact resistance tutorial uses three mesh files.

Run each zone alone first, with a fixed temperature or heat flux at the interface, to find numerical settings that work (advice). The Multizone page gives the same advice.

Interface markers

Each interface has two markers, one on each side. List the pairs in the main file:

  • MARKER_ZONE_INTERFACE: pairs of markers that exchange data.
  • MARKER_CHT_INTERFACE: the same pairs, marked as heat transfer interfaces.

All CHT test cases and tutorials list the pairs in both options (test case, tutorial).

Coupling method

CHT_COUPLING_METHOD decides what crosses the interface (code):

  • DIRECT_TEMPERATURE_ROBIN_HEATFLUX (default): the fluid gets the solid wall temperature. The solid gets a heat flux computed from its own wall temperature and the fluid temperature next to the wall. This is a Robin condition, which mixes temperature and heat flux. All CHT test cases use this method (test case).
  • DIRECT_TEMPERATURE_NEUMANN_HEATFLUX: the solid gets the heat flux computed by the fluid. This is a Neumann condition, a prescribed flux.
  • AVERAGED_TEMPERATURE_ROBIN_HEATFLUX and AVERAGED_TEMPERATURE_NEUMANN_HEATFLUX: the fluid wall temperature is a conductivity-weighted average of the temperatures on both sides.

The Robin methods need the fluid conductivity. With CONDUCTIVITY_MODEL= POLYNOMIAL_CONDUCTIVITY in an incompressible fluid zone, SU2 stops (code). Start with the default, because it is the only method used in the tests (advice, to be reviewed).

Interface interpolation

The two sides of an interface do not need matching meshes (Multizone). KIND_INTERPOLATION chooses how SU2 moves values between them (code):

  • NEAREST_NEIGHBOR (default): each point takes the value of the closest point on the other side. NUM_NEAREST_NEIGHBORS (default 1) sets how many neighbors SU2 uses.
  • ISOPARAMETRIC: interpolation inside the faces of the other side.
  • RADIAL_BASIS_FUNCTION: smooth interpolation with radial basis functions (KIND_RADIAL_BASIS_FUNCTION).

WEIGHTED_AVERAGE is the sliding mesh method for fluid-fluid interfaces, not for CHT. SU2 uses the method of the donor zone, so set it in the main file to apply it everywhere (code). No CHT test case changes the default (test case). With very different mesh sizes on the two sides, ISOPARAMETRIC or RADIAL_BASIS_FUNCTION can give a smoother interface temperature than NEAREST_NEIGHBOR (advice, to be reviewed).

Contact resistance between solids

CHT_INTERFACE_CONTACT_RESISTANCE models imperfect contact between two solids: the temperature jumps across the interface (tutorial).

These rules come from the code (code):

  • Give one value per interface pair, or one value for all pairs. Values must not be negative.
  • It acts only between two HEAT_EQUATION zones, and only with the two ..._ROBIN_HEATFLUX coupling methods. On fluid-solid interfaces it has no effect.
  • The heat flux is (T − T_wall) / (d/k + R), where d is the distance from the wall to the next point and k the conductivity. So R is in m²·K/W, the inverse of a heat transfer coefficient.

The tutorial gives the values in the order of the pairs in MARKER_CHT_INTERFACE: CHT_INTERFACE_CONTACT_RESISTANCE= (1e-4, 0, 0) (tutorial).

Outer and inner iterations

SU2 solves the zones one after the other and exchanges interface data between them. One pass over all zones is an outer iteration.

  • OUTER_ITER (main file): the number of outer iterations of a steady case, or per time step of an unsteady case.
  • INNER_ITER (default 1): the iterations of each zone inside one outer iteration (code, tutorial). You can set it per zone file.
  • MULTIZONE_SOLVER: BLOCK_GAUSS_SEIDEL (default) or BLOCK_JACOBI (code). Gauss-Seidel uses the newest data of the zones already solved, and Jacobi uses the data of the previous outer iteration (advice).
  • RELAXATION_FACTOR_CHT (default 1.0, no relaxation): the new interface value is factor × new + (1 − factor) × old (code).
  • ITER is not allowed in multizone cases: SU2 stops. Use OUTER_ITER and INNER_ITER (code).

The solid often converges more slowly than the fluid, because heat conduction has no convection to carry information. A larger CFL_NUMBER can accelerate the solid solve if the linear system remains adequately solved; the solid-only test case solid_heat_conduction/periodic_pins uses 1e8 (advice, to be reviewed).

Unsteady CHT

Set the time settings in the main file (unsteady CHT tutorial):

TIME_DOMAIN= YES
TIME_MARCHING= DUAL_TIME_STEPPING-2ND_ORDER
TIME_STEP= 0.05
MAX_TIME= 100.0
TIME_ITER= 3
OUTER_ITER= 10

These values are from the test case coupled_cht/incomp_2d_unsteady (test case). The tutorial uses OUTER_ITER= 200 to converge the coupling in each time step (tutorial).

  • Choose TIME_STEP from the time scale of the flow, for example the vortex shedding period (tutorial).
  • In unsteady runs, the solid density and specific heat matter, so set real material values.
  • Solids often respond much more slowly than the fluid. Reaching a periodic state can take many time steps (advice, to be reviewed).

Check convergence and results

  • Coupling residuals. In a multizone case, SU2 prints for each zone how much the solution changed since the last outer iteration. These are the block Gauss-Seidel (BGS) residuals. Fields such as BGS_PRESSURE[0] and BGS_TEMPERATURE[1] are per zone; the number in brackets is the zone. Add the group BGS_RES[i] to HISTORY_OUTPUT for zone i.
  • Default stop rule. Without CONV_FIELD, a multizone case monitors AVG_BGS_RES[0], the averaged BGS residual of zone 0 (code). Set CONV_FIELD and CONV_RESIDUAL_MINVAL in the main file to monitor what you need, for example the solid temperature. The pin array test case sets CONV_RESIDUAL_MINVAL in its main file (test case).
  • Field names. SU2 ignores unknown names in CONV_FIELD and prints Ignoring Convergence Field(s) at the start (code).
  • Heat balance. Monitor TOTAL_HEATFLUX and AVG_TEMPERATURE (group HEAT) on the interface markers, through MARKER_MONITORING in each zone. At steady convergence, integrate conductive heat flux on both sides with a consistent normal convention: heat leaving the solid equals heat entering the fluid. With outward normals for both domains, their signed interface rates sum to zero. Non-matching interpolation also needs a conservation check (advice).
  • Per-zone history. WRT_ZONE_HIST= YES writes a history file per zone. WRT_ZONE_CONV= YES prints the convergence of each zone (code).
  • Visual check. OUTPUT_FILES= (RESTART, PARAVIEW_MULTIBLOCK) writes one ParaView file with all zones. The temperature should be continuous across solid-fluid interfaces (contact resistance tutorial).

Common problems

Symptom Likely cause What to try
SU2 stops: “You probably want to set INC_ENERGY_EQUATION= YES for the fluid solver”. The incompressible fluid zone has no energy equation (code). Set INC_ENERGY_EQUATION= YES in the fluid zone file.
SU2 stops: “ITER must not be used when running multizone”. ITER in a zone file or in the main file (code). Use OUTER_ITER in the main file, and INNER_ITER if needed.
SU2 stops: “Polynomial Conductivity model not implemented for CHT interface”. POLYNOMIAL_CONDUCTIVITY with a Robin coupling method (code). Use CONSTANT_CONDUCTIVITY or CONSTANT_PRANDTL in the fluid, or a Neumann coupling method.
SU2 stops: “Number of CHT interfaces does not match number of contact resistances”. Wrong number of values in CHT_INTERFACE_CONTACT_RESISTANCE (code). Give one value per interface pair, or a single value.
The solid stays at its initial temperature. The interface markers are missing from MARKER_CHT_INTERFACE or MARKER_ZONE_INTERFACE, or the marker names do not match the mesh (advice). Check the start-up output: it prints the interface type between each pair of zones. Check the marker names.
A wall with MARKER_HEATTRANSFER in a solid zone behaves as adiabatic. The heat equation solver does not implement this condition (code). Mesh the outer fluid, or use MARKER_HEATFLUX or MARKER_ISOTHERMAL.
The solid temperatures settle far too slowly. A small CFL number in the solid, or INNER_ITER= 1 with a very stiff solid (advice). Raise CFL_NUMBER in the solid zone, or raise INNER_ITER in the solid zone file (to be reviewed).
The outer iterations oscillate. Strong coupling between zones (advice). Try RELAXATION_FACTOR_CHT below 1, for example 0.5 (to be reviewed).
The solid material behaves like steel or like air. MATERIAL_DENSITY, SPECIFIC_HEAT_CP or THERMAL_CONDUCTIVITY_CONSTANT left at their defaults (code). Set all three in each solid zone file.
The temperature looks blocky along a non-matching interface. NEAREST_NEIGHBOR interpolation between very different meshes (advice). Try KIND_INTERPOLATION= ISOPARAMETRIC (to be reviewed).
The result files of different zones overwrite each other. MULTIZONE_ADAPT_FILENAME= NO (advice). Keep the default YES, which adds the zone number to the restart and solution file names (code).

Tutorials:

Test cases:

User guide pages: Basics of Multi-Zone Computations, Markers and BC, Theory: Heat Conduction, 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