CFD Online Discussion Forums - [NEMO] Divergence for two-directional flow

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- SU2 (https://www.cfd-online.com/Forums/su2/)

- - [NEMO] Divergence for two-directional flow (https://www.cfd-online.com/Forums/su2/254639-nemo-divergence-two-directional-flow.html)

[NEMO] Divergence for two-directional flow

Hi pals!

I am trying to analyse Falcon 9 along its reentry trajectory. To simply the simulation, I'm having a simplified model with one nozzle at the moment in Argon environment.

There are two main parts:
1. Descent w/o plume
2. Descent w plume

For part 1, there are no issues with it and the results are fine. For part 2, I configure the Argon freestream and added MARKER_SUPERSONIC_INLET at the nozzle exit with negative x-velocity component but it diverges immediately.

Code:

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

%                                                                              %

% SU2 configuration file                                                       %

% Case description: Simplified Falcon 9 (Argon)                                       %

% Author: Jesslyn Ong                                                                %

% Institution: Korea Advanced Institute of Science and Technology              %

% Date: 22.02.2024                                                             %

% File Version 8.0.0 "Harrier"                                                 %

%                                                                              %

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



SOLVER= NEMO_NAVIER_STOKES

MATH_PROBLEM= DIRECT

SYSTEM_MEASUREMENTS= SI



TIME_DOMAIN= NO

CFL_NUMBER= 0.5

ITER= 50000



FLUID_MODEL= SU2_NONEQ

GAS_MODEL= ARGON

GAS_COMPOSITION= ( 1.0 )

FROZEN_MIXTURE= YES



VISCOSITY_MODEL= SUTHERLAND

CONDUCTIVITY_MODEL= CONSTANT_PRANDTL



MACH_NUMBER= 4.675

INIT_OPTION= TD_CONDITIONS

FREESTREAM_PRESSURE= 0.1129

FREESTREAM_TEMPERATURE= 198.6

FREESTREAM_TEMPERATURE_VE= 198.6



MARKER_FAR= ( FARFIELD, INLET )

MARKER_SMOLUCHOWSKI_MAXWELL= ( WALL, 300 )

MARKER_SUPERSONIC_INLET= ( NOZZLEEXIT, 1500, 3.55E+4, -3000, 0.0, 0.0 )

INLET_TEMPERATURE_VE= 1500

INLET_GAS_COMPOSITION= ( 1.0 )

MARKER_MONITORING= ( WALL )

MARKER_PLOTTING= ( WALL )

MARKER_ANALYZE= ( WALL )



REF_LENGTH= 13

REF_AREA= 0

NUM_METHOD_GRAD= WEIGHTED_LEAST_SQUARES

TRANSPORT_COEFF_MODEL= WILKE

%CONV_NUM_METHOD_FLOW= ROE

CONV_NUM_METHOD_FLOW= AUSMPLUSUP2

USE_ACCURATE_FLUX_JACOBIANS= YES

TIME_DISCRE_FLOW= EULER_EXPLICIT



MESH_FILENAME= 2dfull.su2

MESH_FORMAT= SU2

SOLUTION_FILENAME= restart_flow

VOLUME_FILENAME= flow

TABULAR_FORMAT= CSV



OUTPUT_FILES= RESTART, PARAVIEW

VOLUME_OUTPUT= ( COORDINATES, SOLUTION, PRIMITIVE, TIME_STEP )

HISTORY_OUTPUT= ( ITER, FLOW_COEFF, AERO_COEFF, HEAT, FLOW_COEFF_SURF, AERO_COEFF_SURF, HEAT_SURF )

CONV_FILENAME= history

OUTPUT_WRT_FREQ= 50

WRT_RESTART_OVERWRITE= YES



RESTART_SOL= NO

RESTART_FILENAME= restart_flow.dat

READ_BINARY_RESTART= YES

The error code is as follow:

Code:

------------------------------ Begin Solver -----------------------------



Simulation Run using the Single-zone Driver





Error in "void CSolver::SetResidual_RMS(const CGeometry*, const CConfig*)": 

-------------------------------------------------------------------------

SU2 has diverged (NaN detected).

------------------------------ Error Exit -------------------------------

Any ideas will be much appreciated! Cheers!

Mesh file:
https://drive.google.com/file/d/1vtG...ew?usp=sharing

Hi Jessowy,

Thanks for using SU2-NEMO! It seems like an interesting problem and look forward to seeing the results. As a quick heads-up, I can't see any of the mesh files - I no longer have access to all my tools.

Your setup looks good.
Some things I would suggest are:
1.) Run using the AUSM or MSW numerical scheme. In my experience, they were much more stable.
2.) I would make sure you are running to a first-order simulation to start (MUSCL=NO).

I think the difficulty is arising due to the nozzle exit flow condition. The numerics, at the beginning of the simulation, see a velocity gradient of M=4.5 flow to a negative value....which I suspect is causing problems.
You can play some games here:
1.) You can use a restart file. Take you good solution from your first solution, then apply the nozzle condition.

2.) You can create/alter your restart file to better initialize the flow. You can manually change the restart csv file to include a plume region where the flow state would more closely resemble the plume. This may alleviate the large gradients.

3.) Finally, (I think this would work - but not confident), is to set your freestream conditions to stationary flow (or close to it). Then the inflow of your domain and the nozzle exit would be initialized as a supersonic inlet. This will allow the plume to develop before interacting with the M=4.5 flow. You may need to run the problem unsteady for this.

I am not aware of anyone trying to simulate any type of retro-propulsion with SU2 in general, so you are in uncharted territory. Please let me know if any of this helps.

Wally