|
[Sponsors] |
![]() |
![]() |
#1 |
New Member
ugurtan
Join Date: May 2020
Location: Munich, Germany
Posts: 19
Rep Power: 6 ![]() |
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) |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Senior Member
Pedro Gomes
Join Date: Dec 2017
Posts: 466
Rep Power: 13 ![]() |
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. |
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
ugurtan
Join Date: May 2020
Location: Munich, Germany
Posts: 19
Rep Power: 6 ![]() |
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! |
|
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Foam::error::printStack(Foam::Ostream&) with simpleFoam -parallel | U.Golling | OpenFOAM Running, Solving & CFD | 52 | September 23, 2023 03:35 |
Initial conditions for uniform flow | andreas | OpenFOAM | 5 | November 16, 2012 15:00 |
[OpenFOAM] ParaView/Parafoam error when making animation | Disco_Caine | ParaView | 6 | September 28, 2010 09:54 |
user subroutine error | CFDUSER | CFX | 2 | December 9, 2006 06:31 |
user defined function | cfduser | CFX | 0 | April 29, 2006 10:58 |