[akki_malik]

I am using SU2 6.0 version and trying to simulate flow over a full aircraft geometry, mesh size is appx. 4 million, I have tried several combinations of multi-grid parameters, But the results never converge, the following is a sample configuration file as I can not attach the original one.

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% %
% SU2 configuration file %
% Case description: ONERA M6 wing in inviscid, transonic flow %
% Author: Thomas D. Economon %
% Institution: Stanford University %
% Date: 2015.08.25 %
% File Version 5.0.0 "Raven" %
% %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
% Physical governing equations (EULER, NAVIER_STOKES)
PHYSICAL_PROBLEM= NAVIER_STOKES
%
% Mathematical problem (DIRECT, CONTINUOUS_ADJOINT)
MATH_PROBLEM= DIRECT
%
% Restart solution (NO, YES)
RESTART_SOL= NO
%
% Write binary restart files (YES, NO)
WRT_BINARY_RESTART= NO
%
% Read binary restart files (YES, NO)
READ_BINARY_RESTART= NO

% -------------------- COMPRESSIBLE FREE-STREAM DEFINITION --------------------%
%
% Mach number (non-dimensional, based on the free-stream values)
MACH_NUMBER= 0.7
%
% Angle of attack (degrees)
AOA= 15.0
%
% Side-slip angle (degrees)
SIDESLIP_ANGLE= 0.0
%
% Free-stream pressure (101325.0 N/m^2 by default, only for Euler equations)
FREESTREAM_PRESSURE= 101325.0
%
% Free-stream temperature (288.15 K by default)
FREESTREAM_TEMPERATURE= 288.15

% ---------------------- REFERENCE VALUE DEFINITION ---------------------------%
%
% Reference origin for moment computation
REF_ORIGIN_MOMENT_X = 7.0
REF_ORIGIN_MOMENT_Y = 0.00
REF_ORIGIN_MOMENT_Z = 1.00
%
% Reference length for pitching, rolling, and yaMAIN_BOX non-dimensional moment
REF_LENGTH= 5.0
%
% Reference area for force coefficients (0 implies automatic calculation)
REF_AREA= 20
%
% Flow non-dimensionalization (DIMENSIONAL, FREESTREAM_PRESS_EQ_ONE,
% FREESTREAM_VEL_EQ_MACH, FREESTREAM_VEL_EQ_ONE)
REF_DIMENSIONALIZATION= FREESTREAM_VEL_EQ_ONE

% ----------------------- BOUNDARY CONDITION DEFINITION -----------------------%
%
% Marker of the Euler boundary (0 implies no marker)
MARKER_HEATFLUX= ( UPPER_SIDE,0.0, LOWER_SIDE,0.0, TIP,0.0 )
%
% Marker of the far field (0 implies no marker)
MARKER_FAR= ( XNORMAL_FACES, ZNORMAL_FACES, YNORMAL_FACE )
%
% Marker of symmetry boundary (0 implies no marker)
MARKER_SYM= ( SYMMETRY_FACE )
%
% Marker of the surface which is going to be plotted
MARKER_PLOTTING= ( UPPER_SIDE, LOWER_SIDE, TIP )
%
% Marker of the surface where the functional (Cd, Cl, etc.) will be evaluated
MARKER_MONITORING= ( UPPER_SIDE, LOWER_SIDE, TIP )

% ------------- COMMON PARAMETERS TO DEFINE THE NUMERICAL METHOD --------------%
%
% Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES)
NUM_METHOD_GRAD= WEIGHTED_LEAST_SQUARES
%
% Objective function in gradient evaluation (DRAG, LIFT, SIDEFORCE, MOMENT_X,
% MOMENT_Y, MOMENT_Z, EFFICIENCY,
% EQUIVALENT_AREA, NEARFIELD_PRESSURE,
% FORCE_X, FORCE_Y, FORCE_Z, THRUST,
% TORQUE, FREE_SURFACE, TOTAL_HEATFLUX,
% MAXIMUM_HEATFLUX, INVERSE_DESIGN_PRESSURE,
% INVERSE_DESIGN_HEATFLUX)
OBJECTIVE_FUNCTION= DRAG
%
% Courant-Friedrichs-Lewy condition of the finest grid
CFL_NUMBER= 0.005
%
% 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= ( 1.5, 0.5, 0.005, 10.0 )
%
% Runge-Kutta alpha coefficients
RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 )
%
% Number of total iterations
EXT_ITER= 99999
%
% Linear solver for the implicit formulation (BCGSTAB, FGMRES)
LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver (ILU, LU_SGS, LINELET, JACOBI)
LINEAR_SOLVER_PREC= ILU
%
% 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

% ----------------------- SLOPE LIMITER DEFINITION ----------------------------%
%
% Coefficient for the limiter
VENKAT_LIMITER_COEFF= 0.03
%
% Coefficient for the sharp edges limiter
ADJ_SHARP_LIMITER_COEFF= 3.0
%
% Reference coefficient (sensitivity) for detecting sharp edges.
REF_SHARP_EDGES= 3.0
%
% Remove sharp edges from the sensitivity evaluation (NO, YES)
SENS_REMOVE_SHARP= YES

% -------------------------- MULTIGRID PARAMETERS -----------------------------%
%
% Multi-Grid Levels (0 = no multi-grid)
MGLEVEL= 3
%
% Multi-grid cycle (V_CYCLE, W_CYCLE, FULLMG_CYCLE)
MGCYCLE= W_CYCLE
%
% Multi-Grid PreSmoothing Level
MG_PRE_SMOOTH= ( 0.5, 0.5, 0.5, 0.5 )
%
% Multi-Grid PostSmoothing Level
MG_POST_SMOOTH= ( 0.5, 0.5, 0.5, 0.5 )
%
% Jacobi implicit smoothing of the correction
MG_CORRECTION_SMOOTH= ( 0.5, 0.5, 0.5, 0.5 )
%
% 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
%
% 2nd and 4th order artificial dissipation coefficients
JST_SENSOR_COEFF= ( 0.5, 0.02 )
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_FLOW= EULER_IMPLICIT

% --------------------------- CONVERGENCE PARAMETERS --------------------------&
%
% Convergence criteria (CAUCHY, RESIDUAL)
CONV_CRITERIA= RESIDUAL
%
% Residual reduction (order of magnitude with respect to the initial value)
RESIDUAL_REDUCTION= 8
%
% Min value of the residual (log10 of the residual)
RESIDUAL_MINVAL= -12
%
% Start convergence criteria at iteration number
STARTCONV_ITER= 25
%
% Number of elements to apply the criteria
CAUCHY_ELEMS= 100
%
% Epsilon to control the series convergence
CAUCHY_EPS= 1E-10
%
% Function to apply the criteria (LIFT, DRAG, NEARFIELD_PRESS, SENS_GEOMETRY,
% SENS_MACH, DELTA_LIFT, DELTA_DRAG)
CAUCHY_FUNC_FLOW= DRAG

% ------------------------- INPUT/OUTPUT INFORMATION --------------------------%
%
% Mesh input file
MESH_FILENAME= mesh_ONERAM6_inv_ffd.su2
%
% Mesh output file
MESH_OUT_FILENAME= mesh_out.su2
%
% Restart flow input file
SOLUTION_FLOW_FILENAME= solution_flow.dat
%
% Restart adjoint input file
SOLUTION_ADJ_FILENAME= solution_adj.dat
%
% Mesh input file format (SU2)
MESH_FORMAT= SU2
%
% Output file format (PARAVIEW, TECPLOT)
OUTPUT_FORMAT= TECPLOT
%
% Output file convergence history
CONV_FILENAME= history
%
% Output file restart flow
RESTART_FLOW_FILENAME= restart_flow.dat
%
% Output file restart adjoint
RESTART_ADJ_FILENAME= restart_adj.dat
%
% Output file flow (w/o extension) variables
VOLUME_FLOW_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_FLOW_FILENAME= surface_flow
%
% Output file surface adjoint coefficient (w/o extension)
SURFACE_ADJ_FILENAME= surface_adjoint
%
% Writing solution frequency
WRT_SOL_FREQ= 100
%
% Writing convergence history frequency
WRT_CON_FREQ= 1



If anyone has done simulation on full aircraft geometry, Please help.

[RcktMan77]

Try turning off multigrid. It tends to require a bit of iteration of its settings in order to get things running in a suitable manner. If the code is stable after turning off multigrid, then you have isolated that as the problem. You can then go back and iterate on settings to see if there are any that are suitable. Given your mesh for a full aircraft is relatively coarse, you may find it difficult. You will have better luck sticking with the V cycle option.


Also, if your mesh consists of multiple element types (i.e. tetrahedra, prisms, pyramids, hexahedra), then you're better off with Green Gauss instead of Weighted Least Squares. After turning off multigrid, then you can probably choose a CFL number a bit greater than 0.005. I would turn on the adaptive CFL feature, and vary it from 1.0 to 10.0 or 20.0 to start.

[akki_malik]

If I turn off multi-grid then it will take lot of time to converge. I tried with fine grid as well (23 Million), But there was no convergence at all, first results seems to be converged, (Cl, Cd and all parameters in history file were constant for almost 5000 iterations, but the value of coefficients was much above the expected value), after that simulation continued for almost 200000 iterations, But no convergence, no stabilization in the results was observed.
Most of the time I played with multi-gird parameters only, along with CFL no and CFL ramping as well, But there was no improvement.
Not only I am looking for convergence, but I want it fast, at least below 30000 iterations.

[RcktMan77]

Using a much larger CFL value than the 0.005 value you're using should help advance the solution towards convergence more quickly. The aero coefficients you're comparing against may also be off from their expected values due to discretization error as a result of having a mesh that is too coarse. If you ramp the CFL value from 1 to 20 or even 30, then your solution will likely be converged within 30,000 iterations even without multigrid. Again, unless you're grid consists of homogenous elements, you're better off calculating spatial gradients with Green Gauss.

[akki_malik]

Thanks a lot for all the answers, I will make changes as suggested and come back again.
However, mesh quality is good enough and it is giving good results on commercial softwares (CFD++ specifically), by good results I mean to say that they are matching with wind tunnel testing.

[pcg]

Hi,
Judging from the header on the config file it had Euler flow specified originally right?
To run for NS you will want to specify the turbulence model and associated settings, look for a RANS config file in the TestCases folder.

If in the output of the code you don't have residuals for turbulence it means it is assuming laminar flow (which is the default setting).
Regards,
Pedro

[akki_malik]

Hi, I am sorry for not posting original configuration file, This uploaded configuration file is actually the one given for onera m6 wing, I have made necessary changes in this one though I forget to mention all of them. As I focused mainly on Multigrid parameters, and CFL ramping, which I have edited correctly.
I have tried both turbulence models, SA and SST. Thats the only thing I have given for turbulence model, I would like to know if we can write more details about the turbulence models in configuration file.
I have also used Green Gauss method for spatial gradients and V cycle for multi-grid cycle.

[pcg]

You have CFL_REDUCTION_TURB (increase or reduce the CFL compared to the one for the flow) and RELAXATION_FACTOR_TURB.
About MG parameters, these MG_PRE_SMOOTH, etc. are integers, i.e. number of smoothing steps, I am not sure what 0.5 gets converted to when reading...
The problem may just be converging from free-stream, have you tried increasing Mach number in steps?

[akki_malik]

I have not seen these two options in configuration file, namely, CFL_REDUCTION_TURB and RELAXATION_FACTOR_TURB. I am not sure if these options are available for 6.0.0 version.
I had no idea about the values of MG pre-smooth and post-smooth factors, I tried some random numbers, I guess the solution was diverging when these values were around 2 or 3. With these values, simulation doesn't diverge. Thanks a lot for these information. I have tried with different Mach numbers, 0.7,0.9,1.2,1.6. But the convergence is no where.

[pcg]

They are, you can see them in the file config_template.cfg in the root directory of the code.
I usually run with MG_PRE_SMOOTH= ( 1, 2, 3, 3 ) and the others all 0.
I don't have experience with full aircraft cases so I don't know of any tricks unfortunately.

[akki_malik]

I will try out this and reach you back.
Results for full geometry are little difficult to converge or I have no idea if they will converge or not using SU2.

[aero_amit]

Allright, I will share my experience.....
1-Do not use multi grid for complex meshes.
2- Try first order simulation for few thousand iterations.
3- Run second order solution from the first order output
4- No need to use small CFL if grid is not too bad. You can go with CFL 1 or 2 and try higher in the later stages.

Let me know