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

Supersonic 2D Ramp Air Intake Outlet Back Pressure

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

Like Tree2Likes
  • 1 Post By pcg
  • 1 Post By pcg

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 5, 2022, 06:43
Default Supersonic 2D Ramp Air Intake Outlet Back Pressure
  #1
New Member
 
Barış Bıçakçı
Join Date: Dec 2021
Location: Turkey
Posts: 7
Rep Power: 3
BarisBicakci is on a distinguished road
Hello everyone,
I'm trying to run viscous simulation for Supersonic flow over 2D Ramp Air Intake of McDonnell Douglas F-15 Eagle. But I have a problem with Outlet boundary conditions. As a result of the simulation, when the flow passes through the throat of the air intake, it slows down as expected due to the oblique shocks and decreases to subsonic speeds. But the problem is that as the flow moves towards the outlet, it speeds up again and reaches supersonic speeds. Everything I tried to prevent this was unsuccessful. No matter how much I changed the Outlet Back Pressure, the result was still the same. Should I define the Outlet back pressure more than the static Pressure I have defined for Inlet? It didn't make sense for me.
You can see my configuration file and my boundary markers below. I'm also attaching the simulation results from Praview. Could someone help me to understand how should I solve this problem? I would be really appriciate for any kind of suggesstion. This is my graduation project.

% ------------- 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, SA_E, SA_COMP, SA_E_COMP, SST_SUST)
KIND_TURB_MODEL= SST
%
% Mathematical problem (DIRECT, CONTINUOUS_ADJOINT)
MATH_PROBLEM= DIRECT
%
% Restart solution (NO, YES)
RESTART_SOL= NO
%
% System of measurements (SI, US)
% International system of units (SI): ( meters, kilograms, Kelvins,
% Newtons = kg m/s^2, Pascals = N/m^2,
% Density = kg/m^3, Speed = m/s,
% Equiv. Area = m^2 )
% United States customary units (US): ( inches, slug, Rankines, lbf = slug ft/s^2,
% psf = lbf/ft^2, Density = slug/ft^3,
% Speed = ft/s, Equiv. Area = ft^2 )
SYSTEM_MEASUREMENTS= SI

% ---- NONEQUILIBRIUM GAS, IDEAL GAS, POLYTROPIC, VAN DER WAALS AND PENG ROBINSON CONSTANTS -------%
%
% Fluid model (STANDARD_AIR, IDEAL_GAS, VW_GAS, PR_GAS,
% CONSTANT_DENSITY, INC_IDEAL_GAS, INC_IDEAL_GAS_POLY, MUTATIONPP, SU2_NONEQ)
FLUID_MODEL= STANDARD_AIR
%

% ----------- COMPRESSIBLE AND INCOMPRESSIBLE FREE-STREAM DEFINITION ----------%
%
% Mach number (non-dimensional, based on the free-stream values)
MACH_NUMBER= 2.2
%
% Reynolds number (non-dimensional, based on the free-stream values)
REYNOLDS_NUMBER= 6947291
% Reynolds length (1 m, 1 inch by default)
REYNOLDS_LENGTH= 1.0
%
% Angle of attack (degrees)
AOA= 3
%
% Side-slip angle (degrees)
SIDESLIP_ANGLE= 0.0
%
% Free-stream pressure (101325.0 N/m^2 by default, only Euler flows)
FREESTREAM_PRESSURE= 8830
%
% Free-stream temperature (288.15 K by default)
FREESTREAM_TEMPERATURE= 216.75
%
% Free-stream velocity (1.0 m/s, 1.0 ft/s by default)
FREESTREAM_VELOCITY= ( 649.5, 0.00, 0.00 )

% --------------------------- 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
%


% ---------------------- REFERENCE VALUE DEFINITION ---------------------------%
%
% Reference origin for moment computation
REF_ORIGIN_MOMENT_X = 0.25
REF_ORIGIN_MOMENT_Y = 0.00
REF_ORIGIN_MOMENT_Z = 0.00
%
% Reference length for pitching, rolling, and yawing non-dimensional moment
REF_LENGTH= 1.0
%
% Reference area for force coefficients (0 implies automatic calculation)
REF_AREA= 1.0

% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Navier-Stokes (no-slip), constant heat flux wall marker(s) (NONE = no marker)
% Format: ( marker name, constant heat flux (J/m^2), ... )
MARKER_HEATFLUX= ( UpperWall, 0, LowerWall, 0 )
%
% Marker of the far field (0 implies no marker)
MARKER_FAR= ( FarField )
%
% Supersonic inlet boundary marker(s) (NONE = no marker)
% Total Conditions: (inlet marker, temperature, static pressure, velocity_x,
% velocity_y, velocity_z, ... ), i.e. all variables specified.
MARKER_SUPERSONIC_INLET= ( Inlet, 216.75, 8830, 649.5, 0.0, 0.0 )
%
% Outlet boundary marker(s) (NONE = no marker)
% Format: ( outlet marker, back pressure (static), ... )
MARKER_OUTLET= ( Outlet, 1000.0 )
%
% Marker(s) of the surface to be plotted or designed
MARKER_PLOTTING= ( Outlet )
%
% Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated
MARKER_MONITORING= ( UpperWall, LowerWall )

% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
% Numerical method for spatial gradients (GREEN_GAUSS, LEAST_SQUARES,
% WEIGHTED_LEAST_SQUARES)
NUM_METHOD_GRAD= WEIGHTED_LEAST_SQUARES
%
% Courant-Friedrichs-Lewy condition of the finest grid
CFL_NUMBER= 5.0
%
% 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= ( 0.1, 2.0, 5.0, 1e10 )
%
% Runge-Kutta alpha coefficients
RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 )
%
% Number of total iterations
ITER= 100000
%
% Linear solver for the implicit formulation (BCGSTAB, FGMRES)
LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver (ILU, JACOBI, LINELET, LU_SGS)
LINEAR_SOLVER_PREC= ILU
%
% Min error of the linear solver for the implicit formulation
LINEAR_SOLVER_ERROR= 1E-6
%
% Max number of iterations of the linear solver for the implicit formulation
LINEAR_SOLVER_ITER= 20

% -------------------------- MULTIGRID PARAMETERS -----------------------------%
%
% Multi-Grid Levels (0 = no multi-grid)
MGLEVEL= 0
%
% Multi-grid cycle (V_CYCLE, W_CYCLE, FULLMG_CYCLE)
MGCYCLE= W_CYCLE
%
% Multi-grid pre-smoothing level
MG_PRE_SMOOTH= ( 1, 2, 3, 3 )
%
% 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= 1.0
%
% Damping factor for the correction prolongation
MG_DAMP_PROLONGATION= 1.0

% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
% Convective numerical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, HLLC,
% TURKEL_PREC, MSW)
CONV_NUM_METHOD_FLOW= JST
%
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the flow equations.
% Required for 2nd order upwind schemes (NO, YES)
MUSCL_FLOW= YES
%
% Slope limiter (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG,
% BARTH_JESPERSEN, VAN_ALBADA_EDGE)
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN
%
% Coefficient for the limiter (smooth regions)
VENKAT_LIMITER_COEFF= 0.006
%
% 2nd and 4th order artificial dissipation coefficients
JST_SENSOR_COEFF= ( 0.5, 0.02 )
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_FLOW= EULER_IMPLICIT

% --------------------------- CONVERGENCE PARAMETERS --------------------------%
%
% Convergence criteria (CAUCHY, RESIDUAL)
CONV_FIELD= RMS_DENSITY
%
% Min value of the residual (log10 of the residual)
CONV_RESIDUAL_MINVAL= -8
%
% 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

% -------------------- 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
Attached Images
File Type: png mach number.png (144.2 KB, 24 views)
BarisBicakci is offline   Reply With Quote

Old   February 5, 2022, 07:43
Default
  #2
New Member
 
Barış Bıçakçı
Join Date: Dec 2021
Location: Turkey
Posts: 7
Rep Power: 3
BarisBicakci is on a distinguished road
Or should I define the outlet marker as INC_OUTLET_TYPE= MASS_FLOW_OUTLET . Then set a appropriate massflow rate for outlet to be able to decrease the mach towards the outlet.
BarisBicakci is offline   Reply With Quote

Old   February 5, 2022, 18:30
Default
  #3
pcg
Senior Member
 
Pedro Gomes
Join Date: Dec 2017
Posts: 428
Rep Power: 11
pcg is on a distinguished road
You should not mix inlets and outlets with farfield when the associated surfaces intersect.
A farfield boundary is both inlet and outlet depending on the flow direction, and both sub and supersonic depending on Mach number.
Your domain also looks too small, look for guidelines on how far the boundaries should be from the surface. If it's all supersonic 10x might be enough but don't quote me on that, when in doubt test the sensitivity to your modelling assumptions.
BarisBicakci likes this.
pcg is offline   Reply With Quote

Old   February 5, 2022, 18:37
Default
  #4
pcg
Senior Member
 
Pedro Gomes
Join Date: Dec 2017
Posts: 428
Rep Power: 11
pcg is on a distinguished road
You are also using a weird mix of methods.
JST is not great for supersonic or for detailed viscous stuff (not our implementation anyway).
Try ROE with the van Albada limiter and green Gauss gradients.
And SST is probably overkill, SA is usually fine for external aero stuff and you can get away with higher y+.
BarisBicakci likes this.
pcg is offline   Reply With Quote

Old   February 5, 2022, 19:08
Default
  #5
New Member
 
Barış Bıçakçı
Join Date: Dec 2021
Location: Turkey
Posts: 7
Rep Power: 3
BarisBicakci is on a distinguished road
Quote:
Originally Posted by pcg View Post
You should not mix inlets and outlets with farfield when the associated surfaces intersect.
A farfield boundary is both inlet and outlet depending on the flow direction, and both sub and supersonic depending on Mach number.
Your domain also looks too small, look for guidelines on how far the boundaries should be from the surface. If it's all supersonic 10x might be enough but don't quote me on that, when in doubt test the sensitivity to your modelling assumptions.
Thank you for your valuable suggestions and I will definitely consider them. I'm really inexperienced in computational fluids dynamics and SU2.
But I'm sorry, I just couldn't understand the point about the not mixing inlets and outlets with Farfield. I also ran another simulation without the outside region for the same geometry before as you can see in the attachment picture. However I had the result with same problem.
Attached Images
File Type: jpg mac.jpg (20.9 KB, 14 views)
BarisBicakci is offline   Reply With Quote

Reply

Tags
su2, supersonic, supersonic inlet, viscous

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
Computation of Aerodynamic Loads for the Air Intake of a Supersonic Airplane BarisBicakci SU2 1 December 22, 2021 17:20
Getting divergence while increasing the back pressure at pressure outlet greenfields15 FLUENT 0 March 19, 2018 00:39
sonicFoam - pressure driven pipe: flow continuity violation and waveTransmissive BC Endel OpenFOAM Running, Solving & CFD 3 September 11, 2014 17:29
the static pressure at one outlet is negative? yuhehuan Main CFD Forum 7 August 15, 2013 22:01
Gas pressure question Dan Moskal Main CFD Forum 0 October 24, 2002 23:02


All times are GMT -4. The time now is 09:10.