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

SU2 cfg file and runtime problems

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

Like Tree1Likes
  • 1 Post By pdp.aero

Reply
 
LinkBack Thread Tools Display Modes
Old   May 6, 2014, 10:27
Default SU2 cfg file and runtime problems
  #1
Member
 
Hedley
Join Date: May 2014
Posts: 48
Rep Power: 3
hedley is on a distinguished road
Does anyone have an explanation of the .cfg file and what each option does in clear plain English ?

When running I get the error message
"The solution contains .......... non-physical points "
followed by
" terminate called after throwing instance of int "

what do these mean ? any help greatly appreciated.
hedley is offline   Reply With Quote

Old   May 18, 2014, 21:57
Default
  #2
Super Moderator
 
Francisco Palacios
Join Date: Jan 2013
Location: Stanford, CA
Posts: 301
Rep Power: 5
fpalacios is on a distinguished road
Quote:
Originally Posted by hedley View Post
Does anyone have an explanation of the .cfg file and what each option does in clear plain English ?

When running I get the error message
"The solution contains .......... non-physical points "
followed by
" terminate called after throwing instance of int "

what do these mean ? any help greatly appreciated.
It means that the code is diverging (non-physical points means that you are obtaining a negative density). Could you please try to reduce the CFL number and remove the multigrid?
CFL_NUMBER= 0.75
MGLEVEL= 0

Thanks for using SU2,

Best Francisco
fpalacios is offline   Reply With Quote

Old   May 20, 2014, 08:09
Default
  #3
New Member
 
Join Date: Feb 2014
Posts: 10
Rep Power: 3
CFDbeginner88 is on a distinguished road
Concerning your question about an explanation of the config file. I have made a start with some other students and until now, this is what we got. It is still work in progress, keep that in mind.

Common parameters defining the numerical method
Spatial gradient calculation
The current version of SU2 (3.0) has the possibility to use Green-Gauss (GG), Least-squares (LS) and Weighted-least-squares (WLS) methods to compute the spatial gradients.
In the case of well ordered meshes, both GG as WLS as LS can be used. [1] In principle all the methods should converge to the same result, the only difference being convergence speed.
In the case of distorted meshes, GG is preferred. Distorted meshes often appear in meshes that represent boundary layers for high Reynolds numbers.

Linear solver definition
BCGSTAB or FGMRES
In case an implicit or discrete adjoint formulation is chosen to solve a problem, one can chose two linear solvers. FGMRES is the more stable one from the two options, working for both Euler and RANS flows. In case Euler is used, one could also use BCGSTAB.
Preconditioner of the krylov linear solver
If one wants to use a preconditioner, a choice can be made between Jacobi, Linelet and LU_SGS. From these three preconditioners, Jacobi is the most simple one and works well for Euler but not for RANS. In case of Jacobi, RANS simulations will not converge. LU_SGS should be used if one uses RANS flow.

Flow numerical method definition
Convective numerical method
Numerical Flow Methods are used to calculate the convective fluxes. The current version of SU2 (3.0) has the possibility to use a large number of different methods. A few are mentioned here.
JST (Jameson-Schmidt-Turkel)
JST is a central scheme with second order accuracy making it more stable but less accurate than ROE. To obtain similar results for JST as those of ROE, the mesh should be increased.
Lax - Friedrich
The Lax - Friedrich method (centered scheme) requires very fine grids in order to achieve correct results. In case the grids are not very fine, the numerical results will be badly smeared. This is due to the fact that the Lax - Friedrich method uses more diffusion than necessary. This method is stable for CFL numbers up to 1. (Finite Volume Methods for Hyperbolic Problems, LeVeque R.J., 2002)
ROE (Roes Approximate Riemann Solver)
ROE has better accuracy than JST and is particularly useful when examining boundary layers.
Time discretization
The current version of SU2 (3.0) has the possibility to use Euler-implicit, Euler-explicit and Runge-Kutta-explicit.
Difference between Implicit and Explicit
Implicit schemes use both the current and latter state of a system to find a solution while explicit schemes only use a latter system. Implicit schemes are known to be more stable over a wide range of time steps at the cost of higher cost per time step since they have to perform an extra calculation. If the differential equation features a rapid decaying solution, it is called a stiff differential equation. When a differential equation is not stiff, one can use explicit methods.
Difference between Runge-Kutta and Euler
Where Euler connects points with a straight line (first order), Runge-Kutta methods uses parabolas (second order) and quartic curves (fourth order) to connects points with a curved line. Derivatives at multiple points are calculated in the evaluation interval after which weighted averages are calculated for the change of the function between these evaluation points. This results in a smaller error compared to Euler. Runge-Kutta methods are preferred for dynamic time varying chaotic systems where very large accuracy is necessary. The room for error in such systems is very small, leading to rapid changing behavior and potential non-convergence.
CFDbeginner88 is offline   Reply With Quote

Old   May 20, 2014, 09:49
Default
  #4
Member
 
Payam D.
Join Date: Aug 2011
Posts: 81
Blog Entries: 3
Rep Power: 6
pdp.aero is on a distinguished road
Quote:
JST (Jameson-Schmidt-Turkel)
JST is a central scheme with second order accuracy making it more stable but less accurate than ROE. To obtain similar results for JST as those of ROE, the mesh should be increased.
Quote:
ROE (Roes Approximate Riemann Solver)
ROE has better accuracy than JST and is particularly useful when examining boundary layers.
CFDbeginner88,

You need more evaluation for making a comparison between the Roe and JST schemes and their accuracy.

Considering the external compressible inviscid flow over an airfoil with AoA ranging from 0 to 6 degree, the resulted aerodynamic coefficients using different schemes and their comparison demonstrate that the JST obtains more accurate aerodynamic coefficients rather than the Roe, in particular moment coefficient. The drag and lift coefficient for both schemes agree very well. However, in the AoA bigger than 3 degree, the moment coefficient resulted from 2nd-order Roe have a considerable vertical offset from the actual trend.

Already, I have compared them for the aforementioned case. Their Cm-Cl comparison has been attached. As the figure demonstrates, 3 schemes are considered for 5 cases. The 2nd-order Roe's test cases differ in their artificial dissipation coefficients, which are (0.25, 0.5, 0.5) and (0.65, 0.5, 0.02). The results from the JST scheme match with the actual trend for the test case.

This is not limited to the SU2 or the inviscid two-dimensional condition. Actually, I had this situation long ago with the 2nd-order Roe scheme for the viscous or inviscid flow around a wing, wing-body or airfoils using the Fluent. I have no idea yet why the 2nd-order Roe originally results in such a vertical offset from the actual trend by increasing the AoA. What I do know is JST obtains accurate coefficients.

Cheers,
PDP
Attached Images
File Type: png JST_Roe_comparison.png (92.6 KB, 39 views)
pdp.aero is offline   Reply With Quote

Old   May 20, 2014, 13:52
Default Basic lift and drag on a 3d wing
  #5
Member
 
Hedley
Join Date: May 2014
Posts: 48
Rep Power: 3
hedley is on a distinguished road
Still trying to figure out why the solver on each iteration increases cl and cd and the values written to the history file are larger than expected . At a basic level if I do an analisys of a 2d airfoil or look up in abbot et al the max cl may be in the order of 1.2 . I then process a wing in SU2 expecting +- 70-80% of section cl and yet get values of > 3 or 4 for cl and cd > 1.

If anyone has done a flow over a 3d wing and got meaningful results ie similar to expected in a wind tunnel please post eg cfd file .

Regards
hedley is offline   Reply With Quote

Old   May 20, 2014, 14:08
Default
  #6
Member
 
Payam D.
Join Date: Aug 2011
Posts: 81
Blog Entries: 3
Rep Power: 6
pdp.aero is on a distinguished road
Quote:
Originally Posted by hedley View Post
Still trying to figure out why the solver on each iteration increases cl and cd and the values written to the history file are larger than expected . At a basic level if I do an analisys of a 2d airfoil or look up in abbot et al the max cl may be in the order of 1.2 . I then process a wing in SU2 expecting +- 70-80% of section cl and yet get values of > 3 or 4 for cl and cd > 1.

If anyone has done a flow over a 3d wing and got meaningful results ie similar to expected in a wind tunnel please post eg cfd file .

Regards
Could you please provide more information on your test case, I mean the flow condition, solver setting and etc. It would be more helpful to see your .cfg file to figure out the issue. It will probably cause by the reference values in your .cfg file; it's just a guess though.
pdp.aero is offline   Reply With Quote

Old   May 20, 2014, 14:17
Default here is the .cfg file
  #7
Member
 
Hedley
Join Date: May 2014
Posts: 48
Rep Power: 3
hedley is on a distinguished road
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% %
% Stanford University Unstructured (SU2) configuration file %
% Case description: __________________________________________________ _______ %
% Author: __________________________________________________ _________________ %
% Institution: __________________________________________________ ____________ %
% Date: __________ %
% File Version 1.1.2 October 1st, 2012 %
% %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
% Physical governing equations (EULER, NAVIER_STOKES,
% PLASMA_EULER, PLASMA_NAVIER_STOKES,
% FREE_SURFACE_EULER, FREE_SURFACE_NAVIER_STOKES,
% FLUID_STRUCTURE_EULER, FLUID_STRUCTURE_NAVIER_STOKES,
% AEROACOUSTIC_EULER, AEROACOUSTIC_NAVIER_STOKES,
% WAVE_EQUATION, HEAT_EQUATION, LINEAR_ELASTICITY)
PHYSICAL_PROBLEM= NAVIER_STOKES
%
% Specify turbulence model (NONE, SA, SST)
KIND_TURB_MODEL= SA
%
% Mathematical problem (DIRECT, ADJOINT, LINEARIZED)
MATH_PROBLEM= DIRECT
%
% Restart solution (NO, YES)
RESTART_SOL= NO

% -------------------- COMPRESSIBLE FREE-STREAM DEFINITION --------------------%
%
% Mach number (non-dimensional, based on the free-stream values)
MACH_NUMBER= 0.1147
%
% Angle of attack (degrees, only for compressible flows)
AoA= 3
%
% Side-slip angle (degrees, only for compressible flows)
SIDESLIP_ANGLE= 0.0
%
% Free-stream temperature (273.15 K by default)
FREESTREAM_TEMPERATURE= 273.15
% this is 15 degrees C HEDLEY
%
% Reynolds number (non-dimensional, based on the free-stream values)
REYNOLDS_NUMBER= 3.282E6
%
% Reynolds length (1 m by default)
REYNOLDS_LENGTH= 1

% -------------- COMPRESSIBLE AND INCOMPRESSIBLE FLUID CONSTANTS --------------%
%
% Ratio of specific heats (1.4 (air), only for compressible flows)
GAMMA_VALUE= 1.4
%
% Specific gas constant (287.87 J/kg*K (air), only for compressible flows)
GAS_CONSTANT= 287.87
%
% Laminar Prandtl number (0.72 (air), only for compressible flows)
PRANDTL_LAM= 0.72
%
% Turbulent Prandtl number (0.9 (air), only for compressible flows)
PRANDTL_TURB= 0.9

% ---------------------- REFERENCE VALUE DEFINITION ---------------------------%
%
% Conversion factor for converting the grid to meters
CONVERT_TO_METER= 1
%
% Write a new mesh converted to meters (NO, YES)
WRITE_CONVERTED_MESH = NO
%
% 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
%
% Reference area for force coefficients (0 implies automatic calculation)
REF_AREA= 0
%
% Reference pressure (101325.0 N/m^2 by default, only for compressible flows)
REF_PRESSURE= 1
%
% Reference temperature (273.15 K by default, only for compressible flows)
REF_TEMPERATURE= 1
%
% Reference density (1.2886 Kg/m^3 by default, only for compressible flows)
REF_DENSITY= 1
%
% Reference element length for computing the slope limiter epsilon
REF_ELEM_LENGTH= 0.1

% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Navier-Stokes wall boundary marker(s) (NONE = no marker)
MARKER_HEATFLUX= ( wing, 0.0 )
%
% Far-field boundary marker(s) (NONE = no marker)
MARKER_FAR= ( farfield )
%
% Symmetry boundary marker(s) (NONE = no marker)
MARKER_SYM= ( symmetry )
%was symmetry hedley
% Adiabatic wall boundary condition (YES, NO)
ADIABATIC_WALL= YES
%
% Marker(s) of the surface to be plotted or designed
MARKER_PLOTTING= ( wing )
% was wing hd
% Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated
MARKER_MONITORING= ( wing)

% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
% Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES)
NUM_METHOD_GRAD= GREEN_GAUSS
%
% Courant-Friedrichs-Lewy condition of the finest grid
CFL_NUMBER= .5
%
% CFL ramp (factor, number of iterations, CFL limit)
CFL_RAMP= ( 1.0, 50, 2.0 )
%
% Runge-Kutta alpha coefficients
RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 )
%
% Number of total iterations
EXT_ITER= 100

% ------------------------ LINEAR SOLVER DEFINITION ---------------------------%
%
% Linear solver for the implicit (or discrete adjoint) formulation (BCGSTAB, FGMRES)
LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver (NONE, JACOBI, LINELET)
LINEAR_SOLVER_PREC= LU_SGS
%
% 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
%
% Linear solver history
LINEAR_SOLVER_HIST= NO

% -------------------------- MULTIGRID PARAMETERS -----------------------------%
%
% Multi-Grid Levels (0 = no multi-grid)
MGLEVEL= 0
%
% Multi-Grid Cycle (0 = V cycle, 1 = W Cycle)
MGCYCLE= 0
%
% CFL reduction factor on the coarse levels
MG_CFL_REDUCTION= 0.5
%
% Maximum number of children in the agglomeration stage
MAX_CHILDREN= 50
%
% Maximum length of an agglomerated element (relative to the domain)
MAX_DIMENSION= 0.1
%
% Multigrid pre-smoothing level
MG_PRE_SMOOTH= ( 1, 2, 2, 2 )
%
% Multigrid 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= 0.85
%
% Damping factor for the correction prolongation
MG_DAMP_PROLONGATION= 0.85
%
% Full Multigrid (NO, YES)
FULLMG= NO
%
% Start up iterations using the fine grid
START_UP_ITER= 0

% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
% Convective numerical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, HLLC,
% TURKEL_PREC, MSW)
CONV_NUM_METHOD_FLOW= JST
%was ROE hedley
% 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
%
% Coefficient for the limiter (smooth regions)
LIMITER_COEFF= 0.3
%
% 1st, 2nd and 4th order artificial dissipation coefficients
AD_COEFF_FLOW= ( 0.15, 0.5, 0.02 )
%
% Viscous numerical method (AVG_GRAD, AVG_GRAD_CORRECTED, GALERKIN)
VISC_NUM_METHOD_FLOW= AVG_GRAD_CORRECTED
%
% Source term numerical method (PIECEWISE_CONSTANT)
SOUR_NUM_METHOD_FLOW= PIECEWISE_CONSTANT
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_FLOW= EULER_IMPLICIT

% -------------------- 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
%
% Viscous numerical method (AVG_GRAD, AVG_GRAD_CORRECTED)
VISC_NUM_METHOD_TURB= AVG_GRAD_CORRECTED
%
% Source term numerical method (PIECEWISE_CONSTANT)
SOUR_NUM_METHOD_TURB= PIECEWISE_CONSTANT
%
% Time discretization (EULER_IMPLICIT)
TIME_DISCRE_TURB= EULER_IMPLICIT

% --------------------------- PARTITIONING STRATEGY ---------------------------%
% Write a tecplot/paraview file for each partition (NO, YES)
VISUALIZE_PART= YES

% ----------------------- GEOMETRY EVALUATION PARAMETERS ----------------------%
%
% Geometrical evaluation mode (FUNCTION, GRADIENT)
GEO_MODE= FUNCTION
%
% Marker(s) of the surface where geometrical based func. will be evaluated
GEO_MARKER= ( airfoil )
%
% Number of airfoil sections
GEO_NUMBER_SECTIONS= 5
%
% Orientation of airfoil sections (X_AXIS, Y_AXIS, Z_AXIS)
GEO_ORIENTATION_SECTIONS= Y_AXIS
%
% Location (coordinate) of the airfoil sections (MinValue, MaxValue)
GEO_LOCATION_SECTIONS= (1.5, 3.5)
%
% Plot loads and Cp distributions on each airfoil section
GEO_PLOT_SECTIONS= YES
%
% Number of section cuts to make when calculating internal volume
GEO_VOLUME_SECTIONS= 101

% ------------------------- 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
%
% Use analytical definition for surfaces (NONE, NACA0012_AIRFOIL, BIPARABOLIC,
% NACA4412_AIRFOIL, CYLINDER)
ANALYTICAL_SURFDEF= NONE
%
% Before each computation do an implicit smoothing of the nodes coord (NO, YES)
SMOOTH_GEOMETRY= NO
%
% Adapt the boundary elements (NO, YES)
ADAPT_BOUNDARY= YES

% ------------------------ GRID DEFORMATION PARAMETERS ------------------------%
%
% Kind of deformation (FFD_SETTING, HICKS_HENNE, PARABOLIC, NACA_4DIGITS,
% DISPLACEMENT, ROTATION, FFD_CONTROL_POINT,
% FFD_DIHEDRAL_ANGLE, FFD_TWIST_ANGLE,
% FFD_ROTATION, FFD_CAMBER, FFD_THICKNESS, FFD_VOLUME)
DV_KIND= FFD_SETTING
%
% Marker of the surface in which we are going apply the shape deformation
DV_MARKER= ( airfoil )
%
% Parameters of the shape deformation
% - HICKS_HENNE ( Lower Surface (0)/Upper Surface (1)/Only one Surface (2), x_Loc )
% - NACA_4DIGITS ( 1st digit, 2nd digit, 3rd and 4th digit )
% - PARABOLIC ( Center, Thickness )
% - DISPLACEMENT ( x_Disp, y_Disp, z_Disp )
% - ROTATION ( x_Orig, y_Orig, z_Orig, x_End, y_End, z_End )
% - OBSTACLE ( Center, Bump size )
% - FFD_CONTROL_POINT ( Chunk ID, i_Ind, j_Ind, k_Ind, x_Disp, y_Disp, z_Disp )
% - FFD_DIHEDRAL_ANGLE ( Chunk ID, x_Orig, y_Orig, z_Orig, x_End, y_End, z_End )
% - FFD_TWIST_ANGLE ( Chunk ID, x_Orig, y_Orig, z_Orig, x_End, y_End, z_End )
% - FFD_ROTATION ( Chunk ID, x_Orig, y_Orig, z_Orig, x_End, y_End, z_End )
% - FFD_CAMBER ( Chunk ID, i_Ind, j_Ind )
% - FFD_THICKNESS ( Chunk ID, i_Ind, j_Ind )
% - FFD_VOLUME ( Chunk ID, i_Ind, j_Ind )
DV_PARAM= ( 1, 0.5 )
%
% New value of the shape deformation
DV_VALUE= 0.01
%
% Grid deformation technique (SPRING, FEA)
GRID_DEFORM_METHOD= SPRING
%
% Hold the grid fixed in a region (NO, YES)
HOLD_GRID_FIXED= NO
%
% Coordinates of the box where the grid will be deformed (Xmin, Ymin, Zmin,
% Xmax, Ymax, Zmax)
HOLD_GRID_FIXED_COORD= ( -0.5, -0.49, 0.0, 2.5, 0.49, 0.0 )
%
% Visualize the deformation (NO, YES)
VISUALIZE_DEFORMATION= NO

% --------------------------- CONVERGENCE PARAMETERS --------------------------%
%
% Convergence criteria (CAUCHY, RESIDUAL)
%
CONV_CRITERIA= RESIDUAL
%
% 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= -8
%
% 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= 1E-10
%
% Function to apply the criteria (LIFT, DRAG, NEARFIELD_PRESS, SENS_GEOMETRY,
% SENS_MACH, DELTA_LIFT, DELTA_DRAG)
CAUCHY_FUNC_FLOW= DRAG
CAUCHY_FUNC_ADJFLOW= SENS_GEOMETRY
CAUCHY_FUNC_LIN= DELTA_DRAG
%
% Epsilon for full multigrid method evaluation
FULLMG_CAUCHY_EPS= 1E-4

% ------------------------- INPUT/OUTPUT INFORMATION --------------------------%
%
% Mesh input file
MESH_FILENAME= wingscaled.su2
% was wing.su2 HEDLEY
% Mesh input file format (SU2, CGNS, NETCDF_ASCII)
MESH_FORMAT= SU2
%
% Divide rectangles into triangles (NO, YES)
DIVIDE_ELEMENTS= NO
%
% Convert a CGNS mesh to SU2 format (YES, NO)
CGNS_TO_SU2= NO
%
% Mesh output file
MESH_OUT_FILENAME= mesh_out.su2
%
% Restart flow input file
SOLUTION_FLOW_FILENAME= solution_flow.dat
%
% Restart linear flow input file
SOLUTION_LIN_FILENAME= solution_lin.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 linear solver history (w/o extension)
LIN_CONV_FILENAME= lin_history
%
% Output file restart flow
RESTART_FLOW_FILENAME= restart_flow.dat
%
% Output file restart adjoint
RESTART_ADJ_FILENAME= restart_adj.dat
%
% Output file linear flow
RESTART_LIN_FILENAME= restart_lin.dat
%
% Output file flow (w/o extension) variables
VOLUME_FLOW_FILENAME= flow
%
% Output file adjoint (w/o extension) variables
VOLUME_ADJ_FILENAME= adjoint
%
% Output file linearized (w/o extension) variables
VOLUME_LIN_FILENAME= linearized
%
% 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
%
% Output file surface linear coefficient (w/o extension)
SURFACE_LIN_FILENAME= surface_linear
%
% Writing solution file frequency
WRT_SOL_FREQ= 100
%
% Writing convergence history frequency
WRT_CON_FREQ= 1
%
% Writing linear solver history frequency
WRT_LIN_CON_FREQ= 1
%
% Write unsteady data adding headers and prefixes (NO, YES)
WRT_UNSTEADY= NO
%
% Write mass averaged solution file (plasma solver only, NO by default)
WRT_MASS_AVG_FLOW= NO

% --------------------- OPTIMAL SHAPE DESIGN DEFINITION -----------------------%
%
% Objective function (DRAG, LIFT, SIDEFORCE, MOMENT_X, MOMENT_Y,
% MOMENT_Z, EFFICIENCY, EQUIVALENT_AREA, NEARFIELD_PRESSURE,
% FORCE_X, FORCE_Y, FORCE_Z, THRUST, TORQUE, FREESURFACE)
OBJFUNC= DRAG
%
% Scale objective function.
OBJFUNC_SCALE= 0.001
%
% Inequality constraints list separated by comma (DRAG, LIFT, SIDEFORCE,
% MOMENT_X, MOMENT_Y, MOMENT_Z, EFFICIENCY, EQUIVALENT_AREA,
% NEARFIELD_PRESSURE, FORCE_X, FORCE_Y, FORCE_Z, THRUST, TORQUE,
% FREESURFACE)
CONST_IEQ= LIFT, MOMENT_Z
%
% Scale inequality constraints (separated by comma)
CONST_IEQ_SCALE= 0.001, 0.001
%
% Min value inequality constraints list (NONE, LESS, GREATER)
CONST_IEQ_SIGN= GREATER, GREATER
%
% Max value inequality constraints list (separated by comma)
CONST_IEQ_VALUE= 0.328188, 0.034068
%
% Equality constraints list separated by comma (DRAG, LIFT, SIDEFORCE, MOMENT_X, MOMENT_Y,
% MOMENT_Z, EFFICIENCY, EQUIVALENT_AREA, NEARFIELD_PRESSURE,
% FORCE_X, FORCE_Y, FORCE_Z, THRUST, TORQUE, FREESURFACE)
CONST_EQ= NONE
%
% Scale equality constraints (separated by comma)
CONST_EQ_SCALE= 0.0
%
% Value equality constraints list (separated by comma)
CONST_EQ_VALUE= 0.0
%
% List of design variables (Design variables are separated by semicolons)
% From 1 to 99, Geometrycal design variables.
% - HICKS_HENNE ( 1, Scale | Mark. List | Lower(0)/Upper(1) side, x_Loc )
% - NACA_4DIGITS ( 4, Scale | Mark. List | 1st digit, 2nd digit, 3rd and 4th digit )
% - DISPLACEMENT ( 5, Scale | Mark. List | x_Disp, y_Disp, z_Disp )
% - ROTATION ( 6, Scale | Mark. List | x_Axis, y_Axis, z_Axis, x_Turn, y_Turn, z_Turn )
% - FFD_CONTROL_POINT ( 7, Scale | Mark. List | Chunk, i_Ind, j_Ind, k_Ind, x_Mov, y_Mov, z_Mov )
% - FFD_DIHEDRAL_ANGLE ( 8, Scale | Mark. List | Chunk, x_Orig, y_Orig, z_Orig, x_End, y_End, z_End )
% - FFD_TWIST_ANGLE ( 9, Scale | Mark. List | Chunk, x_Orig, y_Orig, z_Orig, x_End, y_End, z_End )
% - FFD_ROTATION ( 10, Scale | Mark. List | Chunk, x_Orig, y_Orig, z_Orig, x_End, y_End, z_End )
% - FFD_CAMBER ( 11, Scale | Mark. List | Chunk, i_Ind, j_Ind )
% - FFD_THICKNESS ( 12, Scale | Mark. List | Chunk, i_Ind, j_Ind )
% - FFD_VOLUME ( 13, Scale | Mark. List | Chunk, i_Ind, j_Ind )
% From 100 to 199, Flow solver design variables.
% - MACH_NUMBER ( 101, Scale | Markers List )
% - AOA ( 102, Scale | Markers List )
DEFINITION_DV= ( 1, 0.001 | airfoil | 0, 0.1 ); ( 1, 0.001 | airfoil | 0, 0.2 )
hedley is offline   Reply With Quote

Old   May 20, 2014, 14:45
Default and here is some output with Cl and Cd increasing each loop
  #8
Member
 
Hedley
Join Date: May 2014
Posts: 48
Rep Power: 3
hedley is on a distinguished road
Initialize jacobian structure (Navier-Stokes). MG level: 0.
Initialize jacobian structure (SA model).

----------------- Integration and Numerics Preprocessing ----------------
Integration Preprocessing.
Numerics Preprocessing.

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

Maximum residual: 1.89096, located at point 1648.

Iter Time(s) Res[Rho] Res[nu] CLift(Total) CDrag(Total)
0 25.741053 0.323718 -4.513804 0.839490 0.345001
1 24.044417 0.187468 -4.448524 1.183776 0.487726
2 21.945658 0.126626 -4.477596 1.464226 0.607455
3 21.030338 0.076769 -4.502995 1.693231 0.705232
4 20.238298 0.043514 -4.522412 1.876937 0.785252
5 20.570025 0.016620 -4.534918 2.026783 0.852054
6 20.145987 -0.005051 -4.541085 2.147346 0.907573
7 19.977807 -0.021602 -4.542675 2.242479 0.953327
8 19.858203 -0.034791 -4.541540 2.316662 0.990674
9 20.289774 -0.046206 -4.539163 2.374541 1.021008
hedley is offline   Reply With Quote

Old   May 20, 2014, 14:48
Default
  #9
Member
 
Payam D.
Join Date: Aug 2011
Posts: 81
Blog Entries: 3
Rep Power: 6
pdp.aero is on a distinguished road
In what dimension the grid and geometry is created? Inch or m?
Further, your geometry is a wing, right? what is the root and tip chord length?
Besides, what is the MAC (Mean Aerodynamic Chord) length?
pdp.aero is offline   Reply With Quote

Old   May 20, 2014, 14:53
Default sizing
  #10
Member
 
Hedley
Join Date: May 2014
Posts: 48
Rep Power: 3
hedley is on a distinguished road
The wing is in meters - chord 1.6 meters - tip chord 800mm - half span 3.5 meters . The root airfoil is NACA 64212.5 and tip NACA 64210 .

The grid and volume were created in pointwise which used inches and then after reading previous post I converted down to meters in pointwise by scaling by 0.0254

regards
hedley is offline   Reply With Quote

Old   May 20, 2014, 14:58
Default images attached
  #11
Member
 
Hedley
Join Date: May 2014
Posts: 48
Rep Power: 3
hedley is on a distinguished road
MAC is +- 400mm
Attached Images
File Type: jpg wingmesh11.jpg (61.7 KB, 22 views)
File Type: jpg wingflowfield11.jpg (83.2 KB, 21 views)
hedley is offline   Reply With Quote

Old   May 20, 2014, 16:46
Default
  #12
Member
 
Payam D.
Join Date: Aug 2011
Posts: 81
Blog Entries: 3
Rep Power: 6
pdp.aero is on a distinguished road
Okay, thank you for providing extra information.
The main point is, your Mach number is below the 0.3, so the flow is incompressible. However, you have created a compressible domain which includes hemisphere farfield, symmetric plane and the wall. Typically, for the incompressible external flow we are defining an inlet, outlet with a cylinder-like or rectangular-like domain. Nevertheless, by solving the compressible flow with the incompressible flow condition or initial condition, the results will be obtained same as using the incompressible solver. For this purpose, you need to set your config file for solving the compressible flow, albeit with incompressible flow condition.

Therefore, from the aforementioned points, I have changed some part of your Config file which is stated as follow:

First, your REFERENCE VALUE DEFINITION should be changed for the compressible flow.
Code:
% Reference pressure (101325.0 N/m^2 by default, only for compressible flows)
REF_PRESSURE= 101325.0
%
% Reference temperature (273.15 K by default, only for compressible flows)
REF_TEMPERATURE= 273.15
%
% Reference density (1.2886 Kg/m^3 by default, only for compressible flows)
REF_DENSITY= 1.292319138159549
Second, your Reynolds number should be calculated based on your geometry and the flow condition. The Reynolds length is the MAC. Using the ideal gas formula and sea level condition, we will have this:
MAC calculation for trapezoid wing:
Code:
((2/3)*Croot*(1+taper+(taper)^2))/(1+taper)
Code:
M=0.1147
T=273.15
R=8314.4621
Rs=286.959
MAC=1.1022
ro=(101325)/((R/28.966)*T)
mo=1.79*10e-05
Re=ro*(M*((gama*Rs*T)^0.5))*MAC/mo
So, in the code,

Code:
%COMPRESSIBLE FREE-STREAM DEFINITION
% Reynolds number (non-dimensional, based on the free-stream values)
REYNOLDS_NUMBER= 3.023535797839057E5
%
% Reynolds length (1 m by default)
REYNOLDS_LENGTH= 1.1022

%REFERENCE VALUE DEFINITION
% Reference origin for moment computation
REF_ORIGIN_MOMENT_X = 0.77335
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= 1.1022
The reference origin for moment computation has been set by assuming that the XYZ axes' origin is located at the front point of the root.

Third, in this case, you need more than 100 iterations for obtaining suitable convergence, so I changed the max iteration number.
Code:
% Number of total iterations
EXT_ITER= 100000
Fourth, using convergence acceleration method will help you to reduce the run time, particularly in this case that your using the RANS equations. The AMG setting for the Config file:
Code:
% Multi-Grid Levels (0 = no multi-grid)
MGLEVEL= 2
%
% Multi-Grid Cycle (0 = V cycle, 1 = W Cycle)
MGCYCLE= 1
%
% CFL reduction factor on the coarse levels
MG_CFL_REDUCTION= 0.75

% Multigrid pre-smoothing level
MG_PRE_SMOOTH= ( 1, 2, 3, 3 )
Fifth, you are iterating the RANS equations, so 2nd-order spatial integration for the turbulence model will be helpful in order to obtain accurate results.
Code:
% Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER)
%
SPATIAL_ORDER_TURB= 2ND_ORDER
Sixth, I had noted that you are using the Pointwise for the grid generation. However, you created an unstructured block around the wing, probably without using the T-Rex for creating high anisotropic tetrahedral cell at your boundary layer for capturing the viscous separation drag. This suggestion is optional. You could create structured surface mesh around the wing, then go to the create --> extrude ---> normal, select all the surface mesh on the wing and extrude them outward to create high orthogonal structured boundary layer block. Lastly, you could create an unstructured block for the remaining part of the domain like what you did for the unstructured block creation shown in your picture.
In this way, you will create a Hybrid grid, which definitely improves your results. Then, you could use the SST turbulence model in your Config file, which gives better results in comparison with the SA model.

Note: The modified Config file by me has been attached, however I couldn't find time to check it with my laptop. In case it didn't work, please let me know.
Besides, it didn't let me to attach ".cfg" file, after downloading the file, change the extension to the ".cfg"

Good Luck,
PDP
Attached Files
File Type: txt wing_comp.txt (15.8 KB, 12 views)
hedley likes this.

Last edited by pdp.aero; May 20, 2014 at 19:04. Reason: attachment
pdp.aero is offline   Reply With Quote

Old   May 20, 2014, 18:57
Default
  #13
Member
 
Payam D.
Join Date: Aug 2011
Posts: 81
Blog Entries: 3
Rep Power: 6
pdp.aero is on a distinguished road
The attachment is provided in the previous message.
pdp.aero is offline   Reply With Quote

Old   May 20, 2014, 22:15
Default
  #14
Member
 
Hedley
Join Date: May 2014
Posts: 48
Rep Power: 3
hedley is on a distinguished road
Dear pdp.aero

Thank you for a comprehensive and very well explained and informative reply . It is 4am in South Africa so I will start up the computer and try out when spousal unit awakens to avoid domestic violence - much appreciated . Hedley

Last edited by hedley; May 20, 2014 at 22:24. Reason: Wrong name spelling
hedley is offline   Reply With Quote

Old   May 21, 2014, 01:13
Default try of new cfg file
  #15
Member
 
Hedley
Join Date: May 2014
Posts: 48
Rep Power: 3
hedley is on a distinguished road
All goes well and then Killed ?


------------------- Config file boundary information --------------------
Far-field boundary marker(s): farfield.
Symmetry plane boundary marker(s): symmetry.
Constant heat flux wall boundary marker(s): wing.

---------------- Flow & Non-dimensionalization information ---------------
Viscous flow: Computing pressure using the ideal gas law
based on the freestream temperature and a density computed
from the Reynolds number.
--Input conditions:
Ratio of specific heats: 1.4
Specific gas constant (J/(kg.K)): 287.87
Freestream pressure (N/m^2): 9763.69
Freestream temperature (K): 273.15
Freestream density (kg/m^3): 0.12417
Freestream velocity (m/s): (38.0041,0,1.99171)
Freestream velocity magnitude (m/s): 38.0563
Freestream energy (kg.m/s^2): 197303
Freestream viscosity (N.s/m^2): 1.72261e-05
--Reference values:
Reference pressure (N/m^2): 101325
Reference temperature (K): 273.15
Reference energy (kg.m/s^2): 78405.6
Reference density (kg/m^3): 1.29232
Reference velocity (m/s): 280.01
Reference viscosity (N.s/m^2): 361.862
--Resulting non-dimensional state:
Mach number (non-dimensional): 0.1147
Reynolds number (non-dimensional): 302354
Reynolds length (m): 1.1022
Specific gas constant (non-dimensional): 287.87
Freestream temperature (non-dimensional): 1
Freestream pressure (non-dimensional): 0.0963602
Freestream density (non-dimensional): 0.0960831
Freestream velocity (non-dimensional): (0.135724,0,0.007113)
Freestream velocity magnitude (non-dimensional): 0.13591
Free-stream turb. kinetic energy (non-dimensional): 6.92687e-05
Free-stream specific dissipation (non-dimensional): 13.981
Freestream energy (non-dimensional): 2.51645
Freestream viscosity (non-dimensional): 4.76042e-08
Force coefficients computed using freestream values.
Note: Negative pressure, temperature or density is not allowed!

---------------------- Read grid file information -----------------------
Three dimensional problem.
2819141 interior elements.
2819141 tetrahedra.
485190 points.
3 surface markers.
18306 boundary elements in index 0 (Marker = farfield).
20743 boundary elements in index 1 (Marker = symmetry).
27467 boundary elements in index 2 (Marker = wing).

------------------------- Geometry Preprocessing ------------------------
Setting local point and element connectivity.
Checking the numerical grid orientation.
Identifying edges and vertices.
Computing centers of gravity.
Setting the control volume structure.
Volume of the computational grid: 7.41088e+06.
Searching for the closest normal neighbors to the surfaces.
Compute the surface curvature.
Max K: 90362.6. Mean K: 324.818. Standard deviation K: 3003.99.
Setting the multigrid structure.
CVs of the MG level: 82163. Agglom. rate 1/5.90521. MG level: 1.
CVs of the MG level: 12560. Agglom. rate 1/6.54164. MG level: 2.

------------------------- Solver Preprocessing --------------------------
Computing wall distances.
Area projection in the z-plane = 4.02345.
Initialize jacobian structure (Navier-Stokes). MG level: 0.
Initialize jacobian structure (SA model).
Initialize jacobian structure (Navier-Stokes). MG level: 1.
Killed
hedley is offline   Reply With Quote

Old   May 21, 2014, 03:02
Default test run
  #16
Member
 
Hedley
Join Date: May 2014
Posts: 48
Rep Power: 3
hedley is on a distinguished road
1. Ok the only way I can stop it crashing is to set MGLEVEL=0
2. I thought taper ratio was tip chord / root chord
3. I fixed the one typo changing 2st to 2ND.

Ran the suggested .cfg file which crashes with multi grid and runs with multigrid set to 0 BUT then back to where I started with CLift and Cdrag increasing on each iteration .

There seem to be many input variables and I am sure that there are dependencies between them so unlike my airplane with has a few control inputs SU2 is like a black box with many many knobs that one tweeks without any real idea of how this will affect the solver.

If anyone has ever run a .cfg file on a 3d wing section at anywhere between 60KTS and 175KTS and got outputs for Clift and CDrag that make sense please assist.

Regards
Hedley
hedley is offline   Reply With Quote

Old   May 21, 2014, 03:31
Default
  #17
Member
 
Payam D.
Join Date: Aug 2011
Posts: 81
Blog Entries: 3
Rep Power: 6
pdp.aero is on a distinguished road
Please, turn off the AMG solver.

Code:
% Multi-Grid Levels (0 = no multi-grid)
MGLEVEL= 0
%
% Multi-Grid Cycle (0 = V cycle, 1 = W Cycle)
MGCYCLE= 0
What is your SU2 version?

Okay, after I posted this, I have seen your last post. Yes, I have noticed that using AMG solver with parallel RANS equations is not compatible, and they didn't use them for their tutorial test cases.

You are right, taper ratio is Ctip/Croot, typically it is somewhere between 0.2 to 0.3 for general aviation.
Your wing is similar to the ONERA M6 geometry, one of the SU2's tutorial, but your Mach number is pretty small, and your Reynolds number indicates the Laminar flow (e.g. below the 5e+05).
Therefore, my suggestion is change your Mach number to 0.83 and calculate the Reynolds number, then run the code. In this way you are running test case similar to the tutorial 7, turbulent ONERA M6. I already run this tutorial, and I got the convergence. Continuing this, if you got the convergence, it means you need to change your solver into the incompressible. For checking the convergence, after your iteration finished, plot the residual and see they are going down or not. If they come down 4 order of magnitude, you are obtaining the convergence hopefully. After this, when you concluded that you got the convergence with 0.83 Mach, you need to change into incompressible solver. For this purpose, create a rectangular-like unstructured block around your wing. Consequently, define velocity inlet at the entry, pressure outlet at the outlet, wall or pressure outlet for the surrounding domain and the symmetric boundary condition. For setting your configuration, please refer to the tutorial 3, laminar flat plat, in order to get more information on implementing laminar N-S equations for your case. Run the code on your new configuration.

Sorry if couldn't help you any more.

Good Luck,
Payam

Last edited by pdp.aero; May 21, 2014 at 04:21. Reason: Updating
pdp.aero is offline   Reply With Quote

Old   May 21, 2014, 11:26
Default final attempt
  #18
Member
 
Hedley
Join Date: May 2014
Posts: 48
Rep Power: 3
hedley is on a distinguished road
Thank you for the time spent on this

1. I turned off AMG
2. Am running Latest version see below 3.1.0 Eagle
3. Still comes up with strange values.

I will put this to one side and realize that CFD is not for the faint hearted -

regards and thanks again .

------------------------------------------------------------------------
| _____ _ _ ___ |
| / ____| | | | | |__ \ Web: su2.stanford.edu |
| | (___ | | | | ) | Twitter: @su2code |
| \___ \ | | | | / / Forum: www.cfd-online.com/Forums/su2/ |
| ____) | | |__| | / /_ |
| |_____/ \____/ |____| Suite (Computational Fluid Dynamic Code) |
| Release 3.1.0 "eagle" |
-------------------------------------------------------------------------
| SU2, Copyright (C) 2012-2014 Aerospace Design Laboratory (ADL). |
| SU2 is distributed in the hope that it will be useful, |
| but WITHOUT ANY WARRANTY; without even the implied warranty of |
| MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU |
| Lesser General Public License (version 2.1) for more details. |
-------------------------------------------------------------------------

------------------------ Physical case definition -----------------------
Compressible RANS equations.
Turbulence model: Spalart Allmaras
Mach number: 0.1147.
Angle of attack (AoA): 3 deg, and angle of sideslip (AoS): 0 deg.
Reynolds number: 302354.
No restart solution, use the values at infinity (freestream).
The reference length/area will be computed using y(2D) or z(3D) projection.
The reference length (moment computation) is 1.2444.
Reference origin (moment computation) is (0.77335, 0, 0).
Surface(s) where the force coefficients are evaluated: wing.
Surface(s) plotted in the output file: wing.
Surface(s) affected by the design variables: airfoil.
Input mesh file name: smallwing.su2

---------------------- Space numerical integration ----------------------
Roe solver for the flow inviscid terms.
Second order integration with slope limiter.
Venkatakrishnan slope-limiting method, with constant: 0.3.
The reference element size is: 0.1.
Scalar upwind solver (first order) for the turbulence model.
Second order integration.
Average of gradients with correction (viscous flow terms).
Piecewise constant integration of the flow source terms.
Average of gradients with correction (viscous turbulence terms).
Piecewise constant integration of the turbulence model source terms.
Gradient computation using Green-Gauss theorem.

---------------------- Time numerical integration -----------------------
Local time stepping (steady state simulation).
Euler implicit method for the flow equations.
FGMRES is used for solving the linear system.
Convergence criteria of the linear solver: 1e-06.
Max number of iterations: 20.
Relaxation coefficient: 1.
No CFL ramp.
Courant-Friedrichs-Lewy number: 0.75
Euler implicit time integration for the turbulence model.

------------------------- Convergence criteria --------------------------
Maximum number of iterations: 100.
Reduce the density residual 5 orders of magnitude.
The minimum bound for the density residual is 10^(-8).
Start convergence criteria at iteration 10.

-------------------------- Output information ---------------------------
Writing a flow solution every 100 iterations.
Writing the convergence history every 1 iterations.
The output file format is Paraview ASCII (.vtk).
Convergence history file name: history.
Surface flow coefficients file name: surface_flow.
Flow variables file name: flow.
Restart flow file name: restart_flow.dat.

------------------- Config file boundary information --------------------
Far-field boundary marker(s): farfield.
Symmetry plane boundary marker(s): symmetry.
Constant heat flux wall boundary marker(s): wing.

---------------- Flow & Non-dimensionalization information ---------------
Viscous flow: Computing pressure using the ideal gas law
based on the freestream temperature and a density computed
from the Reynolds number.
--Input conditions:
Ratio of specific heats: 1.4
Specific gas constant (J/(kg.K)): 287.87
Freestream pressure (N/m^2): 8647.98
Freestream temperature (K): 273.15
Freestream density (kg/m^3): 0.109981
Freestream velocity (m/s): (38.0041,0,1.99171)
Freestream velocity magnitude (m/s): 38.0563
Freestream energy (kg.m/s^2): 197303
Freestream viscosity (N.s/m^2): 1.72261e-05
--Reference values:
Reference pressure (N/m^2): 101325
Reference temperature (K): 273.15
Reference energy (kg.m/s^2): 78405.6
Reference density (kg/m^3): 1.29232
Reference velocity (m/s): 280.01
Reference viscosity (N.s/m^2): 361.862
--Resulting non-dimensional state:
Mach number (non-dimensional): 0.1147
Reynolds number (non-dimensional): 302354
Reynolds length (m): 1.2444
Specific gas constant (non-dimensional): 287.87
Freestream temperature (non-dimensional): 1
Freestream pressure (non-dimensional): 0.0853489
Freestream density (non-dimensional): 0.0851035
Freestream velocity (non-dimensional): (0.135724,0,0.007113)
Freestream velocity magnitude (non-dimensional): 0.13591
Free-stream turb. kinetic energy (non-dimensional): 6.92687e-05
Free-stream specific dissipation (non-dimensional): 12.3834
Freestream energy (non-dimensional): 2.51645
Freestream viscosity (non-dimensional): 4.76042e-08
Force coefficients computed using freestream values.
Note: Negative pressure, temperature or density is not allowed!

---------------------- Read grid file information -----------------------
Three dimensional problem.
1573830 interior elements.
946959 tetrahedra.
618440 prisms.
8431 pyramids.
485190 points.
3 surface markers.
18306 boundary elements in index 0 (Marker = farfield).
17850 boundary elements in index 1 (Marker = symmetry).
27467 boundary elements in index 2 (Marker = wing).

------------------------- Geometry Preprocessing ------------------------
Setting local point and element connectivity.
Checking the numerical grid orientation.
Identifying edges and vertices.
Computing centers of gravity.
Setting the control volume structure.
Volume of the computational grid: 7.41088e+06.
Searching for the closest normal neighbors to the surfaces.
Compute the surface curvature.
Max K: 90362.6. Mean K: 345.171. Standard deviation K: 3074.93.

------------------------- Solver Preprocessing --------------------------
Computing wall distances.
Area projection in the z-plane = 4.02345.
Initialize jacobian structure (Navier-Stokes). MG level: 0.
Initialize jacobian structure (SA model).

----------------- Integration and Numerics Preprocessing ----------------
Integration Preprocessing.
Numerics Preprocessing.

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

Maximum residual: -4.9885, located at point 1648.

Iter Time(s) Res[Rho] Res[nu] CLift(Total) CDrag(Total)
0 20.581689 -6.555742 -10.821365 0.840691 0.411578
1 18.891452 -6.682332 -10.750260 1.252222 0.573674
2 19.230903 -6.742428 -10.774174 1.593348 0.706413
hedley is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
SU2 runtime error: cannot find value of GMRES in given map bruzerravi SU2 1 May 1, 2013 07:11
[BEGINNER] Problems running tutorials (incompressible) in OF 2.xx Jaro OpenFOAM Running, Solving & CFD 7 December 4, 2012 21:12
C runtime library internal header file Error gholamghar Fluent UDF and Scheme Programming 1 October 18, 2011 10:38
OpenFOAM 1.7.1 installation problem on OpenSUSE 11.3 flakid OpenFOAM Installation 16 December 28, 2010 09:48
fortran runtime error while calculating Anna (aka new-user) CD-adapco 2 December 2, 2004 12:35


All times are GMT -4. The time now is 14:20.