
[Sponsors] 
November 18, 2021, 08:02 
axial compressor mass flow convergence issue

#1 
New Member
Jyoti Ranjan
Join Date: Oct 2020
Posts: 12
Rep Power: 4 
Hi,
I am simulating an axial compressor in v7.2.0. I am able to get acceptable level of residuals (image included). But, the mass flow rates at the inlet and outlet are not stabilizing. I have included the mass flow convergence history (image 'massflow.png'), where it appears to be correct. But on zooming in, as seen in image 'massflow_zoomed_in.png', the mass flow rates (both at inlet and outlet) are seen to be falling gradually, although the instantaneous imbalance is not very high. I have tried 1) various levels of grid refinement, 2) CFL as low as 1 (improves turbulence residuals) and 3) running it further longer  without any luck. Is there any configuration setting gone wrong or anything else to resolve this issue would be of great help. I am pasting the configuration file below and attaching a truncated console output 'su2.txt'. Thank you, Jyoti Configuration file Code:
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% % % % SU2 configuration file % % Case description: tr fan % % Author: JRM % % % %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %  DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION % % % Physical governing equations (EULER, NAVIER_STOKES, % WAVE_EQUATION, HEAT_EQUATION, FEM_ELASTICITY, % POISSON_EQUATION) SOLVER= RANS % % Specify turbulence model (NONE, SA, SA_NEG, SST) KIND_TURB_MODEL= SST % % Mathematical problem (DIRECT, CONTINUOUS_ADJOINT) MATH_PROBLEM= DIRECT % % Restart solution (NO, YES) RESTART_SOL= NO %  COMPRESSIBLE FREESTREAM DEFINITION % % % Mach number (nondimensional, based on the freestream values) MACH_NUMBER= .5 % % Angle of attack (degrees, only for compressible flows) AOA= 0.0 % % Sideslip angle (degrees, only for compressible flows) SIDESLIP_ANGLE= 0.0 % % Init option to choose between Reynolds (default) or thermodynamics quantities % for initializing the solution (REYNOLDS, TD_CONDITIONS) INIT_OPTION= TD_CONDITIONS % % Freestream option to choose between density and temperature (default) for % initializing the solution (TEMPERATURE_FS, DENSITY_FS) FREESTREAM_OPTION= TEMPERATURE_FS % % Freestream temperature (288.15 K by default) FREESTREAM_TEMPERATURE= 288.15 % FREESTREAM_PRESSURE= 101325 % % Freestream Turbulence Intensity FREESTREAM_TURBULENCEINTENSITY = 0.05 % % Freestream Turbulent to Laminar viscosity ratio FREESTREAM_TURB2LAMVISCRATIO = 100.0 % % Reynolds number (nondimensional, based on the freestream values) REYNOLDS_NUMBER= 2.5E6 % % Reynolds length (1 m by default) REYNOLDS_LENGTH= 0.09 %  IDEAL GAS, POLYTROPIC, VAN DER WAALS AND PENG ROBINSON CONSTANTS % % % Different gas model (STANDARD_AIR, IDEAL_GAS, VW_GAS, PR_GAS) FLUID_MODEL= IDEAL_GAS % % Ratio of specific heats (1.4 default and the value is hardcoded % for the model STANDARD_AIR) GAMMA_VALUE= 1.4 % % Specific gas constant (287.058 J/kg*K default and this value is hardcoded % for the model STANDARD_AIR) GAS_CONSTANT= 287.058 %  VISCOSITY MODEL % % % Viscosity model (SUTHERLAND, CONSTANT_VISCOSITY). VISCOSITY_MODEL= SUTHERLAND % % Sutherland Viscosity Ref (1.716E5 default value for AIR SI) MU_REF= 1.716E5 % % Sutherland Temperature Ref (273.15 K default value for AIR SI) MU_T_REF= 273.15 % % Sutherland constant (110.4 default value for AIR SI) SUTHERLAND_CONSTANT= 110.4 %  THERMAL CONDUCTIVITY MODEL % % % Conductivity model (CONSTANT_CONDUCTIVITY, CONSTANT_PRANDTL). CONDUCTIVITY_MODEL= CONSTANT_PRANDTL % % Laminar Prandtl number (0.72 (air), only for CONSTANT_PRANDTL) PRANDTL_LAM= 0.72 % % Turbulent Prandtl number (0.9 (air), only for CONSTANT_PRANDTL) PRANDTL_TURB= 0.90 %  DYNAMIC MESH DEFINITION % % % Type of dynamic mesh (NONE, RIGID_MOTION, ROTATING_FRAME, % STEADY_TRANSLATION, % ELASTICITY, GUST) GRID_MOVEMENT= ROTATING_FRAME % % Motion mach number (nondimensional). Used for initializing a viscous flow % with the Reynolds number and for computing force coeffs. with dynamic meshes. MACH_MOTION= 0.5 %MACH_MOTION= 0.35 % % Coordinates of the motion origin MOTION_ORIGIN= 0.00 0.0 0.0 % % Angular velocity vector (rad/s) about the motion origin ROTATION_RATE = 0.0 0.0 1680.019 % %  REFERENCE VALUE DEFINITION % % % Reference origin for moment computation REF_ORIGIN_MOMENT_X = 0.00 REF_ORIGIN_MOMENT_Y = 0.00 REF_ORIGIN_MOMENT_Z = 0.00 % % Reference length for pitching, rolling, and yawing nondimensional moment REF_LENGTH= 0.64607 % % Reference area for force coefficients (0 implies automatic calculation) REF_AREA= 0 % % Compressible flow nondimensionalization (DIMENSIONAL, FREESTREAM_PRESS_EQ_ONE, % FREESTREAM_VEL_EQ_MACH, FREESTREAM_VEL_EQ_ONE) REF_DIMENSIONALIZATION= DIMENSIONAL %  BOUNDARY CONDITION DEFINITION % % MARKER_TURBOMACHINERY= (INFLOW , OUTFLOW) TURBOMACHINERY_KIND= AXIAL % Specify ramp option for rotating frame (YES, NO) default NO RAMP_ROTATING_FRAME= NO % % Parameters of the rotating frame ramp (starting rotational speed, % updatingiterationfrequency, total number of iteration for the ramp) RAMP_ROTATING_FRAME_COEFF= (0.0, 100, 500) % % NavierStokes wall boundary marker(s) (NONE = no marker) MARKER_HEATFLUX= ( BLADE, 0.0, HUB, 0.0, SHROUD, 0.0 ) MARKER_SHROUD=(SHROUD) % MARKER_PERIODIC= ( PER1, PER2, 0.0, 0.0, 0.0, 0.0, 0.0, 16.363636363636, 0.0, 0.0, 0.0 ) % % Internal boundary marker(s) e.g. no boundary condition (NONE = no marker) MARKER_INTERNAL= ( PS, SS ) % % Marker(s) of the surface to be plotted or designed %MARKER_PLOTTING= ( BLADE,INFLOW,OUTFLOW ) % % Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated %MARKER_MONITORING= ( BLADE ) % INLET_TYPE= TOTAL_CONDITIONS % Inlet boundary marker(s) (NONE = no marker) % Format: ( inlet marker, total temperature, total pressure, flow_direction_x, % flow_direction_y, flow_direction_z, ... ) where flow_direction is % a unit vector. SPECIFIED_INLET_PROFILE = NO INLET_FILENAME = inlet.dat MARKER_INLET= ( INFLOW, 288.15, 101325, 0.0,0,1.0 ) % % Outlet boundary marker(s) (NONE = no marker) % Format: ( outlet marker, back pressure (static), ... ) MARKER_OUTLET= ( OUTFLOW, 110000 ) %MARKER_GILES= (OUTFLOW, RADIAL_EQUILIBRIUM, 110000, 0.0, 0.0, 0.0, 0.0, 1.0, 1.0) % This option insert an extra under relaxation factor for the Giles BC at the hub % and shroud (under relax factor applied, span percentage to under relax) %GILES_EXTRA_RELAXFACTOR= ( 0.05, 0.05) % YES Non reflectivity activated, NO the Giles BC behaves as a normal 1D characteristicbased BC %SPATIAL_FOURIER= YES % % Specify Kind of average process for linearizing the NavierStokes % equation at inflow and outflow BCs included at the mixingplane interface % (ALGEBRAIC, AREA, MASSFLUX, MIXEDOUT) default AREA AVERAGE_PROCESS_KIND= MIXEDOUT PERFORMANCE_AVERAGE_PROCESS_KIND= MIXEDOUT % Parameters of the Newton method for the MIXEDOUT average algorithm % (under relaxation factor, tollerance, max number of iterations) MIXEDOUT_COEFF= (1.0, 1.0E05, 15) % % Limit of Mach number below which the mixedout algorithm is substituted % with a AREA average algorithm to avoid numerical issues AVERAGE_MACH_LIMIT= 0.05 %  SURFACES IDENTIFICATION % % % Marker(s) of the surface in the surface flow solution file MARKER_PLOTTING= ( INFLOW, OUTFLOW) % Marker(s) of the surface where the nondimensional coefficients are evaluated. MARKER_MONITORING = ( INFLOW, OUTFLOW ) % % Marker(s) of the surface that is going to be analyzed in detail (massflow, average pressure, distortion, etc) MARKER_ANALYZE = ( INFLOW, OUTFLOW ) % % Method to compute the average value in MARKER_ANALYZE (AREA, MASSFLUX). MARKER_ANALYZE_AVERAGE = MASSFLUX % %  COMMON PARAMETERS DEFINING THE NUMERICAL METHOD % % % Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES) NUM_METHOD_GRAD= WEIGHTED_LEAST_SQUARES % Numerical method for spatial gradients to be used for MUSCL reconstruction % Options are (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES, LEAST_SQUARES). Default value is % NONE and the method specified in NUM_METHOD_GRAD is used. NUM_METHOD_GRAD_RECON =WEIGHTED_LEAST_SQUARES % % CourantFriedrichsLewy condition of the finest grid CFL_NUMBER= 20 % % 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= ( .2,2.0, 1, 10 ) % % RungeKutta alpha coefficients RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 ) % % Number of total iterations ITER= 200000 %  LINEAR SOLVER DEFINITION % % % Linear solver for the implicit (or discrete adjoint) formulation (BCGSTAB, FGMRES) LINEAR_SOLVER= FGMRES % % Preconditioner of the Krylov linear solver (NONE, JACOBI, LINELET) LINEAR_SOLVER_PREC= LU_SGS % % Min error of the linear solver for the implicit formulation LINEAR_SOLVER_ERROR= 1E4 % % Max number of iterations of the linear solver for the implicit formulation LINEAR_SOLVER_ITER= 100 %  MULTIGRID PARAMETERS % % % MultiGrid Levels (0 = no multigrid) MGLEVEL= 0 % % Multigrid cycle (V_CYCLE, W_CYCLE, FULLMG_CYCLE) MGCYCLE= V_CYCLE % % Multigrid presmoothing level MG_PRE_SMOOTH= ( 1, 1, 1, 1 ) % % Multigrid postsmoothing level MG_POST_SMOOTH= ( 0, 0, 0, 0 ) % % Jacobi implicit smoothing of the correction MG_CORRECTION_SMOOTH= ( 0, 0, 0, 0 ) % % 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, LAXFRIEDRICH, CUSP, ROE, AUSM, HLLC, % TURKEL_PREC, MSW) CONV_NUM_METHOD_FLOW= ROE % % Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER) MUSCL_FLOW= YES % % Slope limiter (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG, % BARTH_JESPERSEN, VAN_ALBADA_EDGE) SLOPE_LIMITER_FLOW= VAN_ALBADA_EDGE % % Coefficient for the Venkat's limiter (upwind scheme). A larger values decrease % the extent of limiting, values approaching zero cause % lowerorder approximation to the solution (0.05 by default) % VENKAT_LIMITER_COEFF= 0.3 ENTROPY_FIX_COEFF= 0.03 % % 2nd and 4th order artificial dissipation coefficients for % the JST method ( 0.5, 0.02 by default ) JST_SENSOR_COEFF= ( 0.5, 0.02 ) % % Time discretization (RUNGEKUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT) TIME_DISCRE_FLOW= EULER_IMPLICIT %  TURBULENT NUMERICAL METHOD DEFINITION % % % Convective numerical method (SCALAR_UPWIND) CONV_NUM_METHOD_TURB= SCALAR_UPWIND % % Monotonic Upwind Scheme for Conservation Laws (TVD) in the turbulence equations. % Required for 2nd order upwind schemes (NO, YES) MUSCL_TURB= NO % % Slope limiter (VENKATAKRISHNAN, MINMOD) SLOPE_LIMITER_TURB= VAN_ALBADA_EDGE % % Time discretization (EULER_IMPLICIT) TIME_DISCRE_TURB= EULER_IMPLICIT % % Reduction factor of the CFL coefficient in the turbulence problem CFL_REDUCTION_TURB= 1 %  CONVERGENCE PARAMETERS % % % Convergence criteria (CAUCHY, RESIDUAL) CONV_CRITERIA = RESIDUAL CONV_FIELD= RMS_DENSITY %RHO_ENERGY % % Min value of the residual (log10 of the residual) CONV_RESIDUAL_MINVAL= 16 % % Start convergence criteria at iteration number CONV_STARTITER= 10 % % Number of elements to apply the criteria CONV_CAUCHY_ELEMS= 100 % % Epsilon to control the series convergence CONV_CAUCHY_EPS= 1E10 % %  INPUT/OUTPUT INFORMATION % % % Mesh input file MESH_FILENAME= ../../r67_1.6M_5em7m_new.cgns % % Mesh input file format (SU2, CGNS, NETCDF_ASCII) MESH_FORMAT= CGNS % % 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= solution_adj.dat % % Output file format (PARAVIEW, TECPLOT, STL) TABULAR_FORMAT= CSV % % Output file convergence history (w/o extension) CONV_FILENAME= history % % 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 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_FILENAME= surface_flow % % Output file surface adjoint coefficient (w/o extension) SURFACE_ADJ_FILENAME= surface_adjoint % % Writing solution file frequency %WRT_SOL_FREQ= 200 % OUTPUT_WRT_FREQ= 100 % % Writing convergence history frequency %WRT_CON_FREQ= 1 % Output the solution at each surface in the history file %WRT_SURFACE= YES % % Screen output SCREEN_OUTPUT= (INNER_ITER, WALL_TIME, RMS_DENSITY, RMS_NU_TILDE, RMS_MOMENTUMX, RMS_MOMENTUMY, SURFACE_MASSFLOW, SURFACE_TOTAL_PRESSURE, SURFACE_TOTAL_TEMPERATURE) % VOLUME_OUTPUT= (MOMENTUMX, MOMENTUMY, MOMENTUMZ, DENSITY, MACH, PRESSURE, TEMPERATURE, Y_PLUS, EDDY_VISCOSITY, PRIMITIVE) % % History output groups (use 'SU2_CFD d <config_file>' to view list of available fields) HISTORY_OUTPUT= (ITER, RMS_RES, SURFACE_MASSFLOW, SURFACE_TOTAL_PRESSURE, SURFACE_TOTAL_TEMPERATURE) % Files to output % Possible formats : (TECPLOT, TECPLOT_BINARY, SURFACE_TECPLOT, % SURFACE_TECPLOT_BINARY, CSV, SURFACE_CSV, PARAVIEW, PARAVIEW_BINARY, SURFACE_PARAVIEW, % SURFACE_PARAVIEW_BINARY, MESH, RESTART_BINARY, RESTART_ASCII, CGNS, STL) % default : (RESTART, PARAVIEW, SURFACE_PARAVIEW) OUTPUT_FILES= (RESTART, PARAVIEW_MULTIBLOCK, SURFACE_PARAVIEW) %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% 

November 18, 2021, 17:53 

#2 
Member
na
Join Date: Jul 2018
Posts: 78
Rep Power: 6 
By no means am i knowledgeable when it comes to Turbomachinery (or compressible flow to begin with) but in a first shot i would simply say your overall convergence is too low for the massflow to converge.
A few thoughts: 1. Maybe try a less demanding case (lower Mach and Reynoldsnumber) and see whether that converges better to machine zero (like 1e10 and beyond, that always depends a bit) 2. As you have a steady state case go as high of a CFL you can work with (i.e. the one that gives you the fastet rediual drops) 3. dont 100 Linear solver iterations! Take a look if you reach 1e4 in a reasonable amount... if not maybe it caps at 2e4 after e.g. 5 iterations and then you do 95 iteration for the bin... then restrict your iterations to the amount you need to get to that cap 4. Add RESIDUAL to VOLUME_OUTPUT and take a look at where high res are... maybe its just one corner that kills your convergence. I already had (incompressible) cases where rounding a sharpe edge made all the difference Maybe some of that helps, Tobi 

November 18, 2021, 18:01 

#3 
Senior Member
Pedro Gomes
Join Date: Dec 2017
Posts: 428
Rep Power: 11 
Your residuals are only dropping 3 orders which is not good enough IMO.
I would try something like this for the linear solver. LINEAR_SOLVER= FGMRES LINEAR_SOLVER_PREC= ILU LINEAR_SOLVER_ERROR= 0.05 LINEAR_SOLVER_ITER= 10 And you can also try GREEN_GAUSS instead of WEIGHTED_LEAST_SQUARES And VENKATAKRISHNAN_WANG instead of VAN_ALBADA, with the limiter parameter 0.050.1 

November 22, 2021, 10:11 

#4 
New Member
Jyoti Ranjan
Join Date: Oct 2020
Posts: 12
Rep Power: 4 
Thank you Tobi and Pedro for your suggestions.
I have tried to work on your advices. 1. Didn't find a less demanding case (it would be great if someone can point to an axial compressor test case), but tried this same case with a coarse mesh (.34M cells, my earlier mesh was 1.6M cells). I could reach very low level of residuals (~ 1e11 for density) for first order solution; but second order solution does not get through. Upon refining the boundary layer mesh for the coarse mesh to a level when second order solution gets through, I get the similar level of residuals that I got with the original mesh(1.6M cells). 2. Found 10 linear solver iterations to be enough. Saves quite some compute time. 3. Highest residual is not localized to a specific region for my case, keeps changing. 4. Tried the values LINEAR_SOLVER= FGMRES LINEAR_SOLVER_PREC= ILU LINEAR_SOLVER_ERROR= 0.05 LINEAR_SOLVER_ITER= 10 and GREEN_GAUSS and VENKATKRISHNAN_WANG limiter. While, the linear solver settings (LINEAR_SOLVER_ERROR= 0.05 LINEAR_SOLVER_ITER= 10) saved compute time, I could not get any improvements as far as the final result is concerned. Usually, 34 orders fall in residuals is not bad for a real turbomachine as long as the performance parameters (pressure ratio and efficiency) converge at a stable mean flow with an acceptable level of imbalance. I tried running the case a bit (quite a bit!) longer and I see the mass flow rates at inlet and outlet seem to have stabilized but the imbalance at 0.118846% may be a bit higher (image included). I also tried to plot the histories of the inlet/ and outlet applied boundary conditions 'obtained from the solution' (console output displayed when intermediate output files are written; I have written it every 100 iterations) inlet total pressure and outlet static pressure (images included). The solution PT (total pressure) at Inlet has settled to a constant value of 101229 Pa quite soon against the applied BC of PT=101325 Pa, which seems ok. The solution PS (static pressure) at outlet takes very long to settle  in this case it is settling to 110536 Pa against 110000 Pa applied BC; it has taken about 110000 iterations. I was wondering, if there is a need of a tighter relaxation for the outlet BC or a static pressure profile BC possible! (Note: I am getting similar results with RADIAL_EQUILIBRIUM.) Thank you, Jyoti 

November 24, 2021, 07:03 

#5 
Senior Member
Pedro Gomes
Join Date: Dec 2017
Posts: 428
Rep Power: 11 
Ah ok it looked like the difference was higher initially.
It could be because of differences in how those quantities are computed for postprocessing and how they are computed while solving the equations, especially if there is still streamwise variation close to the outlet. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Wind tunnel flow simulation boundary condition issue  charan3007  SU2  0  October 21, 2021 09:27 
Solver parameters to solve convergence issue  WilliamH  SU2  5  February 5, 2021 07:19 
Negative Aorta Flow Convergence Issue  BlueCat  Main CFD Forum  2  June 17, 2016 14:33 
Laminar Pipe Flow convergence issues  preichl  OpenFOAM Running, Solving & CFD  11  September 22, 2014 22:22 
Continuity convergence issue for a multiphase flow in a counterflow heat exchanger  Andrea1984  Fluent Multiphase  2  July 24, 2013 05:55 