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

High drag for airfoil compared to XFOIL and wind tunnel data

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

Like Tree1Likes
  • 1 Post By Ry10

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 22, 2016, 13:11
Default High drag for airfoil compared to XFOIL and wind tunnel data
  #1
New Member
 
Ryan Barrett
Join Date: May 2015
Posts: 15
Rep Power: 6
Ry10 is on a distinguished road
I am trying to get the lift and drag coefficients out of a 2D airfoil using SU2. I am doing a steady 2D incompressible RANS simulation with the SA turbulence model. I have attached two graphs that I compare the results from XFOIL(panel method) and known wind tunnel data for different angles of attack. The lift matches pretty well but the drag is very high. Is there something wrong with my config file that would cause this? I tried to attach my su2 mesh but it was too big, but let me know if you need it. Thanks!

Code:
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%                                                                              %
% SU2 configuration file                                                       %
% Case description: 2D NACA 0012 Airfoil Validation Case (incompressible)      %
%                   http://turbmodels.larc.nasa.gov/naca0012_val_sa.html       %
% Author: Francisco Palacios	                                               %
% Institution: Stanford University                                             %
% Date: Feb 18th, 2013                                                         %
% File Version 4.0.0 "Cardinal"                                                %
%                                                                              %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
% Physical governing equations (EULER, NAVIER_STOKES,
%                               TNE2_EULER, TNE2_NAVIER_STOKES,
%                               WAVE_EQUATION, HEAT_EQUATION, LINEAR_ELASTICITY,
%                               POISSON_EQUATION)
PHYSICAL_PROBLEM= NAVIER_STOKES
%
% Specify turbulent model (NONE, SA, SA_NEG, SST)
KIND_TURB_MODEL= SA
%
% Mathematical problem (DIRECT, ADJOINT, LINEARIZED)
MATH_PROBLEM= DIRECT
%
% Regime type (COMPRESSIBLE, INCOMPRESSIBLE, FREESURFACE)
REGIME_TYPE= INCOMPRESSIBLE
%
% Restart solution (NO, YES)
RESTART_SOL= NO

% ------------------------- UNSTEADY SIMULATION -------------------------------%
%
% Unsteady simulation (NO, TIME_STEPPING, DUAL_TIME_STEPPING-1ST_ORDER, 
%                      DUAL_TIME_STEPPING-2ND_ORDER, TIME_SPECTRAL)
UNSTEADY_SIMULATION= NO
% CONSOLE = CONCISE
% -------------------- INCOMPRESSIBLE FREE-STREAM DEFINITION ------------------%
%
% Mach number
% MACH_NUMBER= 0.15
% Angle of attack (deg)
% AoA= -5.0

% Free-stream density (1.2886 Kg/m^3 (air), 998.2 Kg/m^3 (water))
FREESTREAM_DENSITY= 2.13163
%
% Free-stream velocity (m/s)
FREESTREAM_VELOCITY= ( 10.0, 0.00, 0.00 )
%
% Free-stream viscosity (1.853E-5 Ns/m^2 (air), 0.798E-3 Ns/m^2 (water))
FREESTREAM_VISCOSITY= 1.853e-05

% ---------------------- 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_MOMENT= 1.0
%
% Reference area for force coefficients (0 implies automatic calculation)
REF_AREA= 1.0
%%%%%
% MOTION
%GRID_MOVEMENT = YES
%GRID_MOVEMENT_KIND = NONE
%GRID_MOVEMENT_KIND = ROTATING_FRAME
%MACH_MOTION = 0.7958
%MARKER_MOVING = NONE
%MOTION_ORIGIN_X = 0.5
%MOTION_ORIGIN_Y = -32.0
%MOTION_ORIGIN_Z = 0.0
%ROTATION_RATE_X = 0.0
%ROTATION_RATE_Y = 0.0
%ROTATION_RATE_Z = 0.0 
%8.25

% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Navier-Stokes wall boundary marker(s) (NONE = no marker)
MARKER_HEATFLUX= ( airfoil, 0.0 )
%
% Farfield boundary marker(s) (NONE = no marker)
MARKER_FAR= ( farfield )
%
% Marker(s) of the surface to be plotted or designed
MARKER_PLOTTING= ( airfoil )
%
% Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated
MARKER_MONITORING= ( airfoil )

% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
% Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES)
NUM_METHOD_GRAD= WEIGHTED_LEAST_SQUARES
%
% Courant-Friedrichs-Lewy condition of the finest grid
CFL_NUMBER= 10.0
%
% 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= ( 1.5, 0.5, 1.0, 100.0 )
%
% Number of total iterations
EXT_ITER= 75000

% ----------------------- SLOPE LIMITER DEFINITION ----------------------------%
%
% Reference element length for computing the slope and sharp edges limiters.
REF_ELEM_LENGTH= 0.1
%
% Coefficient for the limiter
LIMITER_COEFF= 0.1
%
%
% Reference coefficient (sensitivity) for detecting sharp edges.
REF_SHARP_EDGES= 3.0
%
% Remove sharp edges from the sensitivity evaluation (NO, YES)
SENS_REMOVE_SHARP= NO

% ------------------------ LINEAR SOLVER DEFINITION ---------------------------%
%
% Linear solver for implicit formulations (BCGSTAB, FGMRES)
LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver (JACOBI, LINELET, LU_SGS)
LINEAR_SOLVER_PREC= LU_SGS
%
% Minimum error of the linear solver for implicit formulations
LINEAR_SOLVER_ERROR= 1E-4
%
% Max number of iterations of the linear solver for the implicit formulation
LINEAR_SOLVER_ITER= 5

% -------------------------- 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, 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= 0.75
%
% Damping factor for the correction prolongation
MG_DAMP_PROLONGATION= 0.75

% -------------------- 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)
%
SPATIAL_ORDER_FLOW= 2ND_ORDER_LIMITER
%
% Slope limiter (VENKATAKRISHNAN, MINMOD)
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN
%
% 1st, 2nd and 4th order artificial dissipation coefficients
AD_COEFF_FLOW= ( 0.15, 0.5, 0.02 )
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_FLOW= EULER_IMPLICIT

% ---------------- ADJOINT-FLOW NUMERICAL METHOD DEFINITION -------------------%
% Adjoint problem boundary condition (DRAG, LIFT, SIDEFORCE, MOMENT_X,
%                                     MOMENT_Y, MOMENT_Z, EFFICIENCY,
%                                     EQUIVALENT_AREA, NEARFIELD_PRESSURE,
%                                     FORCE_X, FORCE_Y, FORCE_Z, THRUST,
%                                     TORQUE, FREE_SURFACE, TOTAL_HEAT,
%                                     MAXIMUM_HEATFLUX, INVERSE_DESIGN_PRESSURE,
%                                     INVERSE_DESIGN_HEATFLUX)
OBJECTIVE_FUNCTION= DRAG
%
% Convective numerical method (JST, LAX-FRIEDRICH, ROE)
CONV_NUM_METHOD_ADJFLOW= ROE
%
% Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER)
%
SPATIAL_ORDER_ADJFLOW= 2ND_ORDER
%
% Slope limiter (VENKATAKRISHNAN, SHARP_EDGES)
SLOPE_LIMITER_ADJFLOW= VENKATAKRISHNAN
%
% Coefficient for the sharp edges limiter
SHARP_EDGES_COEFF= 3.0
%
% 1st, 2nd, and 4th order artificial dissipation coefficients
AD_COEFF_ADJFLOW= ( 0.15, 0.0, 0.002 )
%
% Reduction factor of the CFL coefficient in the adjoint problem
CFL_REDUCTION_ADJFLOW= 0.25
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT)
TIME_DISCRE_ADJFLOW= EULER_IMPLICIT
%
% Adjoint frozen viscosity (NO, YES)
FROZEN_VISC= YES

% -------------------- TURBULENT NUMERICAL METHOD DEFINITION ------------------%
%
% Convective numerical method (SCALAR_UPWIND)
CONV_NUM_METHOD_TURB= SCALAR_UPWIND
%
% Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER)
%
SPATIAL_ORDER_TURB= 1ST_ORDER
%
% Slope limiter (VENKATAKRISHNAN, MINMOD)
SLOPE_LIMITER_TURB= VENKATAKRISHNAN
%
% Time discretization (EULER_IMPLICIT)
TIME_DISCRE_TURB= EULER_IMPLICIT

% --------------------------- CONVERGENCE PARAMETERS --------------------------%
%
% Convergence criteria (CAUCHY, RESIDUAL)
%
CONV_CRITERIA= CAUCHY
%
% Residual reduction (order of magnitude with respect to the initial value)
RESIDUAL_REDUCTION= 5
%
% Min value of the residual (log10 of the residual)
RESIDUAL_MINVAL= -10
%
% Start convergence criteria at iteration number
STARTCONV_ITER= 10
%
% Number of elements to apply the criteria
CAUCHY_ELEMS= 100
%
% Epsilon to control the series convergence
CAUCHY_EPS= 8E-6
%
% Function to apply the criteria (LIFT, DRAG, NEARFIELD_PRESS, SENS_GEOMETRY, 
% 	      	    		 SENS_MACH, DELTA_LIFT, DELTA_DRAG)
CAUCHY_FUNC_FLOW= LIFT
%CAUCHY_FUNC_LIN= DELTA_DRAG
% ------------------------- GRID ADAPTATION STRATEGY --------------------------%
%
% Percentage of new elements (% of the original number of elements)
NEW_ELEMS= 5
%
% Kind of grid adaptation (NONE, FULL, FULL_FLOW, GRAD_FLOW, FULL_ADJOINT,
%                          GRAD_ADJOINT, GRAD_FLOW_ADJ, ROBUST,
%                          FULL_LINEAR, COMPUTABLE, COMPUTABLE_ROBUST,
%                          REMAINING, WAKE, SMOOTHING, SUPERSONIC_SHOCK,
%                          TWOPHASE)
KIND_ADAPT= FULL_FLOW
%
% Scale factor for the dual volume
DUALVOL_POWER= 0.5
%
% Before each computation do an implicit smoothing of the nodes coord (NO, YES)
SMOOTH_GEOMETRY= NO
% ------------------------- INPUT/OUTPUT INFORMATION --------------------------%
%
% Mesh input file
%MESH_FILENAME= mesh_NACA0012_turb_897x257.su2
MESH_FILENAME = mesh_AIRFOIL.su2
%
% Mesh input file format (SU2, CGNS, NETCDF_ASCII)
MESH_FORMAT= SU2
%
% Mesh output file
MESH_OUT_FILENAME= mesh_out.su2
%
% Restart flow input file
SOLUTION_FLOW_FILENAME= solution_flow.dat
%
% Restart adjoint input file
SOLUTION_ADJ_FILENAME= solution_adj.dat
%
% Output file format (PARAVIEW, TECPLOT, STL)
OUTPUT_FORMAT= PARAVIEW
%
% Output file convergence history (w/o extension) 
CONV_FILENAME= history
%
% Output file restart flow
RESTART_FLOW_FILENAME= solution_flow.dat
%
% Output file restart adjoint
RESTART_ADJ_FILENAME= restart_adj.dat
%
% Output file flow (w/o extension) variables
VOLUME_FLOW_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_FLOW_FILENAME= surface_flow
%
% Output file surface adjoint coefficient (w/o extension)
SURFACE_ADJ_FILENAME= surface_adjoint
%
% Writing solution file frequency
WRT_SOL_FREQ= 5000
%
% Writing convergence history frequency
WRT_CON_FREQ= 1000

DV_KIND = HICKS_HENNE
DV_MARKER = ( airfoil )
DV_PARAM = ( 1, 0.5 )
DEFINITION_DV= ( 1, 1.0 | airfoil | 0, 0.05 ); ( 1, 1.0 | airfoil | 0, 0.10 ); ( 1, 1.0 | airfoil | 0, 0.15 ); ( 1, 1.0 | airfoil | 0, 0.20 ); ( 1, 1.0 | airfoil | 0, 0.25 ); ( 1, 1.0 | airfoil | 0, 0.30 ); ( 1, 1.0 | airfoil | 0, 0.35 ); ( 1, 1.0 | airfoil | 0, 0.40 ); ( 1, 1.0 | airfoil | 0, 0.45 ); ( 1, 1.0 | airfoil | 0, 0.50 ); ( 1, 1.0 | airfoil | 0, 0.55 ); ( 1, 1.0 | airfoil | 0, 0.60 ); ( 1, 1.0 | airfoil | 0, 0.65 ); ( 1, 1.0 | airfoil | 0, 0.70 ); ( 1, 1.0 | airfoil | 0, 0.75 ); ( 1, 1.0 | airfoil | 0, 0.80 ); ( 1, 1.0 | airfoil | 0, 0.85 ); ( 1, 1.0 | airfoil | 0, 0.90 ); ( 1, 1.0 | airfoil | 0, 0.95 ); ( 1, 1.0 | airfoil | 1, 0.05 ); ( 1, 1.0 | airfoil | 1, 0.10 ); ( 1, 1.0 | airfoil | 1, 0.15 ); ( 1, 1.0 | airfoil | 1, 0.20 ); ( 1, 1.0 | airfoil | 1, 0.25 ); ( 1, 1.0 | airfoil | 1, 0.30 ); ( 1, 1.0 | airfoil | 1, 0.35 ); ( 1, 1.0 | airfoil | 1, 0.40 ); ( 1, 1.0 | airfoil | 1, 0.45 ); ( 1, 1.0 | airfoil | 1, 0.50 ); ( 1, 1.0 | airfoil | 1, 0.55 ); ( 1, 1.0 | airfoil | 1, 0.60 ); ( 1, 1.0 | airfoil | 1, 0.65 ); ( 1, 1.0 | airfoil | 1, 0.70 ); ( 1, 1.0 | airfoil | 1, 0.75 ); ( 1, 1.0 | airfoil | 1, 0.80 ); ( 1, 1.0 | airfoil | 1, 0.85 ); ( 1, 1.0 | airfoil | 1, 0.90 ); ( 1, 1.0 | airfoil | 1, 0.95 )
% DEFINITION_DV = (( 1, 1.0 | airfoil | 0, 0.961538461538 ); ( 1, 1.0 | airfoil | 0, 0.923076923077 ); ( 1, 1.0 | airfoil | 0, 0.884615384615 ); ( 1, 1.0 | airfoil | 0, 0.846153846154 ); ( 1, 1.0 | airfoil | 0, 0.807692307692 ); ( 1, 1.0 | airfoil | 1, 0.846153846154 ); ( 1, 1.0 | airfoil | 1, 0.884615384615 ); ( 1, 1.0 | airfoil | 1, 0.923076923077 ); ( 1, 1.0 | airfoil | 1, 0.961538461538 )
Attached Images
File Type: png drag_comparison.png (49.1 KB, 112 views)
File Type: png lift_comparison.png (48.4 KB, 95 views)
abonfi likes this.
Ry10 is offline   Reply With Quote

Old   February 22, 2016, 21:03
Default Experienced similar things
  #2
New Member
 
Join Date: Jul 2015
Posts: 7
Rep Power: 6
anon_k is on a distinguished road
Hi,

For what it's worth, I have noticed the same thing. The drag is always higher than the test data I have from an old NACA report. Cl and Cm vary from too high to too low, depending on the solver choice and CFL number. I was using SU2_EDU.
anon_k is offline   Reply With Quote

Old   February 23, 2016, 01:07
Default
  #3
Member
 
Eduardo Molina
Join Date: Sep 2010
Location: Brazil
Posts: 35
Rep Power: 11
EMolina is on a distinguished road
Hi...

Let me ask you some questions. Did your simulation converged? Why you are using Cauchy converge criteria? Can you show us the density residual?

Cheers

Molina
EMolina is offline   Reply With Quote

Old   February 23, 2016, 18:38
Default
  #4
New Member
 
Ryan Barrett
Join Date: May 2015
Posts: 15
Rep Power: 6
Ry10 is on a distinguished road
Quote:
Originally Posted by EMolina View Post
Hi...

Let me ask you some questions. Did your simulation converged? Why you are using Cauchy converge criteria? Can you show us the density residual?

Cheers

Molina
My simulation did converge. I have been using the Cauchy convergence criteria because I am using the CFD in an outer loop and it seemed more robust. My residuals are all pretty low between -7 and -12.
Res[Press] Res[nu]
-7.827376 -10.677632
Ry10 is offline   Reply With Quote

Old   February 24, 2016, 12:01
Default
  #5
New Member
 
Mike
Join Date: Oct 2015
Posts: 11
Rep Power: 6
gunnersnroses is on a distinguished road
Hi

Is the reference area you've set definitely correct/the same as you've used for the wind tunnel/other experiments?

You currently have it set to the default 1m^2 (REF_AREA= 1.0)

Cheers,
M.
gunnersnroses is offline   Reply With Quote

Old   February 24, 2016, 16:54
Default
  #6
New Member
 
Ryan Barrett
Join Date: May 2015
Posts: 15
Rep Power: 6
Ry10 is on a distinguished road
Quote:
Originally Posted by gunnersnroses View Post
Hi

Is the reference area you've set definitely correct/the same as you've used for the wind tunnel/other experiments?

You currently have it set to the default 1m^2 (REF_AREA= 1.0)

Cheers,
M.
Yes. Everything was normalized to 1.0 for all the calculations that are compared. My lift matches pretty well, it is my drag that is quite high in comparison.
Ry10 is offline   Reply With Quote

Old   October 11, 2016, 05:58
Default
  #7
New Member
 
luigi
Join Date: Oct 2016
Posts: 6
Rep Power: 5
luigi22 is on a distinguished road
Hi,
I have to calculate Cl Cd for different type of airfoils to vary the angle of attack (alpha), I do in this way:
naca0018
pane
oper
visc 100000
iter 1000
alfa 0
pacc naca0018.pol
aseq -30.0 30.0 2.0
pacc
quit
The results are different from the datas, maybe cause the large variation of alpha. what do you think?
luigi22 is offline   Reply With Quote

Old   October 13, 2016, 17:35
Default
  #8
hlk
Senior Member
 
Heather Kline
Join Date: Jun 2013
Posts: 306
Rep Power: 9
hlk is on a distinguished road
It looks like this hasn't been mentioned on this thread yet:
Since the panel method and data match well, but the turbulent viscous simulation does not, it could be that the issue is with the turbulence - either that the flow in the experiment was closer to laminar, or that the grid is not refined enough near the wall to accurately capture the boundary layer.

On the angle of attack sweep from -30 to 30 degrees - that is a wide enough range that the flow would certainly be separated and not likely to be providing an accurate solution towards the ends of that range. (unless using very high fidelity CFD - ie unsteady LES methods)
hlk is offline   Reply With Quote

Old   October 14, 2016, 04:58
Default
  #9
New Member
 
Join Date: Dec 2013
Location: Italy
Posts: 26
Rep Power: 7
Jiba is on a distinguished road
Just some other points:

1. did you set the transition point in XFOIL? If not the code will predict a "free" transition, conversely SU2 is fully turbulent. A comparison in terms of cf could be interesting

2. the turbulence model is solved as 1st order, did you check with 2nd order accuracy?
Jiba is offline   Reply With Quote

Old   October 14, 2016, 07:29
Default
  #10
New Member
 
luigi
Join Date: Oct 2016
Posts: 6
Rep Power: 5
luigi22 is on a distinguished road
Hi,
I didn't set the transition point and I didn't check with 2nd order accuracy, the only things that I write in the prompt are:
naca0018
pane
oper
visc 100000
iter 1000
alfa 0
pacc naca0018.pol
aseq -30.0 30.0 2.0
pacc
quit
I read in a document that is better using the command "init" for a large range of alpha and I don't know if the command "alpha 0" (after iter) is necessary. What do you think?
I tryed the same for different Reynold's Numbers and I have the same problems, maybe the issues are linked to an error in my script.
Thank you very much!
luigi22 is offline   Reply With Quote

Old   October 14, 2016, 08:53
Default
  #11
New Member
 
Join Date: Dec 2013
Location: Italy
Posts: 26
Rep Power: 7
Jiba is on a distinguished road
Quote:
Originally Posted by luigi22 View Post
Hi,
I didn't set the transition point and I didn't check with 2nd order accuracy, the only things that I write in the prompt are:
naca0018
pane
oper
visc 100000
iter 1000
alfa 0
pacc naca0018.pol
aseq -30.0 30.0 2.0
pacc
quit
I read in a document that is better using the command "init" for a large range of alpha and I don't know if the command "alpha 0" (after iter) is necessary. What do you think?
I tryed the same for different Reynold's Numbers and I have the same problems, maybe the issues are linked to an error in my script.
Thank you very much!

The script itself is not wrong, anyway you are performing a free transition analysis (so keep in mind that when comparing the results). Could you post the details about SU2 simulation, like y+ and the input file?
Jiba is offline   Reply With Quote

Old   October 15, 2016, 04:15
Default
  #12
New Member
 
luigi
Join Date: Oct 2016
Posts: 6
Rep Power: 5
luigi22 is on a distinguished road
I don't have an SU2 simulation; I had experimental datas (maybe from Sandia Lab) to be compared with my xfoil's results.
luigi22 is offline   Reply With Quote

Old   October 19, 2016, 14:16
Default
  #13
New Member
 
luigi
Join Date: Oct 2016
Posts: 6
Rep Power: 5
luigi22 is on a distinguished road
Hi,
I have another question, like you can see on my script there is the command alpha 0 (after iter 1000); I used this command cause there was in a tutorial but I don't know the utility, I thought that was only to see the Cp at alpha 0 but then I noticed that, with this command (alpha 0), my final results are less correct. Do you know its function?
thank you very much!
luigi22 is offline   Reply With Quote

Old   October 19, 2016, 14:25
Default
  #14
hlk
Senior Member
 
Heather Kline
Join Date: Jun 2013
Posts: 306
Rep Power: 9
hlk is on a distinguished road
Quote:
Originally Posted by luigi22 View Post
I don't have an SU2 simulation; I had experimental datas (maybe from Sandia Lab) to be compared with my xfoil's results.
For more information on running and interpreting xfoil data, I would suggest seeking out a similar support forum for that code, or seeing what their contact/support suggestions are on their website.
hlk is offline   Reply With Quote

Old   October 20, 2016, 15:03
Default
  #15
New Member
 
luigi
Join Date: Oct 2016
Posts: 6
Rep Power: 5
luigi22 is on a distinguished road
Hi,
I have another question, like you can see on my script there is the command alpha 0 (after iter 1000); I used this command cause there was in a tutorial but I don't know the utility, I thought that was only to see the Cp at alpha 0 but then I noticed that, with this command (alpha 0), my final results are less correct. Do you know its function?
thank you very much!

About this what do you think?
luigi22 is offline   Reply With Quote

Old   October 30, 2016, 18:27
Default
  #16
Member
 
C
Join Date: Apr 2013
Posts: 34
Rep Power: 8
whizkid is on a distinguished road
Hello all,
The problem here is possibly because that the flow is transitional (Re = 1.1M and freestream turbulence intensity is around 0.1%). You should solve the case with a transition model. Recently, I have added my own transition model (named BC (Bas-Cakmakcioglu) Model) to the code, and I have opened a pull request (#326). Maybe you can test this case with the BC model, and see the results.

Hopefully, the BC transition model will be merged into the master branch after some testing.

Best,
S. Cakmakcioglu
whizkid is offline   Reply With Quote

Reply

Tags
drag, su2, xfoil

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



All times are GMT -4. The time now is 20:17.