[shahidkhan]

I am trying to run a 3-D case. Flow is supersonic, turbulent. When I am using first order scheme, solution converges to some extent then residuals become almost constant. On using higher order scheme (MUSCL_FLOW=YES) my solution initially converges for some iterations but then starts to diverge. (I have checked mesh. Issue is not with that although not 100% sure). Please look into config file for reference. I have also attached the domain with this for reference.

Note- After 120 iterations it says SU2 has diverged. NaN detected


% ------------- 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, SA_E, SA_COMP, SA_E_COMP, SST_SUST)
KIND_TURB_MODEL= SA
%
% specify transition model (NONE, LM, BC)
%KIND_TRANS_MODEL= NONE
%FREESTREAM_TURBULENCEINTENSITY= 0.10
%
% Mathematical problem (DIRECT, CONTINUOUS_ADJOINT)
MATH_PROBLEM= DIRECT
%
% Axisymmetric simulation, only compressible flows (NO, YES)
%AXISYMMETRIC= NO

% Restart solution (NO, YES)
RESTART_SOL= NO
%
SYSTEM_MEASUREMENTS= SI

% -------------------- COMPRESSIBLE FREE-STREAM DEFINITION --------------------%
%
% Mach number (non-dimensional, based on the free-stream values)
MACH_NUMBER= 2.5
%
% Angle of attack (degrees, only for compressible flows)
AOA= 0.00
%
% 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= 140.0
%
FREESTREAM_PRESSURE= 32500.0
%
% Reynolds number (non-dimensional, based on the free-stream values)
REYNOLDS_NUMBER= 5.3E7
%
% Reynolds length (1 m by default)
REYNOLDS_LENGTH= 1.0

% ---- 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
%
% 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), only for CONSTANT_PRANDTL)
PRANDTL_TURB= 0.90

% ---------------------- 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= 1.0
%
% 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 --------------------------%
%
% Navier-Stokes wall boundary marker(s) (NONE = no marker)
MARKER_HEATFLUX= ( wall, 0.0 )
%
% Inlet boundary type (TOTAL_CONDITIONS, MASS_FLOW)
%INLET_TYPE= TOTAL_CONDITIONS
%
MARKER_SUPERSONIC_INLET= ( inlet, 140.0, 32500.0, 592.9975126, 0.0, 0.0 )
%
MARKER_SUPERSONIC_OUTLET= ( outlet )
%
% Far-field boundary marker(s) (NONE = no marker)
%
% Symmetry boundary marker(s) (NONE = no marker)
MARKER_SYM= ( symmetry )
%
% Marker(s) of the surface to be plotted or designed
MARKER_PLOTTING= ( wall )
%
% Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated
MARKER_MONITORING= ( wall )

% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
% Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES, LEAST_SQUARES)
NUM_METHOD_GRAD= GREEN_GAUSS
%
% Courant-Friedrichs-Lewy condition of the finest grid
CFL_NUMBER= 0.5
%
% 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= ( 1.0, 1.1, 0.5, 5.0 )
%
% Maximum Delta Time in local time stepping simulations
%MAX_DELTA_TIME= 1E6
%
% 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, SMOOTHER, RESTARTED_FGMRES )
LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver (NONE, JACOBI, LINELET, LU_SGS, LINELET)
LINEAR_SOLVER_PREC= ILU
%
% Min error of the linear solver for the implicit formulation
LINEAR_SOLVER_ERROR= 1E-10
%
% 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, JST_KE, JST_MAT, LAX-FRIEDRICH, CUSP, ROE, AUSM,
% AUSMPLUSUP, AUSMPLUSUP2, AUSMPWPLUS, HLLC, TURKEL_PREC,
% SW, MSW, FDS, SLAU, SLAU2, L2ROE, LMROE)
CONV_NUM_METHOD_FLOW= AUSMPLUSUP2
%
% 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= YES
%
% Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER)
MUSCL_FLOW= YES
%
% Slope limiter (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG,
% BARTH_JESPERSEN, VAN_ALBADA_EDGE)
SLOPE_LIMITER_FLOW= VAN_ALBADA_EDGE
%
% 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= 0.03
%
% 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_CRTERIA= RESIDUAL
%
CONV_FIELD= RMS_DENSITY
%
%min value of residual (log10of residual)
CONV_RESIDUAL_MINVAL= -9
%
% 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= extrude_mesh.su2
%
% Mesh input file format (SU2, CGNS, NETCDF_ASCII)
MESH_FORMAT= SU2
%
% Mesh output file
MESH_OUT_FILENAME= mesh_out.su2
%
% Restart flow input file
SOLUTION_FILENAME= restart_after_320_iter.dat
%
% Restart adjoint input file
SOLUTION_ADJ_FILENAME= solution_adj.dat
%
% Output file format (PARAVIEW, TECPLOT, STL)
TABULAR_FORMAT= TECPLOT
%
%Output files
%OUTPUT_FILES= (TECPLOT )
%
% 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
%
%
% Screen output
SCREEN_OUTPUT= (INNER_ITER, WALL_TIME, RMS_DENSITY, RMS_MOMENTUM-X, RMS_MOMENTUM-Y, RMS_MOMENTUM-Z, RMS_ENERGY, AVG_CFL, MIN_CFL, MAX_CFL)
% history output
HISTORY_OUTPUT= (ITER, RMS_RES, AVG_CFL, MIN_CFL, MAX_CFL )
%volume output fields
VOLUME_OUTPUT= (COORDINATES, DENSITY, MOMENTUM-X, MOMENTUM-Y, MOMENTUM-Z, PRESSURE, TEMPERATURE, MACH )
% Writing frequency for volume/surface output
OUTPUT_WRT_FREQ= 10

[pcg]

If you have a viscous wall your outlet is not going to be all supersonic.

[shahidkhan]

Yes you are right. I also thought of this but in my reference paper all the outlet (the top, rear and sides) are considered as supersonic outlet, hence I am trying the same.

[PENGGEGE777]

I meet the same problem for my simulatio of underexpanded jet flow.

converge with 1st order ROE and diverge with 2nd orde ROE....................

[shahidkhan]

Did you found the solution?

[PENGGEGE777]

Originally Posted by shahidkhan

Did you found the solution?

Not yet, I tried to use Fluent with 2nd order method, and it converges.

So I am focusing on the difference of 2nd order method between Fluent and SU2, and how they are implemented.

[shahidkhan]

Oh. I am also trying it on ANSYS. Please update with the progress in SU2 when you make some.

[PENGGEGE777]

Sure, man , let us share our findings here.

[PENGGEGE777]

Hi man ,I can make my simulation converges, with 2nd order ROE scheme.
The following is my config file, you can have a try of this kind of numerical setup.


%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% %
% SU2 configuration file %
% Case description: Non-ideal compressible fluid flow in a converging- %
% diverging supersonic nozzle for siloxane fluid MDM %
% Author: Alberto Guardone %
% Institution: Politecnico di Milano %
% Date: 2019.05.03 %
% File Version 6.2.0 "Falcon" %
% %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
% Physical governing equations (EULER, NAVIER_STOKES,
% FEM_EULER, FEM_NAVIER_STOKES, FEM_RANS, FEM_LES,
% WAVE_EQUATION, HEAT_EQUATION, FEM_ELASTICITY,
% POISSON_EQUATION)
SOLVER= EULER
AXISYMMETRIC = YES
%
% Specify turbulence model (NONE, SA, SA_NEG, SST, SA_E, SA_COMP, SA_E_COMP)
KIND_TURB_MODEL= SA
%
% Mathematical problem (DIRECT, CONTINUOUS_ADJOINT, DISCRETE_ADJOINT)
MATH_PROBLEM= DIRECT
%
% Restart solution (NO, YES)
RESTART_SOL= YES
%
% 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= 1e-9
%
% 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 pressure (101325.0 N/m^2, 2116.216 psf by default)
FREESTREAM_PRESSURE= 803430
%
% Free-stream temperature (288.15 K, 518.67 R by default)
FREESTREAM_TEMPERATURE=336.7
%
% Compressible flow non-dimensionalization (DIMENSIONAL, FREESTREAM_PRESS_EQ_ONE,
% FREESTREAM_VEL_EQ_MACH, FREESTREAM_VEL_EQ_ONE)
REF_DIMENSIONALIZATION= DIMENSIONAL

% ---- 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= 297
%
% Critical Temperature (131.00 K by default)
%CRITICAL_TEMPERATURE= 565.3609
%
% Critical Pressure (3588550.0 N/m^2 by default)
%CRITICAL_PRESSURE= 1437500
%
% Acentric factor (0.035 (air))
%ACENTRIC_FACTOR= 0.524

% --------------------------- 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= 1.21409E-05

% --------------------------- THERMAL CONDUCTIVITY MODEL ----------------------%
%
% Laminar Conductivity model (CONSTANT_CONDUCTIVITY, CONSTANT_PRANDTL,
% POLYNOMIAL_CONDUCTIVITY).
%CONDUCTIVITY_MODEL= CONSTANT_CONDUCTIVITY
%
% Molecular Thermal Conductivity that would be constant (0.0257 by default)
%KT_CONSTANT= 0.030542828

% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Navier-Stokes (no-slip), constant heat flux wall marker(s) (NONE = no marker)
% Format: ( marker name, constant heat flux (J/m^2), ... )

MARKER_EULER= (WALL)
%MARKER_HEATFLUX = (WALL, 0.0)
% Symmetry boundary marker(s) (NONE = no marker)
MARKER_SYM= ( SYMMETRY )
%
% Riemann boundary marker(s) (NONE = no marker)
% Format: (marker, data kind flag, list of data)
%MARKER_RIEMANN= ( INLET, TOTAL_CONDITIONS_PT, 803430, 336.7, 1.0, 0.0, 0.0, OUTLET, STATIC_PRESSURE, 100430, 0.0, 0.0, 0.0, 0.0 )
MARKER_RIEMANN= ( INLET, TOTAL_CONDITIONS_PT, 803430, 336.7, 1.0, 0.0, 0.0, TOP, STATIC_PRESSURE, 100430, 0.0, 0.0, 0.0, 0.0, OUTLET, STATIC_PRESSURE, 100430, 0.0, 0.0, 0.0, 0.0 )

MARKER_PLOTTING = ( TOP,OUTLET )
MARKER_MONITORING = ( TOP,OUTLET )
% ------------- 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 = 10
%
% 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, 1.1, 0.1, 1000.0 )
%
% Maximum Delta Time in local time stepping simulations
MAX_DELTA_TIME= 1E6

% ----------- 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
%
% Slope limiter (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG,
% BARTH_JESPERSEN, VAN_ALBADA_EDGE)
SLOPE_LIMITER_FLOW=VENKATAKRISHNAN

VENKAT_LIMITER_COEFF= 0.01
%
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the turbulence equations.
% Required for 2nd order upwind schemes (NO, YES)
MUSCL_TURB= NO

% ------------------------ LINEAR SOLVER DEFINITION ---------------------------%
%
% Linear solver or smoother for implicit formulations (BCGSTAB, FGMRES, SMOOTHER_JACOBI,
% SMOOTHER_ILU, SMOOTHER_LUSGS,
% SMOOTHER_LINELET)
LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver (ILU, LU_SGS, LINELET, JACOBI)
LINEAR_SOLVER_PREC= ILU
%
% 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= 10

% -------------------------- MULTIGRID PARAMETERS -----------------------------%
%
% Multi-grid levels (0 = no multi-grid)
MGLEVEL= 0

% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
% Convective numrical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, AUSMPLUSUP, AUSMPLUSUP2, HLLC,
% TURKEL_PREC, MSW, FDS)
CONV_NUM_METHOD_FLOW = ROE
%
% Entropy fix coefficient (0.0 implies no entropy fixing, 1.0 implies scalar
% artificial dissipation)
ENTROPY_FIX_COEFF= 0.1
%
% 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
%
% Time discretization (EULER_IMPLICIT)
TIME_DISCRE_TURB= EULER_IMPLICIT
%
% Reduction factor of the CFL coefficient in the turbulence problem
CFL_REDUCTION_TURB= 1.0

% --------------------------- CONVERGENCE PARAMETERS --------------------------%
%
% Number of total iterations
ITER= 100000
%
% Convergence criteria (CAUCHY, RESIDUAL)
%
CONV_CRITERIA= RESIDUAL
%
%
% Min value of the residual (log10 of the residual)
CONV_RESIDUAL_MINVAL= -11
%
% Start convergence criteria at iteration number
CONV_STARTITER= 10

% ------------------------- INPUT/OUTPUT INFORMATION --------------------------%
%
% Mesh input file
MESH_FILENAME= total.su2
%
% Mesh input file format (SU2, CGNS)
MESH_FORMAT= SU2
%
% Mesh output file
MESH_OUT_FILENAME= mesh_out.su2
%
% Restart flow input file
SOLUTION_FILENAME= solution_flow.dat
%
% Output file format (TECPLOT, TECPLOT_BINARY, PARAVIEW, PARAVIEW_BINARY,
% FIELDVIEW, FIELDVIEW_BINARY)
TABULAR_FORMAT= CSV
%
% Output file convergence history (w/o extension)
CONV_FILENAME= history
%
% Output file restart flow
RESTART_FILENAME= restart_flow.dat
%
% Output file flow (w/o extension) variables
VOLUME_FILENAME= flow
%
% Output file surface flow coefficient (w/o extension)
SURFACE_FILENAME= surface_flow
%
% Writing solution file frequency
OUTPUT_WRT_FREQ= 100
%
% Screen output
SCREEN_WRT_FREQ_OUTER = 1
SCREEN_OUTPUT= ( INNER_ITER, RMS_DENSITY, RMS_ENERGY,RMS_TKE, RMS_DISSIPATION,NONPHYSICAL_POINTS)

[PENGGEGE777]

From your description, your simulation can converge with 1st order, but diverge with 2nd order scheme.

Then the main problem should be your numerical scheme.

You can try different scheme, like ROE, HLLC, and so on.

Also, to avoid spurious oscillation around discontinuity, e.g., shock, you should choose appropiate slope limitet, like VENKATAKRISHNAN = 0.01.

THere is no 'a size fits all'. Hence, for scheme, slope limiter and its coeffciient, you have to trial and error.

Good luck man, and if you succeed, please share your config file here, thanks.

[shahidkhan]

Can you please tell me what was the issue in your case and what changes you made which made it to work?

[PENGGEGE777]

I think there are two main changes:

1. add Numerical method for spatial gradients when MUSCL is on

% 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

2. choose suitable slope limiter

SLOPE_LIMITER_FLOW=VENKATAKRISHNAN

VENKAT_LIMITER_COEFF= 0.01

[shahidkhan]

Sure. Really thanks to you. I will try my case with that. Will update it here too.

[ander]

Any luck with finding robust configurations? In general I can say that for my relatively limited experience with SU2, I'm only able to get reliable convergence with the JST central scheme.