[kuzuner]

Hello everyone, i am new to SU2 and trying to test out turbomachinery capabilities of SU2 by running NASA's rotor67 case in 3D.

I am using my own mesh without a tip gap for simplicity. So far the results I am getting are not correct. I am defining relative total temperature and pressure BC at inlet but simulation keeps calculating higher temperatures and pressures than the total inlet conditions. The locations it keeps doing this are mostly at leading and trailing edges. I've used finer meshes, different topologies, etc but couldnt figure out why this keeps happening and nothing I did solved the problem. Also, I am using Giles BC at the outlet with radial equilibrium. The pressure defined at the Giles BC is static pressure at the hub at the outlet.

I've also tested the same mesh with same BCs in CFX and it didnt show any behavior like SU2 and computed a sensible solution. Thus, I think the mesh I am using is most likely fine.

I am sharing my cfg file as well. I will be very glad to hear out any solution idea or anyone that encountered the same issue, calculating higher values than the defined total BC values, from the community.

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%                                                                              %
% SU2 configuration file                                                       %
% Case description: NASA Rotor67 Sim				               %
% Author: K. Uzuner	                                                       %
%                                        				       %
%                                                 		               %
%                                               			       %
%                                                                              %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
% Physical governing equations (EULER, NAVIER_STOKES,
%                               WAVE_EQUATION, HEAT_EQUATION, FEM_ELASTICITY,
%                               POISSON_EQUATION)
SOLVER= RANS
%
% Specify turbulence model (NONE, SA, SA_NEG, SST)
KIND_TURB_MODEL= SST
%
% Mathematical problem (DIRECT, CONTINUOUS_ADJOINT)
MATH_PROBLEM= DIRECT
%
% Restart solution (NO, YES)
RESTART_SOL= NO

% -------------------- 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= 0.0
%
% 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= TD_CONDITIONS
%
% Free-stream option to choose between density and temperature (default) for
% initializing the solution (TEMPERATURE_FS, DENSITY_FS)
FREESTREAM_OPTION= TEMPERATURE_FS
%
% Free-stream temperature (288.15 K by default)
FREESTREAM_TEMPERATURE= 288.15
%
FREESTREAM_PRESSURE= 150000
%
% Free-stream Turbulence Intensity
FREESTREAM_TURBULENCEINTENSITY = 0.01
%
% Free-stream Turbulent to Laminar viscosity ratio
FREESTREAM_TURB2LAMVISCRATIO = 10.0
%
% Reynolds number (non-dimensional, based on the free-stream values)
REYNOLDS_NUMBER= 6.5E6
%
% Reynolds length (1 m by default)
REYNOLDS_LENGTH= 0.3048

% ---- IDEAL GAS, POLYTROPIC, VAN DER WAALS AND PENG ROBINSON CONSTANTS -------%
%
% Different gas model (STANDARD_AIR, IDEAL_GAS, VW_GAS, PR_GAS)
FLUID_MODEL= IDEAL_GAS
%
% Ratio of specific heats (1.4 default and the value is hardcoded
%                          for the model STANDARD_AIR)
GAMMA_VALUE= 1.4
%
% Specific gas constant (287.058 J/kg*K default and this value is hardcoded
%                        for the model STANDARD_AIR)
GAS_CONSTANT= 287.058

% --------------------------- VISCOSITY MODEL ---------------------------------%
%
% Viscosity model (SUTHERLAND, CONSTANT_VISCOSITY).
VISCOSITY_MODEL= SUTHERLAND
%
% 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

% --------------------------- THERMAL CONDUCTIVITY MODEL ----------------------%
%
% Conductivity model (CONSTANT_CONDUCTIVITY, CONSTANT_PRANDTL).
CONDUCTIVITY_MODEL= CONSTANT_PRANDTL
%
% Laminar Prandtl number (0.72 (air), only for CONSTANT_PRANDTL)
PRANDTL_LAM= 0.72
%
% Turbulent Prandtl number (0.9 (air), only for CONSTANT_PRANDTL)
PRANDTL_TURB= 0.90

% ----------------------- DYNAMIC MESH DEFINITION -----------------------------%
%
% Type of dynamic mesh (NONE, RIGID_MOTION, ROTATING_FRAME,
%                       STEADY_TRANSLATION,
%                       ELASTICITY, GUST)
GRID_MOVEMENT= ROTATING_FRAME
%
% 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= 0.0 0.0 0.0
%
% Angular velocity vector (rad/s) about the motion origin
ROTATION_RATE = -1680.0 0.0 0.0
%

% ---------------------- REFERENCE VALUE DEFINITION ---------------------------%
%
% Reference origin for moment computation
REF_ORIGIN_MOMENT_X = 0.00
REF_ORIGIN_MOMENT_Y = 0.00
REF_ORIGIN_MOMENT_Z = 0.00
%
% Reference length for pitching, rolling, and yawing non-dimensional moment
REF_LENGTH= 0.64607
%
% Reference area for force coefficients (0 implies automatic calculation)
REF_AREA= 0
%
% Compressible flow non-dimensionalization (DIMENSIONAL, FREESTREAM_PRESS_EQ_ONE,
%                              FREESTREAM_VEL_EQ_MACH, FREESTREAM_VEL_EQ_ONE)
REF_DIMENSIONALIZATION= DIMENSIONAL

% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
MARKER_TURBOMACHINERY= (INLET , OUTLET)
TURBOMACHINERY_KIND= AXIAL
%
% Navier-Stokes wall boundary marker(s) (NONE = no marker)
MARKER_HEATFLUX= ( BLADE, 0.0, HUB, 0.0, SHROUD, 0.0 )
%
% 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= ( BLADE, STANDARD_WALL_FUNCTION, HUB, STANDARD_WALL_FUNCTION, SHROUD, STANDARD_WALL_FUNCTION )
%
% Symmetry boundary marker(s) (NONE = no marker)
MARKER_PERIODIC= ( PER1, PER2, 0.0, 0.0, 0.0, 16.364, 0.0, 0.0, 0.0, 0.0, 0.0 )
%
% Marker(s) of the surface to be plotted or designed
MARKER_PLOTTING= ( BLADE )
%
% Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated
MARKER_MONITORING= ( BLADE )
%
% Inlet boundary marker(s) (NONE = no marker)
% Format: ( inlet marker, total temperature, total pressure, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
%SPECIFIED_INLET_PROFILE = YES
%INLET_FILENAME = INLET_coarseProperInOut.dat
MARKER_INLET= ( INLET, 351.5, 172253, 0.5, -0.866, 0.0 )
%
% Outlet boundary marker(s) (NONE = no marker)
% Format: ( outlet marker, back pressure (static), ... )
%MARKER_OUTLET= ( OUTLET, 125923 )
MARKER_GILES= (OUTLET, RADIAL_EQUILIBRIUM, 101558.0475, 0.0, 0.0, 0.0, 0.0, 1.0, 1.0)
%
% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
% Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES)
NUM_METHOD_GRAD= GREEN_GAUSS
%
% Courant-Friedrichs-Lewy condition of the finest grid
CFL_NUMBER= 0.6
%
% Adaptive CFL number (NO, YES)
CFL_ADAPT= NO
%
% Parameters of the adaptive CFL number (factor down, factor up, CFL min value,
%                                        CFL max value )
CFL_ADAPT_PARAM= ( 0.1, 0.1, 0.4, 1.2 )
%
% Runge-Kutta alpha coefficients
RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 )
%
% Number of total iterations
ITER= 999999

% ------------------------ LINEAR SOLVER DEFINITION ---------------------------%
%
% Linear solver for the implicit (or discrete adjoint) formulation (BCGSTAB, FGMRES)
LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver (NONE, JACOBI, LINELET)
LINEAR_SOLVER_PREC= ILU
%
% Min error of the linear solver for the implicit formulation
LINEAR_SOLVER_ERROR= 1E-4
%
% Max number of iterations of the linear solver for the implicit formulation
LINEAR_SOLVER_ITER= 10

% -------------------------- 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, 1, 1, 1 )
%
% 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= 0.7
%
% Damping factor for the correction prolongation
MG_DAMP_PROLONGATION= 0.7

% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
% Convective numerical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, HLLC,
%                              TURKEL_PREC, MSW)
CONV_NUM_METHOD_FLOW= ROE
%
% Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER)
MUSCL_FLOW= NO
%
% Slope limiter (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG,
%                BARTH_JESPERSEN, VAN_ALBADA_EDGE)
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN
%
% Coefficient for the Venkat's limiter (upwind scheme). A larger values decrease
%             the extent of limiting, values approaching zero cause
%             lower-order approximation to the solution (0.05 by default)
VENKAT_LIMITER_COEFF= 0.05
%
% 2nd and 4th order artificial dissipation coefficients for
%     the JST method ( 0.5, 0.02 by default )
JST_SENSOR_COEFF= ( 0.5, 0.02 )
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_FLOW= EULER_IMPLICIT

% -------------------- TURBULENT NUMERICAL METHOD DEFINITION ------------------%
%
% Convective numerical method (SCALAR_UPWIND)
CONV_NUM_METHOD_TURB= SCALAR_UPWIND
%
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the turbulence equations.
%           Required for 2nd order upwind schemes (NO, YES)
MUSCL_TURB= NO
%
% Slope limiter (VENKATAKRISHNAN, MINMOD)
SLOPE_LIMITER_TURB= VENKATAKRISHNAN
%
% Time discretization (EULER_IMPLICIT)
TIME_DISCRE_TURB= EULER_IMPLICIT

% --------------------------- CONVERGENCE PARAMETERS --------------------------%
%
% Convergence criteria (CAUCHY, RESIDUAL)
CONV_FIELD= RESIDUAL
%
% 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-6
%

% ------------------------- INPUT/OUTPUT INFORMATION --------------------------%
%
% Mesh input file
MESH_FILENAME= rotor67_1M_3_rot.cgns
%
% Mesh input file format (SU2, CGNS, NETCDF_ASCII)
MESH_FORMAT= CGNS
%
% Mesh output file
MESH_OUT_FILENAME= mesh_out.su2
%
% Restart flow input file
SOLUTION_FILENAME= restart_flow.dat
%
% Restart adjoint input file
SOLUTION_ADJ_FILENAME= solution_adj.dat
%
% Output file format (PARAVIEW, TECPLOT, STL)
TABULAR_FORMAT= CSV
%
% Output file convergence history (w/o extension)
CONV_FILENAME= history
%
% Output file restart flow
RESTART_FILENAME= restart_flow.dat
%
% Output file restart adjoint
RESTART_ADJ_FILENAME= restart_adj.dat
%
% Output file flow (w/o extension) variables
VOLUME_FILENAME= flow
%
% Output file adjoint (w/o extension) variables
VOLUME_ADJ_FILENAME= adjoint
%
% Output objective function gradient (using continuous adjoint)
GRAD_OBJFUNC_FILENAME= of_grad.dat
%
% 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
%
% Writing solution file frequency
%WRT_SOL_FREQ= 200
%
OUTPUT_WRT_FREQ= 50
%
% Writing convergence history frequency
WRT_CON_FREQ= 1
%
% Screen output
SCREEN_OUTPUT= (INNER_ITER, WALL_TIME, RMS_DENSITY, RMS_NU_TILDE, RMS_MOMENTUM-X, RMS_MOMENTUM-Y)
%
VOLUME_OUTPUT= (MOMENTUM-X, MOMENTUM-Y, MOMENTUM-Z, DENSITY, MACH, PRESSURE, TEMPERATURE, Y_PLUS, EDDY_VISCOSITY)
%

% --------------------- 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 )
%    FFD_TWIST_2D           (  22, Scale | Mark. List | FFD_BoxTag, x_Orig, y_Orig )
%    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_DV= ( 30, 0.001 | airfoil | 0, 0.1 ); ( 30, 0.001 | airfoil | 0, 0.2 )

[ashvin]

Originally Posted by kuzuner

Hello everyone, i am new to SU2 and trying to test out turbomachinery capabilities of SU2 by running NASA's rotor67 case in 3D.

I am using my own mesh without a tip gap for simplicity. So far the results I am getting are not correct. I am defining relative total temperature and pressure BC at inlet but simulation keeps calculating higher temperatures and pressures than the total inlet conditions. The locations it keeps doing this are mostly at leading and trailing edges. I've used finer meshes, different topologies, etc but couldnt figure out why this keeps happening and nothing I did solved the problem. Also, I am using Giles BC at the outlet with radial equilibrium. The pressure defined at the Giles BC is static pressure at the hub at the outlet.

I've also tested the same mesh with same BCs in CFX and it didnt show any behavior like SU2 and computed a sensible solution. Thus, I think the mesh I am using is most likely fine.

I am sharing my cfg file as well. I will be very glad to hear out any solution idea or anyone that encountered the same issue, calculating higher values than the defined total BC values, from the community.

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%                                                                              %
% SU2 configuration file                                                       %
% Case description: NASA Rotor67 Sim				               %
% Author: K. Uzuner	                                                       %
%                                        				       %
%                                                 		               %
%                                               			       %
%                                                                              %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
% Physical governing equations (EULER, NAVIER_STOKES,
%                               WAVE_EQUATION, HEAT_EQUATION, FEM_ELASTICITY,
%                               POISSON_EQUATION)
SOLVER= RANS
%
% Specify turbulence model (NONE, SA, SA_NEG, SST)
KIND_TURB_MODEL= SST
%
% Mathematical problem (DIRECT, CONTINUOUS_ADJOINT)
MATH_PROBLEM= DIRECT
%
% Restart solution (NO, YES)
RESTART_SOL= NO

% -------------------- 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= 0.0
%
% 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= TD_CONDITIONS
%
% Free-stream option to choose between density and temperature (default) for
% initializing the solution (TEMPERATURE_FS, DENSITY_FS)
FREESTREAM_OPTION= TEMPERATURE_FS
%
% Free-stream temperature (288.15 K by default)
FREESTREAM_TEMPERATURE= 288.15
%
FREESTREAM_PRESSURE= 150000
%
% Free-stream Turbulence Intensity
FREESTREAM_TURBULENCEINTENSITY = 0.01
%
% Free-stream Turbulent to Laminar viscosity ratio
FREESTREAM_TURB2LAMVISCRATIO = 10.0
%
% Reynolds number (non-dimensional, based on the free-stream values)
REYNOLDS_NUMBER= 6.5E6
%
% Reynolds length (1 m by default)
REYNOLDS_LENGTH= 0.3048

% ---- IDEAL GAS, POLYTROPIC, VAN DER WAALS AND PENG ROBINSON CONSTANTS -------%
%
% Different gas model (STANDARD_AIR, IDEAL_GAS, VW_GAS, PR_GAS)
FLUID_MODEL= IDEAL_GAS
%
% Ratio of specific heats (1.4 default and the value is hardcoded
%                          for the model STANDARD_AIR)
GAMMA_VALUE= 1.4
%
% Specific gas constant (287.058 J/kg*K default and this value is hardcoded
%                        for the model STANDARD_AIR)
GAS_CONSTANT= 287.058

% --------------------------- VISCOSITY MODEL ---------------------------------%
%
% Viscosity model (SUTHERLAND, CONSTANT_VISCOSITY).
VISCOSITY_MODEL= SUTHERLAND
%
% 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

% --------------------------- THERMAL CONDUCTIVITY MODEL ----------------------%
%
% Conductivity model (CONSTANT_CONDUCTIVITY, CONSTANT_PRANDTL).
CONDUCTIVITY_MODEL= CONSTANT_PRANDTL
%
% Laminar Prandtl number (0.72 (air), only for CONSTANT_PRANDTL)
PRANDTL_LAM= 0.72
%
% Turbulent Prandtl number (0.9 (air), only for CONSTANT_PRANDTL)
PRANDTL_TURB= 0.90

% ----------------------- DYNAMIC MESH DEFINITION -----------------------------%
%
% Type of dynamic mesh (NONE, RIGID_MOTION, ROTATING_FRAME,
%                       STEADY_TRANSLATION,
%                       ELASTICITY, GUST)
GRID_MOVEMENT= ROTATING_FRAME
%
% 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= 0.0 0.0 0.0
%
% Angular velocity vector (rad/s) about the motion origin
ROTATION_RATE = -1680.0 0.0 0.0
%

% ---------------------- REFERENCE VALUE DEFINITION ---------------------------%
%
% Reference origin for moment computation
REF_ORIGIN_MOMENT_X = 0.00
REF_ORIGIN_MOMENT_Y = 0.00
REF_ORIGIN_MOMENT_Z = 0.00
%
% Reference length for pitching, rolling, and yawing non-dimensional moment
REF_LENGTH= 0.64607
%
% Reference area for force coefficients (0 implies automatic calculation)
REF_AREA= 0
%
% Compressible flow non-dimensionalization (DIMENSIONAL, FREESTREAM_PRESS_EQ_ONE,
%                              FREESTREAM_VEL_EQ_MACH, FREESTREAM_VEL_EQ_ONE)
REF_DIMENSIONALIZATION= DIMENSIONAL

% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
MARKER_TURBOMACHINERY= (INLET , OUTLET)
TURBOMACHINERY_KIND= AXIAL
%
% Navier-Stokes wall boundary marker(s) (NONE = no marker)
MARKER_HEATFLUX= ( BLADE, 0.0, HUB, 0.0, SHROUD, 0.0 )
%
% 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= ( BLADE, STANDARD_WALL_FUNCTION, HUB, STANDARD_WALL_FUNCTION, SHROUD, STANDARD_WALL_FUNCTION )
%
% Symmetry boundary marker(s) (NONE = no marker)
MARKER_PERIODIC= ( PER1, PER2, 0.0, 0.0, 0.0, 16.364, 0.0, 0.0, 0.0, 0.0, 0.0 )
%
% Marker(s) of the surface to be plotted or designed
MARKER_PLOTTING= ( BLADE )
%
% Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated
MARKER_MONITORING= ( BLADE )
%
% Inlet boundary marker(s) (NONE = no marker)
% Format: ( inlet marker, total temperature, total pressure, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
%SPECIFIED_INLET_PROFILE = YES
%INLET_FILENAME = INLET_coarseProperInOut.dat
MARKER_INLET= ( INLET, 351.5, 172253, 0.5, -0.866, 0.0 )
%
% Outlet boundary marker(s) (NONE = no marker)
% Format: ( outlet marker, back pressure (static), ... )
%MARKER_OUTLET= ( OUTLET, 125923 )
MARKER_GILES= (OUTLET, RADIAL_EQUILIBRIUM, 101558.0475, 0.0, 0.0, 0.0, 0.0, 1.0, 1.0)
%
% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
% Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES)
NUM_METHOD_GRAD= GREEN_GAUSS
%
% Courant-Friedrichs-Lewy condition of the finest grid
CFL_NUMBER= 0.6
%
% Adaptive CFL number (NO, YES)
CFL_ADAPT= NO
%
% Parameters of the adaptive CFL number (factor down, factor up, CFL min value,
%                                        CFL max value )
CFL_ADAPT_PARAM= ( 0.1, 0.1, 0.4, 1.2 )
%
% Runge-Kutta alpha coefficients
RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 )
%
% Number of total iterations
ITER= 999999

% ------------------------ LINEAR SOLVER DEFINITION ---------------------------%
%
% Linear solver for the implicit (or discrete adjoint) formulation (BCGSTAB, FGMRES)
LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver (NONE, JACOBI, LINELET)
LINEAR_SOLVER_PREC= ILU
%
% Min error of the linear solver for the implicit formulation
LINEAR_SOLVER_ERROR= 1E-4
%
% Max number of iterations of the linear solver for the implicit formulation
LINEAR_SOLVER_ITER= 10

% -------------------------- 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, 1, 1, 1 )
%
% 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= 0.7
%
% Damping factor for the correction prolongation
MG_DAMP_PROLONGATION= 0.7

% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
% Convective numerical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, HLLC,
%                              TURKEL_PREC, MSW)
CONV_NUM_METHOD_FLOW= ROE
%
% Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER)
MUSCL_FLOW= NO
%
% Slope limiter (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG,
%                BARTH_JESPERSEN, VAN_ALBADA_EDGE)
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN
%
% Coefficient for the Venkat's limiter (upwind scheme). A larger values decrease
%             the extent of limiting, values approaching zero cause
%             lower-order approximation to the solution (0.05 by default)
VENKAT_LIMITER_COEFF= 0.05
%
% 2nd and 4th order artificial dissipation coefficients for
%     the JST method ( 0.5, 0.02 by default )
JST_SENSOR_COEFF= ( 0.5, 0.02 )
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_FLOW= EULER_IMPLICIT

% -------------------- TURBULENT NUMERICAL METHOD DEFINITION ------------------%
%
% Convective numerical method (SCALAR_UPWIND)
CONV_NUM_METHOD_TURB= SCALAR_UPWIND
%
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the turbulence equations.
%           Required for 2nd order upwind schemes (NO, YES)
MUSCL_TURB= NO
%
% Slope limiter (VENKATAKRISHNAN, MINMOD)
SLOPE_LIMITER_TURB= VENKATAKRISHNAN
%
% Time discretization (EULER_IMPLICIT)
TIME_DISCRE_TURB= EULER_IMPLICIT

% --------------------------- CONVERGENCE PARAMETERS --------------------------%
%
% Convergence criteria (CAUCHY, RESIDUAL)
CONV_FIELD= RESIDUAL
%
% 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-6
%

% ------------------------- INPUT/OUTPUT INFORMATION --------------------------%
%
% Mesh input file
MESH_FILENAME= rotor67_1M_3_rot.cgns
%
% Mesh input file format (SU2, CGNS, NETCDF_ASCII)
MESH_FORMAT= CGNS
%
% Mesh output file
MESH_OUT_FILENAME= mesh_out.su2
%
% Restart flow input file
SOLUTION_FILENAME= restart_flow.dat
%
% Restart adjoint input file
SOLUTION_ADJ_FILENAME= solution_adj.dat
%
% Output file format (PARAVIEW, TECPLOT, STL)
TABULAR_FORMAT= CSV
%
% Output file convergence history (w/o extension)
CONV_FILENAME= history
%
% Output file restart flow
RESTART_FILENAME= restart_flow.dat
%
% Output file restart adjoint
RESTART_ADJ_FILENAME= restart_adj.dat
%
% Output file flow (w/o extension) variables
VOLUME_FILENAME= flow
%
% Output file adjoint (w/o extension) variables
VOLUME_ADJ_FILENAME= adjoint
%
% Output objective function gradient (using continuous adjoint)
GRAD_OBJFUNC_FILENAME= of_grad.dat
%
% 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
%
% Writing solution file frequency
%WRT_SOL_FREQ= 200
%
OUTPUT_WRT_FREQ= 50
%
% Writing convergence history frequency
WRT_CON_FREQ= 1
%
% Screen output
SCREEN_OUTPUT= (INNER_ITER, WALL_TIME, RMS_DENSITY, RMS_NU_TILDE, RMS_MOMENTUM-X, RMS_MOMENTUM-Y)
%
VOLUME_OUTPUT= (MOMENTUM-X, MOMENTUM-Y, MOMENTUM-Z, DENSITY, MACH, PRESSURE, TEMPERATURE, Y_PLUS, EDDY_VISCOSITY)
%

% --------------------- 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 )
%    FFD_TWIST_2D           (  22, Scale | Mark. List | FFD_BoxTag, x_Orig, y_Orig )
%    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_DV= ( 30, 0.001 | airfoil | 0, 0.1 ); ( 30, 0.001 | airfoil | 0, 0.2 )

Hello,
Were you able to get your case to run? I think the flow direction has to be in the Z direction. When the flow direction is in the x direction it gives the wrong number of blade count. When I changed the flow direction to the z direction it gives the correct number of blades. That is one thing I noticed from your card.

One other thing, were you able to scale up the number of processors used in calculating the case? I can only get it to scale up to 6 processors.
Thanks
Ashvin

[kuzuner]

Originally Posted by ashvin

Hello,
Were you able to get your case to run? I think the flow direction has to be in the Z direction. When the flow direction is in the x direction it gives the wrong number of blade count. When I changed the flow direction to the z direction it gives the correct number of blades. That is one thing I noticed from your card.

One other thing, were you able to scale up the number of processors used in calculating the case? I can only get it to scale up to 6 processors.
Thanks
Ashvin

Hello Ashvin,

You are right, I noticed the same thing a while back with rotation axis, it has to be in z-axis for the calculations to be correct.

I encountered the same issue with the multi-core calculations. It is not really a pretty fix but hardcoding the value of nSpanWiseSections worked for me so far. I found out this fix from this issue in SU2 github, https://github.com/su2code/SU2/issues/990

The change I have made is below. This is in CPhysicalGeometry.cpp in SU2/Common/src/geometry/. In my case the number of spanwise points is 57.

.
.
.
if(marker_flag == OUTFLOW){
	nSpanWiseSections[INFLOW - 1] = 57;
	nSpanWiseSections[OUTFLOW - 1] = 57; 
      if(nSpanWiseSections[INFLOW -1] != nSpanWiseSections[OUTFLOW - 1]){
        char buf[100];
        SPRINTF(buf, "nSpan inflow %u, nSpan outflow %u", nSpanWiseSections[INFLOW], nSpanWiseSections[OUTFLOW]);
        SU2_MPI::Error(string(" At the moment only turbomachinery with the same amount of span-wise section can be simulated\n") + buf, CURRENT_FUNCTION);
      }
      else{
        config->SetnSpanWiseSections(nSpanWiseSections[OUTFLOW -1]);
      }
    }

  }

}
void CPhysicalGeometry::SetTurboVertex(CConfig *config, unsigned short val_iZone, unsigned short marker_flag, bool allocate) {
.
.
.

I am yet to see any side effect of this fix may cause, so use it with this also in mind. Hope it will work for you.

[ashvin]

Originally Posted by kuzuner

Hello Ashvin,

You are right, I noticed the same thing a while back with rotation axis, it has to be in z-axis for the calculations to be correct.

I encountered the same issue with the multi-core calculations. It is not really a pretty fix but hardcoding the value of nSpanWiseSections worked for me so far. I found out this fix from this issue in SU2 github, https://github.com/su2code/SU2/issues/990

The change I have made is below. This is in CPhysicalGeometry.cpp in SU2/Common/src/geometry/. In my case the number of spanwise points is 57.

.
.
.
if(marker_flag == OUTFLOW){
	nSpanWiseSections[INFLOW - 1] = 57;
	nSpanWiseSections[OUTFLOW - 1] = 57; 
      if(nSpanWiseSections[INFLOW -1] != nSpanWiseSections[OUTFLOW - 1]){
        char buf[100];
        SPRINTF(buf, "nSpan inflow %u, nSpan outflow %u", nSpanWiseSections[INFLOW], nSpanWiseSections[OUTFLOW]);
        SU2_MPI::Error(string(" At the moment only turbomachinery with the same amount of span-wise section can be simulated\n") + buf, CURRENT_FUNCTION);
      }
      else{
        config->SetnSpanWiseSections(nSpanWiseSections[OUTFLOW -1]);
      }
    }

  }

}
void CPhysicalGeometry::SetTurboVertex(CConfig *config, unsigned short val_iZone, unsigned short marker_flag, bool allocate) {
.
.
.

I am yet to see any side effect of this fix may cause, so use it with this also in mind. Hope it will work for you.

Hello kuzuner,
Thanks. I finally made the choice to hard code the number of spans for my case like you did and it works for any number of cores. Of course, if I change the span-wise sections I will have to change that in the code and re-compile it. For now it works and it is fine. I was hesitant to change anything in the code, but your post gave me the encouragement to do so. I want to thank you for your advice. I am surprised they have not corrected this issue. The bug was posted in May 2020 and it still has not been corrected. I am quite surprised.
Thanks
Ashvin

[ashvin]

Hello kuzuner again,
I am sorry to bother you again. Were you able to get the values for TotalEfficiency_1 and TotalStaticEfficiency_1 for the rotor in your history.csv. I keep getting zero. Sorry to bother you.
Thanks
Ashvin

[kuzuner]

Originally Posted by ashvin

Hello kuzuner again,
I am sorry to bother you again. Were you able to get the values for TotalEfficiency_1 and TotalStaticEfficiency_1 for the rotor in your history.csv. I keep getting zero. Sorry to bother you.
Thanks
Ashvin

Hello Ashvin,

I do not need those values in my study but I checked and they are 0 for my case as well.

I use polytropic efficiency and I calculate it with the values I take from post-processing.

Sorry I couldn't be much of a help on this. Good luck.

[ashvin]

Originally Posted by kuzuner

Hello Ashvin,

I do not need those values in my study but I checked and they are 0 for my case as well.

I use polytropic efficiency and I calculate it with the values I take from post-processing.

Sorry I couldn't be much of a help on this. Good luck.

Hi Kuzuner,
No worries. At least I did not do anything wrong. You have been a lot of help! I really appreciate it!
Thanks so much!
Ashvin