CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > SU2

Time-accurate solution restart from steady state solution

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 30, 2021, 13:25
Default Time-accurate solution restart from steady state solution
  #1
New Member
 
Jyoti Ranjan
Join Date: Oct 2020
Posts: 14
Rep Power: 5
jyotir is on a distinguished road
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 -------------------------------
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
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
jyotir is offline   Reply With Quote

Old   December 1, 2021, 17:29
Default
  #2
Member
 
na
Join Date: Jul 2018
Posts: 83
Rep Power: 7
TKatt is on a distinguished road
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
TKatt is offline   Reply With Quote

Old   December 7, 2021, 12:10
Default
  #3
New Member
 
Jyoti Ranjan
Join Date: Oct 2020
Posts: 14
Rep Power: 5
jyotir is on a distinguished road
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
jyotir is offline   Reply With Quote

Old   December 8, 2021, 05:21
Default
  #4
pcg
Senior Member
 
Pedro Gomes
Join Date: Dec 2017
Posts: 465
Rep Power: 13
pcg is on a distinguished road
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 is offline   Reply With Quote

Old   December 8, 2021, 05:28
Default
  #5
pcg
Senior Member
 
Pedro Gomes
Join Date: Dec 2017
Posts: 465
Rep Power: 13
pcg is on a distinguished road
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.
pcg is offline   Reply With Quote

Old   December 8, 2021, 08:29
Default
  #6
New Member
 
Jyoti Ranjan
Join Date: Oct 2020
Posts: 14
Rep Power: 5
jyotir is on a distinguished road
Quote:
Originally Posted by pcg View Post
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 is offline   Reply With Quote

Old   December 8, 2021, 08:34
Default
  #7
New Member
 
Jyoti Ranjan
Join Date: Oct 2020
Posts: 14
Rep Power: 5
jyotir is on a distinguished road
Quote:
Originally Posted by pcg View Post
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.
jyotir is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 05:52.