Experimental values not matching SU2 values

Kvothe332 · May 14, 2020, 11:58

Hi,
I am new to SU2. I am doing a thesis where I have to first validate experimental value from a paper with SU2 . This is for transonic flow over NACA0012 2D. But for some reason values are not even remotely close to experimental. And sometimes I have "FGMRES failed, linear solution diverged" . To check whether I have any problem with mesh or not, I simulated the mesh in FLUENT and results gave within 6% of the experimental value. I dont know what to do.

[QUOTE]%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% %
%
% %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
% Physical governing equations (EULER, NAVIER_STOKES,
% WAVE_EQUATION, HEAT_EQUATION, FEM_ELASTICITY,
% POISSON_EQUATION)
SOLVER= RANS
%
% Specify turbulent 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
% 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
% -------------------- COMPRESSIBLE FREE-STREAM DEFINITION --------------------%
%
% Mach number (non-dimensional, based on the free-stream values)
MACH_NUMBER= 0.7
%
% Angle of attack (degrees, only for compressible flows)
AOA= 1.55
% 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= 311.0
%
% Reynolds number (non-dimensional, based on the free-stream values)
REYNOLDS_NUMBER= 9E6
%
% Reynolds length (1 m, 1 inch by default)
REYNOLDS_LENGTH= 1
%
% Free-stream density (1.2886 Kg/m^3, 0.0025 slug/ft^3 by default)
FREESTREAM_DENSITY= 1.225
%
%
% Free-stream viscosity (1.853E-5 N s/m^2, 3.87E-7 lbf s/ft^2 by default)
FREESTREAM_VISCOSITY= 1.7894E-5

% Free-stream Turbulence Intensity
FREESTREAM_TURBULENCEINTENSITY = 1
%
% Free-stream Turbulent to Laminar viscosity ratio
FREESTREAM_TURB2LAMVISCRATIO = 1
%
% Compressible flow non-dimensionalization (DIMENSIONAL, FREESTREAM_PRESS_EQ_ONE,
% FREESTREAM_VEL_EQ_MACH, FREESTREAM_VEL_EQ_ONE)
REF_DIMENSIONALIZATION= FREESTREAM_PRESS_EQ_ONE
% ---- IDEAL GAS, POLYTROPIC, VAN DER WAALS AND PENG ROBINSON CONSTANTS -------%
%
% Fluid model (STANDARD_AIR, IDEAL_GAS, VW_GAS, PR_GAS,
% CONSTANT_DENSITY, INC_IDEAL_GAS, INC_IDEAL_GAS_POLY)
FLUID_MODEL= IDEAL_GAS
%
% 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
% --------------------------- VISCOSITY MODEL ---------------------------------%
%
% Viscosity model (SUTHERLAND, CONSTANT_VISCOSITY, POLYNOMIAL_VISCOSITY).
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)
% -------------------------- CL DRIVER DEFINITION -----------------------------%
%
% Activate fixed lift mode (specify a CL instead of AoA, NO/YES)
FIXED_CL_MODE= NO
% ---------------------- REFERENCE VALUE DEFINITION ---------------------------%
%
% Reference origin for moment computation
REF_ORIGIN_MOMENT_X = 0.25
REF_ORIGIN_MOMENT_Y = 0.00
REF_ORIGIN_MOMENT_Z = 0.00
%
% Reference length for pitching, rolling, and yawing non-dimensional moment
REF_LENGTH= 1
%
% Reference area for force coefficients (0 implies automatic calculation)
REF_AREA= 1
% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Navier-Stokes wall boundary marker(s) (NONE = no marker)
MARKER_HEATFLUX= ( AIRFOIL, 0.0 )
MARKER_FAR= ( FF )
%
% Marker(s) of the surface to be plotted or designed
MARKER_PLOTTING= ( AIRFOIL )
%
% Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated
MARKER_MONITORING= ( AIRFOIL )

% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
% Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES)
NUM_METHOD_GRAD= GREEN_GAUSS
%
%
% Adaptive CFL number (NO, YES)
CFL_ADAPT= YES
% Parameters of the adaptive CFL number (factor down, factor up, CFL min value,
% CFL max value )
CFL_ADAPT_PARAM= ( 0.1, 2.0, 5.0, 1e10 )
%
% Number of total iterations
ITER= 5000
%
% Objective function in gradient evaluation (DRAG, LIFT, SIDEFORCE, MOMENT_X,
% MOMENT_Y, MOMENT_Z, EFFICIENCY)
OBJECTIVE_FUNCTION= DRAG
% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
% Convective numerical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, HLLC,
% TURKEL_PREC, MSW)
CONV_NUM_METHOD_FLOW= ROE
%
% Entropy fix coefficient (0.0 implies no entropy fixing, 1.0 implies scalar
% artificial dissipation)
ENTROPY_FIX_COEFF= 0.001
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_FLOW= EULER_IMPLICIT
% Roe Low Dissipation function for Hybrid RANS/LES simulations (FD, NTS, NTS_DUCROS)
ROE_LOW_DISSIPATION= FD
% -------------------- TURBULENT NUMERICAL METHOD DEFINITION ------------------%
%
% Convective numerical method (SCALAR_UPWIND)
CONV_NUM_METHOD_TURB= SCALAR_UPWIND
%
% Time discretization (EULER_IMPLICIT)
TIME_DISCRE_TURB= EULER_IMPLICIT
%
% Reduction factor of the CFL coefficient in the turbulence problem
CFL_REDUCTION_TURB= 1.0

% ------------------------ LINEAR SOLVER DEFINITION ---------------------------%
%
% Linear solver or smoother for implicit formulations:
% BCGSTAB, FGMRES, RESTARTED_FGMRES, CONJUGATE_GRADIENT (self-adjoint problems only), SMOOTHER.
LINEAR_SOLVER= FGMRES
%
%
% Preconditioner of the Krylov linear solver or type of smoother (ILU, LU_SGS, LINELET, JACOBI)
LINEAR_SOLVER_PREC= LU_SGS
%
% Linael 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
LINEAR_SOLVER_RESTART_FREQUENCY= 10
%
% Relaxation factor for smoother-type solvers (LINEAR_SOLVER= SMOOTHER)
LINEAR_SOLVER_SMOOTHER_RELAXATION= 0.5
% -------------------------- 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
% ----------------------- 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, FUSELAGE)
GEO_DESCRIPTION= AIRFOIL
%
% Geometrical evaluation mode (FUNCTION, GRADIENT)
GEO_MODE= FUNCTION

% --------------------------- CONVERGENCE PARAMETERS --------------------------%
%
% Convergence criteria (CAUCHY, RESIDUAL)
CONV_CRITERIA= RESIDUAL
%
% Min value of the residual (log10 of the residual)
CONV_RESIDUAL_MINVAL= -12
%
% 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-4
%

% ------------------------- INPUT/OUTPUT INFORMATION --------------------------%
%
% Mesh input file
MESH_FILENAME= testing.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= solution_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= 10000
%
% Writing convergence history frequency
WRT_CON_FREQ= 1
%
% Screen output
SCREEN_OUTPUT=(INNER_ITER, RMS_DENSITY, RMS_NU_TILDE, LIFT, DRAG)
%
% Output files
OUTPUT_FILES= (RESTART, PARAVIEW, SURFACE_PARAVIEW, SURFACE_CSV)

test.txt

pcg · May 14, 2020, 15:03

Hi,
What is your reference for the experimental results? I can help putting together a better config for your problem.

Few notes:
You are using a first order scheme, your CFL is probably going to very high values, SU2 does not have wall functions you need y+ around 1, but try to keep the aspect ratio near the wall below 1000.

Kvothe332 · May 14, 2020, 15:12

Quote:

Originally Posted by pcg

Hi,
What is your reference for the experimental results? I can help putting together a better config for your problem.

Few notes:
You are using a first order scheme, your CFL is probably going to very high values, SU2 does not have wall functions you need y+ around 1, but try to keep the aspect ratio near the wall below 1000.

Hi,
thanks for the reply
I am using this paper as a reference for now : https://www.researchgate.net/publica...A_0012_Airfoil [this paper has the experimental and fluent simulation also, for my thesis i have to first prove that su2 is reliable]

i dont have any wall. Only farfield and airfoil. My y+ around airfoil should be around 1. Should i limit CFL maximum to some values? And how can i go for 2nd order?

pcg · May 14, 2020, 15:32

With Roe I usually stick with fixed CFL of 20 to 50.
For second order:
NUM_METHOD_GRAD= GREEN_GAUSS
CONV_NUM_METHOD_FLOW= ROE
ENTROPY_FIX_COEFF= 0.01
MUSCL_FLOW= YES
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN_WANG
VENKAT_LIMITER_COEFF= 0.05

If the case goes into a limit cycle oscillation and the residuals stop falling you may need to increase either the limiter coefficient or the entropy correction.

Make sure your farfield boundary really is far just to be safe (more than 50 chords radius).
And if you want to validate, you must do a mesh refinement study, no point drawing conclusions if you are not sure the results are mesh independent.

Kvothe332 · May 14, 2020, 15:42

Quote:

Originally Posted by pcg

With Roe I usually stick with fixed CFL of 20 to 50.
For second order:
NUM_METHOD_GRAD= GREEN_GAUSS
CONV_NUM_METHOD_FLOW= ROE
ENTROPY_FIX_COEFF= 0.01
MUSCL_FLOW= YES
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN_WANG
VENKAT_LIMITER_COEFF= 0.05

If the case goes into a limit cycle oscillation and the residuals stop falling you may need to increase either the limiter coefficient or the entropy correction.

Make sure your farfield boundary really is far just to be safe (more than 50 chords radius).
And if you want to validate, you must do a mesh refinement study, no point drawing conclusions if you are not sure the results are mesh independent.

Thank you for replying.
I will try the second-order and comment back. It's kinda weird that in FLUENT the result is produced and the result is within 6%.

I will also do mesh refinement.

I actually used this video as a reference point for my meshing (more nodes)
https://www.youtube.com/watch?v=9Bc0NBk-urM&t=134s

Kvothe332 · May 14, 2020, 16:50

Quote:

Originally Posted by pcg

With Roe I usually stick with fixed CFL of 20 to 50.
For second order:
NUM_METHOD_GRAD= GREEN_GAUSS
CONV_NUM_METHOD_FLOW= ROE
ENTROPY_FIX_COEFF= 0.01
MUSCL_FLOW= YES
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN_WANG
VENKAT_LIMITER_COEFF= 0.05

If the case goes into a limit cycle oscillation and the residuals stop falling you may need to increase either the limiter coefficient or the entropy correction.

Make sure your farfield boundary really is far just to be safe (more than 50 chords radius).
And if you want to validate, you must do a mesh refinement study, no point drawing conclusions if you are not sure the results are mesh independent.

Hi,
I did try 2nd order and making fixed CFL. but after like 200 iteration the error appears " FGMRES ortogonalization failed, Linear solver diverged"
I dont know why in SU2, it's diverging. In FLUENT it didnt.

pcg · May 14, 2020, 18:54

If your mesh is made up of quadrilaterals, multigrid will help with convergence
MGLEVEL= 2
MGCYCLE= V_CYCLE
MG_PRE_SMOOTH= ( 1, 1, 2, 2 )
MG_POST_SMOOTH= ( 0, 0, 0, 0 )
MG_CORRECTION_SMOOTH= ( 0, 0, 0, 0 )
MG_DAMP_RESTRICTION= 0.7
MG_DAMP_PROLONGATION= 0.7

I played around a bit and I don't think you will match these particular results, I get CL ~ 0.25 and CD ~ 0.009, with farfield radius of 100c.
The wall effects for those results seem very strong (difference between the measured and corrected columns) for example with farfield radius of 5c the CL goes down to 0.22 (the working section of that wind tunnel is about 3c).
Back when I started using SU2 I compared the results with what is available from NASA's TMR (https://turbmodels.larc.nasa.gov/naca0012_val.html) and that SU2 matches quite well.
There is also a V&V SU2 repository (https://github.com/su2code/VandV) have a look at the settings they use, types of meshes and so on, it should help you get going with SU2.
Despite our best efforts the code is a lot less forgiving than commercial CFD software...

Kvothe332 · May 14, 2020, 19:09

Quote:

Originally Posted by pcg

If your mesh is made up of quadrilaterals, multigrid will help with convergence
MGLEVEL= 2
MGCYCLE= V_CYCLE
MG_PRE_SMOOTH= ( 1, 1, 2, 2 )
MG_POST_SMOOTH= ( 0, 0, 0, 0 )
MG_CORRECTION_SMOOTH= ( 0, 0, 0, 0 )
MG_DAMP_RESTRICTION= 0.7
MG_DAMP_PROLONGATION= 0.7

I played around a bit and I don't think you will match these particular results, I get CL ~ 0.25 and CD ~ 0.009, with farfield radius of 100c.
The wall effects for those results seem very strong (difference between the measured and corrected columns) for example with farfield radius of 5c the CL goes down to 0.22 (the working section of that wind tunnel is about 3c).
Back when I started using SU2 I compared the results with what is available from NASA's TMR (https://turbmodels.larc.nasa.gov/naca0012_val.html) and that SU2 matches quite well.
There is also a V&V SU2 repository (https://github.com/su2code/VandV) have a look at the settings they use, types of meshes and so on, it should help you get going with SU2.
Despite our best efforts the code is a lot less forgiving than commercial CFD software...

Thank you for your reply and having patience with a newbie like me.
I appreciate you did the simulation and provided me with solutions. I never used SU2 and never knew farfield can have this much effect on the result bcs fluent never complained even if i gave like 5c.
I will do the meshing from scratch with bigger farfield and do miltigrid( my mesh is quadrilateral) and comment back here.
Do you think i should change any other setting from the config file?
Do you think 20c which i am using right now is making the divergeance problem?

Kvothe332 · May 15, 2020, 03:47

Quote:

Originally Posted by pcg

With Roe I usually stick with fixed CFL of 20 to 50.
For second order:
NUM_METHOD_GRAD= GREEN_GAUSS
CONV_NUM_METHOD_FLOW= ROE
ENTROPY_FIX_COEFF= 0.01
MUSCL_FLOW= YES
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN_WANG
VENKAT_LIMITER_COEFF= 0.05

If the case goes into a limit cycle oscillation and the residuals stop falling you may need to increase either the limiter coefficient or the entropy correction.

Make sure your farfield boundary really is far just to be safe (more than 50 chords radius).
And if you want to validate, you must do a mesh refinement study, no point drawing conclusions if you are not sure the results are mesh independent.

Quote:

Originally Posted by pcg

If your mesh is made up of quadrilaterals, multigrid will help with convergence
MGLEVEL= 2
MGCYCLE= V_CYCLE
MG_PRE_SMOOTH= ( 1, 1, 2, 2 )
MG_POST_SMOOTH= ( 0, 0, 0, 0 )
MG_CORRECTION_SMOOTH= ( 0, 0, 0, 0 )
MG_DAMP_RESTRICTION= 0.7
MG_DAMP_PROLONGATION= 0.7

I played around a bit and I don't think you will match these particular results, I get CL ~ 0.25 and CD ~ 0.009, with farfield radius of 100c.
The wall effects for those results seem very strong (difference between the measured and corrected columns) for example with farfield radius of 5c the CL goes down to 0.22 (the working section of that wind tunnel is about 3c).
Back when I started using SU2 I compared the results with what is available from NASA's TMR (https://turbmodels.larc.nasa.gov/naca0012_val.html) and that SU2 matches quite well.
There is also a V&V SU2 repository (https://github.com/su2code/VandV) have a look at the settings they use, types of meshes and so on, it should help you get going with SU2.
Despite our best efforts the code is a lot less forgiving than commercial CFD software...

I did the meshing again and this time with 500c. But the same error message comes in after 200-300 iteration (FGMRES orthogonalization failed, Linear solver diverged)

pcg · May 15, 2020, 04:21

Having the farfield too close will influence the results but not the convergence (if anything it will make it easier). I'm attaching my config maybe it will work better.
Be careful with the mesh quality, especially the cell aspect ratio near the wall and the skewness (aka orthogonality, angle between sides of the primal cells).
These are the stats for the mesh I used:

Code:

+--------------------------------------------------------------+
|           Mesh Quality Metric|        Minimum|        Maximum|
+--------------------------------------------------------------+
|    Orthogonality Angle (deg.)|        50.3543|             90|
|     CV Face Area Aspect Ratio|        1.00151|        4489.01|
|           CV Sub-Volume Ratio|        1.00027|        3.35962|
+--------------------------------------------------------------+

config.txt

Kvothe332 · May 15, 2020, 04:49

Quote:

Originally Posted by pcg

Having the farfield too close will influence the results but not the convergence (if anything it will make it easier). I'm attaching my config maybe it will work better.
Be careful with the mesh quality, especially the cell aspect ratio near the wall and the skewness (aka orthogonality, angle between sides of the primal cells).
These are the stats for the mesh I used:

Code:

+--------------------------------------------------------------+
|           Mesh Quality Metric|        Minimum|        Maximum|
+--------------------------------------------------------------+
|    Orthogonality Angle (deg.)|        50.3543|             90|
|     CV Face Area Aspect Ratio|        1.00151|        4489.01|
|           CV Sub-Volume Ratio|        1.00027|        3.35962|
+--------------------------------------------------------------+

Attachment 77655

I think there are some problems in my meshing. maximum aspect ratio is way too high. May be that's why my solution is diverging.

pcg · May 15, 2020, 05:00

That's 100% why it is diverging.

May 14, 2020, 11:58	Experimental values not matching SU2 values	#1
Kvothe332 New Member Md Anwar Parvez Join Date: May 2020 Posts: 8 Rep Power: 5	Hi, I am new to SU2. I am doing a thesis where I have to first validate experimental value from a paper with SU2 . This is for transonic flow over NACA0012 2D. But for some reason values are not even remotely close to experimental. And sometimes I have "FGMRES failed, linear solution diverged" . To check whether I have any problem with mesh or not, I simulated the mesh in FLUENT and results gave within 6% of the experimental value. I dont know what to do. [QUOTE]%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%% % % % % % %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%% % ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------% % % Physical governing equations (EULER, NAVIER_STOKES, % WAVE_EQUATION, HEAT_EQUATION, FEM_ELASTICITY, % POISSON_EQUATION) SOLVER= RANS % % Specify turbulent 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 % 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 % -------------------- COMPRESSIBLE FREE-STREAM DEFINITION --------------------% % % Mach number (non-dimensional, based on the free-stream values) MACH_NUMBER= 0.7 % % Angle of attack (degrees, only for compressible flows) AOA= 1.55 % 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= 311.0 % % Reynolds number (non-dimensional, based on the free-stream values) REYNOLDS_NUMBER= 9E6 % % Reynolds length (1 m, 1 inch by default) REYNOLDS_LENGTH= 1 % % Free-stream density (1.2886 Kg/m^3, 0.0025 slug/ft^3 by default) FREESTREAM_DENSITY= 1.225 % % % Free-stream viscosity (1.853E-5 N s/m^2, 3.87E-7 lbf s/ft^2 by default) FREESTREAM_VISCOSITY= 1.7894E-5 % Free-stream Turbulence Intensity FREESTREAM_TURBULENCEINTENSITY = 1 % % Free-stream Turbulent to Laminar viscosity ratio FREESTREAM_TURB2LAMVISCRATIO = 1 % % Compressible flow non-dimensionalization (DIMENSIONAL, FREESTREAM_PRESS_EQ_ONE, % FREESTREAM_VEL_EQ_MACH, FREESTREAM_VEL_EQ_ONE) REF_DIMENSIONALIZATION= FREESTREAM_PRESS_EQ_ONE % ---- IDEAL GAS, POLYTROPIC, VAN DER WAALS AND PENG ROBINSON CONSTANTS -------% % % Fluid model (STANDARD_AIR, IDEAL_GAS, VW_GAS, PR_GAS, % CONSTANT_DENSITY, INC_IDEAL_GAS, INC_IDEAL_GAS_POLY) FLUID_MODEL= IDEAL_GAS % % 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/kgK default and this value is hardcoded % for the model STANDARD_AIR, compressible only) GAS_CONSTANT= 287.058 % --------------------------- VISCOSITY MODEL ---------------------------------% % % Viscosity model (SUTHERLAND, CONSTANT_VISCOSITY, POLYNOMIAL_VISCOSITY). 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 + b1T + b2T^2 + b3T^3 + b4*T^4 MU_POLYCOEFFS= (0.0, 0.0, 0.0, 0.0, 0.0) % -------------------------- CL DRIVER DEFINITION -----------------------------% % % Activate fixed lift mode (specify a CL instead of AoA, NO/YES) FIXED_CL_MODE= NO % ---------------------- REFERENCE VALUE DEFINITION ---------------------------% % % Reference origin for moment computation REF_ORIGIN_MOMENT_X = 0.25 REF_ORIGIN_MOMENT_Y = 0.00 REF_ORIGIN_MOMENT_Z = 0.00 % % Reference length for pitching, rolling, and yawing non-dimensional moment REF_LENGTH= 1 % % Reference area for force coefficients (0 implies automatic calculation) REF_AREA= 1 % -------------------- BOUNDARY CONDITION DEFINITION --------------------------% % % Navier-Stokes wall boundary marker(s) (NONE = no marker) MARKER_HEATFLUX= ( AIRFOIL, 0.0 ) MARKER_FAR= ( FF ) % % Marker(s) of the surface to be plotted or designed MARKER_PLOTTING= ( AIRFOIL ) % % Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated MARKER_MONITORING= ( AIRFOIL ) % ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------% % % Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES) NUM_METHOD_GRAD= GREEN_GAUSS % % % Adaptive CFL number (NO, YES) CFL_ADAPT= YES % Parameters of the adaptive CFL number (factor down, factor up, CFL min value, % CFL max value ) CFL_ADAPT_PARAM= ( 0.1, 2.0, 5.0, 1e10 ) % % Number of total iterations ITER= 5000 % % Objective function in gradient evaluation (DRAG, LIFT, SIDEFORCE, MOMENT_X, % MOMENT_Y, MOMENT_Z, EFFICIENCY) OBJECTIVE_FUNCTION= DRAG % -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------% % % Convective numerical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, HLLC, % TURKEL_PREC, MSW) CONV_NUM_METHOD_FLOW= ROE % % Entropy fix coefficient (0.0 implies no entropy fixing, 1.0 implies scalar % artificial dissipation) ENTROPY_FIX_COEFF= 0.001 % % Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT) TIME_DISCRE_FLOW= EULER_IMPLICIT % Roe Low Dissipation function for Hybrid RANS/LES simulations (FD, NTS, NTS_DUCROS) ROE_LOW_DISSIPATION= FD % -------------------- TURBULENT NUMERICAL METHOD DEFINITION ------------------% % % Convective numerical method (SCALAR_UPWIND) CONV_NUM_METHOD_TURB= SCALAR_UPWIND % % Time discretization (EULER_IMPLICIT) TIME_DISCRE_TURB= EULER_IMPLICIT % % Reduction factor of the CFL coefficient in the turbulence problem CFL_REDUCTION_TURB= 1.0 % ------------------------ LINEAR SOLVER DEFINITION ---------------------------% % % Linear solver or smoother for implicit formulations: % BCGSTAB, FGMRES, RESTARTED_FGMRES, CONJUGATE_GRADIENT (self-adjoint problems only), SMOOTHER. LINEAR_SOLVER= FGMRES % % % Preconditioner of the Krylov linear solver or type of smoother (ILU, LU_SGS, LINELET, JACOBI) LINEAR_SOLVER_PREC= LU_SGS % % Linael 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 LINEAR_SOLVER_RESTART_FREQUENCY= 10 % % Relaxation factor for smoother-type solvers (LINEAR_SOLVER= SMOOTHER) LINEAR_SOLVER_SMOOTHER_RELAXATION= 0.5 % -------------------------- 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 % ----------------------- 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, FUSELAGE) GEO_DESCRIPTION= AIRFOIL % % Geometrical evaluation mode (FUNCTION, GRADIENT) GEO_MODE= FUNCTION % --------------------------- CONVERGENCE PARAMETERS --------------------------% % % Convergence criteria (CAUCHY, RESIDUAL) CONV_CRITERIA= RESIDUAL % % Min value of the residual (log10 of the residual) CONV_RESIDUAL_MINVAL= -12 % % 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-4 % % ------------------------- INPUT/OUTPUT INFORMATION --------------------------% % % Mesh input file MESH_FILENAME= testing.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= solution_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= 10000 % % Writing convergence history frequency WRT_CON_FREQ= 1 % % Screen output SCREEN_OUTPUT=(INNER_ITER, RMS_DENSITY, RMS_NU_TILDE, LIFT, DRAG) % % Output files OUTPUT_FILES= (RESTART, PARAVIEW, SURFACE_PARAVIEW, SURFACE_CSV) test.txt

May 15, 2020, 04:21		#10
pcg Senior Member Pedro Gomes Join Date: Dec 2017 Posts: 465 Rep Power: 13	Having the farfield too close will influence the results but not the convergence (if anything it will make it easier). I'm attaching my config maybe it will work better. Be careful with the mesh quality, especially the cell aspect ratio near the wall and the skewness (aka orthogonality, angle between sides of the primal cells). These are the stats for the mesh I used: Code: +--------------------------------------------------------------+ \| Mesh Quality Metric\| Minimum\| Maximum\| +--------------------------------------------------------------+ \| Orthogonality Angle (deg.)\| 50.3543\| 90\| \| CV Face Area Aspect Ratio\| 1.00151\| 4489.01\| \| CV Sub-Volume Ratio\| 1.00027\| 3.35962\| +--------------------------------------------------------------+ config.txt

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Introducing SU2 International Developers Society (IDS)	fpalacios	SU2 News & Announcements	1	June 17, 2019 22:38
using chemkin	JMDag2004	OpenFOAM Pre-Processing	2	March 8, 2016 22:38
Pressure value not matching to experimental result	Bisht	STAR-CCM+	10	November 25, 2015 00:58
Flow 3d results and real Experimental results not matching?	Subodh21	FLOW-3D	0	July 21, 2014 14:52
Need Help- Values not matching	umm..	FLUENT	0	February 22, 2008 09:28

May 14, 2020, 15:03		#2
pcg Senior Member Pedro Gomes Join Date: Dec 2017 Posts: 465 Rep Power: 13	Hi, What is your reference for the experimental results? I can help putting together a better config for your problem. Few notes: You are using a first order scheme, your CFL is probably going to very high values, SU2 does not have wall functions you need y+ around 1, but try to keep the aspect ratio near the wall below 1000.

May 14, 2020, 15:32		#4
pcg Senior Member Pedro Gomes Join Date: Dec 2017 Posts: 465 Rep Power: 13	With Roe I usually stick with fixed CFL of 20 to 50. For second order: NUM_METHOD_GRAD= GREEN_GAUSS CONV_NUM_METHOD_FLOW= ROE ENTROPY_FIX_COEFF= 0.01 MUSCL_FLOW= YES SLOPE_LIMITER_FLOW= VENKATAKRISHNAN_WANG VENKAT_LIMITER_COEFF= 0.05 If the case goes into a limit cycle oscillation and the residuals stop falling you may need to increase either the limiter coefficient or the entropy correction. Make sure your farfield boundary really is far just to be safe (more than 50 chords radius). And if you want to validate, you must do a mesh refinement study, no point drawing conclusions if you are not sure the results are mesh independent.

May 14, 2020, 18:54		#7
pcg Senior Member Pedro Gomes Join Date: Dec 2017 Posts: 465 Rep Power: 13	If your mesh is made up of quadrilaterals, multigrid will help with convergence MGLEVEL= 2 MGCYCLE= V_CYCLE MG_PRE_SMOOTH= ( 1, 1, 2, 2 ) MG_POST_SMOOTH= ( 0, 0, 0, 0 ) MG_CORRECTION_SMOOTH= ( 0, 0, 0, 0 ) MG_DAMP_RESTRICTION= 0.7 MG_DAMP_PROLONGATION= 0.7 I played around a bit and I don't think you will match these particular results, I get CL ~ 0.25 and CD ~ 0.009, with farfield radius of 100c. The wall effects for those results seem very strong (difference between the measured and corrected columns) for example with farfield radius of 5c the CL goes down to 0.22 (the working section of that wind tunnel is about 3c). Back when I started using SU2 I compared the results with what is available from NASA's TMR (https://turbmodels.larc.nasa.gov/naca0012_val.html) and that SU2 matches quite well. There is also a V&V SU2 repository (https://github.com/su2code/VandV) have a look at the settings they use, types of meshes and so on, it should help you get going with SU2. Despite our best efforts the code is a lot less forgiving than commercial CFD software...

May 15, 2020, 05:00		#12
pcg Senior Member Pedro Gomes Join Date: Dec 2017 Posts: 465 Rep Power: 13	That's 100% why it is diverging.