|
[Sponsors] |
Time-accurate solution restart from steady state solution |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
November 30, 2021, 13:25 |
Time-accurate solution restart from steady state solution
|
#1 |
New Member
Jyoti Ranjan
Join Date: Oct 2020
Posts: 14
Rep Power: 5 |
Hi,
I am trying to simulate a time accurate flow solution of an axial compressor in v7.2.0. I am using a full-annulus model. I have to restart the unsteady case with a steady state solution of the same model. I am just renaming the steady state solution restat_flow.dat to restat_flow_00000.dat, restat_flow_00001.dat, restat_flow_00002.dat, and trying to run the unsteady cases. With both DUAL_TIME_STEPPING-2ND_ORDER and DUAL_TIME_STEPPING-1ST_ORDER options , I get the following error, which looks a bit strange to me. Code:
Error in "void CSolver::Restart_OldGeometry(CGeometry *, CConfig *)": ------------------------------------------------------------------------- There is no flow restart file restart_flow_00002.csv ------------------------------ Error Exit ------------------------------- So, does the restart option (for dual time stepping) not work with ROTATING_FRAME? If so, is there any other way to get a time-accurate solution for this kind of a problem? I am pasting my .cfg here 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= YES %-----------------------TIME DOMAIN--------------------------------------------% % Time domain simulation TIME_DOMAIN= YES % % Unsteady simulation (NO, TIME_STEPPING, DUAL_TIME_STEPPING-1ST_ORDER, % DUAL_TIME_STEPPING-2ND_ORDER, HARMONIC_BALANCE) TIME_MARCHING= DUAL_TIME_STEPPING-2ND_ORDER % % Time Step for dual time stepping simulations (s) -- Only used when UNST_CFL_NUMBER = 0.0 % For the DG-FEM solver it is used as a synchronization time when UNST_CFL_NUMBER != 0.0 TIME_STEP= 1.0E-6 % % Total Physical Time for dual time stepping simulations (s) MAX_TIME= 10.0 % % Unsteady Courant-Friedrichs-Lewy number of the finest grid %UNST_CFL_NUMBER= 10 % TIME_ITER=300000 % Number of internal iterations (dual time method) INNER_ITER= 100 % % Specify unsteady restart iter RESTART_ITER = 3 % -------------------- COMPRESSIBLE FREE-STREAM DEFINITION --------------------% % % Mach number (non-dimensional, based on the free-stream values) MACH_NUMBER= 0.5 % % Angle of attack (degrees, only for compressible flows) AOA= 0.0 % % Side-slip 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 % % Free-stream option to choose between density and temperature (default) for % initializing the solution (TEMPERATURE_FS, DENSITY_FS) FREESTREAM_OPTION= TEMPERATURE_FS % % Free-stream temperature (288.15 K by default) FREESTREAM_TEMPERATURE= 288.15 % FREESTREAM_PRESSURE= 101325 % % Free-stream Turbulence Intensity FREESTREAM_TURBULENCEINTENSITY = 0.05 % % Free-stream Turbulent to Laminar viscosity ratio FREESTREAM_TURB2LAMVISCRATIO = 100.0 % % Reynolds number (non-dimensional, based on the free-stream values) REYNOLDS_NUMBER= 2.5E6 % % Reynolds length (1 m by default) REYNOLDS_LENGTH= .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 (1.716E-5 default value for AIR SI) MU_REF= 1.716E-5 % % 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 (non-dimensional). 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 non-dimensional moment REF_LENGTH= 0.64607 % % Reference area for force coefficients (0 implies automatic calculation) REF_AREA= 0 % % Compressible flow non-dimensionalization (DIMENSIONAL, FREESTREAM_PRESS_EQ_ONE, % FREESTREAM_VEL_EQ_MACH, FREESTREAM_VEL_EQ_ONE) REF_DIMENSIONALIZATION= DIMENSIONAL % -------------------- BOUNDARY CONDITION DEFINITION --------------------------% % Navier-Stokes wall boundary marker(s) (NONE = no marker) MARKER_HEATFLUX= ( BLADE, 0.0, BLADE_0, 0.0, BLADE_1, 0.0, BLADE_2, 0.0, BLADE_3, 0.0, BLADE_4, 0.0, BLADE_5, 0.0, BLADE_6, 0.0, BLADE_7, 0.0, BLADE_8, 0.0, BLADE_9, 0.0, BLADE_10, 0.0, BLADE_11, 0.0, BLADE_12, 0.0, BLADE_13, 0.0, BLADE_14, 0.0, BLADE_15, 0.0, BLADE_16, 0.0, BLADE_17, 0.0, BLADE_18, 0.0, BLADE_19, 0.0, BLADE_20, 0.0, HUB, 0.0, SHROUD, 0.0 ) MARKER_SHROUD=(SHROUD) % % Viscous wall markers for which wall functions must be applied. (NONE = no marker) % Format: ( marker name, wall function type -NO_WALL_FUNCTION, STANDARD_WALL_FUNCTION, % ADAPTIVE_WALL_FUNCTION, SCALABLE_WALL_FUNCTION, EQUILIBRIUM_WALL_MODEL, % NONEQUILIBRIUM_WALL_MODEL-, ... ) %MARKER_WALL_FUNCTIONS= ( BLADE, STANDARD_WALL_FUNCTION, HUB, STANDARD_WALL_FUNCTION, SHROUD, STANDARD_WALL_FUNCTION ) % % Symmetry boundary marker(s) (NONE = no marker) % % Internal boundary marker(s) e.g. no boundary condition (NONE = no marker) MARKER_INTERNAL= (PER1, PER2, 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 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_wo_komega.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, 115000 ) % Specify Kind of average process for linearizing the Navier-Stokes % equation at inflow and outflow BCs included at the mixing-plane 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, 1.0E-08, 100) % % Limit of Mach number below which the mixedout algorithm is substituted % with a AREA average algorithm to avoid numerical issues AVERAGE_MACH_LIMIT= 0.01 % ------------------------ SURFACES IDENTIFICATION ----------------------------% % % Marker(s) of the surface in the surface flow solution file MARKER_PLOTTING= ( INFLOW, OUTFLOW) % Marker(s) of the surface where the non-dimensional coefficients are evaluated. MARKER_MONITORING = ( INFLOW, OUTFLOW ) % %Viscous wall markers for which wall functions must be applied. (NONE = no marker) % Format: ( marker name, wall function type -NO_WALL_FUNCTION, STANDARD_WALL_FUNCTION, % ADAPTIVE_WALL_FUNCTION, SCALABLE_WALL_FUNCTION, EQUILIBRIUM_WALL_MODEL, % NONEQUILIBRIUM_WALL_MODEL-, ... ) %MARKER_WALL_FUNCTIONS= ( airfoil, NO_WALL_FUNCTION ) % %Marker(s) of the surface where custom thermal BC's are defined. %MARKER_PYTHON_CUSTOM = ( NONE ) % %Marker(s) of the surface where obj. func. (design problem) will be evaluated %MARKER_DESIGNING = ( airfoil ) % % 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 % % Courant-Friedrichs-Lewy condition of the finest grid CFL_NUMBER= 1 % % 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 ) % % Runge-Kutta alpha coefficients RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 ) % % Number of total iterations %ITER= 300000 %INNER_ITER= 1000 % Start convergence criteria at iteration number % % ------------------------ 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= ILU % % Min error of the linear solver for the implicit formulation LINEAR_SOLVER_ERROR= .05 % % Max number of iterations of the linear solver for the implicit formulation LINEAR_SOLVER_ITER= 10 % -------------------------- MULTIGRID PARAMETERS -----------------------------% % % Multi-Grid Levels (0 = no multi-grid) MGLEVEL= 0 % % Multi-grid cycle (V_CYCLE, W_CYCLE, FULLMG_CYCLE) MGCYCLE= V_CYCLE % % Multi-grid pre-smoothing level MG_PRE_SMOOTH= ( 1, 1, 1, 1 ) % % Multi-grid post-smoothing 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, LAX-FRIEDRICH, 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 % lower-order approximation to the solution (0.05 by default) % VENKAT_LIMITER_COEFF= 0.05 % 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 (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT) TIME_DISCRE_FLOW= EULER_IMPLICIT %TIME_DISCRE_FLOW= EULER_EXPLICIT % -------------------- 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= 1E-10 % % ------------------------- INPUT/OUTPUT INFORMATION --------------------------% % % Mesh input file MESH_FILENAME=../../r67_grid1_.35M_5em7m_FA.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_MOMENTUM-X, RMS_MOMENTUM-Y, SURFACE_MASSFLOW, SURFACE_TOTAL_PRESSURE, SURFACE_TOTAL_TEMPERATURE) % VOLUME_OUTPUT= (MOMENTUM-X, MOMENTUM-Y, MOMENTUM-Z, 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) %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% Thank you, Jyoti |
|
December 1, 2021, 17:29 |
|
#2 |
Member
na
Join Date: Jul 2018
Posts: 90
Rep Power: 8 |
well, are you maybe mixing up binary .dat and ascii .csv files? ... But I am not sure if anything weird is happening. We have the option READ_BINARY_RESTART= YES/NO where the default is YES. And I guess you always write binary .dat files via OUTPUT_FILES= RESTART
Maybe you could try switching to ASCII files by OUTPUT_FILES= RESTART_ASCII and then try to restart with READ_BINARY_RESTART= NO maybe that helps already |
|
December 7, 2021, 12:10 |
|
#3 |
New Member
Jyoti Ranjan
Join Date: Oct 2020
Posts: 14
Rep Power: 5 |
Hello Tobi,
I was using .dat only. I tried switching to ASCII files - that does not work either. It says the solution file mesh is different even though I am using the same mesh. Code:
Error in "void CSolver::Read_SU2_Restart_ASCII(CGeometry *, const CConfig *, std::__cxx11::string)": ------------------------------------------------------------------------- The solution file does not match the mesh, currently only binary files can be interpolated. ------------------------------ Error Exit ------------------------------- Thank you, Jyoti |
|
December 8, 2021, 05:21 |
|
#4 |
Senior Member
Pedro Gomes
Join Date: Dec 2017
Posts: 466
Rep Power: 13 |
Hi,
Can you try your initial method (binary restart) but in addition create the ascii outputs. So, in your steady-state use OUTPUT_FILES= RESTART_ASCII, RESTART, ... like TKatt suggested, but do not use READ_BINARY_RESTART= NO. |
|
December 8, 2021, 05:28 |
|
#5 |
Senior Member
Pedro Gomes
Join Date: Dec 2017
Posts: 466
Rep Power: 13 |
Also, to my shame I have not done many turbomachinery simulations in SU2, but if you are doing full-annulus unsteady, shouldn't you be using a RIGID_MOTION instead of a rotating frame?
i.e. the entire mesh is moved every time step. I guess the two modelling options are equivalent if you only have one stage. |
|
December 8, 2021, 08:29 |
|
#6 |
New Member
Jyoti Ranjan
Join Date: Oct 2020
Posts: 14
Rep Power: 5 |
Yes, I have tried this in the process of trying out combinations of binary, ascii, etc. and the case was running at least. I was waiting to see if it is converging (still in progress). Thanks.
|
|
December 8, 2021, 08:34 |
|
#7 | |
New Member
Jyoti Ranjan
Join Date: Oct 2020
Posts: 14
Rep Power: 5 |
Quote:
|
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[Other] Contribution a new utility: refine wall layer mesh based on yPlus field | lakeat | OpenFOAM Community Contributions | 58 | December 23, 2021 02:36 |
laplacianFoam with source term | Herwig | OpenFOAM Running, Solving & CFD | 17 | November 19, 2019 13:47 |
Setting up Lid driven Cavity Benchmark with 1M cells for multiple cores | puneet336 | OpenFOAM Running, Solving & CFD | 11 | April 7, 2019 00:58 |
Domain Reference Pressure and mass flow inlet boundary | AdidaKK | CFX | 75 | August 20, 2018 05:37 |
Solution does not advance with time: steady state too soon? | Noix_V | FLUENT | 7 | June 21, 2018 00:01 |