[Kamranh01]

Hey, guys for some reason I cannot get my simulation to run past 100 iterations and I am confused about why. I get the following error message too and I have no idea what it means, help would be appreciated, here's the config file below!

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% %
% SU2 configuration file %
% Case description: NACA 0012 Rotor %
% Author:K.Hussain %
% Institution: University of Strathclyde %
% Date: Feb 28th, 2023 %
% File Version 7.5.1 "Blackbird" %
% %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
SOLVER= EULER
%
KIND_TURB_MODEL= NONE
%
MATH_PROBLEM= DIRECT
%
RESTART_SOL= NO
%
SYSTEM_MEASUREMENTS= SI
%
% -------------------- COMPRESSIBLE FREE-STREAM DEFINITION --------------------%
%
MACH_NUMBER= 0.0
%
AOA= 7.0
%
FREESTREAM_PRESSURE= 101327.0
%
FREESTREAM_TEMPERATURE= 288.15
%
FREESTREAM_DENSITY= 1.225
%
FREESTREAM_OPTION= TEMPERATURE_FS
%%
REYNOLDS_NUMBER= 165389.9181
%%
REYNOLDS_LENGTH= 0.05
%%
INIT_OPTION= TD_CONDITIONS
%
REF_DIMENSIONALIZATION= DIMENSIONAL
%%
% ---------------------- REFERENCE VALUE DEFINITION ---------------------------%
REF_ORIGIN_MOMENT_X = 0.00
%%
REF_ORIGIN_MOMENT_Y = 0.00
%%
REF_ORIGIN_MOMENT_Z = -0.1
%
%
REF_LENGTH= 0.05
%
%
REF_AREA= 0

% --------------------------------- FLUID MODEL -----------------------------------%
%
FLUID_MODEL= IDEAL_GAS
%%
GAMMA_VALUE= 1.4
%%
GAS_CONSTANT= 287.06

%
% --------------------------- VISCOSITY MODEL ---------------------------------%
%
VISCOSITY_MODEL= SUTHERLAND
%%
MU_CONSTANT= 1.716E-5
%%
MU_REF= 1.716E-5
%%
MU_T_REF= 273.15
%%
SUTHERLAND_CONSTANT= 110.4
%
%
% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
MARKER_HEATFLUX= ( BLADE, 0.0 )

MARKER_FAR= ( FAR )

MARKER_INLET= ( INLET, 288.15, 101327, 0.0, 1.0, 0.0)

MARKER_OUTLET= ( OUTLET, 101327)

MARKER_PERIODIC= ( SIDE_1, SIDE_2, 0.0, 0.0, -0.1, 0.0, 120.0, 0.0, 0.0, 0.0, 0.0 )
%%%
% ------------------------ SURFACES IDENTIFICATION ----------------------------%
%
MARKER_PLOTTING= ( BLADE )
%
%
MARKER_MONITORING= ( BLADE )

% ----------------------- DYNAMIC MESH DEFINITION -----------------------------%
%
GRID_MOVEMENT= ROTATING_FRAME
%
MACH_MOTION= 0.3456
%
MOTION_ORIGIN= 0.0 0.0 -0.1
%
ROTATION_RATE= 0.0, 62.44, 0.0

% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
NUM_METHOD_GRAD= WEIGHTED_LEAST_SQUARES

CFL_NUMBER= 0.01
%%
CFL_ADAPT= NO
%%
CFL_ADAPT_PARAM= ( 0.1, 1.2, 10.0, 1000.0)
%%
RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 )
%
% ------------------------ LINEAR SOLVER DEFINITION ---------------------------%
%
LINEAR_SOLVER= FGMRES
%%
LINEAR_SOLVER_PREC= ILU
%%%
LINEAR_SOLVER_ERROR= 1E-16
%%
LINEAR_SOLVER_ITER= 50
%
% ----------------------- SLOPE LIMITER DEFINITION ----------------------------%
%
VENKAT_LIMITER_COEFF= 0.05
LIMITER_ITER= 999999
%
% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
CONV_NUM_METHOD_FLOW= JST
%
MUSCL_FLOW= NO
%
ENTROPY_FIX_COEFF= 0.001
%
JST_SENSOR_COEFF= ( 0.5, 0.02 )
%
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN
%
TIME_DISCRE_FLOW= EULER_IMPLICIT
%

% --------------------------- SOLVER CONTROLS --------------------------%
%convergeance criteria
%%%
TIME_DOMAIN= NO
%%
INNER_ITER= 999999
%%%
ITER= 999999
%%
CONV_RESIDUAL_MINVAL= 1E-8
%%
CONV_STARTITER= 0
%%
%%
CONV_FIELD= (LIFT,DRAG)
%
% ------------------------- INPUT/OUTPUT INFORMATION --------------------------%
%
MESH_FILENAME= MARK1TALL.su2
%
MESH_FORMAT= SU2
%
MESH_OUT_FILENAME= MESH1_out.su2
%
SOLUTION_FILENAME= restart_flow.csv
%
SOLUTION_ADJ_FILENAME= solution_adj.csv
%
TABULAR_FORMAT= CSV
%
OUTPUT_FILES= (PARAVIEW, SURFACE_PARAVIEW, RESTART_ASCII)
%
CONV_FILENAME= history
%
RESTART_FILENAME= restart_flow.csv
%
RESTART_ADJ_FILENAME= restart_adj.csv
VOLUME_FILENAME= flow
%
VOLUME_ADJ_FILENAME= adjoint
%
VALUE_OBJFUNC_FILENAME= of_eval.csv
%
GRAD_OBJFUNC_FILENAME= of_grad.csv
%
SURFACE_FILENAME= surface_flow
%
SURFACE_ADJ_FILENAME= surface_adjoint
%%
OUTPUT_WRT_FREQ= 100
%
%
WRT_FORCES_BREAKDOWN = YES
%
HISTORY_OUTPUT = (ITER, RMS_RES, AERO_COEFF)
SCREEN_OUTPUT = (INNER_ITER, RMS_DENSITY, LIFT, DRAG, CAUCHY_LIFT,CAUCHY_DRAG)

as again any help is hugely appreciated!

[bigfootedrockmidget]

It looks like at 100 iterations it wants to write the skin friction to the paraview output files, put it cannot find this field. This might be a bug.

If you remove the surface_paraview output, does the problem go away?

OUTPUT_FILES= (PARAVIEW, RESTART_ASCII)

Or if you do not write primitive information to the file:

VOLUME_OUTPUT= (SOLUTION)

[Kamranh01]

I tried both but it didn't do anything, its a really strange bug I have never seen anything like it before on any of the forums

[pcg]

You cannot use MARKER_HEATFLUX with an Euler solver.
Euler is inviscid and MARKER_HEATFLUX is a no-slip boundary, you need to use MARKER_EULER instead.

[Kamranh01]

that did the trick, thank you, sir. I was initially using navier stokes but decided to just use Euler for the mesh convergence process, I just didn't remove the heat flux as I assumed it would run fine with it. You are a lifesaver thank you