[ari003]

Hello everyone, hope you all are doing fine and happy 2022. I am here seeking for some advice or suggestion related to my simulation work. I am running a transonic case of super-critical airfoil with Mach 0.8 and do observe immense oscillation in the lift curve field which is inhibiting it towards convergence. I am using AUSM +up convective scheme with MUSCL and the .cfg file is as below

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% %
% SU2 configuration file %
% Case description: Unsteady periodic detached NACA0012 simulation %
% Author: Steffen Schotthöfer %
% Institution: TU Kaiserslautern %
% Date: Jan 21, 2020 %
% File Version 7.0.1 "Blackbird" (or newer) %
% %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
% Physical governing equations (EULER, NAVIER_STOKES, NS_PLASMA)
%
SOLVER= RANS
%
% Specify turbulent model (NONE, SA, SA_NEG, SST)
KIND_TURB_MODEL= SST
%
% Mathematical problem (DIRECT, CONTINUOUS_ADJOINT)
MATH_PROBLEM= DIRECT
%
TIME_DOMAIN = NO
%
% ------------------------- UNSTEADY SIMULATION -------------------------------%
%
%
% Numerical Method for Unsteady simulation(NO, TIME_STEPPING, DUAL_TIME_STEPPING-1ST_ORDER, DUAL_TIME_STEPPING-2ND_ORDER, TIME_SPECTRAL)
%TIME_MARCHING= DUAL_TIME_STEPPING-2ND_ORDER
%
% Time Step for dual time stepping simulations (s)
%TIME_STEP= 5e-4
%
% Maximum Number of physical time steps.
%TIME_ITER= 2200
%
% Number of internal iterations (dual time method)
%INNER_ITER= 100
%
% Restart after the transient phase has passed
RESTART_SOL = YES
%
% Specify unsteady restart iter
%RESTART_ITER = 6
% -------------------- 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
%
% De-Dimensionalization
REF_DIMENSIONALIZATION = DIMENSIONAL
%
%FREESTREAM_OPTION= TEMPERATURE_FS
%
%FREESTREAM_PRESSURE= 66486.2
% Free-stream temperature (288.15 K by default)
FREESTREAM_TEMPERATURE= 263.3
%
% Reynolds number (non-dimensional, based on the free-stream values)
REYNOLDS_NUMBER= 1.37e+7
%
% Reynolds length (1 m by default)
REYNOLDS_LENGTH= 1.0
% --------------------------- VISCOSITY MODEL ---------------------------------%
%
% Viscosity model (SUTHERLAND, CONSTANT_VISCOSITY).
VISCOSITY_MODEL= SUTHERLAND
%
% Molecular Viscosity that would be constant (1.716E-5 by default)
MU_CONSTANT= 1.81e-05
%
% ---------------------- 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= 1.0
%
% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Navier-Stokes wall boundary marker(s) (NONE = no marker)
MARKER_HEATFLUX= ( wall_upper,0.0, wall_lower,0.0)
%
% Farfield boundary marker(s) (NONE = no marker)
MARKER_FAR= ( farfield)
%
% Marker(s) of the surface to be plotted or designed
MARKER_PLOTTING= (wall_upper)
%
%INC_INLET_TYPE= TOTAL_CONDITIONS
%MARKER_INLET = (inlet, 293, 101325.0, 1, 0.0, 0.0)
%
%INC_OUTLET_TYPE= PRESSURE_OUTLET
%MARKER_OUTLET = (outlet, 1e3)
%
% Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated
MARKER_MONITORING= (wall_upper, wall_lower)
%
% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
% Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES)
NUM_METHOD_GRAD= WEIGHTED_LEAST_SQUARES
%
% Courant-Friedrichs-Lewy condition of the finest grid
CFL_NUMBER= 20
%
% 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= ( 0.5, 1.5, 1, 50.0 )
%
% Runge-Kutta alpha coefficients
RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 )
%
%
% Linear solver for the implicit formulation (BCGSTAB, FGMRES)
%LINEAR_SOLVER= FGMRES
%
% Min error of the linear solver for the implicit formulation
%LINEAR_SOLVER_ERROR= 1E-6
%
% Max number of iterations of the linear solver for the implicit formulation
%LINEAR_SOLVER_ITER= 5
%
% Number of total iterations
ITER= 35000
%
% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
% Convective numerical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, HLLC,
% TURKEL_PREC, MSW)
CONV_NUM_METHOD_FLOW= AUSMPLUSUP
%
% Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER)
MUSCL_FLOW= YES
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN
%
% 1st, 2nd and 4th order artificial dissipation coefficients
JST_SENSOR_COEFF= ( 0.5, 0.01 )
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_FLOW= EULER_IMPLICIT
%
% Linear solver for implicit formulations (BCGSTAB, FGMRES)
LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver (JACOBI, LINELET, LU_SGS)
LINEAR_SOLVER_PREC= ILU
% -------------------- TURBULENT NUMERICAL METHOD DEFINITION ------------------%
%
% Convective numerical method (SCALAR_UPWIND)
CONV_NUM_METHOD_TURB= SCALAR_UPWIND
%
% Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER)
%
MUSCL_TURB= NO
%
% Time discretization (EULER_IMPLICIT)
TIME_DISCRE_TURB= EULER_IMPLICIT
%
% --------------------------- CONVERGENCE PARAMETERS --------------------------%
%
% Convergence criteria (CAUCHY, RESIDUAL)
CONV_CRITERIA= CAUCHY
%
CONV_FIELD= LIFT, DRAG
% Min value of the residual (log10 of the residual)
CONV_RESIDUAL_MINVAL= -6
%
% Start convergence criteria at iteration number
CONV_STARTITER= 10
%
% Number of elements to apply the criteria
CONV_CAUCHY_ELEMS= 20
%
% Epsilon to control the series convergence
CONV_CAUCHY_EPS= 1E-6
%
%
% ------------------------- INPUT/OUTPUT INFORMATION --------------------------%
%
HISTORY_WRT_FREQ_INNER=1
SCREEN_WRT_FREQ_INNER =1
OUTPUT_WRT_FREQ=100
%
% Mesh input file
MESH_FILENAME= qq.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_flow.dat
%
% Restart adjoint input file
SOLUTION_ADJ_FILENAME= restart_adj.dat
%
% Output file format (PARAVIEW, TECPLOT, STL)
OUTPUT_FILES= RESTART, TECPLOT_ASCII, SURFACE_TECPLOT_ASCII
%
% Output file convergence history (w/o extension)
CONV_FILENAME= history15
%
% 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 surface flow coefficient (w/o extension)
SURFACE_FILENAME= surface_flow
%
%
SCREEN_OUTPUT = (INNER_ITER, WALL_TIME, RMS_PRESSURE, RMS_DENSITY, LIFT, DRAG, AVG_CFL, LINSOL_ITER LINSOL_RESIDUAL )
HISTORY_OUTPUT=(ITER,WALL_TIME,REL_RMS_RES,RMS_RES , AERO_COEFF,AERO_COEFF)
VOLUME_OUTPUT =(PRESSURE_COEFF, Y_PLUS, MACH, ORTHOGONALITY )
%

When I use the central scheme (JST) it do converge pretty well but with 2nd order upwind it is even taking 15k iteration but no convergence.
I have attached the lift plot in the section, please find it below. Any sort of advice will be really appreciated.

[ugurtan666]

It is normal to have a converged result by JST which is central scheme with artificial dissipation. Since its dissipation is also function of spectral radius of the Jacobian (U+A), imho in transonic region JST is not a good choice with its highly diffusive nature especially in terms of lower acoustic mode, U-A.

When it comes to AUSMPLUSUP, I can't see in your cfg file if you enter VENKAT_LIMITER_COEFF which is given as 0.05 default. Entering it 0.01 can make it more stable i.e. more decreasing residuals. However it decreases the spatial accuracy of the scheme.

If you cannot see any improvement in oscillations with lower VENKAT_LIMITER_COEFF, maybe you can consider improving your mesh quality.

[pcg]

Try the option USE_ACCURATE_FLUX_JACOBIANS=YES

[ari003]

Originally Posted by pcg

Try the option USE_ACCURATE_FLUX_JACOBIANS=YES

Thanks Ugurtan and Pedro for your valuable inputs. I was running the simulation with the stated modification and it helped to some extent.

VENKAT_LIMITER_COEFF= 0.005
%
USE_ACCURATE_FLUX_JACOBIANS= YES

The oscillation diminished a little but still finding it hard for the convergence. I decreased the value of Venkat coeff in steps and also noticed that as I reduced, the oscillation diminishes successively. But, I wonder there must be a limit in lower value of this coefficient. I am yet to do an intensive research behind what are the physical aspect of these two function but any advice how to reach convergence even after that is always welcome. I am attaching the pic as well, please find it below.
And really sorry for bothering you people with my problem and any advice will be really appreciated.

[ugurtan666]

AUSM is a member of flux splitting algorithm family. Since the Riemann problem is nonlinear in Euler/Navier Stokes Equations, flux splitting algorithms are generally used like AUSM, SLAU, Steger Warming etc...

Flux is splitted as advection and pressure terms in AUSM, then the flux on the interface is calculated by left and right fluxes and polynomials as specified in Liou's papers related with AUSM.

USE_ACCURATE_FLUX_JACOBIANS= YES option is only available for SLAU and AUSM algorithms in SU2. I am not sure but this option might use higher order polynomials to increase the performance of Riemann solution with an increase in computational cost.

Limiters are used in upwind schemes to calculate left and right fluxes in each cell by linear reconstruction in spatially second order methods. A good limiter must satisfy the minimum principle (monotonicity), must be differentiable and must be high enough to keep spatial order close to second order. These requirements cause a tradeoff obviously.

For having an idea about venkat_coeff, I can suggest you to read Venkatakrishnan's paper Convergence to Steady State Solutions of the Euler Equations on Unstructured Grids with Limiters, Journal of Computational Physics, pp. 120-130, 1995.

PS: If Pedro says something contradictory of mine, please obey him, not me.

[ari003]

Originally Posted by ugurtan666

AUSM is a member of flux splitting algorithm family. Since the Riemann problem is nonlinear in Euler/Navier Stokes Equations, flux splitting algorithms are generally used like AUSM, SLAU, Steger Warming etc...

Flux is splitted as advection and pressure terms in AUSM, then the flux on the interface is calculated by left and right fluxes and polynomials as specified in Liou's papers related with AUSM.

USE_ACCURATE_FLUX_JACOBIANS= YES option is only available for SLAU and AUSM algorithms in SU2. I am not sure but this option might use higher order polynomials to increase the performance of Riemann solution with an increase in computational cost.

Limiters are used in upwind schemes to calculate left and right fluxes in each cell by linear reconstruction in spatially second order methods. A good limiter must satisfy the minimum principle (monotonicity), must be differentiable and must be high enough to keep spatial order close to second order. These requirements cause a tradeoff obviously.

For having an idea about venkat_coeff, I can suggest you to read Venkatakrishnan's paper Convergence to Steady State Solutions of the Euler Equations on Unstructured Grids with Limiters, Journal of Computational Physics, pp. 120-130, 1995.

PS: If Pedro says something contradictory of mine, please obey him, not me.

Thanks again for spending your valuable time for me to providing the insight. I will definitely go through step by step and will be time consuming for me. But meanwhile regarding this problem, I need to get some satisfactory result with upwind scheme( as you told before that central scheme shouldn't be used in convective discretization) and best will be to use the flux splitting mechanism. SLAU is mostly advised to be used for low Mach prob and the only remaining is AUSM. So, after short research I found that AUSM+ will be a good scheme to proceed with. But again the problem is convergence. The Cauchy lift and drag residual is not attaining the convergence. I can hardly find any mesh fault. Do you think there can be any further alteration can be made in this .cfg file? Your advice will really help me Sir.

[pcg]

At Mach 0.8 the ROE convective scheme should be easier to converge than ausm+up.
Try MG_LEVEL=0, I don't remember the default.
You may also try the config I shared at the end of this thread https://github.com/su2code/SU2/discussions/1522
(After adapting it to your case)

[ari003]

Originally Posted by pcg

At Mach 0.8 the ROE convective scheme should be easier to converge than ausm+up.
Try MG_LEVEL=0, I don't remember the default.
You may also try the config I shared at the end of this thread https://github.com/su2code/SU2/discussions/1522
(After adapting it to your case)

Hi Pedro, thank for responding. I tried keeping all your suggestion in mind but still convergence is the issue even with ROE scheme. With MG off the lift and drag residual oscillates and convergence is far off.
With MG =3 which acclerates in convergence I somewhat found the residual declining and might converge in few iteration but the issue is computational resource. It is taking ample time for each iteration like 188 sec. I have attached the .cfg file. Any input will be of help. Struggling with this since long but I believe happiness overcoming struggle is par apart.

[ari003]

Hello peeps, thanks to everyone for your generous responses. I switched to

SLOPE_LIMITER_FLOW= VAN_ALBADA_EDGE

and gave a proper convergence with ROE as well as AUSM+ disc scheme. Hence the case is solved.

[ugurtan666]

Originally Posted by ari003

Hello peeps, thanks to everyone for your generous responses. I switched to

and gave a proper convergence with ROE as well as AUSM+ disc scheme. Hence the case is solved.

It makes sense. van Albada limiter is more aggressive than that of Venkatakrishnan, yet both of them are TVD algorithms. Since van Albada is free of min/max functions unlike Venkatakrishnan, it is differentiable everywhere in the r-psi domain.

BTW, I would expect the aerodynamic coefficients with van Albada to be smaller than or equal to average of Venkat.