[jyotir]

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.

Error in "void CSolver::Restart_OldGeometry(CGeometry *, CConfig *)": 
-------------------------------------------------------------------------
There is no flow restart file restart_flow_00002.csv
------------------------------ Error Exit -------------------------------

I observed that, switching off GRID_MOVEMENT which needs to be set as ROTATING_FRAME for my case, gets the case running.
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

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%                                                                              %
% 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

[TKatt]

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

[jyotir]

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.

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

[pcg]

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.

[pcg]

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.

[jyotir]

Originally Posted by pcg

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.

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.

[jyotir]

Originally Posted by pcg

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.

Not sure. Usually a moving reference frame is much more efficient computationally. And, RIGID_MOTION may not work IMO as one surface (shroud) has to be stationary; I will see, at some time, if it works.