[t.teschner]

I'm test driving SU2 at the moment to evaluate if I can use it for a few projects that I have lined up (after many years of frustration with OpenFOAM) and thus far I am rather pleased with SU2. The schemes and algorithms that are implemented are working rather well, not something I a used to from OpenFOAM (let's not go there ...).

The compressible setup seems straight forward and I can achieve what I want. I also wanted to evaluate the incompressible solver characteristics, and thus set up a simple NACA 0012 example for the classical NASA validation test case at Re=6E6 and Ma=0.15. I get good results for that with the RANS solver, but for INC_RANS, I seem to always get a magnitude of 1 at the velocity inlet, despite specifying a velocity inlet boundary condition with a non-zero value.

I have tried now a few things, and probably I am just missing something here (I have also checked my setup against the available tutorial case), but my velocity vector always has a magnitude of 1 at the inlet.

Here is my input:

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
SOLVER= INC_RANS
% Specify turbulence model (NONE, SA, SST)
KIND_TURB_MODEL= SST
%
MATH_PROBLEM= DIRECT
%
% Restart solution (NO, YES)
RESTART_SOL= NO
%
SYSTEM_MEASUREMENTS= SI
%
% ------------------------------- SOLVER CONTROL ------------------------------%
%
% Number of iterations for single-zone problems
ITER= 1
%
% Maximum number of inner iterations
INNER_ITER= 500
%
% Convergence field
CONV_FIELD= DRAG
%
% Min value of the residual (log10 of the residual)
CONV_RESIDUAL_MINVAL= -8
%
% Number of elements to apply the criteria
CONV_CAUCHY_ELEMS= 40
%
% Epsilon to control the series convergence
CONV_CAUCHY_EPS= 1E-4
%
% ---------------- INCOMPRESSIBLE FLOW CONDITION DEFINITION -------------------%
%
% Density model within the incompressible flow solver.
% Options are CONSTANT (default), BOUSSINESQ, VARIABLE, or FLAMELET. If VARIABLE,
% an appropriate fluid model must be selected. For FLAMELET, the density is
% retrieved directly from the flamelet manifold.
INC_DENSITY_MODEL= CONSTANT
%
% Solve the energy equation in the incompressible flow solver
INC_ENERGY_EQUATION = NO
%
% Initial density for incompressible flows
% (1.2886 kg/m^3 by default (air), 998.2 Kg/m^3 (water))
INC_DENSITY_INIT= 1.2886
%
% Initial velocity for incompressible flows (1.0,0,0 m/s by default)
INC_VELOCITY_INIT= ( 84.96890112 , 14.98230979 , 0.00 )
%
% Non-dimensionalization scheme for incompressible flows. Options are
% INITIAL_VALUES (default), REFERENCE_VALUES, or DIMENSIONAL.
% INC_*_REF values are ignored unless REFERENCE_VALUES is chosen.
INC_NONDIM= INITIAL_VALUES
%
% List of inlet types for incompressible flows. List length must
% match number of inlet markers. Options: VELOCITY_INLET, PRESSURE_INLET.
INC_INLET_TYPE= VELOCITY_INLET
%
% List of outlet types for incompressible flows. List length must
% match number of outlet markers. Options: PRESSURE_OUTLET, MASS_FLOW_OUTLET
INC_OUTLET_TYPE= PRESSURE_OUTLET
%
% ---------------------- REFERENCE VALUE DEFINITION ---------------------------%
%
% Reference origin for moment computation (m or in)
REF_ORIGIN_MOMENT_X = 0.25
REF_ORIGIN_MOMENT_Y = 0.00
REF_ORIGIN_MOMENT_Z = 0.00
%
% Reference length for moment non-dimensional coefficients (m or in)
REF_LENGTH= 1.0
%
% Reference velocity (incompressible only)
REF_VELOCITY= 8.63E1
%
% Reference viscosity (incompressible only)
REF_VISCOSITY= 1.853E-5
%
% Reference area for non-dimensional force coefficients (0 implies automatic
% calculation) (m^2 or in^2)
REF_AREA= 1.0
%
% --------------------------- VISCOSITY MODEL ---------------------------------%
%
% Viscosity model (SUTHERLAND, CONSTANT_VISCOSITY, POLYNOMIAL_VISCOSITY, FLAMELET).
VISCOSITY_MODEL= CONSTANT_VISCOSITY
%
% Molecular Viscosity that would be constant (1.716E-5 by default)
MU_CONSTANT= 1.853E-5
%
% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Navier-Stokes (no-slip), isothermal wall marker(s) (NONE = no marker)
% Format: ( marker name, constant wall temperature (K), ... )
MARKER_ISOTHERMAL= ( upper, 288.15, lower, 288.15, te, 288.15 )
%
% Inlet boundary type (TOTAL_CONDITIONS, MASS_FLOW)
INLET_TYPE= TOTAL_CONDITIONS
%
% Inlet boundary marker(s) with the following formats (NONE = no marker)
% Total Conditions: (inlet marker, total temp, total pressure, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
% Mass Flow: (inlet marker, density, velocity magnitude, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
% Inc. Velocity: (inlet marker, temperature, velocity magnitude, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
% Inc. Pressure: (inlet marker, temperature, total pressure, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
MARKER_INLET= ( inlet, 0.0, 86.28, 0.984807753, 0.173648178, 0.0 )
MARKER_INLET_TURBULENT= ( inlet, 0.00052, 10.0 )
%
% Outlet boundary marker(s) (NONE = no marker)
% Compressible: ( outlet marker, back pressure (static thermodynamic), ... )
% Inc. Pressure: ( outlet marker, back pressure (static gauge in Pa), ... )
% Inc. Mass Flow: ( outlet marker, mass flow target (kg/s), ... )
MARKER_OUTLET= ( outlet, 0.0 )
%
% ------------------------ SURFACES IDENTIFICATION ----------------------------%
%
% Marker(s) of the surface in the surface flow solution file
MARKER_PLOTTING = ( upper, lower, te )
%
% Marker(s) of the surface where the non-dimensional coefficients are evaluated.
MARKER_MONITORING = ( upper, lower, te )
%
% Viscous wall markers for which wall functions must be applied. (NONE = no marker)
% Format: ( marker name, wall function type -NO_WALL_FUNCTION, STANDARD_WALL_FUNCTION,
%           ADAPTIVE_WALL_FUNCTION, SCALABLE_WALL_FUNCTION, EQUILIBRIUM_WALL_MODEL,
%           NONEQUILIBRIUM_WALL_MODEL-, ... )
MARKER_WALL_FUNCTIONS= ( upper, NO_WALL_FUNCTION, lower, NO_WALL_FUNCTION, te, NO_WALL_FUNCTION )
%
% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
% Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES)
NUM_METHOD_GRAD= WEIGHTED_LEAST_SQUARES
%
% Numerical method for spatial gradients to be used for MUSCL reconstruction
% Options are (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES, LEAST_SQUARES). Default value is
% NONE and the method specified in NUM_METHOD_GRAD is used.
NUM_METHOD_GRAD_RECON = WEIGHTED_LEAST_SQUARES
%
% CFL number (initial value for the adaptive CFL number)
CFL_NUMBER= 10.0
%
% Adaptive CFL number (NO, YES)
CFL_ADAPT= YES
%
% Parameters of the adaptive CFL number (factor-down, factor-up, CFL min value,
%                                        CFL max value, acceptable linear solver convergence)
% Local CFL increases by factor-up until max if the solution rate of change is not limited,
% and acceptable linear convergence is achieved. It is reduced if rate is limited, or if there
% is not enough linear convergence, or if the nonlinear residuals are stagnant and oscillatory.
% It is reset back to min when linear solvers diverge, or if nonlinear residuals increase too much.
CFL_ADAPT_PARAM= ( 0.1, 2.0, 10.0, 1e10, 0.1 )
%
% Maximum Delta Time in local time stepping simulations
MAX_DELTA_TIME= 1E6
%
% External iteration offset due to restart
EXT_ITER_OFFSET= 0
%
% Runge-Kutta alpha coefficients
RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 )
%
% ----------- SLOPE LIMITER AND DISSIPATION SENSOR DEFINITION -----------------%
%
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the flow equations.
%           Required for 2nd order upwind schemes (NO, YES)
MUSCL_FLOW= NO
%
% Slope limiter (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG, BARTH_JESPERSEN, VAN_ALBADA_EDGE,
%                NISHIKAWA_R3, NISHIKAWA_R4, NISHIKAWA_R5)
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN
%
% Same as MUSCL_FLOW but for turbulence.
%
MUSCL_TURB= NO
%
% Slope limiter (same as SLOPE_LIMITER_FLOW except VAN_ALBADA_EDGE)
%
SLOPE_LIMITER_TURB= VENKATAKRISHNAN
%
% Same as MUSCL_FLOW but for the continuous adjoint equations.
%
MUSCL_ADJFLOW= YES
%
% Slope limiter (same as SLOPE_LIMITER_FLOW plus SHARP_EDGES, WALL_DISTANCE)
%
SLOPE_LIMITER_ADJFLOW= VENKATAKRISHNAN
%
% Same as MUSCL_FLOW but for continuous adjoint turbulence equations.
%
MUSCL_ADJTURB= NO
%
% Slope limiter (see SLOPE_LIMITER_ADJFLOW)
%
SLOPE_LIMITER_ADJTURB= VENKATAKRISHNAN
%
% Coefficient for Venkatakrishnan-type limiters (upwind scheme).
% A larger value decreases the extent of limiting, values approaching zero
% cause lower-order approximation to the solution (0.05 by default)
VENKAT_LIMITER_COEFF= 0.05
%
% Reference coefficient for detecting sharp edges (3.0 by default).
REF_SHARP_EDGES = 3.0
%
% Coefficient for the adjoint sharp edges limiter (3.0 by default).
ADJ_SHARP_LIMITER_COEFF= 3.0
%
% Remove sharp edges from the sensitivity evaluation (NO, YES)
SENS_REMOVE_SHARP = NO
%
SENS_SMOOTHING= NONE
%
% Freeze the value of the limiter after a number of iterations
LIMITER_ITER= 999999
%
% 1st order artificial dissipation coefficients for
%     the Lax–Friedrichs method ( 0.15 by default )
LAX_SENSOR_COEFF= 0.15
%
% 2nd and 4th order artificial dissipation coefficients for
%     the JST method ( 0.5, 0.02 by default )
JST_SENSOR_COEFF= ( 0.5, 0.02 )
%
% 1st order artificial dissipation coefficients for
%     the adjoint Lax–Friedrichs method ( 0.15 by default )
ADJ_LAX_SENSOR_COEFF= 0.15
%
% 2nd, and 4th order artificial dissipation coefficients for
%     the adjoint JST method ( 0.5, 0.02 by default )
ADJ_JST_SENSOR_COEFF= ( 0.5, 0.02 )
%
% ------------------------ LINEAR SOLVER DEFINITION ---------------------------%
%
% Linear solver or smoother for implicit formulations:
% BCGSTAB, FGMRES, RESTARTED_FGMRES, CONJUGATE_GRADIENT (self-adjoint problems only), SMOOTHER.
LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver or type of smoother (ILU, LU_SGS, LINELET, JACOBI)
LINEAR_SOLVER_PREC= LU_SGS
%
% Linear solver ILU preconditioner fill-in level (0 by default)
LINEAR_SOLVER_ILU_FILL_IN= 0
%
% Minimum error of the linear solver for implicit formulations
LINEAR_SOLVER_ERROR= 1E-10
%
% Max number of iterations of the linear solver for the implicit formulation
LINEAR_SOLVER_ITER= 10
%
% Restart frequency for RESTARTED_FGMRES
LINEAR_SOLVER_RESTART_FREQUENCY= 10
%
% Relaxation factor for smoother-type solvers (LINEAR_SOLVER= SMOOTHER)
LINEAR_SOLVER_SMOOTHER_RELAXATION= 1.0
%
% -------------------------- MULTIGRID PARAMETERS -----------------------------%
%
% Multi-grid levels (0 = no multi-grid)
MGLEVEL= 4
%
% Multi-grid cycle (V_CYCLE, W_CYCLE, FULLMG_CYCLE)
MGCYCLE= V_CYCLE
%
% Multi-grid pre-smoothing level
MG_PRE_SMOOTH= ( 5, 5, 5, 5, 5 )
%
% Multi-grid post-smoothing level
MG_POST_SMOOTH= ( 5, 5, 5, 5, 5 )
%
% Jacobi implicit smoothing of the correction
MG_CORRECTION_SMOOTH= ( 5, 5, 5, 5, 5 )
%
% Damping factor for the residual restriction
MG_DAMP_RESTRICTION= 0.5
%
% Damping factor for the correction prolongation
MG_DAMP_PROLONGATION= 0.5
%
% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
% Convective numerical method (JST, JST_KE, JST_MAT, LAX-FRIEDRICH, ROE, AUSM,
%                              AUSMPLUSUP, AUSMPLUSUP2, AUSMPLUSM, HLLC, TURKEL_PREC,
%                              SW, MSW, FDS, SLAU, SLAU2, L2ROE, LMROE)
CONV_NUM_METHOD_FLOW= LAX-FRIEDRICH
%
% Roe Low Dissipation function for Hybrid RANS/LES simulations (FD, NTS, NTS_DUCROS)
ROE_LOW_DISSIPATION= FD
%
% Roe dissipation coefficient
ROE_KAPPA= 0.5
%
% Minimum value for beta for the Roe-Turkel preconditioner
MIN_ROE_TURKEL_PREC= 0.01
%
% Maximum value for beta for the Roe-Turkel preconditioner
MAX_ROE_TURKEL_PREC= 0.2
%
% Post-reconstruction correction for low Mach number flows (NO, YES)
LOW_MACH_CORR= NO
%
% Roe-Turkel preconditioning for low Mach number flows (NO, YES)
LOW_MACH_PREC= NO
%
% Use numerically computed Jacobians for AUSM+up(2) and SLAU(2)
% Slower per iteration but potentialy more stable and capable of higher CFL
USE_ACCURATE_FLUX_JACOBIANS= NO
%
% Use the vectorized version of the selected numerical method (available for JST family and Roe).
% SU2 should be compiled for an AVX or AVX512 architecture for best performance.
% NOTE: Currently vectorization always used for schemes that support it.
USE_VECTORIZATION= YES
%
% Entropy fix coefficient (0.0 implies no entropy fixing, 1.0 implies scalar
%                          artificial dissipation)
ENTROPY_FIX_COEFF= 0.5
%
% Higher values than 1 (3 to 4) make the global Jacobian of central schemes (compressible flow
% only) more diagonal dominant (but mathematically incorrect) so that higher CFL can be used.
CENTRAL_JACOBIAN_FIX_FACTOR= 4.0
%
% Control numerical properties of the global Jacobian matrix using a multiplication factor
% for incompressible central schemes
CENTRAL_INC_JACOBIAN_FIX_FACTOR= 1.0
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT)
TIME_DISCRE_FLOW= EULER_IMPLICIT
%
% Use a Newton-Krylov method on the flow equations, see TestCases/rans/oneram6/turb_ONERAM6_nk.cfg
% For multizone discrete adjoint it will use FGMRES on inner iterations with restart frequency
% equal to "QUASI_NEWTON_NUM_SAMPLES".
NEWTON_KRYLOV= NO
%
% Integer parameters {startup iters, precond iters, initial tolerance relaxation}.
NEWTON_KRYLOV_IPARAM= (10, 3, 2)
%
% Double parameters {startup residual drop, precond tolerance, full tolerance residual drop, findiff step}.
NEWTON_KRYLOV_DPARAM= (1.0, 0.1, -6.0, 1e-5)
%
% ------------------- FEM FLOW NUMERICAL METHOD DEFINITION --------------------%
%
% FEM numerical method (DG)
NUM_METHOD_FEM_FLOW= DG
%
% Riemann solver used for DG (ROE, LAX-FRIEDRICH, AUSM, HLLC, VAN_LEER)
RIEMANN_SOLVER_FEM= HLLC
%
% Constant factor applied for quadrature with straight elements (2.0 by default)
QUADRATURE_FACTOR_STRAIGHT_FEM = 2.0
%
% Constant factor applied for quadrature with curved elements (3.0 by default)
QUADRATURE_FACTOR_CURVED_FEM = 3.0
%
% Factor for the symmetrizing terms in the DG FEM discretization (1.0 by default)
THETA_INTERIOR_PENALTY_DG_FEM = 1.0
%
% Compute the entropy in the fluid model (YES, NO)
COMPUTE_ENTROPY_FLUID_MODEL= YES
%
% Use the lumped mass matrix for steady DGFEM computations (NO, YES)
USE_LUMPED_MASSMATRIX_DGFEM= NO
%
% Only compute the exact Jacobian of the spatial discretization (NO, YES)
JACOBIAN_SPATIAL_DISCRETIZATION_ONLY= NO
%
% Number of aligned bytes for the matrix multiplications. Multiple of 64. (128 by default)
ALIGNED_BYTES_MATMUL= 128
%
% Time discretization (RUNGE-KUTTA_EXPLICIT, CLASSICAL_RK4_EXPLICIT, ADER_DG)
TIME_DISCRE_FEM_FLOW= RUNGE-KUTTA_EXPLICIT
%
% Number of time DOFs for the predictor step of ADER-DG (2 by default)
TIME_DOFS_ADER_DG= 2
% Factor applied during quadrature in time for ADER-DG. (2.0 by default)
%QUADRATURE_FACTOR_TIME_ADER_DG = 2.0
%
% Type of discretization used in the predictor step of ADER-DG (ADER_ALIASED_PREDICTOR, ADER_NON_ALIASED_PREDICTOR)
ADER_PREDICTOR= ADER_ALIASED_PREDICTOR
% Number of time levels for time accurate local time stepping. (1 by default, max. allowed 15)
LEVELS_TIME_ACCURATE_LTS= 1
%
% Specify the method for matrix coloring for Jacobian computations (GREEDY_COLORING, NATURAL_COLORING)
KIND_MATRIX_COLORING= GREEDY_COLORING
%
% Specify shock capturing method for DG
KIND_FEM_DG_SHOCK= NONE
%
% ------------------------- SCREEN/HISTORY VOLUME OUTPUT --------------------------%
%
% Screen output fields (use 'SU2_CFD -d <config_file>' to view list of available fields)
SCREEN_OUTPUT= (INNER_ITER, RMS_PRESSURE, DRAG, LIFT, MIN_CFL, AVG_CFL, MAX_CFL, MAX_VELOCITY-X)
%
% History output groups (use 'SU2_CFD -d <config_file>' to view list of available fields)
HISTORY_OUTPUT= (ITER, RMS_PRESSURE, RMS_MOMENTUM-X, RMS_MOMENTUM-Y, DRAG, LIFT)
%
% Volume output fields/groups (use 'SU2_CFD -d <config_file>' to view list of available fields)
VOLUME_OUTPUT= (COORDINATES, SOLUTION, PRIMITIVE)
%
% Writing frequency for screen output
SCREEN_WRT_FREQ_INNER= 10
%
SCREEN_WRT_FREQ_OUTER= 1
%
SCREEN_WRT_FREQ_TIME= 1
%
% Writing frequency for history output
HISTORY_WRT_FREQ_INNER= 1
%
HISTORY_WRT_FREQ_OUTER= 1
%
HISTORY_WRT_FREQ_TIME= 1
%
% list of writing frequencies corresponding to the list in OUTPUT_FILES
OUTPUT_WRT_FREQ= 250, 250, 250
%
% Output the performance summary to the console at the end of SU2_CFD
WRT_PERFORMANCE= YES
%
% Output the tape statistics (discrete adjoint)
WRT_AD_STATISTICS= NO
%
%
% Overwrite or append iteration number to the restart files when saving
WRT_RESTART_OVERWRITE= YES
%
% Overwrite or append iteration number to the surface files when saving
WRT_SURFACE_OVERWRITE= YES
%
% Overwrite or append iteration number to the volume files when saving
WRT_VOLUME_OVERWRITE= YES
%
% Determines if the forces breakdown is written out
WRT_FORCES_BREAKDOWN= NO
%
% MPI communication level (NONE, MINIMAL, FULL)
COMM_LEVEL= FULL
%
% Node number for the CV to be visualized (tecplot) (delete?)
VISUALIZE_CV= -1
%
% Write extra output (EXPERIMENTAL, NOT FOR GENERAL USE)
EXTRA_OUTPUT= NO
%
% Write extra heat output for a given heat solver zone
EXTRA_HEAT_ZONE_OUTPUT= -1
%
% ------------------------- INPUT/OUTPUT FILE INFORMATION --------------------------%
%
% Mesh input file
MESH_FILENAME= naca_0012.su2
%
% Mesh input file format (SU2, CGNS)
MESH_FORMAT= SU2
%
% Restart flow input file
SOLUTION_FILENAME= restart_flow.dat
%
% Output tabular file format (TECPLOT, CSV)
TABULAR_FORMAT= CSV
%
OUTPUT_PRECISION= 10
%
% Files to output
OUTPUT_FILES= (RESTART, PARAVIEW, SURFACE_PARAVIEW)
%
% Output file convergence history (w/o extension)
CONV_FILENAME= history
%
% Output file with the forces breakdown
BREAKDOWN_FILENAME= forces_breakdown.dat
%
% Output file restart flow
RESTART_FILENAME= restart_flow.dat
%
% Output file flow (w/o extension) variables
VOLUME_FILENAME= flow
%
% Output file surface flow coefficient (w/o extension)
SURFACE_FILENAME= surface_flow
%

If anyone with more experience than me could have a look over the setup and let me know where I go wrong it would be much appreciated!

[bigfootedrockmidget]

You are using nondimensionalization of the results:

% Non-dimensionalization scheme for incompressible flows. Options are
% INITIAL_VALUES (default), REFERENCE_VALUES, or DIMENSIONAL.
% INC_*_REF values are ignored unless REFERENCE_VALUES is chosen.
INC_NONDIM= INITIAL_VALUES

That means your result is made dimensionless using your initial values from INC_VELOCITY_INIT.

You can change your code to:

INC_NONDIM=DIMENSIONAL

Alternatively, you can also multiply your velocity field by your initial velocity values in paraview.

We have some explanation here:
https://su2code.github.io/docs_v7/Ph...incompressible

[t.teschner]

I suspected as much, but for some reason, I missed that! Thanks for the help, it is much appreciated!