
[Sponsors] 
Divergence of L2ROE scheme for low Mach numbers 

LinkBack  Thread Tools  Search this Thread  Display Modes 
September 9, 2021, 06:43 
Divergence of L2ROE scheme for low Mach numbers

#1 
Member
Ravi
Join Date: May 2017
Posts: 31
Rep Power: 6 
I am currently trying to obtain the plots of and vs. convective time units (nondimensional) for an airfoil in deep stall (having an angle of attack of ) using the DDES approach, using the SA turbulence model and a 2nd order numerical scheme (dualtime stepping scheme).
My freestream properties are as follows: %  COMPRESSIBLE AND INCOMPRESSIBLE FREESTREAM DEFINITION % % % Specify Turbulence Intensity (%) FREESTREAM_TURBULENCEINTENSITY = 0.6 % Mach number (nondimensional, based on the freestream values) MACH_NUMBER= 0.10 % % Angle of attack (degrees) AOA= 60 % % Sideslip angle (degrees) SIDESLIP_ANGLE= 0.0 % % Freestream pressure (101325.0 N/m^2 by default, only Euler flows) %FREESTREAM_PRESSURE= 101325 % % Freestream temperature (273.15 K by default) FREESTREAM_TEMPERATURE= 300 % % Reynolds number (nondimensional, based on the freestream values) REYNOLDS_NUMBER= 2.75E5 % % Reynolds length (1 m, 1 inch by default) REYNOLDS_LENGTH= 1 I currently have the following relevant numerical settings for space and time, leading up to the L2ROE scheme solution: %  TIMEDEPENDENT SIMULATION % % % Time domain simulation TIME_DOMAIN= YES % % Unsteady simulation (NO, TIME_STEPPING, DUAL_TIME_STEPPING1ST_ORDER, % DUAL_TIME_STEPPING2ND_ORDER, HARMONIC_BALANCE) TIME_MARCHING= DUAL_TIME_STEPPING2ND_ORDER % % Time Step for dual time stepping simulations (s)  Only used when UNST_CFL_NUMBER = 0.0 % For the DGFEM solver it is used as a synchronization time when UNST_CFL_NUMBER != 0.0 TIME_STEP= 0.000864 % % Total Physical Time for dual time stepping simulations (s) MAX_TIME= 150 % % Unsteady CourantFriedrichsLewy number of the finest grid UNST_CFL_NUMBER= 5 % %% Windowed output time averaging % Time iteration to start the windowed time average in a direct run % WINDOW_START_ITER = 500 % % Window used for reverse sweep and direct run. Options (SQUARE, HANN, HANN_SQUARE, BUMP) Square is default. WINDOW_FUNCTION = SQUARE %% Number of internal iterations (dual time method) INNER_ITER= 40 % Iteration number to begin unsteady restarts RESTART_ITER= 2 %  COMMON PARAMETERS TO DEFINE THE NUMERICAL METHOD % % Numerical method for spatial gradients (GREEN_GAUSS, LEAST_SQUARES, % WEIGHTED_LEAST_SQUARES) NUM_METHOD_GRAD= WEIGHTED_LEAST_SQUARES %NUM_METHOD_GRAD= GREEN_GAUSS % % CourantFriedrichsLewy condition of the finest grid CFL_NUMBER= 5.0 % % 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= ( 0.0, 0.5, 1.25, 50.0 ) % % RungeKutta alpha coefficients RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 ) % % Number of total iterations TIME_ITER= 20000000 %  LINEAR SOLVER DEFINITION % % % Linear solver or smoother for implicit formulations (BCGSTAB, FGMRES, SMOOTHER_JACOBI, % SMOOTHER_ILU0, SMOOTHER_LUSGS, % SMOOTHER_LINELET) LINEAR_SOLVER= FGMRES % % Preconditioner of the Krylov linear solver (ILU0, LU_SGS, LINELET, JACOBI) LINEAR_SOLVER_PREC= ILU %LINEAR_SOLVER_ILU_FILL_IN= 0 % % Minimum error of the linear solver for implicit formulations LINEAR_SOLVER_ERROR= 1E6 % % Max number of iterations of the linear solver for the implicit formulation LINEAR_SOLVER_ITER= 20 % %  FLOW NUMERICAL METHOD DEFINITION % % % Convective numerical method (JST, LAXFRIEDRICH, CUSP, ROE, AUSM, HLLC, % TURKEL_PREC, MSW) CONV_NUM_METHOD_FLOW= L2ROE %CONV_NUM_METHOD_FLOW= ROE %ROE_LOW_DISSIPATION= FD % % Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER) %MUSCL_FLOW= YES MUSCL_FLOW= NO % % Slope limiter (VENKATAKRISHNAN, BARTH_JESPERSEN) SLOPE_LIMITER_FLOW=VENKATAKRISHNAN % % Entropy fix coefficient (0.0 implies no entropy fixing, 1.0 implies scalar % artificial dissipation) ENTROPY_FIX_COEFF= 0.0 % % 1st, 2nd and 4th order artificial dissipation coefficients %AD_COEFF_FLOW= ( 0.15, 0.5, 0.02 ) % % Viscous limiter (NO, YES) %VISCOUS_LIMITER_FLOW= NO % % Time discretization (RUNGEKUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT) TIME_DISCRE_FLOW= EULER_IMPLICIT % % Relaxation coefficient %RELAXATION_FACTOR_FLOW= 1.0 %  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 % % Slope limiter (VENKATAKRISHNAN) SLOPE_LIMITER_TURB= NONE % % Viscous limiter (NO, YES) %VISCOUS_LIMITER_TURB= NO % % Time discretization (EULER_IMPLICIT) TIME_DISCRE_TURB= EULER_IMPLICIT % % Reduction factor of the CFL coefficient in the turbulence problem %CFL_REDUCTION_TURB= 1.0 % % Relaxation coefficient %RELAXATION_FACTOR_TURB= 1.0 I have an issue with the solver diverging after the first four iterations as attached in the log file of this post. This is despite trying to use the MUSCL flow setting for numerical integration. Given that as of now, the MUSCL turbulent setting is still a work in progress for such low Mach numbers as of the information given in the SU2 website, I would not change that. Has anyone else faced this issue with the L2ROE scheme diverging using the FD wall function? I have tried the NTS function and it still converges. The purpose of doing this is to validate some results. Hoping to hear from you all soon. Ravi 

September 9, 2021, 13:05 

#2 
Member
bigfoot
Join Date: Dec 2011
Location: Netherlands
Posts: 71
Rep Power: 12 
Hi,
Could you obtain a converged steady state solution on this mesh? I find that it helps to first simplify the problem until it works. You can plot the inner residuals to screen to check if they are converging. If not, you can set LINEAR_SOLVER_ERROR= 1e12 and LINEAR_SOLVER_ITERATIONS= 200 to see if you get convergence at all. If this is not the case, try setting the timestep to a much lower value . Also, first order methods are less accurate (especially in transient simulations) but their errors are diffusive, so they tend to be more stable. Did this method converge for a first order setup? 

September 12, 2021, 05:51 

#3  
Member
Ravi
Join Date: May 2017
Posts: 31
Rep Power: 6 
Quote:
Thanks a lot for your suggestions. I have actually implemented what you mentioned, i.e., by changing the linear solver settings, as well as reducing the time step (I used a dt = dt/4, wherein my dt is of the order of 10^4 s). However, in either case, I get a diverged solution. And regarding obtaining a converged steady state solution, yes indeed, I had started the DDES 2nd order simulation only after obtaining a converged result for the RANS 2nd order solution. Even then I am facing this issue, which I find to be quite strange. I did check my density residuals though, and it does hover around the 10E6.5 mark. One weird thing that I observed is that my solution converges if I use the regular Roe scheme along with the lowdissipation FD function. Is there a physical reason I am missing out here? Hoping to hear from you soon. Ravi 

September 14, 2021, 18:06 

#4  
Senior Member

Quote:
L2ROE for me works. Though I have a course grid. You also can plot residual and see where they get stuck. 

September 15, 2021, 05:43 

#5  
Member
Ravi
Join Date: May 2017
Posts: 31
Rep Power: 6 
Quote:
Thank you for your insight. I did try what you have mentioned as well, but I am unable to make it work. The residuals are what cause the divergence  they diverge within the first few outer iterations. Would you suggest that I modify the unsteady CFL in the unsteady simulation settings (UNST_CFL_NUMBER) as well? Hoping to hear from you soon. Ravi 

September 15, 2021, 11:33 

#6  
Senior Member

Quote:
set TIME_DOMAIN= NO and run it and see if it converges. Then, if so set TIME_DOMAIN= YES without UNST_CFL_NUMBER. I wasn't using UNST_CFL_NUMBER only TIME_STEP. 

September 16, 2021, 11:08 

#7  
Member
Ravi
Join Date: May 2017
Posts: 31
Rep Power: 6 
Quote:
Thank you for your reply. I did try to remove the influence of the unsteady CFL number from the simulation by running TIME_DOMAIN = YES without it, but the problem still persists for some reason. I have also tried to include an adaptive CFL setting for the same, and it still did not converge. I have tried to use a CFL of 0.1 for the same, and I am not able to make it converge. Hoping to hear from you and the others regarding alternative suggestions based on your experience, as I am still quite inexperienced with this issue. Ravi 

September 20, 2021, 08:11 

#8  
Senior Member

Quote:
Go with TIME_DOMAIN = NO and see if you could converge. Only if you did then you can assume there should be no problem switching to time dependent simulation. If you didn't converge with TIME_DOMAIN = NO, then there is something wrong with your numerical setting or mesh for this flow physics. 

September 20, 2021, 09:36 

#9  
Member
Ravi
Join Date: May 2017
Posts: 31
Rep Power: 6 
Quote:
Thank you for your insights. Indeed, you might be correct  there could be an issue with the numerical scheme. I am currently trying to use the ROE solver along with the FD scheme for low wall dissipation in my DDES simulation. I had also tried to run it with RANS 1st and 2nd order, but they had also diverged using both the L2ROE and ROE's schemes in tandem with the FD dissipation scheme. Therefore, I would be grateful to hear of other insights regarding this as well. Hoping to hear from you all soon. With warm regards, Ravi 

September 20, 2021, 13:38 

#10 
Senior Member
Pedro Gomes
Join Date: Dec 2017
Posts: 353
Rep Power: 9 
Low dissipation does not apply to L2 Roe
https://su2code.github.io/docs_v7/Co...upwindschemes 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Roe scheme with low mach preconditioning in the Mach 0.2 flat plate turbulent case?  Shenren_CN  SU2  0  September 25, 2017 08:40 
Local mach number  jacobH  Main CFD Forum  3  October 1, 2014 11:20 
Constructing Surface Interpolation Scheme from Divergence Scheme Information  ngj  OpenFOAM Programming & Development  1  December 9, 2013 12:19 
About compressible flow at low mach  hit  Main CFD Forum  2  October 26, 2009 22:21 
nondimensional analysis in Fluent  Endee  FLUENT  8  September 7, 2005 17:16 