config_template.cfg

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%                                                                              %
% SU2 configuration file                                                       %
% Case description: _________________________________________________________  %
% Author: ___________________________________________________________________  %
% Institution: ______________________________________________________________  %
% Date: __________                                                             %
% File Version 8.4.0 "Harrier"                                                 %
%                                                                              %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
% Solver type (EULER, NAVIER_STOKES, RANS,
%              INC_EULER, INC_NAVIER_STOKES, INC_RANS,
%              NEMO_EULER, NEMO_NAVIER_STOKES,
%              FEM_EULER, FEM_NAVIER_STOKES, FEM_RANS, FEM_LES,
%              HEAT_EQUATION_FVM, ELASTICITY)
SOLVER= EULER
%
% Specify turbulence model (NONE, SA, SST)
KIND_TURB_MODEL= NONE
%
% Specify versions/corrections of the SST model (V2003m, V1994m, VORTICITY, KATO_LAUNDER, UQ, SUSTAINING, COMPRESSIBILITY-WILCOX, COMPRESSIBILITY-SARKAR, DIMENSIONLESS_LIMIT)
SST_OPTIONS= NONE
%
% Specify versions/corrections of the SA model (NEGATIVE, EDWARDS, WITHFT2, QCR2000, COMPRESSIBILITY, ROTATION, BCM, EXPERIMENTAL)
SA_OPTIONS= NONE
%
% Transition model (NONE, LM)
KIND_TRANS_MODEL= NONE
%
% Value of RMS roughness for transition model
HROUGHNESS= 1.0e-6
%
% Specify versions/correlations of the LM model (LM2015, MALAN, SULUKSNA, KRAUSE, KRAUSE_HYPER, MEDIDA, MEDIDA_BAEDER, MENTER_LANGTRY)
LM_OPTIONS= NONE
%
% Specify subgrid scale model(NONE, IMPLICIT_LES, SMAGORINSKY, WALE, VREMAN)
KIND_SGS_MODEL= NONE
%
% Specify the verification solution(NO_VERIFICATION_SOLUTION, INVISCID_VORTEX,
%                                   RINGLEB, NS_UNIT_QUAD, TAYLOR_GREEN_VORTEX,
%                                   MMS_NS_UNIT_QUAD, MMS_NS_UNIT_QUAD_WALL_BC,
%                                   MMS_NS_TWO_HALF_CIRCLES, MMS_NS_TWO_HALF_SPHERES,
%                                   MMS_INC_EULER, MMS_INC_NS, INC_TAYLOR_GREEN_VORTEX,
%                                   USER_DEFINED_SOLUTION)
KIND_VERIFICATION_SOLUTION= NO_VERIFICATION_SOLUTION
%
% Mathematical problem (DIRECT, CONTINUOUS_ADJOINT, DISCRETE_ADJOINT)
% Defaults to DISCRETE_ADJOINT for the SU2_*_AD codes, and to DIRECT otherwise.
MATH_PROBLEM= DIRECT
%
% Axisymmetric simulation for 2D problems. (NO, YES)
AXISYMMETRIC= NO
%
% Gravity force
GRAVITY_FORCE= NO
%
% Restart solution (NO, YES)
RESTART_SOL= NO
%
% Only save the minimum required variables for restarting to restart files (NO, YES).
% If this option is set to NO, then all fields will be written to all output files.
% To minimize the size of other output files (e.g. paraview, tecplot) by not including
% default restart fields in them, add the keyword COMPACT to VOLUME_OUTPUT.
WRT_RESTART_COMPACT= YES
%
% Discard the data storaged in the solution and geometry files
% e.g. AOA, dCL/dAoA, dCD/dCL, iter, etc.
% Note that AoA in the solution and geometry files is critical
% to aero design using AoA as a variable. (NO, YES)
DISCARD_INFILES= NO
%
% System of measurements (SI, US)
% International system of units (SI): ( meters, kilograms, Kelvins,
%                                       Newtons = kg m/s^2, Pascals = N/m^2,
%                                       Density = kg/m^3, Speed = m/s,
%                                       Equiv. Area = m^2 )
% United States customary units (US): ( inches, slug, Rankines, lbf = slug ft/s^2,
%                                       psf = lbf/ft^2, Density = slug/ft^3,
%                                       Speed = ft/s, Equiv. Area = ft^2 )
SYSTEM_MEASUREMENTS= SI
%
% List of config files for each zone in a multizone setup with SOLVER=MULTIPHYSICS
% Order here has to match the order in the meshfile if just one is used.
CONFIG_LIST= (configA.cfg, configB.cfg, ...)
%
% ------------------------------- SOLVER CONTROL ------------------------------%
%
% Number of iterations for single-zone problems
ITER= 1
%
% Maximum number of inner iterations
INNER_ITER= 9999
%
% Maximum number of outer iterations (only for multizone problems)
OUTER_ITER= 1
%
% Maximum number of time iterations
TIME_ITER= 1
%
% Convergence field
CONV_FIELD= DRAG
%
% Min value of the residual (log10 of the residual)
CONV_RESIDUAL_MINVAL= -8
%
% Start convergence criteria at iteration number
CONV_STARTITER= 10
%
% Number of elements to apply the criteria
CONV_CAUCHY_ELEMS= 100
%
% Epsilon to control the series convergence
CONV_CAUCHY_EPS= 1E-10
%
% Iteration number to begin unsteady restarts
RESTART_ITER= 0
%
%% Time convergence monitoring
WINDOW_CAUCHY_CRIT = YES
%
% List of time convergence fields
CONV_WINDOW_FIELD = (TAVG_DRAG, TAVG_LIFT)
%
% Time Convergence Monitoring starts at Iteration WINDOW_START_ITER + CONV_WINDOW_STARTITER
CONV_WINDOW_STARTITER = 0
%
% Epsilon to control the series convergence
CONV_WINDOW_CAUCHY_EPS = 1E-3
%
% Number of elements to apply the criteria
CONV_WINDOW_CAUCHY_ELEMS = 10
%
% Maximum ratio for updating density and energy variables evaluated by the linear solver relative
% to the non-linear solution at previous iteration. Low values ensure stability but may result
% in longer convergence times, based on numerical experiments Default= 0.2
MAX_UPDATE_FLOW= 0.2
%
% Same as MAX_UPDATE_FLOW but for updating nu_tilde variable in SA model, not applicable for Neg model (Default= 0.99)
MAX_UPDATE_SA= 0.99
%
% Same as MAX_UPDATE_FLOW but for updating TKE and Omega variables in SST model (Default= 1.0)
MAX_UPDATE_SST= 1.0
%
% ------------------------- TIME-DEPENDENT SIMULATION -------------------------------%
%
% Time domain simulation
TIME_DOMAIN= NO
%
% Unsteady simulation (NO, TIME_STEPPING, DUAL_TIME_STEPPING-1ST_ORDER,
%                      DUAL_TIME_STEPPING-2ND_ORDER, HARMONIC_BALANCE)
TIME_MARCHING= NO
%
% Time Step for dual time stepping simulations (s) -- Only used when UNST_CFL_NUMBER = 0.0
% For the DG-FEM solver it is used as a synchronization time when UNST_CFL_NUMBER != 0.0
TIME_STEP= 0.0
%
% Total Physical Time for dual time stepping simulations (s)
MAX_TIME= 50.0
%
% Unsteady Courant-Friedrichs-Lewy number of the finest grid
UNST_CFL_NUMBER= 0.0
%
%%  Windowed output time averaging
% Time iteration to start the windowed time average in a direct run
WINDOW_START_ITER = 500
%
% Window used for reverse sweep and direct run. Options (SQUARE, HANN, HANN_SQUARE, BUMP) Square is default.
WINDOW_FUNCTION = SQUARE
%
% Starting direct solver iteration for the unsteady adjoint
UNST_ADJOINT_ITER= 0
%
% ------------------------------- DES Parameters ------------------------------%
%
% Specify Hybrid RANS/LES model (SA_DES, SA_DDES, SA_ZDES, SA_EDDES)
HYBRID_RANSLES= SA_DDES
%
% DES Constant (0.65)
DES_CONST= 0.65

% -------------------- COMPRESSIBLE FREE-STREAM DEFINITION --------------------%
%
% Mach number (non-dimensional, based on the free-stream values)
MACH_NUMBER= 0.8
%
% Angle of attack (degrees, only for compressible flows)
AOA= 1.25
%
% Side-slip angle (degrees, only for compressible flows)
SIDESLIP_ANGLE= 0.0
%
% Init option to choose between Reynolds (default) or thermodynamics quantities
% for initializing the solution (REYNOLDS, TD_CONDITIONS)
INIT_OPTION= REYNOLDS
%
% Free-stream option to choose between density and temperature (default) for
% initializing the solution (TEMPERATURE_FS, DENSITY_FS)
FREESTREAM_OPTION= TEMPERATURE_FS
%
% Free-stream pressure (101325.0 N/m^2, 2116.216 psf by default)
FREESTREAM_PRESSURE= 101325.0
%
% Free-stream temperature (288.15 K, 518.67 R by default)
FREESTREAM_TEMPERATURE= 288.15
%
% Free-stream VIBRATIONAL temperature (288.15 K, 518.67 R by default)
FREESTREAM_TEMPERATURE_VE= 288.15
%
% Reynolds number (non-dimensional, based on the free-stream values)
REYNOLDS_NUMBER= 6.5E6
%
% Reynolds length (1 m, 1 inch by default)
REYNOLDS_LENGTH= 1.0
%
% Free-stream density (1.2886 Kg/m^3, 0.0025 slug/ft^3 by default)
FREESTREAM_DENSITY= 1.2886
%
% Free-stream velocity (1.0 m/s, 1.0 ft/s by default)
FREESTREAM_VELOCITY= ( 1.0, 0.00, 0.00 )
%
% Free-stream viscosity (1.853E-5 N s/m^2, 3.87E-7 lbf s/ft^2 by default)
FREESTREAM_VISCOSITY= 1.853E-5
%
% Free-stream turbulence intensity
FREESTREAM_TURBULENCEINTENSITY= 0.05
%
% Value for freestream intermittency
FREESTREAM_INTERMITTENCY= 1.0
%
% Fix turbulence quantities to far-field values inside an upstream half-space
TURB_FIXED_VALUES= NO
%
% Shift of the half-space on which fixed values are applied.
% It consists of those coordinates whose dot product with the
% normalized far-field velocity is less than this parameter.
TURB_FIXED_VALUES_DOMAIN= -1.0
%
% Free-stream ratio between turbulent and laminar viscosity
FREESTREAM_TURB2LAMVISCRATIO= 10.0
%
% Compressible flow non-dimensionalization (DIMENSIONAL, FREESTREAM_PRESS_EQ_ONE,
%                              FREESTREAM_VEL_EQ_MACH, FREESTREAM_VEL_EQ_ONE)
REF_DIMENSIONALIZATION= DIMENSIONAL

% ---------------- INCOMPRESSIBLE FLOW CONDITION DEFINITION -------------------%
%
% Density model within the incompressible flow solver.
% Options are CONSTANT (default), BOUSSINESQ, VARIABLE, or FLAMELET. If VARIABLE,
% an appropriate fluid model must be selected. For FLAMELET, the density is
% retrieved directly from the flamelet manifold.
INC_DENSITY_MODEL= CONSTANT
%
% Solve the energy equation in the incompressible flow solver
INC_ENERGY_EQUATION = NO
%
% Temperature limits for incompressible flows (0.0, 5000.0 K by default).
TEMPERATURE_LIMITS= 0.0, 5000.0
%
% Initial density for incompressible flows
% (1.2886 kg/m^3 by default (air), 998.2 Kg/m^3 (water))
INC_DENSITY_INIT= 1.2886
%
% Initial velocity for incompressible flows (1.0,0,0 m/s by default)
INC_VELOCITY_INIT= ( 1.0, 0.0, 0.0 )
%
% Initial temperature for incompressible flows that include the
% energy equation (288.15 K by default). Value is ignored if
% INC_ENERGY_EQUATION is false.
INC_TEMPERATURE_INIT= 288.15
%
% Non-dimensionalization scheme for incompressible flows. Options are
% INITIAL_VALUES (default), REFERENCE_VALUES, or DIMENSIONAL.
% INC_*_REF values are ignored unless REFERENCE_VALUES is chosen.
INC_NONDIM= INITIAL_VALUES
%
% Reference density for incompressible flows (1.0 kg/m^3 by default)
INC_DENSITY_REF= 1.0
%
% Reference velocity for incompressible flows (1.0 m/s by default)
INC_VELOCITY_REF= 1.0
%
% Reference temperature for incompressible flows that include the
% energy equation (1.0 K by default)
INC_TEMPERATURE_REF = 1.0
%
% List of inlet types for incompressible flows. List length must
% match number of inlet markers. Options: VELOCITY_INLET, PRESSURE_INLET.
INC_INLET_TYPE= VELOCITY_INLET
%
% Damping coefficient for iterative updates at pressure inlets. (0.1 by default)
INC_INLET_DAMPING= 0.1
%
% Impose inlet velocity magnitude in the direction of the normal of the inlet face.
% used for incompressible velocity inlet and for compressible pressure and mass flow inlets.
INLET_USE_NORMAL= NO
%
% List of outlet types for incompressible flows. List length must
% match number of outlet markers. Options: PRESSURE_OUTLET, MASS_FLOW_OUTLET
INC_OUTLET_TYPE= PRESSURE_OUTLET
%
% Damping coefficient for iterative updates at mass flow outlets. (0.1 by default)
INC_OUTLET_DAMPING= 0.1
%
% Bulk Modulus for computing the Mach number
BULK_MODULUS= 1.42E5
% Epsilon^2 multipier in Beta calculation for incompressible preconditioner.
BETA_FACTOR= 4.1
%
% ----------------------------- SOLID ZONE HEAT VARIABLES-----------------------%
%
% Thermal conductivity used for heat equation
THERMAL_CONDUCTIVITY_CONSTANT= 0.0
%
% Solids temperature at freestream conditions
FREESTREAM_TEMPERATURE= 288.15
%
% Density used in solids
MATERIAL_DENSITY= 2710.0
%
% ----------------------------- CL DRIVER DEFINITION ---------------------------%
%
% Activate fixed lift mode (specify a CL instead of AoA, NO/YES)
FIXED_CL_MODE= NO
%
% Target coefficient of lift for fixed lift mode (0.80 by default)
TARGET_CL= 0.80
%
% Estimation of dCL/dAlpha (0.2 per degree by default)
DCL_DALPHA= 0.2
%
% Maximum number of iterations between AoA updates
UPDATE_AOA_ITER_LIMIT= 100
%
% Number of times Alpha is updated in a fix CL problem.
UPDATE_IH= 5
%
% Number of iterations to evaluate dCL_dAlpha by using finite differences (500 by default)
ITER_DCL_DALPHA= 500
%
% Evaluate the dOF_dCL or dOF_dCMy during run time
EVAL_DOF_DCX= NO
%
% Damping factor for thrust BC (actuator disk).
NETTHRUST_DBCTHRUST= 1.0
%
% parameter for the definition of a complex objective function
DCD_DCL_VALUE= 0.0
%
% parameter for the definition of a complex objective function
DCMX_DCL_VALUE= 0.0
%
% parameter for the definition of a complex objective function
DCMY_DCL_VALUE= 0.0
%
% parameter for the definition of a complex objective function
DCMZ_DCL_VALUE= 0.0

% ---------------------- REFERENCE VALUE DEFINITION ---------------------------%
%
% Reference origin for moment computation (m or in)
REF_ORIGIN_MOMENT_X = 0.25
REF_ORIGIN_MOMENT_Y = 0.00
REF_ORIGIN_MOMENT_Z = 0.00
%
% Reference length for moment non-dimensional coefficients (m or in)
REF_LENGTH= 1.0
%
% Reference velocity (incompressible only)
REF_VELOCITY= 1.0
%
% Reference viscosity (incompressible only)
REF_VISCOSITY= 1.0
%
% Reference area for non-dimensional force coefficients (0 implies automatic
% calculation) (m^2 or in^2)
REF_AREA= 1.0
%
% Aircraft semi-span (0 implies automatic calculation) (m or in)
SEMI_SPAN= 0.0

% ---- NONEQUILIBRIUM GAS, IDEAL GAS, POLYTROPIC, VAN DER WAALS AND PENG ROBINSON CONSTANTS, CoolProp library -------%
%
% Fluid model (STANDARD_AIR, IDEAL_GAS, VW_GAS, PR_GAS,
%              CONSTANT_DENSITY, INC_IDEAL_GAS, INC_IDEAL_GAS_POLY, MUTATIONPP, SU2_NONEQ, FLUID_MIXTURE, COOLPROP, FLUID_FLAMELET, DATADRIVEN_FLUID)
FLUID_MODEL= STANDARD_AIR
% To find all available fluid name for CoolProp library, clikc the following link:
% http://www.coolprop.org/fluid_properties/PurePseudoPure.html#list-of-fluids
FLUID_NAME = nitrogen
% Ratio of specific heats (1.4 default and the value is hardcoded
%                          for the model STANDARD_AIR, compressible only)
GAMMA_VALUE= 1.4
%
% Specific gas constant (287.058 J/kg*K default and this value is hardcoded
%                        for the model STANDARD_AIR, compressible only)
GAS_CONSTANT= 287.058
%
% Critical Temperature (131.00 K by default)
CRITICAL_TEMPERATURE= 131.00
%
% Critical Pressure (3588550.0 N/m^2 by default)
CRITICAL_PRESSURE= 3588550.0
%
% Critical Density (263.0 kg/m^3 by default)
CRITICAL_DENSITY= 263.0
%
% Acentric factor (0.035 (air))
ACENTRIC_FACTOR= 0.035
%
% Thermodynamics(operating) Pressure (101325 Pa default value, only for incompressible flow and FLUID_MIXTURE)
THERMODYNAMIC_PRESSURE= 101325.0
%
% Specific heat at constant pressure, Cp (1004.703 J/kg*K (air)).
% Incompressible fluids with energy eqn. (CONSTANT_DENSITY, INC_IDEAL_GAS) and the heat equation.
SPECIFIC_HEAT_CP= 1004.703
%
% Thermal expansion coefficient (0.00347 K^-1 (air))
% Used with Boussinesq approx. (incompressible, BOUSSINESQ density model only)
THERMAL_EXPANSION_COEFF= 0.00347
%
% Molecular Weights of species for an incompressible ideal gas (28.96 g/mol (air) default),
% For multispecies, we have N Molecular weights: W_1, W_2,...., W_N
MOLECULAR_WEIGHT= 28.96, 16.043
%
% Temperature polynomial coefficients (up to quartic) for specific heat Cp.
% Format -> Cp(T) : b0 + b1*T + b2*T^2 + b3*T^3 + b4*T^4
CP_POLYCOEFFS= (0.0, 0.0, 0.0, 0.0, 0.0)
%
% --- Nonequilibrium fluid options
%
% Gas model - mixture
GAS_MODEL= AIR-5
%
% Initial gas composition in mass fractions
GAS_COMPOSITION= (0.77, 0.23, 0.0, 0.0, 0.0)
%
% Freeze chemical reactions
FROZEN_MIXTURE= NO

%
% Datadriven fluid model
% For data-driven fluid models, an interpolation algorithm is used to retrieve the thermodynamic state for a given density and internal energy

% Interpolation method for thermodynamic state calculation for data-driven fluid model or flamelet fluid model.
% (MLP for multi-layer perceptron, LUT for 2D or 3D, unstructured look-up table)
INTERPOLATION_METHOD= MLP

% Name of the input file containing the information required for the interpolator to function.
% Provide list of .mlp files (See https://github.com/EvertBunschoten/MLPCpp for more information.)
% when using the MLP option for INTERPOLATION_METHOD
% or a single .drg file for the LUT INTERPOLATION_METHOD option.
FILENAMES_INTERPOLATOR= (MLP_1.mlp, MLP_2.mlp, MLP_3.mlp)

% Relaxation factor for the Newton solvers in the data-driven fluid model
DATADRIVEN_NEWTON_RELAXATION= 0.8

% Use physics-informed neural network for calculation of the fluid caloric properties.
USE_PINN= YES

% Specify if there is ionization
IONIZATION= NO
%
% Specify if there is VT transfer residual limiting
VT_RESIDUAL_LIMITING= NO
%
% NEMO Inlet Options
INLET_TEMPERATURE_VE = 288.15
INLET_GAS_COMPOSITION = (0.77, 0.23, 0.0, 0.0, 0.0)

% --------------------------- VISCOSITY MODEL ---------------------------------%
%
% Viscosity model (SUTHERLAND, CONSTANT_VISCOSITY, POLYNOMIAL_VISCOSITY, FLAMELET).
VISCOSITY_MODEL= SUTHERLAND
%
% Molecular Viscosity that would be constant (1.716E-5 by default)
MU_CONSTANT= 1.716E-5
%
% Sutherland Viscosity Ref (1.716E-5 default value for AIR SI)
MU_REF= 1.716E-5
%
% Sutherland Temperature Ref (273.15 K default value for AIR SI)
MU_T_REF= 273.15
%
% Sutherland constant (110.4 default value for AIR SI)
SUTHERLAND_CONSTANT= 110.4
%
% Temperature polynomial coefficients (up to quartic) for viscosity.
% Format -> Mu(T) : b0 + b1*T + b2*T^2 + b3*T^3 + b4*T^4
MU_POLYCOEFFS= (0.0, 0.0, 0.0, 0.0, 0.0)

% --------------------------- THERMAL CONDUCTIVITY MODEL ----------------------%
%
% Laminar Conductivity model (CONSTANT_CONDUCTIVITY, CONSTANT_PRANDTL,
% POLYNOMIAL_CONDUCTIVITY, FLAMELET).
CONDUCTIVITY_MODEL= CONSTANT_PRANDTL
%
% Molecular Thermal Conductivity that would be constant (0.0257 by default)
THERMAL_CONDUCTIVITY_CONSTANT= 0.0257
%
% Laminar Prandtl number (0.72 (air), only for CONSTANT_PRANDTL)
PRANDTL_LAM= 0.72
%
% Temperature polynomial coefficients (up to quartic) for conductivity.
% Format -> Kt(T) : b0 + b1*T + b2*T^2 + b3*T^3 + b4*T^4
KT_POLYCOEFFS= (0.0, 0.0, 0.0, 0.0, 0.0)
%
% Definition of the turbulent thermal conductivity model for RANS
% (CONSTANT_PRANDTL_TURB by default, NONE).
TURBULENT_CONDUCTIVITY_MODEL= CONSTANT_PRANDTL_TURB
%
% Turbulent Prandtl number (0.9 (air) by default)
PRANDTL_TURB= 0.90

% ----------------------- DYNAMIC MESH DEFINITION -----------------------------%
%
% Type of dynamic mesh (NONE, RIGID_MOTION, ROTATING_FRAME,
%                       STEADY_TRANSLATION, GUST)
% ROTATING_FRAME: This option considers both parameters ROTATION_RATE and
% TRANSLATION_RATE, which allows to simulate a free-flying aircraft (in a flight
% mechanical sense) which moves and rotates in all six degrees of freedom about
% the center of gravity. In this context, the farfield MACH number is set to
% zero and MACH_MOTION is used instead to compute force coefficients.
% STEADY_TRANSLATION: This option considers only the parameter TRANSLATION_RATE.
%
GRID_MOVEMENT= NONE
%
% Motion mach number (non-dimensional). Used for initializing a viscous flow
% with the Reynolds number and for computing force coeffs. with dynamic meshes.
MACH_MOTION= 0.8
%
% Coordinates of the motion origin
MOTION_ORIGIN= 0.25 0.0 0.0
%
% Angular velocity vector (rad/s) about the motion origin
ROTATION_RATE = 0.0 0.0 0.0
%
% Pitching angular freq. (rad/s) about the motion origin
PITCHING_OMEGA= 0.0 0.0 0.0
%
% Pitching amplitude (degrees) about the motion origin
PITCHING_AMPL= 0.0 0.0 0.0
%
% Pitching phase offset (degrees) about the motion origin
PITCHING_PHASE= 0.0 0.0 0.0
%
% Translational velocity (m/s or ft/s) in the x, y, & z directions
TRANSLATION_RATE = 0.0 0.0 0.0
%
% Plunging angular freq. (rad/s) in x, y, & z directions
PLUNGING_OMEGA= 0.0 0.0 0.0
%
% Plunging amplitude (m or ft) in x, y, & z directions
PLUNGING_AMPL= 0.0 0.0 0.0
%
% Type of dynamic surface movement (NONE, DEFORMING, MOVING_WALL,
% AEROELASTIC, AEROELASTIC_RIGID_MOTION EXTERNAL, EXTERNAL_ROTATION)
SURFACE_MOVEMENT= NONE
%
% Moving wall boundary marker(s) (NONE = no marker, ignored for RIGID_MOTION)
MARKER_MOVING= ( NONE )
%
% Coordinates of the motion origin
SURFACE_MOTION_ORIGIN= 0.25
%
% Angular velocity vector (rad/s) about the motion origin
SURFACE_ROTATION_RATE = 0.0 0.0 0.0
%
% Pitching angular freq. (rad/s) about the motion origin
SURFACE_PITCHING_OMEGA= 0.0 0.0 0.0
%
% Pitching amplitude (degrees) about the motion origin
SURFACE_PITCHING_AMPL= 0.0 0.0 0.0
%
% Pitching phase offset (degrees) about the motion origin
SURFACE_PITCHING_PHASE= 0.0 0.0 0.0
%
% Translational velocity (m/s or ft/s) in the x, y, & z directions
SURFACE_TRANSLATION_RATE = 0.0 0.0 0.0
%
% Plunging angular freq. (rad/s) in x, y, & z directions
SURFACE_PLUNGING_OMEGA= 0.0 0.0 0.0
%
% Plunging amplitude (m or ft) in x, y, & z directions
SURFACE_PLUNGING_AMPL= 0.0 0.0 0.0
%
% Move Motion Origin for marker moving (1 or 0)
MOVE_MOTION_ORIGIN = 0

% ------------------------- BUFFET SENSOR DEFINITION --------------------------%
%
% Compute the Kenway-Martins separation sensor for buffet-onset detection
% If BUFFET objective/constraint is specified, the objective is given by
% the integrated sensor normalized by reference area
%
% See doi: 10.2514/1.J055172
%
% Evaluate buffet sensor on Navier-Stokes markers  (NO, YES)
BUFFET_MONITORING= NO
%
% Sharpness coefficient for the buffet sensor Heaviside function
BUFFET_K= 10.0
%
% Offset parameter for the buffet sensor Heaviside function
BUFFET_LAMBDA= 0.0

% -------------- AEROELASTIC SIMULATION (Typical Section Model) ---------------%
%
% Activated by GRID_MOVEMENT_KIND option
%
% The flutter speed index (modifies the freestream condition in the solver)
FLUTTER_SPEED_INDEX = 0.6
%
% Natural frequency of the spring in the plunging direction (rad/s)
PLUNGE_NATURAL_FREQUENCY = 100
%
% Natural frequency of the spring in the pitching direction (rad/s)
PITCH_NATURAL_FREQUENCY = 100
%
% The airfoil mass ratio
AIRFOIL_MASS_RATIO = 60
%
% Distance in semichords by which the center of gravity lies behind
% the elastic axis
CG_LOCATION = 1.8
%
% The radius of gyration squared (expressed in semichords)
% of the typical section about the elastic axis
RADIUS_GYRATION_SQUARED = 3.48
%
% Solve the aeroelastic equations every given number of internal iterations
AEROELASTIC_ITER = 3

% --------------------------- GUST SIMULATION ---------------------------------%
%
% Apply a wind gust (NO, YES)
WIND_GUST = NO
%
% Type of gust (NONE, TOP_HAT, SINE, ONE_M_COSINE, VORTEX, EOG)
GUST_TYPE = NONE
%
% Direction of the gust (X_DIR, Y_DIR or Z_DIR)
GUST_DIR = Y_DIR
%
% Gust wavelenght (meters)
% Note for 1-cos gusts: this is the full gust length, not the gust gradient H (half gust length) as used for example in CS-25.
GUST_WAVELENGTH= 10.0
%
% Number of gust periods
GUST_PERIODS= 1.0
%
% Gust amplitude (m/s)
GUST_AMPL= 10.0
%
% Time at which to begin the gust (sec)
GUST_BEGIN_TIME= 0.0
%
% Location at which the gust begins (meters) */
GUST_BEGIN_LOC= 0.0

% ------------------------ SUPERSONIC SIMULATION ------------------------------%
% MARKER_NEARFIELD needs to be defined on a circumferential boundary within
% calculation domain so that it captures pressure disturbance from the model.
% The boundary should have a structured grid with the same number of nodes
% along each azimuthal angle.
% To run inverse design using target equivalent area, TargetEA.dat is required.
%
% Evaluate equivalent area on the Near-Field (NO, YES)
EQUIV_AREA= NO
%
% Integration limits of the equivalent area ( xmin, xmax, Dist_NearField )
EA_INT_LIMIT= ( 1.6, 2.9, 1.0 )
%
% Equivalent area scale factor ( EA should be ~ force based objective functions )
EA_SCALE_FACTOR= 1.0
%
% Fix an azimuthal line due to misalignments of the near-field
FIX_AZIMUTHAL_LINE= 90.0
%
% Drag weight in sonic boom Objective Function (from 0.0 to 1.0)
DRAG_IN_SONICBOOM= 0.0

% -------------------------- ENGINE SIMULATION --------------------------------%
%
% Evaluate a problem with engines
ENGINE= NO
%
% Highlite area to compute MFR (1 in2 by default)
HIGHLITE_AREA= 1.0
%
% Fan polytropic efficiency (1.0 by default)
FAN_POLY_EFF= 1.0
%
% Only half engine is in the computational grid (NO, YES)
ENGINE_HALF_MODEL= NO
%
% Evaluation Frequency for Engine and Actuator Disk Markers
BC_EVAL_FREQ = 40
%
% Damping factor for the engine inflow.
DAMP_ENGINE_INFLOW= 0.95
%
% Damping factor for the engine exhaust.
DAMP_ENGINE_EXHAUST= 0.95
%
% Engine nu factor (SA model).
ENGINE_NU_FACTOR= 3.0
%
% Actuator disk jump definition using ratio or difference (DIFFERENCE, RATIO)
ACTDISK_JUMP= DIFFERENCE
%
% secondary flow value for actuator disk
ACTDISK_SECONDARY_FLOW= 0.0
%
% Actuator disk double surface
ACTDISK_DOUBLE_SURFACE= NO
%
%
% Number of times BC Thrust is updated in a fix Net Thrust problem (5 by default)
UPDATE_BCTHRUST= 100
%
% Initial BC Thrust guess for POWER or D-T driver (4000.0 lbf by default)
INITIAL_BCTHRUST= 4000.0
%
% Initialization with a subsonic flow around the engine.
SUBSONIC_ENGINE= NO
%
% Axis of the cylinder that defines the subsonic region (A_X, A_Y, A_Z, B_X, B_Y, B_Z, Radius)
SUBSONIC_ENGINE_CYL= ( 0.0, 0.0, 0.0, 1.0, 0.0 , 0.0, 1.0 )
%
% Flow variables that define the subsonic region (Mach, Alpha, Beta, Pressure, Temperature)
SUBSONIC_ENGINE_VALUES= ( 0.4, 0.0, 0.0, 2116.216, 518.67 )
%
% Definition of the distortion rack (radial number of proves / circumferential density (degree)
DISTORTION_RACK= (0.0, 0.0)

% ------------------------- TURBOMACHINERY SIMULATION -------------------------%
%
% Specify kind of architecture for each zone (AXIAL, CENTRIPETAL, CENTRIFUGAL,
%                                             CENTRIPETAL_AXIAL, AXIAL_CENTRIFUGAL)
TURBOMACHINERY_KIND= CENTRIPETAL CENTRIPETAL_AXIAL
%
% Specify the machine architecture for performance analysis (TURBINE, COMPRESSOR, PROPELLOR)
%
TURBO_PERF_KIND = TURBINE TURBINE
%
% Specify kind of interpolation for the mixing-plane (LINEAR_INTERPOLATION,
%                                                     NEAREST_SPAN, MATCHING)
MIXINGPLANE_INTERFACE_KIND= LINEAR_INTERPOLATION
%
% Specify option for turbulent mixing-plane (YES, NO) default NO
TURBULENT_MIXINGPLANE= YES
%
% Specify ramp option for Outlet Giles value (YES, NO) default NO
RAMP_OUTLET= NO
%
% Parameters of the outlet Giles ramp (starting outlet value,
% updating-iteration-frequency, total number of iteration for the ramp)
RAMP_OUTLET_COEFF= (400000.0, 10.0, 500)
%
%
% Specify ramp option for frame of motion (YES, NO) default NO
RAMP_MOTION_FRAME= YES
%
% Parameters of the frame of motion ramp (starting frame of motion speed,
% updating-iteration-frequency, total number of iteration for the ramp)
RAMP_MOTION_FRAME_COEFF= (0.0, 39.0, 500)
%
%
% Specify Kind of average process for linearizing the Navier-Stokes
% equation at inflow and outflow BCs included at the mixing-plane interface
% (ALGEBRAIC, AREA, MASSSFLUX, MIXEDOUT) default AREA
AVERAGE_PROCESS_KIND= MIXEDOUT
%
% Specify Kind of average process for computing turbomachinery performance parameters
% (ALGEBRAIC, AREA, MASSSFLUX, MIXEDOUT) default AREA
PERFORMANCE_AVERAGE_PROCESS_KIND= MIXEDOUT
%
% Parameters of the Newton method for the MIXEDOUT average algorithm
% (under relaxation factor, tollerance, max number of iterations)
MIXEDOUT_COEFF= (1.0, 1.0E-05, 15)
%
% Limit of Mach number below which the mixedout algorithm is substituted
% with a AREA average algorithm to avoid numerical issues
AVERAGE_MACH_LIMIT= 0.05
%
% Integer number of periodic time instances for Harmonic Balance
TIME_INSTANCES= 1
%
% Time period for Harmonic Balance wihtout moving meshes
HB_PERIOD= -1
%
% Turn on/off harmonic balance preconditioning
HB_PRECONDITION= NO
%
% Omega_HB = 2*PI*frequency - frequencies for Harmonic Balance method
OMEGA_HB= (0,1.0,-1.0)
%
% Determines if the single-zone driver is used. (deprecated)
SINGLEZONE_DRIVER= NO
%
% Determines if the special output is written out
SPECIAL_OUTPUT= NO

% ------------------- RADIATIVE HEAT TRANSFER SIMULATION ----------------------%
%
% Type of radiation model (NONE, P1)
RADIATION_MODEL = NONE
%
% Kind of initialization of the P1 model (ZERO, TEMPERATURE_INIT)
P1_INITIALIZATION = TEMPERATURE_INIT
%
% Absorption coefficient
ABSORPTION_COEFF = 1.0
%
% Scattering coefficient
SCATTERING_COEFF = 0.0
%
% Apply a volumetric heat source as a source term (NO, YES) in the form of an ellipsoid (YES, NO)
HEAT_SOURCE = NO
%
% Value of the volumetric heat source
HEAT_SOURCE_VAL = 1.0E6
%
% Rotation of the volumetric heat source respect to Z axis (degrees)
HEAT_SOURCE_ROTATION_Z = 0.0
%
% Position of heat source center (Heat_Source_Center_X, Heat_Source_Center_Y, Heat_Source_Center_Z)
HEAT_SOURCE_CENTER = ( 0.0, 0.0, 0.0 )
%
% Vector of heat source radii (Heat_Source_Radius_A, Heat_Source_Radius_B, Heat_Source_Radius_C)
HEAT_SOURCE_AXES = ( 1.0, 1.0, 1.0 )
%
% Wall emissivity of the marker for radiation purposes
MARKER_EMISSIVITY = ( MARKER_NAME, 1.0 )
%
% Courant-Friedrichs-Lewy condition of the finest grid in radiation solvers
CFL_NUMBER_RAD = 1.0E3
%
% Time discretization for radiation problems (EULER_IMPLICIT)
TIME_DISCRE_RADIATION = EULER_IMPLICIT

% --------------------- SPECIES TRANSPORT SIMULATION --------------------------%
%
% Specify scalar transport model (NONE, SPECIES_TRANSPORT, FLAMELET)
KIND_SCALAR_MODEL= NONE
%
% mixing model for species transport (DAVIDSON, WILKE)
MIXING_VISCOSITY_MODEL= DAVIDSON
%
% Mass diffusivity model (CONSTANT_DIFFUSIVITY, CONSTANT_SCHMIDT, UNITY_LEWIS, CONSTANT_LEWIS, FLAMELET)
DIFFUSIVITY_MODEL= CONSTANT_DIFFUSIVITY
%
% Mass diffusivity if DIFFUSIVITY_MODEL= CONSTANT_DIFFUSIVITY is chosen. D_air ~= 0.001
DIFFUSIVITY_CONSTANT= 0.001
%
% Laminar Schmidt number for mass diffusion (for constant schmidt number model)
SCHMIDT_NUMBER_LAMINAR= 1.0
% Turbulent Schmidt number of mass diffusion
SCHMIDT_NUMBER_TURBULENT= 0.7
%
% list of constant Lewis numbers for all species for
CONSTANT_LEWIS_NUMBER= (1,1,1)
%
% Inlet Species boundary marker(s) with the following format:
% (inlet_marker, Species1, Species2, ..., SpeciesN-1, inlet_marker2, Species1, Species2, ...)
% For N species, N-1 transport equations are solved, the last one Y_N is solved algebraically as 1-(sum of the species 1 to (N-1))
MARKER_INLET_SPECIES= (inlet, 0.5, ..., inlet2, 0.6, ...)
%
% Convective numerical method for species transport (SCALAR_UPWIND, BOUNDED_SCALAR)
CONV_NUM_METHOD_SPECIES= SCALAR_UPWIND
%
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the species equations.
% Required for 2nd order upwind schemes (NO, YES)
MUSCL_SPECIES= NO
%
% Same as MUSCL_KAPPA_FLOW but for species transport.
MUSCL_KAPPA_SPECIES= 0.0
%
% Slope limiter for species equations (same as SLOPE_LIMITER_TURB)
SLOPE_LIMITER_SPECIES = NONE
%
% Time discretization for species equations (EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_SPECIES= EULER_IMPLICIT
%
% Reduction factor of the CFL coefficient in the species problem
CFL_REDUCTION_SPECIES= 1.0
%
% Initial values for scalar transport
SPECIES_INIT= 1.0
%
% Activate clipping for scalar transport equations
SPECIES_CLIPPING= NO
%
% Maximum values for scalar clipping
SPECIES_CLIPPING_MAX= 1.0
%
% Minimum values for scalar clipping
SPECIES_CLIPPING_MIN= 0.0

% --------------------- FLAMELET MODEL -----------------------------%
% The flamelet model uses the prompts INTERPOLATION_METHOD and FILENAMES_INTERPOLATOR
% for definition of the flamelet manifold. Either LUT or MLP can be used as options.
% If the terms "Beta_ProgVar", "Beta_Enth_Thermal", "Beta_Enth", and "Beta_Mixfrac" are
% found in the variables list of the manifold, preferential diffusion is assumed.

%
% Names of the user defined (auxiliary) transport equations.
USER_SCALAR_NAMES= (Y-CO)
%
% Names of the source terms for the user defined transport equations. The source term
% has the form
%  S = S_production + S_consumption * Y, with Y the mass fraction of the user scalar
%  S = S_production + S_consumption * X, with X the mole fraction of the user scalar
% The second term can have the name "zero" or "null" to indicate that only a total source
% will be used.
USER_SOURCE_NAMES= ( ProdRateTot_Y-CO,  zero)
%
% Names of variables from the LUT that will be looked up for visualization
LOOKUP_NAMES= (MolarWeightMix, Conductivity, HeatRelease, Diffusivity)
%

% Names of the controlling variables used to evaluate the look-up table and for which
% transported scalar variables are generated. These names should coincide with those
% listed in the look-up table.
CONTROLLING_VARIABLE_NAMES= (ProgressVariable, EnthalpyTot)

% Names of the source term variables as they are present in the look-up table. For
% controlling variables without source terms, use "zero" or "null", similar to the
% option USER_SOURCE_NAMES.
CONTROLLING_VARIABLE_SOURCE_NAMES= (ProdRateTot_PV, NULL)

% Method used to ignite the solution:
% FLAME_FRONT : the flame is initialized using a plane, defined by a point and a normal. On one side, the solution is initialized
% using 'burnt' conditions and on the other side 'unburnt' conditions. The normal points in the direction of the 'burnt'
% condition.
% SPARK : the solution is ignited through application of a set of source terms within a specified region for a set number
% of solver iterations. This artificial spark can be applied after a certain number of iterations has passed, allowing for
% the flow to evolve before igniting the mixture.
% NONE : no artificial solution ignition.
% By default, this option is set to NONE
FLAME_INIT_METHOD= FLAME_FRONT

% Enable preferential diffusion for progress variable, total enthalpy, mixture fraction FGM problems.
% If 'YES', the preferential diffusion model from Efimov et al.(2021) is used for computing the viscous residual terms.
% If enabled, make sure the variables "Beta_ProgVar", "Beta_Enth_Thermal", "Beta_Enth", and "Beta_MixFrac", corresponding
% to the preferential diffusion terms of the progress variable, temperature, total enthalpy, and mixture fraction
% respectively are included in the manifold.
% By default, this option is disabled.
PREFERENTIAL_DIFFUSION= NO

% FLAME_FRONT initialization
% the flame is initialized using a plane, defined by a point and a normal. On one side, the solution is initialized
% using 'burnt' conditions and on the other side 'unburnt' conditions. The normal points in the direction of the 'burnt'
% condition.
% (x1,x2,x3) = point on the plane.
% (x4,x5,x6) = normal of the plane.
% (x7) = thickness of the reaction zone, this is the transition from unburnt to burnt conditions.
% (x8) = Thickness of the 'burnt' zone, after this length, the conditions will be 'unburnt' again.
FLAME_INIT= (0.004, 0.0, 0.0, 1.0, 0.0, 0.0, 0.2e-3, 1.0)

% SPARK initialization
% the solution is ignited through application of a set of source terms within a specified region for a set number
% of solver iterations. This artificial spark can be applied after a certain number of iterations has passed, allowing for
% the flow to evolve before igniting the mixture.
% (x1,x2,x3) = spark center location.
% (x4) = spark radius where within the artificial spark is applied.
% (x5,x6) = spark iteration start and number of iterations in which the artifical spark is applied. For single-zone problems
% the number of iterations are inner-loop iterations, for multi-zone problems, outer-loop iterations are considered.
SPARK_INIT= (0.004, 0.0, 0.0, 1e-4, 100, 10)

% Source terms (density times species time rate of change) applied to the species equations in the spark region for the duration of the spark.
% The number of terms should equate the total number of species in the flamelet problem.
SPARK_REACTION_RATES= (1000, 0, 0)

% Thickened flame correction
% Approximate the thickness of the flame and suppress source terms and enhance diffusivity in cells with a lengthscale higher
% than the flame thickness.
THICKENED_FLAME_CORRECTION= YES

%
% --------------------- INVERSE DESIGN SIMULATION -----------------------------%
%
% Evaluate an inverse design problem using Cp (NO, YES)
INV_DESIGN_CP= NO
%
% Evaluate an inverse design problem using heat flux (NO, YES)
INV_DESIGN_HEATFLUX= NO

% ----------------------- BODY FORCE DEFINITION -------------------------------%
%
% Apply a body force as a source term (NO, YES)
BODY_FORCE= NO
%
% Vector of body force values (BodyForce_X, BodyForce_Y, BodyForce_Z)
BODY_FORCE_VECTOR= ( 0.0, 0.0, 0.0 )

% --------------------------- VORTICITY_CONFINEMENT ---------------------------%
%
% Enable vorticity confinement (YES/NO)
VORTICITY_CONFINEMENT = NO
% Set confinement parameter (0.00 by default)
CONFINEMENT_PARAM = 0.00

% --------------------- STREAMWISE PERIODICITY DEFINITION ---------------------%
%
% Generally for streamwise periodictiy one has to set MARKER_PERIODIC= (<inlet>, <outlet>, ...)
% appropriately as a boundary condition.
%
% Specify type of streamwise periodictiy (default=NONE, PRESSURE_DROP, MASSFLOW)
KIND_STREAMWISE_PERIODIC= NONE
%
% Delta P [Pa] value that drives the flow as a source term in the momentum equations.
% Defaults to 1.0.
STREAMWISE_PERIODIC_PRESSURE_DROP= 1.0
%
% Target massflow [kg/s]. Necessary pressure drop is determined iteratively.
% Initial value is given via STREAMWISE_PERIODIC_PRESSURE_DROP. Default value 1.0.
% Use INC_OUTLET_DAMPING as a relaxation factor. Default value 0.1 is a good start.
STREAMWISE_PERIODIC_MASSFLOW= 0.0
%
% Use streamwise periodic temperature (default=NO, YES)
% If NO, the heatflux is taken out at the outlet.
% This option is only necessary if INC_ENERGY_EQUATION=YES
STREAMWISE_PERIODIC_TEMPERATURE= NO
%
% Prescribe integrated heat [W] extracted at the periodic "outlet".
% Only active if STREAMWISE_PERIODIC_TEMPERATURE= NO.
% If set to zero, the heat is integrated automatically over all present MARKER_HEATFLUX.
% Upon convergence, the area averaged inlet temperature will be INC_TEMPERATURE_INIT.
% Defaults to 0.0.
STREAMWISE_PERIODIC_OUTLET_HEAT= 0.0

% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Euler wall boundary marker(s) (NONE = no marker)
% Implementation identical to MARKER_SYM.
MARKER_EULER= ( airfoil )
%
% Navier-Stokes (no-slip), constant heat flux wall  marker(s) (NONE = no marker)
% Format: ( marker name, constant heat flux (J/m^2), ... )
MARKER_HEATFLUX= ( NONE )
%
% Navier-Stokes (no-slip), heat-transfer/convection wall marker(s) (NONE = no marker)
% Available for compressible and incompressible flow.
% Format: ( marker name, constant heat-transfer coefficient (J/(K*m^2)), constant reservoir Temperature (K) ... )
MARKER_HEATTRANSFER= ( NONE )
%
% Navier-Stokes (no-slip), isothermal wall marker(s) (NONE = no marker)
% Format: ( marker name, constant wall temperature (K), ... )
MARKER_ISOTHERMAL= ( NONE )
%
% Wall species boundary condition marker(s) for species transport (NONE = no marker)
% Specify either a Neumann flux boundary condition (FLUX) or a Dirichlet value boundary condition (VALUE)
% for each species independently. All markers must specify the same number of species.
% Format: ( marker_name, BC_TYPE_1, value_1, BC_TYPE_2, value_2, ..., BC_TYPE_N, value_N, ... )
% where BC_TYPE is either FLUX (Neumann) or VALUE (Dirichlet) for each species
% Example for 3 species: MARKER_WALL_SPECIES= (wall1, FLUX, 0.0, VALUE, 0.3, VALUE, 0.2, wall2, VALUE, 0.1, VALUE, 0.4, FLUX, 0.0)
% If MARKER_WALL_SPECIES is not specified, a zero-flux boundary condition will be used.
MARKER_WALL_SPECIES= ( NONE )
%
% Far-field boundary marker(s) (NONE = no marker)
MARKER_FAR= ( farfield )
%
% Symmetry boundary marker(s) (NONE = no marker)
% Implementation identical to MARKER_EULER.
MARKER_SYM= ( NONE )
%
% Internal boundary marker(s) e.g. no boundary condition (NONE = no marker)
MARKER_INTERNAL= ( NONE )
%
% Near-Field boundary marker(s) (NONE = no marker)
MARKER_NEARFIELD= ( NONE )
%
%
% Inlet boundary type (TOTAL_CONDITIONS, MASS_FLOW)
INLET_TYPE= TOTAL_CONDITIONS
%
% Read inlet profile from a file (YES, NO) default: NO
SPECIFIED_INLET_PROFILE= NO
%
% File specifying inlet profile
INLET_FILENAME= inlet.dat
%
% If a file is provided to specify the inlet profile,
% this tolerance will be used to match the coordinates in the input file to
% the points on the grid.
% INLET_MATCHING_TOLERANCE= 1e-6
%
% Type of spanwise interpolation to use for the inlet face (LINEAR_1D, AKIMA_1D, CUBIC_1D).
INLET_INTERPOLATION_FUNCTION= NONE
%
% Type of radial spanwise interpolation type for the inlet face (VR_VTHETA or ALPHA_PHI).
INLET_INTERPOLATION_DATA_TYPE= VRVTHETA
%
% Write interpolated inlet vertex data to the file Interpolated_Data_<MARKERNAME>.dat
PRINT_INLET_INTERPOLATED_DATA= NO
%
% Inlet boundary marker(s) with the following formats (NONE = no marker)
% Total Conditions: (inlet marker, total temp, total pressure, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
% Mass Flow: (inlet marker, density, velocity magnitude, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
% Inc. Velocity: (inlet marker, temperature, velocity magnitude, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
% Inc. Pressure: (inlet marker, temperature, total pressure, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
MARKER_INLET= ( NONE )
%
% Outlet boundary marker(s) (NONE = no marker)
% Compressible: ( outlet marker, back pressure (static thermodynamic), ... )
% Inc. Pressure: ( outlet marker, back pressure (static gauge in Pa), ... )
% Inc. Mass Flow: ( outlet marker, mass flow target (kg/s), ... )
MARKER_OUTLET= ( NONE )
%
% Propeller blade element actuator disk double surface (inlet, outlet) boundary condition
ACTDISK_DOUBLE_SURFACE = NO
%
% Actuator disk boundary type (VARIABLE_LOAD, VARIABLES_JUMP, BC_THRUST,
%                              DRAG_MINUS_THRUST, BLADE_ELEMENT)
ACTDISK_TYPE= VARIABLES_JUMP
%
% Actuator disk boundary marker(s) with the following formats (NONE = no marker)
% Variable Load: (inlet face marker, outlet face marker, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0)
% Variables Jump: ( inlet face marker, outlet face marker,
%                   Takeoff pressure jump (psf), Takeoff temperature jump (R), Takeoff rev/min,
%                   Cruise  pressure jump (psf), Cruise temperature jump (R), Cruise rev/min )
% BC Thrust: ( inlet face marker, outlet face marker,
%              Takeoff BC thrust (lbs), 0.0, Takeoff rev/min,
%              Cruise BC thrust (lbs), 0.0, Cruise rev/min )
% Drag-Thrust: ( inlet face marker, outlet face marker,
%                Takeoff Drag-Thrust (lbs), 0.0, Takeoff rev/min,
%                Cruise Drag-Thrust (lbs), 0.0, Cruise rev/min )
% Blade element: ( inlet face marker, outlet face marker,
%                  Takeoff Drag-Thrust (lbs), 0.0, Takeoff rev/min,
%                  Cruise Drag-Thrust (lbs), 0.0, Cruise rev/min )
MARKER_ACTDISK= ( NONE )
%
% Blade element: ( inlet face marker, outlet face marker,
%                  X_CG of inlet, Y_CG of inlet, Z_CG of inlet,
%                  X_CG of outlet, Y_CG of outlet, Z_CG of outlet )
MARKER_ACTDISK_BEM_CG= ( NONE )
%
% Blade element: ( inlet face marker, outlet face marker,
%                  X_Axis of inlet, Y_Axis of inlet, Z_Axis of inlet,
%                  X_Axis of outlet, Y_Axis of outlet, Z_Axis of outlet )
MARKER_ACTDISK_BEM_AXIS= ( NONE )
%
% Actuator disk data input file name
ACTDISK_FILENAME= actuatordisk.dat
%
% Propeller blade element section and aerodynamic data input file name
BEM_PROP_FILENAME = prop_geom_alfclcd_data.txt
%
% Propeller blade angle (degrees) at (0.75 * radius)
BEM_PROP_BLADE_ANGLE = 25.0
%
% BEM calculation frequency
BEM_FREQ = 40
%
% Supersonic inlet boundary marker(s) (NONE = no marker)
% Format: (inlet marker, temperature, static pressure, velocity_x,
%           velocity_y, velocity_z, ... ), i.e. primitive variables specified.
MARKER_SUPERSONIC_INLET= ( NONE )
%
% Supersonic outlet boundary marker(s) (NONE = no marker)
MARKER_SUPERSONIC_OUTLET= ( NONE )
%
% Periodic boundary marker(s) (NONE = no marker)
% Format: ( periodic marker, donor marker, rotation_center_x, rotation_center_y,
% rotation_center_z, rotation_angle_x-axis, rotation_angle_y-axis,
% rotation_angle_z-axis, translation_x, translation_y, translation_z, ... )
MARKER_PERIODIC= ( NONE )
%
% Engine Inflow boundary type (FAN_FACE_MACH, FAN_FACE_PRESSURE, FAN_FACE_MDOT)
ENGINE_INFLOW_TYPE= FAN_FACE_MACH
%
% Engine inflow boundary marker(s) (NONE = no marker)
% Format: (engine inflow marker, fan face Mach, ... )
MARKER_ENGINE_INFLOW= ( NONE )
%
% Engine exhaust boundary marker(s) with the following formats (NONE = no marker)
% Format: (engine exhaust marker, total nozzle temp, total nozzle pressure, ... )
MARKER_ENGINE_EXHAUST= ( NONE )
%
% Flag to allow mass-flow rate coupling between all exhaust surfaces and the engine inlet (YES, NO)
ENGINE_EXHAUST_TO_INLET= NO
%
% Displacement boundary marker(s) (NONE = no marker)
% Format: ( displacement marker, displacement value normal to the surface, ... )
MARKER_NORMAL_DISPL= ( NONE )
%
% Pressure boundary marker(s) (NONE = no marker)
% Format: ( pressure marker )
MARKER_PRESSURE= ( NONE )
%
% Riemann boundary marker(s) (NONE = no marker)
% Format: (marker, data kind flag, list of data)
MARKER_RIEMANN= ( NONE )
%
% Shroud boundary marker(s) (NONE = no marker)
% Format: (marker)
% If the ROTATING_FRAME option is activated, this option force
% the velocity on the boundaries specified to 0.0
MARKER_SHROUD= (NONE)
%
% Interface (s) definition, identifies the surface shared by
% two different zones. The interface is defined by listing pairs of
% markers (one from each zone connected by the interface)
% Example:
%   Given an arbitrary number of zones (A, B, C, ...)
%   A and B share a surface, interface 1
%   A and C share a surface, interface 2
% Format: ( marker_A_on_interface_1, marker_B_on_interface_1,
%           marker_A_on_interface_2, marker_C_on_interface_2, ... )
%
MARKER_ZONE_INTERFACE= ( NONE )
%
% CHT interface boundary marker(s)
MARKER_CHT_INTERFACE= ( NONE )
%
% Specifies the interface (s)
% The kind of interface is defined by listing pairs of markers (one from each
% zone connected by the interface)
% Example:
%   Given an arbitrary number of zones (A, B, C, ...)
%   A and B share a surface, interface 1
%   A and C share a surface, interface 2
% Format: ( marker_A_on_interface_1, marker_B_on_interface_1,
%           marker_A_on_interface_2, marker_C_on_interface_2, ... )
%
MARKER_FLUID_INTERFACE= ( NONE )
%
% Marker(s) in which the flow load is computed/applied
MARKER_FLUID_LOAD= ( NONE )
%
% Kind of interface interpolation among different zones (NEAREST_NEIGHBOR, WEIGHTED_AVERAGE,
%                                                        ISOPARAMETRIC, RADIAL_BASIS_FUNCTION)
KIND_INTERPOLATION= NEAREST_NEIGHBOR
%
% Use conservative approach for interpolating between meshes
CONSERVATIVE_INTERPOLATION= YES
%
% Type of radial basis function to use for radial basis function interpolation
% (WENDLAND_C2, INV_MULTI_QUADRIC, GAUSSIAN, THIN_PLATE_SPLINE, MULTI_QUADRIC).
KIND_RADIAL_BASIS_FUNCTION = WENDLAND_C2
%
% Radius for radial basis function.
RADIAL_BASIS_FUNCTION_PARAMETER = 0.015
%
% Use polynomial term in radial basis function interpolation.
RADIAL_BASIS_FUNCTION_POLYNOMIAL_TERM = YES
%
% Tolerance to prune small coefficients from the RBF interpolation matrix.
RADIAL_BASIS_FUNCTION_PRUNE_TOLERANCE = 0
%
% Inflow and Outflow markers must be specified, for each blade (zone), following
% the natural groth of the machine (i.e, from the first blade to the last)
MARKER_TURBOMACHINERY= ( NONE )
%
% Integer number of spanwise sections to compute 3D turbo BC and Performance for turbomachinery
NUM_SPANWISE_SECTIONS= 1
%
% type of algorithm to identify the span-wise sections at the turbo boundaries. 1 means automatic.
SPANWISE_KIND= 1
%
% Mixing-plane interface markers must be specified to activate the transfer of
% information between zones
MARKER_MIXINGPLANE_INTERFACE= ( NONE )
%
% Giles boundary condition for inflow, outflow and mixing-plane
% Format inlet:  ( marker, TOTAL_CONDITIONS_PT, Total Pressure , Total Temperature,
% Flow dir-norm, Flow dir-tang, Flow dir-span, under-relax-avg, under-relax-fourier)
% Format outlet: ( marker, STATIC_PRESSURE, Static Pressure value, -, -, -, -, under-relax-avg, under-relax-fourier)
% Format mixing-plane in and out: ( marker, MIXING_IN or MIXING_OUT, -, -, -, -, -, -, under-relax-avg, under-relax-fourier)
MARKER_GILES= ( NONE )
%
% This option insert an extra under relaxation factor for the Giles BC at the hub
% and shroud (under relax factor applied, span percentage to under relax)
GILES_EXTRA_RELAXFACTOR= ( 0.05, 0.05)
%
% YES Non reflectivity activated, NO the Giles BC behaves as a normal 1D characteristic-based BC
SPATIAL_FOURIER= NO
%
% Catalytic wall marker(s) (NONE = no marker)
% Format: ( marker name, ... )
CATALYTIC_WALL= ( NONE )
% specify if catalytic wall is a supercatalytic wall
SUPERCATALYTIC_WALL= NO
% species composition at the supercatalytic wall
SUPERCATALYTIC_WALL_COMPOSITION= (0,0,0)
% catalytic efficiency
CATALYTIC_EFFICIENCY= 0.2
%
% Inlet Turbulent boundary marker(s) with the following format:
% SA Model: (inlet_marker1, NuFactor1, inlet_marker2, NuFactor2, ...)
% SST Model: (inlet_marker1, TurbIntensity1, RatioTurbLamViscosity1, inlet_marker2, TurbIntensity2, RatioTurbLamViscosity2, ...)
MARKER_INLET_TURBULENT= (inlet1, 0.05, 15, inlet2, 0.02, ...)
%
% Custom boundary marker(s) (this has to be implemented by users in the code).
MARKER_CUSTOM= ( NONE )
%
% Smoluchowski/Maxwell slip wall boundary marker(s)
MARKER_SMOLUCHOWSKI_MAXWELL= ( NONE )
%
% Clamped boundary marker(s)
MARKER_CLAMPED= ( NONE )
%
% Load boundary marker(s)
MARKER_DAMPER= ( NONE )
%
% Load boundary marker(s)
% Format: (inlet marker, load, multiplier, dir_x, dir_y, dir_z, ... ),
% i.e. primitive variables specified.
MARKER_LOAD= ( NONE )
%
% option to apply the load as a sine
SINE_LOAD= NO
% the 1st coeff is the amplitude,
% the 2nd is the frequency,
% the 3rd is the phase in radians
SINE_LOAD_COEFF= (0.0, 0.0, 0.0)
%
RAMP_AND_RELEASE_LOAD= NO
%
% Apply the load as a ramp
RAMP_LOADING= NO
%
% Time while the load is to be increased linearly
RAMP_TIME= 1.0
%
% Number of FSI iterations during which a ramp is applied
RAMP_FSI_ITER= 2
%
% Aitken static relaxation factor
STAT_RELAX_PARAMETER= 0.4
%
% Aitken dynamic maximum relaxation factor for the first iteration
AITKEN_DYN_MAX_INITIAL= 0.5
%
% Aitken dynamic minimum relaxation factor for the first iteration
AITKEN_DYN_MIN_INITIAL= 0.5
%
% Kind of relaxation
BGS_RELAXATION= NONE
%
% Relaxation required
RELAXATION= NO
%
% Transfer method used for multiphysics problems
DYNAMIC_LOAD_TRANSFER= RAMP
%
% Load boundary marker(s)
% Format: (inlet marker, load, multiplier, dir_x, dir_y, dir_z, ... ),
% i.e. primitive variables specified.
MARKER_DISPLACEMENT= ( NONE )

% ------------------------ WALL ROUGHNESS DEFINITION --------------------------%
% The equivalent sand grain roughness height (k_s) on each of the wall. This must be in m.
% This is a list of (string, double) each element corresponding to a wall marker.
WALL_ROUGHNESS = (wall1, ks1, wall2, ks2)
%WALL_ROUGHNESS = (wall1, ks1, wall2, 0.0) %is also allowed
%
% Roughness model used for SST (WILCOX1998, WILCOX2006, LIMITER_KNOPP, LIMITER_AUPOIX).
KIND_ROUGHSST_MODEL = WILCOX1998

% ------------------------ WALL FUNCTION DEFINITION --------------------------%
%
% The von Karman constant, the constant below only affects the standard wall function model
WALLMODEL_KAPPA= 0.41
%
% The wall function model constant B
WALLMODEL_B= 5.5
%
% The y+ value below which the wall function is switched off and we resolve the wall
WALLMODEL_MINYPLUS= 5.0
%
% [Expert] Max Newton iterations used for the standard wall function
WALLMODEL_MAXITER= 200
%
% [Expert] relaxation factor for the Newton iterations of the standard wall function
WALLMODEL_RELFAC= 0.5

% ------------------------ CONJUGATE HEAT TRANSFER (CHT) --------------------------%
%
% Relaxation of the CHT coupling
RELAXATION_FACTOR_CHT= 1.0
%
% CHT interface coupling methods
CHT_COUPLING_METHOD= DIRECT_TEMPERATURE_ROBIN_HEATFLUX

% ------------------------ SURFACES IDENTIFICATION ----------------------------%
%
% Marker(s) of the surface in the surface flow solution file
MARKER_PLOTTING = ( airfoil )
%
% Marker(s) of the surface where the non-dimensional coefficients are evaluated.
MARKER_MONITORING = ( airfoil )
%
% Viscous wall markers for which wall functions must be applied. (NONE = no marker)
% Format: ( marker name, wall function type -NO_WALL_FUNCTION, STANDARD_WALL_FUNCTION,
%           ADAPTIVE_WALL_FUNCTION, SCALABLE_WALL_FUNCTION, EQUILIBRIUM_WALL_MODEL,
%           NONEQUILIBRIUM_WALL_MODEL-, ... )
MARKER_WALL_FUNCTIONS= ( airfoil, NO_WALL_FUNCTION )
%
% Marker(s) of the surface where custom thermal BC's are defined.
MARKER_PYTHON_CUSTOM = ( NONE )
%
% Marker(s) of the surface where obj. func. (design problem) will be evaluated
MARKER_DESIGNING = ( airfoil )
%
% Marker(s) of the surface that is going to be analyzed in detail (massflow, average pressure, distortion, etc)
MARKER_ANALYZE = ( airfoil )
%
% Method to compute the average value in MARKER_ANALYZE (AREA, MASSFLUX).
MARKER_ANALYZE_AVERAGE = MASSFLUX
%
% Duplicate markers while reading the mesh. Currently this is only used for thermoelastic simulations
% to allow specifying two boundary conditions (thermal and structural) on the same boundary.
MARKER_CREATE_COPY= ( original_1, copy_1, ..., original_n, copy_n )

% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
% Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES)
NUM_METHOD_GRAD= GREEN_GAUSS
%
% Numerical method for spatial gradients to be used for MUSCL reconstruction
% Options are (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES, LEAST_SQUARES). Default value is
% NONE and the method specified in NUM_METHOD_GRAD is used.
NUM_METHOD_GRAD_RECON = LEAST_SQUARES
%
% CFL number (initial value for the adaptive CFL number)
CFL_NUMBER= 15.0
%
% Adaptive CFL number (NO, YES)
CFL_ADAPT= NO
%
% Parameters of the adaptive CFL number (factor-down, factor-up, CFL min value,
%                                        CFL max value, acceptable linear solver convergence, starting iteration)
% After the starting iteration has passed, local CFL increases by factor-up until max if the solution rate of
% change is not limited, and acceptable linear convergence is achieved. It is reduced if rate is limited, or if there
% is not enough linear convergence, or if the nonlinear residuals are stagnant and oscillatory.
% It is reset back to min when linear solvers diverge, or if nonlinear residuals increase too much.
CFL_ADAPT_PARAM= ( 0.1, 2.0, 10.0, 1e10, 0.001, 0)
%
% Maximum Delta Time in local time stepping simulations
MAX_DELTA_TIME= 1E6
%
% External iteration offset due to restart
EXT_ITER_OFFSET= 0
%
% Runge-Kutta alpha coefficients
RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 )
%
% Objective function in gradient evaluation  (DRAG, LIFT, SIDEFORCE, MOMENT_X,
%                                             MOMENT_Y, MOMENT_Z, EFFICIENCY, BUFFET,
%                                             EQUIVALENT_AREA, NEARFIELD_PRESSURE,
%                                             FORCE_X, FORCE_Y, FORCE_Z, THRUST,
%                                             TORQUE, TOTAL_HEATFLUX, CUSTOM_OBJFUNC
%                                             MAXIMUM_HEATFLUX, INVERSE_DESIGN_PRESSURE,
%                                             INVERSE_DESIGN_HEATFLUX, SURFACE_TOTAL_PRESSURE,
%                                             SURFACE_MASSFLOW, SURFACE_STATIC_PRESSURE, SURFACE_MACH)
% For a weighted sum of objectives: separate by commas, add OBJECTIVE_WEIGHT and MARKER_MONITORING in matching order.
OBJECTIVE_FUNCTION= DRAG
%
% List of weighting values when using more than one OBJECTIVE_FUNCTION. Separate by commas and match with MARKER_MONITORING.
OBJECTIVE_WEIGHT = 1.0
%
% Expression used when "OBJECTIVE_FUNCTION= CUSTOM_OBJFUNC", any history/screen output can be used together with common
% math functions (sqrt, cos, exp, etc.). This can be used for constraint aggregation (as below) or to compute something
% SU2 does not, see TestCases/user_defined_functions/.
CUSTOM_OBJFUNC= 'DRAG + 10 * pow(fmax(0.4-LIFT, 0), 2)'

% ----------- SLOPE LIMITER AND DISSIPATION SENSOR DEFINITION -----------------%
%
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the flow equations.
%           Required for 2nd order upwind schemes (NO, YES)
MUSCL_FLOW= YES
%
% Option to ramp the MUSCL reconstruction scheme gradually from first to second order
RAMP_MUSCL= NO
%
% Coefficients for the MUSCL ramp, 1st is ramp start iteration,
% 2nd is the ramp update frequency, 3rd is the total number of iterations of the ramp
RAMP_MUSCL_COEFF= (1000.0, 10.0, 500.0)
%
% Value for modifying how aggresively the ramp is applied (cannot be less than or equal to 0)
% < 1 = Aggresive ramp up early, slower later, > 1 slow initial ramping, more aggresive towards end
RAMP_MUSCL_POWER = 1
%
% Type of MUSCL ramp function used
% ITERATION = [min(1.0, iter/endIter)]^RAMP_MUSCL_POWER
% SMOOTH_FUNCTION = [1/2 * ( 1 - cos ( pi * min(1.0, iter/endIter)))]^RAMP_MUSCL_POWER
KIND_MUSCL_RAMP= ITERATION
%
% Coefficient for blending upwind and central differences in MUSCL scheme.
% Values range from -1 (fully one-sided) to 1 (central difference).
MUSCL_KAPPA_FLOW= 0.0
%
% Slope limiter (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG, BARTH_JESPERSEN, VAN_ALBADA_EDGE,
%                NISHIKAWA_R3, NISHIKAWA_R4, NISHIKAWA_R5)
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN
%
% Same as MUSCL_FLOW but for turbulence.
%
MUSCL_TURB= NO
%
% Same as MUSCL_KAPPA_FLOW but for turbulence.
%
MUSCL_KAPPA_TURB= 0.0
%
% Slope limiter (same as SLOPE_LIMITER_FLOW except VAN_ALBADA_EDGE)
%
SLOPE_LIMITER_TURB= VENKATAKRISHNAN
%
% Same as MUSCL_FLOW but for the continuous adjoint equations.
%
MUSCL_ADJFLOW= YES
%
% Same as MUSCL_KAPPA_FLOW but for the continuous adjoint equations.
%
MUSCL_KAPPA_ADJFLOW= 0.0
%
% Slope limiter (same as SLOPE_LIMITER_FLOW plus SHARP_EDGES, WALL_DISTANCE)
%
SLOPE_LIMITER_ADJFLOW= VENKATAKRISHNAN
%
% Same as MUSCL_FLOW but for continuous adjoint turbulence equations.
%
MUSCL_ADJTURB= NO
%
% Slope limiter (see SLOPE_LIMITER_ADJFLOW)
%
SLOPE_LIMITER_ADJTURB= VENKATAKRISHNAN
%
% Coefficient for Venkatakrishnan-type limiters (upwind scheme).
% A larger value decreases the extent of limiting, values approaching zero
% cause lower-order approximation to the solution (0.05 by default)
VENKAT_LIMITER_COEFF= 0.05
%
% Reference coefficient for detecting sharp edges (3.0 by default).
REF_SHARP_EDGES = 3.0
%
% Coefficient for the adjoint sharp edges limiter (3.0 by default).
ADJ_SHARP_LIMITER_COEFF= 3.0
%
% Remove sharp edges from the sensitivity evaluation (NO, YES)
SENS_REMOVE_SHARP = NO
%
SENS_SMOOTHING= NONE
%
% Freeze the value of the limiter after a number of iterations
LIMITER_ITER= 999999
%
% 1st order artificial dissipation coefficients for
%     the Lax–Friedrichs method ( 0.15 by default )
LAX_SENSOR_COEFF= 0.15
%
% 2nd and 4th order artificial dissipation coefficients for
%     the JST method ( 0.5, 0.02 by default )
JST_SENSOR_COEFF= ( 0.5, 0.02 )
%
% 1st order artificial dissipation coefficients for
%     the adjoint Lax–Friedrichs method ( 0.15 by default )
ADJ_LAX_SENSOR_COEFF= 0.15
%
% 2nd, and 4th order artificial dissipation coefficients for
%     the adjoint JST method ( 0.5, 0.02 by default )
ADJ_JST_SENSOR_COEFF= ( 0.5, 0.02 )

% ------------------------ LINEAR SOLVER DEFINITION ---------------------------%
%
% Linear solver or smoother for implicit formulations:
% BCGSTAB, FGMRES, FGCRODR, RESTARTED_FGMRES, CONJUGATE_GRADIENT (self-adjoint problems only), SMOOTHER.
LINEAR_SOLVER= FGMRES

% Inner solver used for nested preconditioning (BCGSTAB is only possible with flexible linear solvers).
% Options: NONE, BCGSTAB, SMOOTHER
% Inner BCGSTAB does up to the number of iterations of the outer solver or sqrt(LINEAR_SOLVER_ERROR).
% Inner SMOOTHER does max(2, sqrt(LINEAR_SOLVER_ITER))
LINEAR_SOLVER_INNER= NONE

% Same for discrete adjoint (smoothers not supported), replaces LINEAR_SOLVER in SU2_*_AD codes.
DISCADJ_LIN_SOLVER= FGMRES
%
% Use CUDA GPU Acceleration for FGMRES Linear Solver Only
ENABLE_CUDA=NO
%
% Preconditioner of the Krylov linear solver or type of smoother (ILU, LU_SGS, LINELET, JACOBI)
LINEAR_SOLVER_PREC= ILU
%
% Same for discrete adjoint (JACOBI or ILU), replaces LINEAR_SOLVER_PREC in SU2_*_AD codes.
DISCADJ_LIN_PREC= ILU
%
% Linear solver ILU preconditioner fill-in level (0 by default)
LINEAR_SOLVER_ILU_FILL_IN= 0
%
% Minimum error of the linear solver for implicit formulations
LINEAR_SOLVER_ERROR= 1E-6
%
% Max number of iterations of the linear solver for the implicit formulation
LINEAR_SOLVER_ITER= 5
%
% Restart frequency for RESTARTED_FGMRES and FGCRODR
LINEAR_SOLVER_RESTART_FREQUENCY= 10
%
% Number of vectors used by FGCRODR for deflation
LINEAR_SOLVER_RESTART_DEFLATION= 4
%
% Relaxation factor for smoother-type solvers (LINEAR_SOLVER= SMOOTHER)
LINEAR_SOLVER_SMOOTHER_RELAXATION= 1.0

% -------------------------- MULTIGRID PARAMETERS -----------------------------%
%
% Multi-grid levels (0 = no multi-grid)
MGLEVEL= 0
%
% Multi-grid cycle (V_CYCLE, W_CYCLE, FULLMG_CYCLE)
MGCYCLE= V_CYCLE
%
% Multi-grid pre-smoothing level
MG_PRE_SMOOTH= ( 1, 2, 3, 3 )
%
% Multi-grid post-smoothing level
MG_POST_SMOOTH= ( 0, 0, 0, 0 )
%
% Jacobi implicit smoothing of the correction
MG_CORRECTION_SMOOTH= ( 0, 0, 0, 0 )
%
% Damping factor for the residual restriction
MG_DAMP_RESTRICTION= 0.75
%
% Damping factor for the correction prolongation
MG_DAMP_PROLONGATION= 0.75

% -------------------------- MESH SMOOTHING -----------------------------%
%
% Before each computation, implicitly smooth the nodal coordinates
SMOOTH_GEOMETRY= 0

% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
% Convective numerical method (JST, JST_KE, JST_MAT, LAX-FRIEDRICH, ROE, AUSM,
%                              AUSMPLUSUP, AUSMPLUSUP2, AUSMPLUSM, HLLC, TURKEL_PREC,
%                              SW, MSW, FDS, SLAU, SLAU2, L2ROE, LMROE)
CONV_NUM_METHOD_FLOW= ROE
%
% Roe Low Dissipation function for Hybrid RANS/LES simulations (FD, NTS, NTS_DUCROS)
ROE_LOW_DISSIPATION= FD
%
% Roe dissipation coefficient
ROE_KAPPA= 0.5
%
% Minimum value for beta for the Roe-Turkel preconditioner
MIN_ROE_TURKEL_PREC= 0.01
%
% Maximum value for beta for the Roe-Turkel preconditioner
MAX_ROE_TURKEL_PREC= 0.2
%
% Post-reconstruction correction for low Mach number flows (NO, YES)
LOW_MACH_CORR= NO
%
% Roe-Turkel preconditioning for low Mach number flows (NO, YES)
LOW_MACH_PREC= NO
%
% Use numerically computed Jacobians for AUSM+up(2) and SLAU(2)
% Slower per iteration but potentialy more stable and capable of higher CFL
USE_ACCURATE_FLUX_JACOBIANS= NO
%
% Use the vectorized version of the selected numerical method (available for JST family and Roe).
% SU2 should be compiled for an AVX or AVX512 architecture for best performance.
% NOTE: Currently vectorization always used for schemes that support it.
USE_VECTORIZATION= YES
%
% Entropy fix coefficient (0.0 implies no entropy fixing, 1.0 implies scalar
%                          artificial dissipation)
ENTROPY_FIX_COEFF= 0.0
%
% MSW coefficient for blending states based on pressure jump.
% Using 0 makes the scheme average left and right regardless of pressure.
MSW_ALPHA= 5.0
%
% Higher values than 1 (3 to 4) make the global Jacobian of central schemes (compressible flow
% only) more diagonal dominant (but mathematically incorrect) so that higher CFL can be used.
CENTRAL_JACOBIAN_FIX_FACTOR= 4.0
%
% Control numerical properties of the global Jacobian matrix using a multiplication factor
% for incompressible central schemes
CENTRAL_INC_JACOBIAN_FIX_FACTOR= 1.0
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_FLOW= EULER_IMPLICIT
%
% Use a Newton-Krylov method on the flow equations, see TestCases/rans/oneram6/turb_ONERAM6_nk.cfg
% For multizone discrete adjoint it will use FGMRES on inner iterations with restart frequency
% equal to "QUASI_NEWTON_NUM_SAMPLES".
NEWTON_KRYLOV= NO
%
% Integer parameters {startup iters, precond iters, initial tolerance relaxation}.
NEWTON_KRYLOV_IPARAM= (20, 3, 2)
%
% Double parameters {startup residual drop, precond tolerance, full tolerance residual drop, findiff step,
% and MUSCL relaxation for the finite difference products}.
NEWTON_KRYLOV_DPARAM= (-2.0, 0.1, -6.0, 1e-5, 1.0)

% ------------------- FEM FLOW NUMERICAL METHOD DEFINITION --------------------%
%
% FEM numerical method (DG)
NUM_METHOD_FEM_FLOW= DG
%
% Riemann solver used for DG (ROE, LAX-FRIEDRICH, AUSM, HLLC, VAN_LEER)
RIEMANN_SOLVER_FEM= ROE
%
% Constant factor applied for quadrature with straight elements (2.0 by default)
QUADRATURE_FACTOR_STRAIGHT_FEM = 2.0
%
% Constant factor applied for quadrature with curved elements (3.0 by default)
QUADRATURE_FACTOR_CURVED_FEM = 3.0
%
% Factor for the symmetrizing terms in the DG FEM discretization (1.0 by default)
THETA_INTERIOR_PENALTY_DG_FEM = 1.0
%
% Compute the entropy in the fluid model (YES, NO)
COMPUTE_ENTROPY_FLUID_MODEL= YES
%
% Use the lumped mass matrix for steady DGFEM computations (NO, YES)
USE_LUMPED_MASSMATRIX_DGFEM= NO
%
% Only compute the exact Jacobian of the spatial discretization (NO, YES)
JACOBIAN_SPATIAL_DISCRETIZATION_ONLY= NO
%
% Number of aligned bytes for the matrix multiplications. Multiple of 64. (128 by default)
ALIGNED_BYTES_MATMUL= 128
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, CLASSICAL_RK4_EXPLICIT, ADER_DG)
TIME_DISCRE_FEM_FLOW= RUNGE-KUTTA_EXPLICIT
%
% Number of time DOFs for the predictor step of ADER-DG (2 by default)
TIME_DOFS_ADER_DG= 2
% Factor applied during quadrature in time for ADER-DG. (2.0 by default)
%QUADRATURE_FACTOR_TIME_ADER_DG = 2.0
%
% Type of discretization used in the predictor step of ADER-DG (ADER_ALIASED_PREDICTOR, ADER_NON_ALIASED_PREDICTOR)
ADER_PREDICTOR= ADER_ALIASED_PREDICTOR
% Number of time levels for time accurate local time stepping. (1 by default, max. allowed 15)
LEVELS_TIME_ACCURATE_LTS= 1
%
% Specify the method for matrix coloring for Jacobian computations (GREEDY_COLORING, NATURAL_COLORING)
KIND_MATRIX_COLORING= GREEDY_COLORING
%
% Specify shock capturing method for DG
KIND_FEM_DG_SHOCK= NONE

% ------------------- TOPOLOGY OPTIMIZATION --------------------%
%
% "Classic" density approach to topology optimization. Each element is
% assigned a density variable that is used to penalize its stiffness.
TOPOLOGY_OPTIMIZATION= NO
%
% Output file for the derivatives of the OBJECTIVE_FUNCTION w.r.t. the
% design densities.
TOPOL_OPTIM_OUTFILE= element_derivatives.dat
%
% The penalization exponent for the Simplified Isotropic Material with
% Penalization.
TOPOL_OPTIM_SIMP_EXPONENT= 1.0
%
% The stiffness of void elements (normalized by ELASTICITY_MODULUS)
TOPOL_OPTIM_SIMP_MINSTIFF= 0.001
%
% Filtering is required to avoid numerical issues, see [Sigmund, 2007]
% (DOI 10.1007/s00158-006-0087-x). Currently available options:
% CONSTANT;  CONICAL (default);  GAUSSIAN;  DILATE;  ERODE.
% The filter can have multiple sequential stages (2 in this case).
TOPOL_OPTIM_FILTER_KERNEL= (DILATE, ERODE)
%
% Each kernel can have its own radius (R1, R2, ...) or one value can be
% specified for all.
TOPOL_OPTIM_FILTER_RADIUS= 0.0
%
% The Gaussian, Erode, and Dilate filters, have a constant parameter.
% Again this can be a list.
TOPOL_OPTIM_KERNEL_PARAM= 0.01
%
% The filtering may become very expensive if the mesh has very refined
% regions. If different from 0 this option mitigates that by limiting the
% "logical radius" (for immediate neighbors that radius is 1, etc.).
TOPOL_OPTIM_SEARCH_LIMIT= 0
%
% After the filtering, a projection step can be applied to increase the
% solid-void contrast, i.e. the discreteness of the solution. Options:
% NO_PROJECTION (default);  HEAVISIDE_UP;  HEAVISIDE_DOWN.
TOPOL_OPTIM_PROJECTION_TYPE= NO_PROJECTION
%
% The continuous Heaviside function (step) approximations require a
% parameter, large value equals more discrete.
TOPOL_OPTIM_PROJECTION_PARAM= 0.0

% ------------------- FEA SOLVER FOR FLUID-STRUCTURE INTERACTION --------------------%
%
% Filename to input for element-based properties
FEA_FILENAME= default_element_properties.dat
%
% Determine if advanced features are used from the element-based FEA analysis (NO, YES = experimental)
FEA_ADVANCED_MODE= NO
%
% Modulus of elasticity
ELASTICITY_MODULUS= 1000.0
%
% Poisson ratio
POISSON_RATIO= 0.35
%
% Thermal expansion coefficient
MATERIAL_THERMAL_EXPANSION_COEFF= 0
%
% Freestream temperature at which there is no stress from thermal expansion
MATERIAL_REFERENCE_TEMPERATURE= 288.15
%
% Knowles B constant
KNOWLES_B= 1.0
%
% Knowles N constant
KNOWLES_N= 1.0
%
% ID of the region we want to compute the sensitivities using direct differentiation
FEA_ID_DIRECTDIFF= 0
%
RESTART_STEADY_STATE= NO
%
% Time discretization
TIME_DISCRE_FEA= NEWMARK_IMPLICIT
%
% Iterative method for non-linear structural analysis
NONLINEAR_FEM_SOLUTION_METHOD= NEWTON_RAPHSON
%
% Pseudo static analysis (no density in dynamic analysis)
PSEUDO_STATIC= NO
%
% Parameter alpha for Newmark scheme (s)
NEWMARK_BETA= 0.25
%
% Parameter gamma for Newmark scheme (s)
NEWMARK_GAMMA= 0.50
%
% Newmark - Generalized alpha - coefficients
TIME_INT_STRUCT_COEFFS= 0.0
%
% Apply dead loads
INCREMENTAL_LOAD= NO
%
% Maximum number of increments of the
NUMBER_INCREMENTS= 10
%
% Definition of the  UTOL RTOL ETOL
INCREMENTAL_CRITERIA= (0.0, 0.0, 0.0)
%
% Use of predictor
PREDICTOR= NO
%
% Order of the predictor
PREDICTOR_ORDER= 0
%
% Geometric conditions
GEOMETRIC_CONDITIONS= SMALL_DEFORMATIONS
%
% Material model
MATERIAL_MODEL= LINEAR_ELASTIC
%
% Compressibility of the material
MATERIAL_COMPRESSIBILITY= COMPRESSIBLE
%
% Formulation for 2-dimensional elasticity solver
FORMULATION_ELASTICITY_2D= PLANE_STRAIN
%
% -------------------- Dielectric effects  ------------------%
%
% Include DE effects
DE_EFFECTS= NO
%
% Value of the Dielectric Elastomer constant
ELECTRIC_FIELD_CONST= 4.25e-11
%
% Modulus of the Electric Fields
ELECTRIC_FIELD_MOD= 20e5
%
% Direction of the Electic Fields
ELECTRIC_FIELD_DIR= (0.0, 1.0)
%
% ------------------------ Prestretch -----------------------%
%
% Consider a prestretch in the structural domain
PRESTRETCH= NO
%
% Filename to input for prestretching membranes
PRESTRETCH_FILENAME= prestretch_file
%
% ----------------------- Body Forces -----------------------%
%
% Centrifugal forces due to ROTATION_RATE around MOTION_ORIGIN.
% GRAVITY_FORCE and BODY_FORCE can also be used with the FEA solver.
CENTRIFUGAL_FORCE= NO

% -------------------- Weakly Coupled Heat ------------------%
%
WEAKLY_COUPLED_HEAT_EQUATION= NO
%
% -------------------- TURBULENT NUMERICAL METHOD DEFINITION ------------------%
%
% Convective numerical method (SCALAR_UPWIND, BOUNDED_SCALAR)
CONV_NUM_METHOD_TURB= SCALAR_UPWIND
%
% Time discretization (EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_TURB= EULER_IMPLICIT
%
% Reduction factor of the CFL coefficient in the turbulence problem
CFL_REDUCTION_TURB= 1.0

% Control lower limit constants of the SST model (C*phi_infinity)
LOWER_LIMIT_K_FACTOR= 1e-15
LOWER_LIMIT_OMEGA_FACTOR= 1e-5

% Use numerically computed exact Jacobians for turbulence models
% Slower per iteration but potentialy more stable and capable of higher CFL
USE_ACCURATE_TURB_JACOBIANS= NO
%
% --------------------- HEAT NUMERICAL METHOD DEFINITION ----------------------%
%
% Value of the thermal diffusivity
THERMAL_DIFFUSIVITY= 1.0
%
% Convective numerical method for the heat equation (only SCALAR_UPWIND)
CONV_NUM_METHOD_HEAT= SCALAR_UPWIND
%
% Check if the MUSCL scheme should be used
MUSCL_HEAT= YES
%
% Same as MUSCL_KAPPA_FLOW but for the heat equation.
MUSCL_KAPPA_HEAT= 0.0
%
% Slope limiter for the heat equation (same options as SLOPE_LIMITER_SPECIES)
SLOPE_LIMITER_HEAT = NONE
%
% Time discretization
TIME_DISCRE_HEAT= EULER_IMPLICIT

% ---------------- ADJOINT-FLOW NUMERICAL METHOD DEFINITION -------------------%
%
% Frozen the slope limiter in the discrete adjoint formulation (NO, YES)
FROZEN_LIMITER_DISC= NO
%
% Continuous Adjoint frozen viscosity
% FROZEN_VISC_CONT= NO
%
% Frozen the turbulent viscosity in the discrete adjoint formulation (NO, YES)
FROZEN_VISC_DISC= NO
%
% Use an inconsistent spatial integration (primal-dual) in the discrete
% adjoint formulation. The AD will use the numerical methods in
% the ADJOINT-FLOW NUMERICAL METHOD DEFINITION section (NO, YES)
INCONSISTENT_DISC= NO
%
% Convective numerical method (JST, LAX-FRIEDRICH, ROE)
CONV_NUM_METHOD_ADJFLOW= JST
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT)
TIME_DISCRE_ADJFLOW= EULER_IMPLICIT
%
% Relaxation coefficient (also for discrete adjoint problems)
RELAXATION_FACTOR_ADJOINT= 1.0
%
% Enable (if != 0) quasi-Newton acceleration/stabilization of discrete adjoints
QUASI_NEWTON_NUM_SAMPLES= 20
%
% Reduction factor of the CFL coefficient in the adjoint problem
CFL_REDUCTION_ADJFLOW= 0.8
%
% Limit value for the adjoint variable
LIMIT_ADJFLOW= 1E6
%
% Use multigrid in the adjoint problem (NO, YES)
MG_ADJFLOW= YES

% ---------------- MULTIZONE DEFINITION --------------%
%
% Determine if the mesh file supports multizone. \n DEFAULT: true (temporarily)
MULTIZONE_MESH= YES
%
% Determine if we need to allocate memory to store the multizone residual. \n DEFAULT: true (temporarily)
MULTIZONE_RESIDUAL= NO
%
% Determines if the convergence history of each individual zone is written to screen
WRT_ZONE_CONV= NO
%
% Determines if the convergence history of each individual zone is written to file
WRT_ZONE_HIST= NO

% ---------------- ADJOINT-TURBULENT NUMERICAL METHOD DEFINITION --------------%
%
% Convective numerical method (SCALAR_UPWIND)
CONV_NUM_METHOD_ADJTURB= SCALAR_UPWIND
%
% Time discretization (EULER_IMPLICIT)
TIME_DISCRE_ADJTURB= EULER_IMPLICIT
%
% Reduction factor of the CFL coefficient in the adjoint turbulent problem
CFL_REDUCTION_ADJTURB= 0.01

% -------------------- NEMO NUMERICAL METHOD DEFINITION -----------------------%
%
% Mixture transport properties (WILKE,GUPTA-YOS,CHAPMANN-ENSKOG, SUTHERLAND)
TRANSPORT_COEFF_MODEL = WILKE

% ----------------------- GEOMETRY EVALUATION PARAMETERS ----------------------%
%
% Marker(s) of the surface where geometrical based function will be evaluated
GEO_MARKER= ( airfoil )
%
% Description of the geometry to be analyzed (AIRFOIL, WING)
GEO_DESCRIPTION= AIRFOIL
%
% Z location of the waterline
GEO_WATERLINE_LOCATION= 0.0
%
% Coordinate of the stations to be analyzed
GEO_LOCATION_STATIONS= (0.0, 0.5, 1.0)
%
% Definition of the nacelle location (higlite coordinates, tilt angle, toe angle)
GEO_NACELLE_LOCATION= (0.0, 0.0, 0.0, 0.0, 0.0)
% Geometrical bounds (Y coordinate) for the wing geometry analysis or
% fuselage evaluation (X coordinate)
GEO_BOUNDS= (1.5, 3.5)
%
% Plot loads and Cp distributions on each airfoil section
GEO_PLOT_STATIONS= NO
%
% Number of section cuts to make when calculating wing geometry
GEO_NUMBER_STATIONS= 25
%
% Geometrical evaluation mode (FUNCTION, GRADIENT)
GEO_MODE= FUNCTION

% ----------------------- DESIGN VARIABLE PARAMETERS --------------------------%
%
% Kind of deformation (NO_DEFORMATION, SCALE_GRID, TRANSLATE_GRID, ROTATE_GRID,
%                      FFD_SETTING, FFD_NACELLE,
%                      FFD_CONTROL_POINT, FFD_CAMBER, FFD_THICKNESS, FFD_TWIST
%                      FFD_CONTROL_POINT_2D, FFD_CAMBER_2D, FFD_THICKNESS_2D,
%                      HICKS_HENNE, SURFACE_BUMP, SURFACE_FILE)
DV_KIND= FFD_SETTING
%
% Marker of the surface in which we are going apply the shape deformation
DV_MARKER= ( airfoil )
%
% Parameters of the shape deformation
% - NO_DEFORMATION ( 1.0 )
% - TRANSLATE_GRID ( x_Disp, y_Disp, z_Disp ), as a unit vector
% - ROTATE_GRID ( x_Orig, y_Orig, z_Orig, x_End, y_End, z_End ) axis, DV_VALUE in deg.
% - SCALE_GRID ( 1.0 )
% - ANGLE_OF_ATTACK ( 1.0 )
% - FFD_SETTING ( 1.0 )
% - FFD_CONTROL_POINT ( FFD_BoxTag, i_Ind, j_Ind, k_Ind, x_Disp, y_Disp, z_Disp )
% - FFD_NACELLE ( FFD_BoxTag, rho_Ind, theta_Ind, phi_Ind, rho_Disp, phi_Disp )
% - FFD_GULL ( FFD_BoxTag, j_Ind )
% - FFD_ANGLE_OF_ATTACK ( FFD_BoxTag, 1.0 )
% - FFD_CAMBER ( FFD_BoxTag, i_Ind, j_Ind )
% - FFD_THICKNESS ( FFD_BoxTag, i_Ind, j_Ind )
% - FFD_TWIST ( FFD_BoxTag, j_Ind, x_Orig, y_Orig, z_Orig, x_End, y_End, z_End )
% - FFD_CONTROL_POINT_2D ( FFD_BoxTag, i_Ind, j_Ind, x_Disp, y_Disp )
% - FFD_CAMBER_2D ( FFD_BoxTag, i_Ind )
% - FFD_THICKNESS_2D ( FFD_BoxTag, i_Ind )
% - HICKS_HENNE ( Lower Surface (0)/Upper Surface (1)/Only one Surface (2), x_Loc )
% - SURFACE_BUMP ( x_Start, x_End, x_Loc )
DV_PARAM= ( 1, 0.5 )
%
% Value of the shape deformation
DV_VALUE= 0.01
%
% For DV_KIND = SURFACE_FILE: With SU2_DEF, give filename for surface
% deformation prescribed by an external parameterization. List moving markers
% in DV_MARKER and provide an ASCII file with name specified with DV_FILENAME
% and with format:
% GlobalID_0, x_0, y_0, z_0
% GlobalID_1, x_1, y_1, z_1
%   ...
% GlobalID_N, x_N, y_N, z_N
% where N is the total number of vertices on all moving markers, and x/y/z are
% the new position of each vertex. Points can be in any order. When SU2_DOT
% is called in SURFACE_FILE mode, sensitivities on surfaces will be written
% to an ASCII file with name given by DV_SENS_FILENAME and with format as
% rows of x, y, z, dJ/dx, dJ/dy, dJ/dz for each surface vertex.
DV_FILENAME= surface_positions.dat
DV_SENS_FILENAME= surface_sensitivity.dat
%
% Format for volume sensitivity file read by SU2_DOT (SU2_NATIVE,
% UNORDERED_ASCII). SU2_NATIVE is the native SU2 restart file (default),
% while UNORDERED_ASCII provide a file of field sensitivities
% as an ASCII file with name given by DV_SENS_FILENAMEand with format as
% rows of x, y, z, dJ/dx, dJ/dy, dJ/dz for each grid point.
DV_SENSITIVITY_FORMAT= SU2_NATIVE
%
DV_UNORDERED_SENS_FILENAME= unordered_sensitivity.dat
%
% Hold the grid fixed in a region
HOLD_GRID_FIXED= NO
%
% Coordinates of the box where the grid will be deformed (Xmin, Ymin, Zmin, Xmax, Ymax, Zmax)
HOLD_GRID_FIXED_COORDS= (-1e15, -1e15, -1e15, 1e15, 1e15, 1e15)
%
% Design variable for FEA problems
% options: NONE, YOUNG_MODULUS, POISSON_RATIO, DENSITY, DEAD_WEIGHT, ELECTRIC_FIELD
DESIGN_VARIABLE_FEA= NONE
%
% Penalty weight value to maintain the total sum of DV constant
TOTAL_DV_PENALTY= 0.0
%
% Parameters for the corresponding OF (allowed stress and KS multiplier).
STRESS_PENALTY_PARAM= (1.0, 10.0)

% ---------------- AUTOMATIC DIFFERENTIATION -------------------%
%
% Preaccumulation in the AD mode.
PREACC= YES

% ---------------- AUTOMATIC DIFFERENTIATION (TAPE TEST DEBUG MODE) -------------------%
%
% Specify the kind of tape that is checked (OBJECTIVE_FUNCTION_TAPE, FULL_SOLVER_TAPE)
CHECK_TAPE_TYPE = FULL_SOLVER_TAPE
%
% Specify the variables for which the tape is checked (SOLVER_VARIABLES, SOLVER_VARIABLES_AND_MESH_COORDINATES)
CHECK_TAPE_VARIABLES = SOLVER_VARIABLES

% ---------------- MESH DEFORMATION PARAMETERS (NEW SOLVER) -------------------%
%
% Use the reformatted pseudo-elastic solver for grid deformation
DEFORM_MESH= YES
%
% Moving markers which deform the mesh
MARKER_DEFORM_MESH = ( airfoil )
MARKER_DEFORM_MESH_SYM_PLANE = ( wall )

% ------------------------ GRID DEFORMATION PARAMETERS ------------------------%
%
% Linear solver or smoother for implicit formulations (same options as LINEAR_SOLVER)
DEFORM_LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver (ILU, LU_SGS, JACOBI)
DEFORM_LINEAR_SOLVER_PREC= ILU
%
% Number of smoothing iterations for mesh deformation
DEFORM_LINEAR_SOLVER_ITER= 1000
%
% Number of nonlinear deformation iterations (surface deformation increments)
DEFORM_NONLINEAR_ITER= 1
%
% Minimum residual criteria for the linear solver convergence of grid deformation
DEFORM_LINEAR_SOLVER_ERROR= 1E-14
%
% Print the residuals during mesh deformation to the console (YES, NO)
DEFORM_CONSOLE_OUTPUT= YES
%
% Deformation coefficient (linear elasticity limits from -1.0 to 0.5, a larger
% value is also possible)
DEFORM_COEFF = 1E6
%
% Type of element stiffness imposed for FEA mesh deformation (INVERSE_VOLUME,
%                                           WALL_DISTANCE, CONSTANT_STIFFNESS)
DEFORM_STIFFNESS_TYPE= WALL_DISTANCE
%
% Deform the grid only close to the surface. It is possible to specify how much
% of the volumetric grid is going to be deformed in meters or inches (1E6 by default)
DEFORM_LIMIT = 1E6
%
% Young modulus for constant stiffness FEA method of grid deformation
DEFORM_ELASTICITY_MODULUS= 2e11
%
% Poisson ratio for constant stiffness FEA method of grid deformation
DEFORM_POISSON_RATIO= 0.3
%
% Size of the layer of highest stiffness for wall distance-based mesh stiffness
DEFORM_STIFF_LAYER_SIZE= 0.0

% -------------------- REFERENCE GEOMETRY -----------------------%
%
% Consider a reference solution for the structure (optimization applications)
REFERENCE_GEOMETRY= NO
%
% Penalty weight value for the objective function
REFERENCE_GEOMETRY_PENALTY= 1.0E6
%
% Reference geometry filename
REFERENCE_GEOMETRY_FILENAME= reference_geometry
%
% Format of the reference geometry file
REFERENCE_GEOMETRY_FORMAT= SU2_REF
%
% If true consider only the surfaces where loads are applied.
REFERENCE_GEOMETRY_SURFACE= NO
%
% Reference node for the structure (optimization applications)
REFERENCE_NODE= 0
%
% Target displacement of the reference node
REFERENCE_NODE_DISPLACEMENT= (0.0, 0.0)
%
% Penalty weight value for the objective function
REFERENCE_NODE_PENALTY= 1.0E3

% -------------------- FREE-FORM DEFORMATION PARAMETERS -----------------------%
%
% Tolerance of the Free-Form Deformation point inversion
FFD_TOLERANCE= 1E-10
%
% Maximum number of iterations in the Free-Form Deformation point inversion
FFD_ITERATIONS= 500
%
% Parameters for prevention of self-intersections within FFD box
FFD_INTPREV = YES
FFD_INTPREV_ITER = 10
FFD_INTPREV_DEPTH = 3
%
% Parameters for prevention of nonconvex elements in mesh after deformation
CONVEXITY_CHECK = YES
CONVEXITY_CHECK_ITER = 10
CONVEXITY_CHECK_DEPTH = 3
%
%
% FFD box definition: 3D case (FFD_BoxTag, X1, Y1, Z1, X2, Y2, Z2, X3, Y3, Z3, X4, Y4, Z4,
%                              X5, Y5, Z5, X6, Y6, Z6, X7, Y7, Z7, X8, Y8, Z8)
%                     2D case (FFD_BoxTag, X1, Y1, 0.0, X2, Y2, 0.0, X3, Y3, 0.0, X4, Y4, 0.0,
%                              0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0)
FFD_DEFINITION= (MAIN_BOX, 0.5, 0.25, -0.25, 1.5, 0.25, -0.25, 1.5, 0.75, -0.25, 0.5, 0.75, -0.25, 0.5, 0.25, 0.25, 1.5, 0.25, 0.25, 1.5, 0.75, 0.25, 0.5, 0.75, 0.25)
%
% FFD box degree: 3D case (i_degree, j_degree, k_degree)
%                 2D case (i_degree, j_degree, 0)
FFD_DEGREE= (10, 10, 1)
%
% Surface grid continuity at the intersection with the faces of the FFD boxes.
% To keep a particular level of surface continuity, SU2 automatically freezes the right
% number of control point planes (NO_DERIVATIVE, 1ST_DERIVATIVE, 2ND_DERIVATIVE, USER_INPUT)
FFD_CONTINUITY= 2ND_DERIVATIVE
%
% Definition of the FFD planes to be frozen in the FFD (x,y,z).
% Value from 0 FFD degree in that direction. Pick a value larger than degree if you don't want to fix any plane.
FFD_FIX_I= (0,2,3)
FFD_FIX_J= (0,2,3)
FFD_FIX_K= (0,2,3)
%
% There is a symmetry plane (j=0) for all the FFD boxes (YES, NO)
FFD_SYMMETRY_PLANE= NO
%
% FFD coordinate system (CARTESIAN)
FFD_COORD_SYSTEM= CARTESIAN
%
% Vector from the cartesian axis the cylindrical or spherical axis (using cartesian coordinates)
% Note that the location of the axis will affect the wall curvature of the FFD box as well as the
% design variable effect.
FFD_AXIS= (0.0, 0.0, 0.0)
%
% FFD Blending function: Bezier curves with global support (BEZIER), uniform BSplines with local support (BSPLINE_UNIFORM)
FFD_BLENDING= BEZIER
%
% Order of the BSplines
FFD_BSPLINE_ORDER= 2, 2, 2
%
% ------------------- UNCERTAINTY QUANTIFICATION DEFINITION -------------------%
%
% Eigenvalue perturbation definition (1, 2, or 3)
UQ_COMPONENT= 1
%
% Permuting eigenvectors (YES, NO)
UQ_PERMUTE= NO
%
% Under-relaxation factor (float [0,1], default = 0.1)
UQ_URLX= 0.1
%
% Perturbation magnitude (float [0,1], default= 1.0)
UQ_DELTA_B= 1.0
%
% --------------------- HYBRID PARALLEL (MPI+OpenMP) OPTIONS ---------------------%
%
% An advanced performance parameter for FVM solvers, a large-ish value should be best
% when relatively few threads per MPI rank are in use (~4). However, maximum parallelism
% is obtained with EDGE_COLORING_GROUP_SIZE=1, consider using this value only if SU2
% warns about low coloring efficiency during preprocessing (performance is usually worse).
% Setting the option to 0 disables coloring and a different strategy is used instead,
% that strategy is automatically used when the coloring efficiency is less than 0.875.
% The optimum value/strategy is case-dependent.
EDGE_COLORING_GROUP_SIZE= 512
%
% Coloring tends to perform better for the discrete adjoint than reductions because
% it uses less memory and enables the shared reading optimization for color loops.
% This option allows an automatic fallback to smaller edge color group sizes on ranks
% where the requested edge color group size is not efficient. Specifically, the largest
% edge color group size up to EDGE_COLORING_GROUP_SIZE is chosen that is at least
% 0.875 efficient. Also, this option allows using more colors, up to 255 instead of up to 64.
EDGE_COLORING_RELAX_DISC_ADJ= YES
%
% Independent "threads per MPI rank" setting for LU-SGS and ILU preconditioners.
% For problems where time is spend mostly in the solution of linear systems (e.g. elasticity,
% very high CFL central schemes), AND, if the memory bandwidth of the machine is saturated
% (4 or more cores per memory channel) better performance (via a reduction in linear iterations)
% may be possible by using a smaller value than that defined by the system or in the call to
% SU2_CFD (via the -t/--threads option).
% The default (0) means "same number of threads as for all else".
LINEAR_SOLVER_PREC_THREADS= 0
%
% ----------------------- PARTITIONING OPTIONS (ParMETIS) ------------------------ %
%
% Load balancing tolerance, lower values will make ParMETIS work harder to evenly
% distribute the work-estimate metric across all MPI ranks, at the expense of more
% edge cuts (i.e. increased communication cost).
PARMETIS_TOLERANCE= 0.02
%
% The work-estimate metric is a weighted function of the work-per-edge (e.g. spatial
% discretization, linear system solution) and of the work-per-point (e.g. source terms,
% temporal discretization) the former usually accounts for >90% of the total.
% These weights are INTEGERS (for compatibility with ParMETIS) thus not [0, 1].
% To balance memory usage (instead of computation) the point weight needs to be
% increased (especially for explicit time integration methods).
PARMETIS_EDGE_WEIGHT= 1
PARMETIS_POINT_WEIGHT= 0
%
% ----------------------- SOBOLEV GRADIENT SMOOTHING OPTIONS ----------------------%
%
% Activate the gradient smoothing solver for the discrete adjoint driver (NO, YES)
% see TestCases/grad_smooth/naca0012/inv_NACA0012_gradsmooth.cfg for a detailed explanantion
% on the config options shown here.
SMOOTH_GRADIENT= NO
%
% Mode how the Sobolev method is applied to the discrete adjoint gradient.
SOBOLEV_MODE= NO_MODUS
%
% Scaling factor for the identity part of the Laplace-Beltrami operator
SMOOTHING_EPSILON1= 1.0
%
% Scaling factor for the Laplace part of the Laplace-Beltrami operator
SMOOTHING_EPSILON2= 1.0
%
% Switch for applying the Sobolev smoothing to the design surface mesh, i.e., instead of the whole volume mesh (NO, YES).
SMOOTH_ON_SURFACE= NO
%
% Switch for running the smoothing procedure seperately in each space dimension (NO, YES).
SEPARATE_DIMENSIONS= NO
%
% Use Dirichlet boundary conditions when working on the design surface, only used for SMOOTH_ON_SURFACE= YES (NO, YES).
DIRICHLET_SURFACE_BOUNDARY= NO
%
% Marker for boundaries where Dirichlet boundary conditions are applied, only valid if working on the volume mesh.
MARKER_SOBOLEVBC= ( airfoil )
%
% Output filename for the assembled Sobolev smoothing system matrix
HESS_OBJFUNC_FILENAME= of_hess.dat
%
% Linear solver or smoother for implicit formulations (same options as LINEAR_SOLVER)
GRAD_LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver (ILU, LU_SGS, JACOBI)
GRAD_LINEAR_SOLVER_PREC= ILU
%
% Number of linear solver iterations for the Sobolev smoothing solver
GRAD_LINEAR_SOLVER_ITER= 1000
%
% Minimum residual criteria for the linear solver convergence of the Sobolev smoothing solver
GRAD_LINEAR_SOLVER_ERROR= 1E-14
%
% ------------------------- SCREEN/HISTORY VOLUME OUTPUT --------------------------%
%
% Screen output fields (use 'SU2_CFD -d <config_file>' to view list of available fields)
SCREEN_OUTPUT= (INNER_ITER, RMS_DENSITY, RMS_MOMENTUM-X, RMS_MOMENTUM-Y, RMS_ENERGY)
%
% History output groups (use 'SU2_CFD -d <config_file>' to view list of available fields)
HISTORY_OUTPUT= (ITER, RMS_RES)
%
% User defined functions available on screen and history output. See TestCases/user_defined_functions/.
CUSTOM_OUTPUTS= ''
%
% Volume output fields/groups (use 'SU2_CFD -d <config_file>' to view list of available fields)
VOLUME_OUTPUT= (COORDINATES, SOLUTION, PRIMITIVE)
%
% Writing frequency for screen output
SCREEN_WRT_FREQ_INNER= 1
%
SCREEN_WRT_FREQ_OUTER= 1
%
SCREEN_WRT_FREQ_TIME= 1
%
% Writing frequency for history output
HISTORY_WRT_FREQ_INNER= 1
%
HISTORY_WRT_FREQ_OUTER= 1
%
HISTORY_WRT_FREQ_TIME= 1
%
% list of writing frequencies corresponding to the list in OUTPUT_FILES
OUTPUT_WRT_FREQ= 10, 250, 42
%
% Output the performance summary to the console at the end of SU2_CFD
WRT_PERFORMANCE= NO
%
% Output the tape statistics (discrete adjoint)
WRT_AD_STATISTICS= NO
%
%
% Overwrite or append iteration number to the restart files when saving
WRT_RESTART_OVERWRITE= YES
%
% Overwrite or append iteration number to the surface files when saving
WRT_SURFACE_OVERWRITE= YES
%
% Overwrite or append iteration number to the volume files when saving
WRT_VOLUME_OVERWRITE= YES
%
% Determines if the forces breakdown is written out
WRT_FORCES_BREAKDOWN= NO
%
% MPI communication level (NONE, MINIMAL, FULL)
COMM_LEVEL= FULL
%
% Node number for the CV to be visualized (tecplot) (delete?)
VISUALIZE_CV= -1
%
% Write extra output (EXPERIMENTAL, NOT FOR GENERAL USE)
EXTRA_OUTPUT= NO
%
% Write extra heat output for a given heat solver zone
EXTRA_HEAT_ZONE_OUTPUT= -1

% ------------------------- INPUT/OUTPUT FILE INFORMATION --------------------------%
%
% Mesh input file
MESH_FILENAME= mesh_NACA0012_inv
%
% Mesh input file format (SU2, CGNS)
MESH_FORMAT= SU2
%
% List of the number of grid points in the RECTANGLE or BOX grid in the x,y,z directions. (default: (33,33,33) ).
MESH_BOX_SIZE= (33, 33, 33)
%
% List of the length of the RECTANGLE or BOX grid in the x,y,z directions. (default: (1.0,1.0,1.0) ).
MESH_BOX_LENGTH= (1.0, 1.0, 1.0)
%
% List of the offset from 0.0 of the RECTANGLE or BOX grid in the x,y,z directions. (default: (0.0,0.0,0.0) ).
MESH_BOX_OFFSET= (0.0, 0.0, 0.0)
%
% Mesh output file
MESH_OUT_FILENAME= mesh_out
%
% Restart flow input file
SOLUTION_FILENAME= solution_flow
%
% Restart adjoint input file
SOLUTION_ADJ_FILENAME= solution_adj
%
% Output tabular file format (TECPLOT, CSV)
TABULAR_FORMAT= CSV
%
% Set <ofstream>.precision(value) to specified value for SU2_DOT and HISTORY output. Useful for exact gradient validation.
OUTPUT_PRECISION= 10
%
% For multizone problems, extend solution and restart filenames automatically by zone number
MULTIZONE_ADAPT_FILENAME= YES
%
% Files to output
% Possible formats : (TECPLOT_ASCII, TECPLOT, SURFACE_TECPLOT_ASCII,
%  SURFACE_TECPLOT, CSV, SURFACE_CSV, PARAVIEW_ASCII, PARAVIEW_LEGACY, SURFACE_PARAVIEW_ASCII,
%  SURFACE_PARAVIEW_LEGACY, PARAVIEW, SURFACE_PARAVIEW, RESTART_ASCII, RESTART, CGNS, SURFACE_CGNS, STL_ASCII, STL_BINARY)
% default : (RESTART, PARAVIEW, SURFACE_PARAVIEW)
OUTPUT_FILES= (RESTART, PARAVIEW, SURFACE_PARAVIEW)
%
% Output file convergence history (w/o extension)
CONV_FILENAME= history
%
% Output file with the forces breakdown
BREAKDOWN_FILENAME= forces_breakdown.dat
%
% Output file restart flow
RESTART_FILENAME= restart_flow
%
% Output file restart adjoint
RESTART_ADJ_FILENAME= restart_adj
%
% Output file flow (w/o extension) variables
VOLUME_FILENAME= flow
%
% Output file adjoint (w/o extension) variables
VOLUME_ADJ_FILENAME= adjoint
%
% Output Objective function (in tecplot .dat or .csv format)
VALUE_OBJFUNC_FILENAME= of_eval
%
% Output objective function gradient (using continuous adjoint)
GRAD_OBJFUNC_FILENAME= of_grad
%
% Output file surface flow coefficient (w/o extension)
SURFACE_FILENAME= surface_flow
%
% Output file surface adjoint coefficient (w/o extension)
SURFACE_ADJ_FILENAME= surface_adjoint
%
% Output file surface sensitivity (discrete adjoint) (w/o extension)
SURFACE_SENS_FILENAME= surface_sens
%
% Output file volume sensitivity (discrete adjoint))
VOLUME_SENS_FILENAME= volume_sens
%
% Read binary restart files (YES, NO)
READ_BINARY_RESTART= YES
%
% Reorient elements based on potential negative volumes (YES/NO)
REORIENT_ELEMENTS= YES
%
% --------------------- OPTIMAL SHAPE DESIGN DEFINITION -----------------------%
%
% Available flow based objective functions or constraint functions
%    DRAG, LIFT, SIDEFORCE, EFFICIENCY, BUFFET,
%    FORCE_X, FORCE_Y, FORCE_Z,
%    MOMENT_X, MOMENT_Y, MOMENT_Z,
%    THRUST, TORQUE, FIGURE_OF_MERIT,
%    EQUIVALENT_AREA, NEARFIELD_PRESSURE,
%    TOTAL_HEATFLUX, MAXIMUM_HEATFLUX,
%    INVERSE_DESIGN_PRESSURE, INVERSE_DESIGN_HEATFLUX,
%    SURFACE_TOTAL_PRESSURE, SURFACE_MASSFLOW
%    SURFACE_STATIC_PRESSURE, SURFACE_MACH
%
% Available geometrical based objective functions or constraint functions
%    AIRFOIL_AREA, AIRFOIL_THICKNESS, AIRFOIL_CHORD, AIRFOIL_TOC, AIRFOIL_AOA,
%    WING_VOLUME, WING_MIN_THICKNESS, WING_MAX_THICKNESS, WING_MAX_CHORD, WING_MIN_TOC, WING_MAX_TWIST, WING_MAX_CURVATURE, WING_MAX_DIHEDRAL
%    STATION#_WIDTH, STATION#_AREA, STATION#_THICKNESS, STATION#_CHORD, STATION#_TOC,
%    STATION#_TWIST (where # is the index of the station defined in GEO_LOCATION_STATIONS)
%
% Available design variables
% 2D Design variables
%    FFD_CONTROL_POINT_2D   (  19, Scale | Mark. List | FFD_BoxTag, i_Ind, j_Ind, x_Mov, y_Mov )
%    FFD_CAMBER_2D          (  20, Scale | Mark. List | FFD_BoxTag, i_Ind )
%    FFD_THICKNESS_2D       (  21, Scale | Mark. List | FFD_BoxTag, i_Ind )
%    HICKS_HENNE            (  30, Scale | Mark. List | Lower(0)/Upper(1) side, x_Loc )
%    ANGLE_OF_ATTACK        ( 101, Scale | Mark. List | 1.0 )
%
% 3D Design variables
%    FFD_CONTROL_POINT      (  11, Scale | Mark. List | FFD_BoxTag, i_Ind, j_Ind, k_Ind, x_Mov, y_Mov, z_Mov )
%    FFD_NACELLE            (  12, Scale | Mark. List | FFD_BoxTag, rho_Ind, theta_Ind, phi_Ind, rho_Mov, phi_Mov )
%    FFD_GULL               (  13, Scale | Mark. List | FFD_BoxTag, j_Ind )
%    FFD_CAMBER             (  14, Scale | Mark. List | FFD_BoxTag, i_Ind, j_Ind )
%    FFD_TWIST              (  15, Scale | Mark. List | FFD_BoxTag, j_Ind, x_Orig, y_Orig, z_Orig, x_End, y_End, z_End )
%    FFD_THICKNESS          (  16, Scale | Mark. List | FFD_BoxTag, i_Ind, j_Ind )
%    FFD_ROTATION           (  18, Scale | Mark. List | FFD_BoxTag, x_Axis, y_Axis, z_Axis, x_Turn, y_Turn, z_Turn )
%    FFD_ANGLE_OF_ATTACK    (  24, Scale | Mark. List | FFD_BoxTag, 1.0 )
%
% Global design variables
%    TRANSLATION            (   1, Scale | Mark. List | x_Disp, y_Disp, z_Disp )
%    ROTATION               (   2, Scale | Mark. List | x_Axis, y_Axis, z_Axis, x_Turn, y_Turn, z_Turn )
%
% Definition of multipoint design problems, this option should be combined with the
% the prefix MULTIPOINT in the objective function or constraint (e.g. MULTIPOINT_DRAG, MULTIPOINT_LIFT, etc.)
MULTIPOINT_MACH_NUMBER= (0.79, 0.8, 0.81)
MULTIPOINT_WEIGHT= (0.33333, 0.33333, 0.33333)
MULTIPOINT_AOA= (1.25, 1.25, 1.25)
MULTIPOINT_SIDESLIP_ANGLE= (0.0, 0.0, 0.0)
MULTIPOINT_TARGET_CL= (0.8, 0.8, 0.8)
MULTIPOINT_REYNOLDS_NUMBER= (1E6, 1E6, 1E6)
MULTIPOINT_FREESTREAM_TEMPERATURE= (288.15, 288.15, 288.15)
MULTIPOINT_FREESTREAM_PRESSURE= (101325.0, 101325.0, 101325.0)
MULTIPOINT_OUTLET_VALUE= (0.0, 0.0, 0.0)
MULTIPOINT_MESH_FILENAME= (mesh_NACA0012_m79.su2, mesh_NACA0012_m8.su2, mesh_NACA0012_m81.su2)
%
% Optimization objective function with scaling factor, separated by semicolons.
% To include quadratic penalty function: use OPT_CONSTRAINT option syntax within the OPT_OBJECTIVE list.
% ex= Objective * Scale
OPT_OBJECTIVE= DRAG
%
% Optimization constraint functions with pushing factors (affects its value, not the gradient  in the python scripts), separated by semicolons
% ex= (Objective = Value ) * Scale, use '>','<','='
OPT_CONSTRAINT= ( LIFT > 0.328188 ) * 0.001; ( MOMENT_Z > 0.034068 ) * 0.001; ( AIRFOIL_THICKNESS > 0.11 ) * 0.001
%
% Factor to reduce the norm of the gradient (affects the objective function and gradient in the python scripts)
% In general, a norm of the gradient ~1E-6 is desired.
OPT_GRADIENT_FACTOR= 1E-6
%
% Factor to relax or accelerate the optimizer convergence (affects the line search in SU2_DEF)
% In general, surface deformations of 0.01'' or 0.0001m are desirable
OPT_RELAX_FACTOR= 1E3
%
% Maximum number of iterations
OPT_ITERATIONS= 100
%
% Requested accuracy
OPT_ACCURACY= 1E-10
%
% Optimization bound (bounds the line search in SU2_DEF)
OPT_LINE_SEARCH_BOUND= 1E6
%
% Upper bound for each design variable (bound in the python optimizer)
OPT_BOUND_UPPER= 1E10
%
% Lower bound for each design variable (bound in the python optimizer)
OPT_BOUND_LOWER= -1E10
%
% Finite difference step size for python scripts (0.001 default, recommended
%                                                 0.001 x REF_LENGTH)
FIN_DIFF_STEP = 0.001
%
% Optimization design variables, separated by semicolons
DEFINITION_DV= ( 1, 1.0 | airfoil | 0, 0.05 ); ( 1, 1.0 | airfoil | 0, 0.10 ); ( 1, 1.0 | airfoil | 0, 0.15 ); ( 1, 1.0 | airfoil | 0, 0.20 ); ( 1, 1.0 | airfoil | 0, 0.25 ); ( 1, 1.0 | airfoil | 0, 0.30 ); ( 1, 1.0 | airfoil | 0, 0.35 ); ( 1, 1.0 | airfoil | 0, 0.40 ); ( 1, 1.0 | airfoil | 0, 0.45 ); ( 1, 1.0 | airfoil | 0, 0.50 ); ( 1, 1.0 | airfoil | 0, 0.55 ); ( 1, 1.0 | airfoil | 0, 0.60 ); ( 1, 1.0 | airfoil | 0, 0.65 ); ( 1, 1.0 | airfoil | 0, 0.70 ); ( 1, 1.0 | airfoil | 0, 0.75 ); ( 1, 1.0 | airfoil | 0, 0.80 ); ( 1, 1.0 | airfoil | 0, 0.85 ); ( 1, 1.0 | airfoil | 0, 0.90 ); ( 1, 1.0 | airfoil | 0, 0.95 ); ( 1, 1.0 | airfoil | 1, 0.05 ); ( 1, 1.0 | airfoil | 1, 0.10 ); ( 1, 1.0 | airfoil | 1, 0.15 ); ( 1, 1.0 | airfoil | 1, 0.20 ); ( 1, 1.0 | airfoil | 1, 0.25 ); ( 1, 1.0 | airfoil | 1, 0.30 ); ( 1, 1.0 | airfoil | 1, 0.35 ); ( 1, 1.0 | airfoil | 1, 0.40 ); ( 1, 1.0 | airfoil | 1, 0.45 ); ( 1, 1.0 | airfoil | 1, 0.50 ); ( 1, 1.0 | airfoil | 1, 0.55 ); ( 1, 1.0 | airfoil | 1, 0.60 ); ( 1, 1.0 | airfoil | 1, 0.65 ); ( 1, 1.0 | airfoil | 1, 0.70 ); ( 1, 1.0 | airfoil | 1, 0.75 ); ( 1, 1.0 | airfoil | 1, 0.80 ); ( 1, 1.0 | airfoil | 1, 0.85 ); ( 1, 1.0 | airfoil | 1, 0.90 ); ( 1, 1.0 | airfoil | 1, 0.95 )
%
% Use combined objective within gradient evaluation: may reduce cost to compute gradients when using the adjoint formulation.
OPT_COMBINE_OBJECTIVE = NO
%
%
% Number of iterations to average the objective function for unsteady adjoints,
% 0 averages over all time iterations, "N" averages over the last N iterations.
ITER_AVERAGE_OBJ= 0

% --------------------- LIBROM PARAMETERS -----------------------%
% LibROM can be found here: https://github.com/LLNL/libROM
%
% Toggle saving to librom (NO, YES)
SAVE_LIBROM = NO
%
% Prefix to the saved libROM files (default: su2)
LIBROM_BASE_FILENAME = su2
%
% Specify POD basis generation algorithm (STATIC_POD, INCREMENTAL_POD)
% STATIC_POD recommended for steady problems
BASIS_GENERATION = STATIC_POD
%
% Maximum number of basis vectors to keep (default: 100)
MAX_BASIS_DIM = 100
%
% Frequency of snapshots saves, for unsteady problems (default: 1. 2 means every other)
ROM_SAVE_FREQ = 1

% --------------------- PASTIX PARAMETERS -----------------------%
%
% Number of calls to 'Build' that trigger re-factorization (0 means only once)
PASTIX_FACTORIZATION_FREQUENCY= 1
%
% 0 - Quiet, 1 - During factorization and cleanup, 2 - Even more detail
PASTIX_VERBOSITY_LEVEL= 0
%
% Level of fill for PaStiX incomplete LU factorization
PASTIX_FILL_LEVEL= 1