[ugurtan666]

Dear SU2 users;

I have a hypersonic test case at M=10. After nearly 500 iterations, I have seen that the aerodynamic coefficients seem to be converging in a 2-3% variation. I have also checked flow domain and I haven't seen any anomaly in domain.

However, I got suddenly FGMRES orthogonalization failed, linear solver diverged error. While I tried same problem at M=7, I haven't seen such a problem. I have also converged solution when I tuned MUSCL_FLOW as NO but I don't want to have first order spatial accurate solution.

Do you have any ideas/suggestions?

My config file setting as;

% ---- 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= 1.3448
% Specific gas constant (287.058 J/kg*K default and this value is hardcoded
% for the model STANDARD_AIR, compressible only)
GAS_CONSTANT= 287.15

% Temperature polynomial coefficients (up to quartic) for specific heat Cp.
% Format -> Cp(T) : b0 + b1*T + b2*T^2 + b3*T^3 + b4*T^4
CP_POLYCOEFFS= (926.55709422388, 0.169323866173782, 1.26310949215E-4, -1.07657580419E-7, 2.10452345942872E-11)

% ----------- 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
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the turbulence equations.
% Required for 2nd order upwind schemes (NO, YES)
MUSCL_TURB= NO
% Slope limiter (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG,
% BARTH_JESPERSEN, VAN_ALBADA_EDGE)
SLOPE_LIMITER_TURB= 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= 0.05
LIMITER_ITER= 9999999 % Freeze the value of the limiter after a number of iterations
% 2nd and 4th order artificial dissipation coefficients for
% the JST method ( 0.5, 0.02 by default )
JST_SENSOR_COEFF= ( 0.5, 0.02 )

% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
% Convective numerical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, AUSMPLUSUP,
% AUSMPLUSUP2, HLLC, TURKEL_PREC, MSW, FDS, SLAU, SLAU2)
CONV_NUM_METHOD_FLOW= HLLC
% Entropy fix coefficient (0.0 implies no entropy fixing, 1.0 implies scalar
% artificial dissipation)
%ENTROPY_FIX_COEFF= 1
% Higher values than 1 (3 to 4) make the global Jacobian of central schemes (compressible flow
% only) more diagonal dominant (but mathematically incorrect) so that higher CFL can be used.
%CENTRAL_JACOBIAN_FIX_FACTOR= 1.0
TIME_DISCRE_FLOW= EULER_IMPLICIT % Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT)

[pcg]

Try ROE instead of HLLC, HLLC does not support entropy correction, also lower this value to reasonable levels, less than 0.1.
If your simulation is dimensional use VENKATAKRISHNAN_WANG, run the case a bit first order and then restart 2nd order.
If you are using Weighted Least Squares gradients, switch to Green-Gauss.
If you are using the SA model, switch to SA_NEG.

Post your CFL and linear solver settings please, and a plot of the residuals and coefficients you are monitoring.

[ugurtan666]

Hello Pedro,

Sorry for my late response. I altered the settings as you specified. I have also posted my CFL settings. below. I have attached the residual plots.

NUM_METHOD_GRAD=GREEN_GAUSS
CFL_NUMBER=0.5
CFL_ADAPT=YES
CFL_ADAPT_PARAM=(0.25, 1.02, 0.3, 10)
RUNGE_KUTTA_ALPHA_COEFF=(0.66667, 0.66667, 1.000000)

It looks better now and thank you for your suggestion. I have a couple of questions if you have time for me

1) I have a 0-50 nonphysical points. Is it normal to have some nonphysical points in hypersonic flows?

2) May I use flux split schemes like AUSMPLUSUP or SLAU for hypersonic problems or ROE scheme is better?

3) I could not find on the internet so I ask you. Is there any basic tutorial for thermally perfect gas or chemically reacting flow models for SU2_NONEQ fluid model?

Thank you very much!