[Madsskjaerbaek]

Hello everyone,

I'm currently working on simulating unsteady subsonic nozzle flow into a large box with a single outlet, using SU2. The setup aims to study the fluid mixing between the inlet flow and the existing fluid within the box. Although the steady-state simulation provides accurate results with an expected outlet velocity of approximately 110 m/s, I'm facing challenges with the unsteady simulation.

Issue:
In the unsteady simulation, the fluid movement is unusually slow. It takes about 500 ms for the flow field to visibly develop near the outlet, which is significantly slower than expected. Based on my experimental data, the inlet fluid should reach the nozzle's outlet in less than 1 ms. However, the simulation results at 500 ms show little to no movement of the species from the inlet.

Attachments:

- Mesh configuration and geometry
- CFG file settings
- Snapshot of the results at 500 ms

I've attached relevant images and files for reference. Given these observations, I suspect there might be an issue with my simulation setup, possibly related to the mesh, time step, or boundary conditions.

I would greatly appreciate any insights or suggestions on potential misconfigurations or adjustments needed to resolve this discrepancy. Has anyone encountered a similar issue, or does anyone have recommendations on parameters to check or modify?

Thank you in advance for your help!

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%                                                                              %
% SU2 configuration file                                                       %
% Case description: Transient jet flow of a converging nozzle                  %
%                                                                              %
% Author: Mads Sjærbæk and Johan Ildor                                         %
% Institution: The Technical University of Denmark                             %
% Date: 2024.03.26                                                             %
%                                                                              %
%                                                                              %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%
% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
% Physical governing equations
%
SOLVER= RANS
%
% Turbulence model
%
KIND_TURB_MODEL= SST
%
% Version
%
SST_OPTIONS= V2003m 
%
% Mathematical problem
%
MATH_PROBLEM= DIRECT
% 
% Axisymmetric simulation (only compressible flows)
%
AXISYMMETRIC= YES
%
% Gravity force
%
GRAVITY_FORCE= NO 
%
% Resume simulation?
%
RESTART_SOL= YES
SOLUTION_FILENAME= restart_flow.dat
RESTART_ITER= 4161
%
% System of measurements
%
SYSTEM_MEASUREMENTS= SI
%
% -------------------- COMPRESSIBLE FREE-STREAM DEFINITION --------------------%
%
% Mach number
%
MACH_NUMBER= 1E-9
%
% Angle of attack
%
AOA= 0
%
% Thermodynamic initial quantities for initializing the solution
%
INIT_OPTION= TD_CONDITIONS
%
% Free-stream temperature for initializing the solution 
%
FREESTREAM_OPTION= TEMPERATURE_FS
%
% Free-stream pressure
%
FREESTREAM_PRESSURE= 101325.0
%
% Free-stream temperature
%
FREESTREAM_TEMPERATURE= 298.15
%
% Compressible flow non-dimensionalization
%
REF_DIMENSIONALIZATION= DIMENSIONAL
%
% ---- IDEAL GAS, POLYTROPIC, VAN DER WAALS AND PENG ROBINSON CONSTANTS -------%
%
% Fluid model
%
FLUID_MODEL= STANDARD_AIR
%
%
% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Navier-Stokes wall boundary marker (NONE = no marker)
%
MARKER_HEATFLUX= ( wall, 0.0 )
%
% Inlet boundary marker (NONE = no marker) 
% Format: ( inlet marker, total temperature, total pressure, flow_direction_x, 
%           flow_direction_y, flow_direction_z, ... )
%
INLET_TYPE= TOTAL_CONDITIONS
MARKER_INLET = (inlet, 298.15, 109858.8, -1.0, 0.0, 0.0)
%
MARKER_OUTLET = (outlet, 101325.0)
%
%MARKER_RIEMANN= ( inlet, TOTAL_CONDITIONS_PT, 109858.8, 298.15, 1, 0.0, 0.0, outlet, STATIC_PRESSURE, 101325.0, 0.0, 0.0, 0.0, 0.0 )
%
%
% Symmetry boundary marker(s) (NONE = no marker)
%
MARKER_SYM= ( symmetry )
%
% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
%
% CFL number (initial value for the adaptive CFL number)
%
CFL_NUMBER= 10  
%
% Adaptive CFL number
%
CFL_ADAPT= YES
%
% Parameters of the adaptive CFL number (factor down, factor up, CFL min value,
%                                        CFL max value )
CFL_ADAPT_PARAM= ( 0.1, 2.0, 0.5, 1000.0 )
%
% ----------- SLOPE LIMITER AND DISSIPATION SENSOR DEFINITION -----------------%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the flow equations.
%           Required for 2nd order upwind schemes (NO, YES)
% MUSCL_FLOW= NO
%
% Slope limiter (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG,
%                BARTH_JESPERSEN, VAN_ALBADA_EDGE)
%SLOPE_LIMITER_FLOW= VENKATAKRISHNAN
%
% 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
%
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the turbulence equations.
%           Required for 2nd order upwind schemes (NO, YES)
%MUSCL_TURB= NO
% ------------------------ LINEAR SOLVER DEFINITION ---------------------------%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%
% Linear solver or smoother for implicit formulations (BCGSTAB, FGMRES, SMOOTHER_JACOBI,
%                                                      SMOOTHER_ILU, SMOOTHER_LUSGS,
%                                                      SMOOTHER_LINELET)
LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver (ILU, LU_SGS, LINELET, JACOBI)
LINEAR_SOLVER_PREC= ILU
%
% Linael solver ILU preconditioner fill-in level (0 by default)
LINEAR_SOLVER_ILU_FILL_IN= 0
%
% Minimum error of the linear solver for implicit formulations
LINEAR_SOLVER_ERROR= 1E-6
%
% 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
% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%
%
% Entropy fix coefficient (0.0 implies no entropy fixing, 1.0 implies scalar
%                          artificial dissipation)
%ENTROPY_FIX_COEFF= 0.1
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_FLOW= EULER_IMPLICIT

% DISCRETIZATION
%
TIME_DOMAIN= YES
TIME_MARCHING= DUAL_TIME_STEPPING-1ST_ORDER
%TIME_STEP= 1e-3
UNST_CFL_NUMBER= 10
%
%NUM_METHOD_GRAD= WEIGHTED_LEAST_SQUARES
CONV_NUM_METHOD_FLOW= JST
JST_SENSOR_COEFF= ( 0.5, 0.005 )
% -------------------- TURBULENT NUMERICAL METHOD DEFINITION ------------------%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%
% Convective numerical method (SCALAR_UPWIND)
CONV_NUM_METHOD_TURB= SCALAR_UPWIND
%
% Time discretization (EULER_IMPLICIT)
TIME_DISCRE_TURB= EULER_IMPLICIT
%
% Reduction factor of the CFL coefficient in the turbulence problem
% CFL_REDUCTION_TURB= 1.0

% --------------------------- CONVERGENCE PARAMETERS --------------------------%
% INNER CONVERGENCE
%
INNER_ITER= 100
CONV_FIELD= REL_RMS_DENSITY
CONV_RESIDUAL_MINVAL= -8
CONV_STARTITER= 0
 
% TIME CONVERGENCE
%
TIME_ITER= 5000000
%
% Starting iteration and type for windowed-time-averaging
%WINDOW_CAUCHY_CRIT= YES
%WINDOW_START_ITER= 500
%
% ------------------------- Time-dependent Simulation -------------------------------%
%
%TIME_DOMAIN= YES
%
% Time Step for dual time stepping simulations (s)
%TIME_STEP= 1e-3
%
% Total Physical Time for dual time stepping simulations (s)
%MAX_TIME= 25e-3
%
% Number of internal iterations 
% INNER_ITER= 2
% CONV_FIELD= REL_RMS_DENSITY
% CONV_RESIDUAL_MINVAL= -5
% CONV_STARTITER= 0
%
%
% TIME_ITER = 2000
%
% --------------------- SPECIES TRANSPORT SIMULATION --------------------------%
%
% Specify scalar transport model (NONE, SPECIES_TRANSPORT)
KIND_SCALAR_MODEL= SPECIES_TRANSPORT
%
% Mass diffusivity model (CONSTANT_DIFFUSIVITY)
DIFFUSIVITY_MODEL= CONSTANT_DIFFUSIVITY
%
% Mass diffusivity if DIFFUSIVITY_MODEL= CONSTANT_DIFFUSIVITY is chosen. D_air ~= 0.001
DIFFUSIVITY_CONSTANT= 0.001
%
% Turbulent Schmidt number of mass diffusion
SCHMIDT_NUMBER_TURBULENT= 0.7
%
% Inlet Species boundary marker(s) with the following format:
% (inlet_marker, Species1, Species2, ..., SpeciesN-1, inlet_marker2, Species1, Species2, ...)
MARKER_INLET_SPECIES= (inlet, 1.0)
%
% Convective numerical method for species transport (SCALAR_UPWIND)
CONV_NUM_METHOD_SPECIES= SCALAR_UPWIND
%
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the species equations.
% Required for 2nd order upwind schemes (NO, YES)
MUSCL_SPECIES= NO
%
% Slope limiter for species equations (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG, BARTH_JESPERSEN, VAN_ALBADA_EDGE)
SLOPE_LIMITER_SPECIES = NONE
%
% Time discretization for species equations (EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_SPECIES= EULER_IMPLICIT
%
% Reduction factor of the CFL coefficient in the species problem
CFL_REDUCTION_SPECIES= 1.0
%
% Initial values for scalar transport
SPECIES_INIT= 0.0
%
% Activate clipping for scalar transport equations
SPECIES_CLIPPING= NO
%
%
% ------------------------- INPUT/OUTPUT INFORMATION --------------------------%
%
% Mesh input file
MESH_FILENAME= NozzleMesh_Allsquares_2.su2
%
% Mesh input file format (SU2, CGNS)
MESH_FORMAT= SU2
%
% Mesh output file
MESH_OUT_FILENAME= mesh_out.su2
%
% Restart flow input file
% SOLUTION_FILENAME= restart_flow.dat
% SOLUTION_ADJ_FILENAME= restart_adj.dat
%
% Output file format (TECPLOT, TECPLOT_BINARY, PARAVIEW, PARAVIEW_BINARY,
%                     FIELDVIEW, FIELDVIEW_BINARY)
%
% Output file format
OUTPUT_FILES= (RESTART, PARAVIEW)
%
TABULAR_FORMAT= CSV
%
% Output file convergence history (w/o extension)
CONV_FILENAME= history
%
%
%
% ------ Transient -----
% Output file restart flow
RESTART_FILENAME= restart.dat
% RESTART_ADJ_FILENAME= restart_adj.dat
WRT_RESTART_OVERWRITE= YES	
%
% ----------------------
%
% Output file flow (w/o extension) variables
VOLUME_FILENAME= flow
%
% Output file surface flow coefficient (w/o extension)
SURFACE_FILENAME= surface_flow
%
% Writing solution file frequency
OUTPUT_WRT_FREQ= (8)
%
% Screen output
SCREEN_OUTPUT= (TIME_INNER, INNER_ITER, RMS_DENSITY, RMS_TKE, RMS_DISSIPATION, cur_TIME, TIME_STEP, WALL_TIME)

[bigfootedrockmidget]

Indeed, it looks like the species are not being propagated into the domain correctly. I did a small test and I could reproduce this with another geometry.
This is strange, because much of what the species do is the same as for turbulent transport, and that seems to work fine in the same test case.
I will investigate some more to see where this comes from.

[bigfootedrockmidget]

I am very sorry to inform you that there was a bug in the update of the time-step for species transport. I have added a fix in a branch and created a pull request:
https://github.com/su2code/SU2/pull/2260


You can checkout the branch with the fix by git using

git checkout fix_unsteady_species

I hope this is sufficient for your purposes. This again proves that every part of the code needs a regression and validation test.


PS: for scalar transport we also have the numerical scheme BOUNDED_SCALAR, which is mass conserving.

[bigfootedrockmidget]

This fix was merged with the develop branch. Let me know if this fixes the issue for you. If you have validated a case for unsteady species transport, consider adding it to our testcases repository.