TURBULENCE [MODEL] model [Options] [ITERATIONS iter] [zone_selector] 
The TURBULENCE keyword is used to request an inviscid or viscous solution, and to select a turbulence model for one or more zones. In addition to the TURBULENCE keyword itself, several additional keywords affect various aspects of the turbulence modeling procedure.
Model Selection
The TURBULENCE keyword (see above for the syntax) is used to select inviscid, laminar, or turbulent flow, and for turbulent flow, the turbulence model to be used. The choice is determined by the input value model, which must be one of the following. Unless noted otherwise, these apply to both structured and unstructured grids. The SpalartAllmaras oneequation model and the Menter shear stress transport (SST) twoequation model are the most widely used, tested, and supported models.
Model Keyword(s)  Description
 

{INVISCID  EULER} [NOSLIP]  Inviscid flow.
If NOSLIP is specified, noslip boundary conditions
will be applied at adiabatic and viscous walls; otherwise, slip
boundary conditions will be applied.
 
LAMINAR  Laminar flow.
 
CEBECI [SMITH]  CebeciSmith algebraic turbulence model.
This model is only available for structured grids.
 
[BALDWIN] LOMAX  BaldwinLomax algebraic turbulence model.
This model is only available for structured grids.
 
PDT  Combination BaldwinLomax and P. D. Thomas algebraic
shear layer model.
This model is only available for structured grids.
 
[BALDWIN] BARTH  BaldwinBarth oneequation turbulence model.
This model is only available for structured grids.
 
POINTWISE  Goldberg pointwise oneequation turbulence model.
This model is only available for unstructured grids.
The FREE_ANUT keyword
can be used to specify the freestream turbulence level.
In multizone problems, the Goldberg pointwise model may only be used with inviscid or laminar flow in other zones.
 
SPALART [ALLMARAS]  SpalartAllmaras oneequation turbulence model,
which is the most widely used oneequation turbulence model
and a practical choice for many applications.
The FREE_ANUT keyword
can be used to specify the freestream turbulence level.
In multizone problems, the SpalartAllmaras model may only be used with inviscid or laminar flow in other zones.
 
SpalartAllmaras Options: 
 
{RC  ROTATION}  Activates a correction for system rotation and streamline curvature.
 
ROUGHNESS hgt  Includes the effects of wall roughness.
The default roughness height is 0.0.
 
{DES  MDES  DDES} [CDES coef]  Activates the
DES,
MDES, or
DDES
option described below in the section on combined RANS/LES modeling.
The DDES option is only available for use with
unstructured grids.
 
{PRNS [RCP coef]  \ DETACHEDPRNS [RCP coef] [DPRNS coef]}  Activates the
PRNS, or
DETACHEDPRNS
option described below in the section on Partially Resolved Numerical
Simulation.
 
BSL and SST models:  Twoequation kω turbulence models of Menter.  
BSL  Baseline model without the shear stress limiter.  
SST  Shear stress transport model. SST is considered an industry standard model and is recommended for use in most applications.  
Additional keywords specific to the BSL and SST models are available for specifying freestream values of k and ω. Additional keywords may also be used to modify the SST stress limiter coefficient. In multizone problems, the BSL and SST models may be used interchangeably or with inviscid or laminar zones. However, it is recommended to use the same model in all zones.  
BSL and SST Options: 
 
F2FIX dmax  For structured grids, this option may be used to specify a
maximum distance from the wall, dmax, within which the
F_{2} term may be nonzero.
Beyond that distance, the term is set to zero.
F_{2} is a blending function, designed to limit
the effects of the shear stress transport term to regions near
walls.
 
{COMPRESSIBLE  TRANSITION}  The COMPRESSIBLE option uses the compressibility
corrections of Suzen and Hoffmann.
If TRANSITION is specified, a compressible version of the SST model with transition modeling is used. This model was developed by Menter, et al.
This option is only available for structured grids, and is fairly sensitive to grid resolution, particularly in the streamwise direction. Additional keywords control the specific compressibility terms that are included and the production term modification coefficient for transition modeling.  
{LESB [CBLES coef]  \ HYBRID [VERSION value] [CLES value] [DELTA value]} 
 
Activates the
LESB or
HYBRID
option described below in the section on combined RANS/LES modeling.
 
Structured grid ke models:  Low Reynolds number twoequation kε
turbulence models.
These models are only available for structured grids.
The user should be aware of additional keywords specific to the kε models, particularly those used to control initialization. In multizone problems, these models may be used with inviscid, laminar, or other structured grid kε models. However, it is recommended to use the same model in all zones.  
AKN [KE]  ABEKONDOHNAGANO [KE] 
 
CHIEN [KE] 
 
CRAFTTECH [KE] 
 
NTT [KE]  NAGANOTAGAWATSUJI [KE] 
 
SSGZ [KE]  SOSARKARGERODIMOSZHANG [KE] 
 
SZS [KE]  SOZHANGSPEZIALE [KE] 
 
Structured grid ke Options: 
 
HYBRID [VERSION value] [CLES value] [DELTA value] 
 
Activates the
HYBRID
option described below in the section on combined RANS/LES modeling.
 
RUMSEYGATSKI [ASM] [KE]  Low Reynolds number twoequation kε
algebraic Reynolds stress model of Rumsey and Gatski.
This model is only available for structured grids.
The user should be aware of additional keywords specific to the kε models, particularly those used to control initialization.
In multizone problems, the RumseyGatski model may be used
with inviscid, laminar, or another structured grid
kε model in other zones.
However, it is recommended to use the same model in all zones.
 
REALIZABLE [KE]  Nonlinear low Reynolds number twoequation
kε model of Goldberg.
This model is only available for unstructured grids.
The user should be aware of additional
keywords specific to the unstructured kε
models.
In multizone problems, the Realizable model may not be used
with different turbulence models in other zones.
It also may not be used with inviscid or laminar flow in other
zones.
 
Realizable ke Options: 
 
{LINEAR  QUADRATIC  CUBIC}  Controls whether the Reynolds stress tensor is computed using
terms that are linear, quadratic, or cubic functions of the
mean strain and rotation rate tensors.
The linear option is similar to the Boussinesq approximation
used by most eddy viscosity models. Highorder terms may
capture the secondary motion in the corners of rectangular
ducts.
 
SHIH [KE]  Nonlinear low Reynolds number twoequation
kε model of Shih.
This model is only available for unstructured grids.
The user should be aware of additional
keywords specific to the unstructured kε
models.
In multizone problems, the Shih model may not be used
with different turbulence models in other zones.
It also may not be used with inviscid or laminar flow in other
zones.
 
Shih ke Options: 
 
{LINEAR  QUADRATIC  CUBIC}  Controls whether the Reynolds stress tensor is computed using
terms that are linear, quadratic, or cubic functions of the
mean strain and rotation rate tensors.
The linear option is similar to the Boussinesq approximation
used by most eddy viscosity models. Highorder terms may
capture the secondary motion in the corners of rectangular
ducts.

Note that, with the exceptions noted above, different turbulence models, or inviscid or laminar flow, may be specified in different zones. However, you must specify a "default" turbulence model (or inviscid or laminar flow) in the input data file. WindUS will stop if you do not. By "default", we mean without specifying zones. In addition, due to a coding limitation, the zone_selector can't be used when inviscid flow is being specified.
For example, for a threezone problem with inviscid flow in zone 1 and the SpalartAllmaras turbulence model in zones 2 and 3, the following will not work because a "default" turbulence model has not been specified, and the code will stop:
TURBULENCE SPALART ZONE 2,3 TURBULENCE INVISCID ZONE 1The following will also not work, because a zone_selector can't be used with INVISCID:
TURBULENCE SPALART TURBULENCE INVISCID ZONE 1Instead, one would specify the following, which will work:
TURBULENCE INVISCID TURBULENCE SPALART ZONE 2,3
Additional common options that may be specified with the TURBULENCE keyword are:
URANS  Indicates the desire to run in unsteady RANS mode.
 

ITERATIONS iter  WindUS organizes the equations to be solved into logical
"groups" that are solved together.
It also allows multiple iterations of a specific group
(i.e., subiterations) for each
"iteration per cycle".
For the one and twoequation turbulence models, the
ITERATIONS option allows the user to request iter
subiterations of the turbulence model equation group for each
iteration per cycle.
If NAVIERSTOKES ITERATIONS
is defaulted, this corresponds to iter iterations of the
turbulence model equations for each iteration of the mean flow
equations.
The default value for iter is one, indicating that each iteration per cycle corresponds to one iteration of the turbulence model equations. 
Note that for the one and twoequation turbulence models, the turbulence model equations may be solved without simultaneously solving the NavierStokes equations. Of course, the turbulence variables depend on the mean flow field, so a reasonable mean flow solution must already exist.
As an example, suppose a mean flow solution has been computed using the SST turbulence model. The Chien kε variables consistent with the existing mean flow field may be computed by restarting from the SST solution, and solving just the Chien kε equations.
ITERATIONS PER CYCLE 2 ZONE ALL NAVIERSTOKES ITERATIONS 0 ZONE ALL TURBULENCE MODEL CHIEN ITERATIONS 5 ZONE ALL
The above keywords specify that, for all zones, there will be two iterations per cycle, with no NavierStokes subiterations and five Chien model subiterations for each "iteration per cycle". There will thus be a total of ten iterations of the Chien kε equations in each zone prior to completing a cycle and exchanging information between zones.
See Also: ITERATIONS, NAVIERSTOKES ITERATIONS, DEBUG 82, DEBUG 83, TEST 21, TEST 67
Wall Distance
MAX_WALL_DISTANCE DistMax {GRID_UNITS  {BOUNDARY_LAYER_THICKNESSES  BLT}} \ [PROGRESS {OFF  [PERCENT] integer_percent}] 
This keyword may be used to specify the maximum distance from the wall that will be used in many of the turbulence models. The value DistMax may be specified in either grid units (i.e., the same units that are used in the .cgd file) by using the GRID_UNITS modifier, or as a multiple of the "nominal" boundary layer thickness by using the BOUNDARY_LAYER_THICKNESSES (or BLT) modifier. Note that the modifier GRID_UNITS or BOUNDARY_LAYER_THICKNESSES (or BLT) must be specified.
The "nominal" boundary layer thickness is defined as 0.37 Re^{−1/5}L_{c}, where L_{c} is a characteristic length equal to the diagonal of the bounding box containing all the viscous grid points, and the Reynolds number Re is based on L_{c} and the freestream flow conditions. This is empirically equal to the boundary layer thickness for incompressible turbulent flow past a flat plate at those conditions.
The default for DistMax is 1,000,000 grid units.
A message is periodically written to the .lis file for each zone, showing the progress of the calculation. The optional PROGRESS keyword may be used to specify how often this message is written, or to prevent it from being written at all. The value integer_percent is the frequency for writing the message, expressed as a percentage of grid cells to be searched. E.g., if integer_percent = 5, the message will be written when the wall distance for 5% of the cells have been computed, 10% of the cells, etc. The default is to write the message, with integer_percent equal to 10.
Note/Warning
The default setting for DistMax of 1,000,000 grid units is intentionally very large so that there will be essentially no chance that the cap on the distance from the wall will corrupt turbulent flow simulations. In general, users should not need to modify this setting.
Some older versions of the code used a slower algorithm for computing the wall distance. Even though the calculation is only done once and the results are saved in the .tda file for later use, there was occasionally a very significant penalty in computational time required at startup for flow problems with many zones and large numbers of grid points. In order to significantly reduce this computational time penalty, the user would set DistMax to a lower value. As a general rule of thumb, if a flow problem is expected only to have attached (i.e., nonseparated), relatively thin boundary layers, DistMax may be set to a smaller value than is needed for problems with large wakes, separated regions, or jets. In practice, it has been found that for simulations with wellbehaved boundary layers, using
MAX_WALL_DISTANCE DistMax BOUNDARY_LAYER_THICKNESSESwhere the multiplier DistMax is a value from 210, may be sufficient. However, users are again cautioned to only adjust this setting if they experience a significant time delay with the wall distance calculation prior to the first solution cycle. The PROGRESS keyword will inform you how the calculation is proceeding.
SpalartAllmaras and Goldberg Models
FREE_ANUT anutinf 
When TURBULENCE SPALART or TURBULENCE POINTWISE is specified, indicating use of the SpalartAllmaras or Goldberg model, the separate keyword FREE_ANUT may be used to specify the freestream value of the eddy viscosity ν_{t}. The default value is 5.0.
Specifying Freestream k and ω
FREE_K val_k FREE_OM val_om 
If TURBULENCE {BSL  SST} is specified, indicating that the BSL or SST model is to be used, the separate keywords FREE_K and FREE_OM may be used to input freestream values of k and ω. The following options are possible:
val_k > 0  The turbulent kinetic energy k and the specific dissipation
rate ω are specified directly, with
ω = val_om (1/sec) The turbulent viscosity ν_{t} is then equal to k/ω.  

val_k < 0  The turbulence intensity is set equal to abs(val_k),
expressed as a percentage of the freestream velocity
U_{∞}.
Thus, the turbulent kinetic energy is computed as
The turbulent viscosity ν_{t} is automatically set equal to 0.001 ν_{l}, where ν_{l} is the laminar viscosity, and the specific dissipation rate is computed as ω = k/ν_{t}.  
val_om < 0  The specific dissipation rate ω is set equal to
val_om percent of U_{∞} / L_{ref},
where U_{∞} is the freestream velocity,
and L_{ref} is the reference length
from the grid (.cgd) file.
Thus
The turbulent viscosity ν_{t} is set to the same percentage of the laminar viscosity.
The turbulent kinetic energy is then computed as k = ων_{t}. 
The default, and recommended, values are
Note that
These inflow values will be used to initialize the flow and applied during each cycle update. If the flow exits the boundary at any time during the solution procedure, values from the interior will be extrapolated to that boundary point. Should the flow subsequently reestablish itself as entering the domain, the specified inflow turbulence will once again be applied.
Inflow turbulence levels may also be specified for the BSL and SST models in the ARBITRARY INFLOW keyword block. If this is done, the TURBULENCE keyword must come before the ARBITRARY INFLOW keyword block in the input data (.dat) file.
See Also: ARBITRARY INFLOW
Compressibility Corrections
COMPRESSIBLE [DISSIPATION] {ONOFF} [zone_selector] PRESSURE [DILATATION] {ONOFF} [zone_selector] 
If TURBULENCE {BSL  SST} {COMPRESSIBLE  TRANSITION} is specified, the BSL or SST model will use the compressibility corrections of Suzen and Hoffmann. The two keywords shown above may also be used to control which specific compressibility terms are included. The COMPRESSIBLE [DISSIPATION] keyword controls whether or not a compressible (dilatational) dissipation correction is used, and the PRESSURE [DILATATION] keyword controls whether or not the pressure dilatation term is included. Both of these are ON by default.
Production Term Modification
SST [TRANSITION] COEF_PTM1 value 
When TURBULENCE SST TRANSITION is specified, indicating that the compressible version of the SST model with transition modeling is to be used, the separate keyword SST COEF_PTM1 may be used to set the value of the coefficient φ_{PTM1}. This coefficient adjusts how much the turbulence production is limited in laminar regions. For a flat plate test case, a value of 1.0 was found to best reproduce the axial location of fully turbulent flow, while a value of 2.0 better predicted the transition onset location. The default value is 1.0.
Stress Limiter Modification
SST STRESS [LIMITER] COEFFICIENT value 
One of the key features of the Menter SST model is the inclusion of a limiter in boundary layer regions that prevents the ratio of turbulent shear stress to turbulent kinetic energy from exceeding a prescribed value. The default value is 0.31, often noted in the literature as Bradshaw's constant. This keyword allows the user to specify a different value of the coefficient. For shock wave/boundary layer interactions, a value of 0.355 has been shown to significantly improve separation regions. The specified value is applied to all zones.
Test Options
Several test options are specifically related to the BSL and SST turbulence models.
TEST 15  Modifies the filter width used with the LESB option.  

TEST 20  Reverts to an older nondimensionalization for k and ω.  
TEST 34, 38, 41, 44  Controls Net Vorticity Transport modification of the turbulent kinetic energy production term.  
TEST 39  Activates freestream sustainment terms.  
TEST 43  Modifies the diffusion coefficient in the ω transport equation.  
TEST 45  Activates additional limiters recommended by Menter after the initial development of the the BSL and SST models.  
TEST 46, 67  Modifies the wall treatment when bleed or blowing are used.  
TEST 57  Forces implicit solution of the turbulence equations when the mean flow is solved explicitly.  
TEST 188  Controls how turbulence model data is passed across coupled zones. 
kε Models
Several additional keywords may be used with the
kε models to control the initialization procedure,
enhance their stability, and improve their accuracy in adverse pressure
gradients and at high Mach numbers.
For convenience, all keyword phrases associated with the
kε models begin with KE.
Note that these keywords apply to structured grids only, unless otherwise
indicated.
KE FREE_K val1 KE FREE_MUT val2 
These keywords may be used to specify the freestream turbulence values to be used when initializing the turbulence variables to uniform values (i.e., with the KE INITIALIZE FROM FREESTREAM keyword). The interpretation of the input depends on the signs of val1 and val2.
For the turbulence kinetic energy k_{∞},
k_{∞} =  3 I^{2}u^{2}_{∞} / 2  for val1 < 0, and where val1 = I  
=  [k_{∞} / a^{2}_{∞}]_{dim}  for val1 > 0, and where val1 = (k_{∞})_{dim} (ft/sec)^{2} 
and for the turbulent viscosity (μ_{t})_{∞},
(μ_{t})_{∞} =  (μ_{t})_{∞}  for val2 < 0, and where val2 = (μ_{t})_{∞}  
=  [(μ_{t})_{∞} / μ_{∞}]_{dim}  for val2 > 0, and where val2 = [(μ_{t})_{∞}]_{dim} (slug/ftsec) 
where the subscript dim denotes a dimensional value.
If the KE FREE_K keyword is not used, or if val1 = 0, then a default value of val1 = −0.01 is used, which corresponds to a turbulence intensity I of 1%. If the KE FREE_MUT keyword is not used, or if val2 = 0, then a default value of val2 = −0.001 is used for structured grids. This sets the freestream turbulent viscosity to be 0.001 times the freestream laminar viscosity. Note that for values greater than zero, the expected units for val1 and val2 are (ft/s)^{2} and slug/fts, respectively.
For structured grids, the kε models extrapolate to get turbulence values at all inflow and outflow boundaries. Thus, KE FREE_K and KE FREE_MUT can be used to initialize the flow, but not to specify inflow conditions.
For unstructured grids, the default setting for KE FREE_MUT is
5 and 50 for the Goldberg realizable and Shih kε
models respectively.
At the end of each cycle, these models reapply the freestream
turbulence values along all freestream boundaries that have
flow entering the domain.
KE INITIALIZE [FROM] {EXISTING  EQUILIBRIUM  FREESTREAM} 
This keyword determines how the turbulent transport variables (k, ε, and μ_{t}) for the kε models will be initialized.
It is recommended that the user first obtain an intermediate solution using another turbulence model, before switching to one of the kε models. Initializing from an existing turbulent solution rather than uniform values aids somewhat in convergence and improves the stability of the models by reducing the dramatic changes in turbulence values that occur during the first few iterations after initialization.
This intermediate solution need not be fully converged, but should have reached a state where the the turbulence is well established within the shear regions (boundary layers, mixing layers, etc.) of each zone. Users can examine values of mut/muinf with CFPOST to check the state of turbulence in the flow prior to switching models. Low values of mut/muinf (say < 50 or 100) may be insufficient to sustain turbulence, causing the solution to relaminarize as additional cycles are performed. The SST and Spalart models are good choices for obtaining the intermediate solution.
There are three methods for establishing the initial values for the kε models.
The first method, given by the EXISTING parameter, performs an "intelligent" initialization, based on the type of turbulence model used in the previous run. This is the default. When initializing from another twoequation model, direct conversion of turbulence values is performed. For lowerorder models, the procedure is equivalent to using the EQUILIBRIUM parameter. When initializing from inviscid or laminar solutions, the procedure is equivalent to using the FREESTREAM parameter.
The second method, given by the EQUILIBRIUM parameter, uses an assumption of turbulent equilibrium, namely that the production, Π, of turbulent kinetic energy equals the rate of dissipation, together with an existing turbulent viscosity profile to initialize the k and ε variables.
The third method, given by the FREESTREAM parameter, initializes the turbulence variables to uniform values within each zone.
KE REINITIALIZE 
This keyword signals the code to ignore the old kε
information in the flow (.cfl) file and perform a fresh
initialization from uniform values.
This command must be removed on subsequent runs or else the model will
reinitialize itself each time.
Under normal operation, this keyword should not be used.
KE [TVD] ORDER {123} 
This keyword sets the spatial order of accuracy of the TVD upwinding
used in solving the kε equations.
The default is firstorder.
KE RELAX [FOR] val [ITERATIONS] 
Updated values of k, ε, and μ_{t}
will be relaxed for val iterations (the default is 500) following
the initialization.
Relaxation of each of these variables reduces the amount they may change
during any single iteration.
Immediately after initialization, the allowed changes are significantly
reduced.
This restriction is then gradually lifted as the last relaxation iteration
is approached.
KE [MAXIMUM] [TURBULENT] VISCOSITY val1 KE [TURBULENT] [REFERENCE] VELOCITY val2 
The kε model uses limiters within the interior of each zone to increase convergence and stability by capping the values of the turbulence quantities at both the high and low extremes. This is usually only necessary during the first few iterations after initialization, when the fluctuations in k and ε tend to be the most dramatic.
Nondimensional values of the minimum limiters have been preset to small numbers. k_{min} is set to 10^{−10}, ε_{min} is set to 10^{−12}, and (μ_{t})_{min} is computed from the turbulent viscosity relation using an assumed reference density of 1, C_{μ} = 0.09, and F_{μ} = 1.
The above keywords determine the maximum limiting values for the turbulence quantities. The first keyword sets the maximum turbulent viscosity to be val1 (the default is 10,000) times the freestream viscosity. The second keyword sets the turbulent reference velocity equal to val2 (the default is 1.0) times the freestream speed of sound. The maximum turbulent kinetic energy allowed is 10% of the kinetic energy of the turbulent reference velocity:
The use of these limiters can be summarized as follows:
If the maximum limiters cause the turbulence variables to be capped within
the flowfield, a warning message will be written to the list output
(.lis) file during the final cycle.
By using CFPOST to examine the
normalized variable mut muinf, one can observe where these
limiters are being used and adjust them using the above keywords.
It is important that the turbulence values not be limited upon convergence.
KE SOURCE [CORRECTION] {NONE  OFF  POPE [COEF value]  CHENKIM [COEF value]} 
This keyword may be used to activate and control optional source term corrections for all structured kε turbulence models. The default setting for the source term is NONE (or OFF).
The POPE option activates a vortex stretching correction of Pope (1978) that is intended to increase the turbulent dissipation rate in axisymmetric or threedimensional jets. This results in a reduction of the turbulent kinetic energy and turbulent shear stress, slower mixing, and longer potential core lengths. The default value for the Pope coefficient is 0.79. Unfortunately, this correction adversely affects radial jet predictions. In addition, experimental results have since shown that lateral divergence causes the shear stress to increase rather than decrease. Some people regard the Pope correction as more of an empirical fix for better prediction of the jet spreading rate.
The CHENKIM option activates an additional term of Chen and Kim (1987). that is intended to better represent the energy transfer rate from largescale turbulence to smallscale turbulence. In regions where the mean strain is large, leading to increased production of turbulent kinetic energy, this term enhances the turbulent dissipation rate. It has been used as a means to improve the prediction of turbulent jets. The default value for the ChenKim coefficient is 0.06, as recommended by Kenzakowski (2004).
For compressible flows, each of these correction terms is multiplied by an exponential damping function to reduce its effectiveness. Additional details, including the equations used by the models, may be found in the description of the KE COMPRESSIBILITY keyword.
KE COMPRESSIBILITY [CORRECTION] {NONE  OFF  SARKAR  WILCOX  \ CRAFT  SUZEN  AUPOIX  USER coef value} 
This keyword may be used to specify compressibility corrections designed to enhance predictions of free shear flows (i.e., jets and mixing layers) at higher Mach numbers. The effect of these corrections is to reduce the turbulent kinetic energy in regions where the flow is supersonic. In terms of supersonic jet predictions, this results in slower spreading rates, reduced mixing, and a longer potential core length.
Many of the turbulence correlation terms which these models are intended to represent have since been shown to make only minor contributions to the turbulent kinetic energy equation. However, many people still use these models as empirical corrections, since they often shift the results in the correct direction.
The following source terms will be selectively added to the righthandside of the ρk or ρε transport equations. \[ \begin{align} S_{\rho k} = & \left\{  \alpha_1 \hat{M}_t^2  \alpha_2 \hat{M}_t^2 \frac{\cal P}{\rho \epsilon} + \alpha_3 \hat{M}_t^2  \alpha_4 \hat{M}_t^2 \frac{ \nabla \rho }{\rho} \frac{k^{3/2}}{\epsilon} \left( \frac{{\cal P}}{\rho \epsilon} + 1 \right) \right\} \rho \epsilon \\ S_{\rho \epsilon} = & \left\{ C_{\epsilon 3} e^{\beta_3 \hat{M}_t^2} \chi_p + C_{\epsilon 4} e^{\beta_4 \hat{M}_t^2} \left( \frac{\cal P}{\rho\epsilon} \right)^2 + C_{A1} \max{\left[ 0; 1C_{A2} \frac{a}{\Omega} \frac{\epsilon}{k^{3/2}} \right]} \right\} \frac{\rho\epsilon^2}{k} \\ \hat{M}_t^2 = & \max{ \left[ 0; \left( \max{\left[ 0; M_t  M_{t01} \right]} \right)^2  \hat{M}_{t02}^2 \right] } \\ M_t = & \sqrt{2k} / {a} \\ \chi_p = & \frac{k}{\epsilon}^3 R_{ij} R_{jk} S_{ki} \end{align} \]
The α_{1} term represents contributions from dilatation dissipation, sometimes referred to as compressible dissipation. The α_{2} and α_{3} terms represent compressible contributions from pressure dilatation. The α_{4} term represents an additional compressibility correction for heated jet flows. The β_{3} and β_{4} coefficients apply compressibility damping factors to the Pope and ChenKim axisymmetric jet correction terms respectively, but the terms must first be activated with the KE SOURCE keyword. The C_{A1} and C_{A3} coefficients control an additional compressibility correction by Aupoix.
In the above expressions, M_{t01} and M_{t02} represent cutoff turbulent Mach numbers, below which the correction terms will have no effect. Some models apply this cutoff to the turbulent Mach number itself, while others apply it to the squared value. Thus, M_{t01} is intended to apply to the linear term, while M_{t02} applies to the square. Usually only one or the other is used.
The following table summarizes the available predefined compressibility corrections. Only one correction may be used at a time, and the default option is NONE (or OFF). One should note that the SUZEN settings are the same as those used in the compressible BSL and SST models.
Compressibility Corrections  

Variable  coef  NONE  SARKAR  WILCOX  CRAFT  SUZEN  AUPOIX 
α_{1}  ALPHA1  0.00  1.00  1.50  2.50  1.00  0.00 
α_{2}  ALPHA2  0.00  0.00  0.00  2.50  0.40  0.00 
α_{3}  ALPHA3  0.00  0.00  0.00  0.00  0.20  0.00 
α_{4}  ALPHA4  0.00  0.00  0.00  5.00  0.00  0.00 
β_{3}  BETA_POPE  0.00  0.00  0.00  75.00  0.00  0.00 
β_{4}  BETA_CHENKIM  0.00  0.00  0.00  0.00  0.00  0.00 
M_{t01}  MT01  0.00  0.00  0.00  0.20  0.00  0.00 
M_{t02}  MT02  0.00  0.00  0.25  0.00  0.00  0.00 
C_{A1}  AUPOIX1  0.00  0.00  0.00  0.00  0.00  0.90 
C_{A2}  AUPOIX2  0.00  0.00  0.00  0.00  0.00  0.32 
In addition, the USER option only adjusts the coefficient/value pairs that are specified. Thus it may be used after loading one of the predefined sets in order to make minor adjustments. The coefficients used will be printed in the .lis file.
Example
The following loads the SARKAR compressibility coefficients and then alters the values to those used by WILCOX.
KE COMPRESSIBILITY CORRECTION SARKAR KE COMPRESSIBILITY CORRECTION USER ALPHA1 1.50 MT02 0.25
The following references describe the predefined compressibility models:
KE [VARIABLE] CMU {ONOFF} 
It is well known that the baseline kε model is poorly suited to adverse pressure gradient flows, such as those found in diffusers. Rodi and Scheuerer
The variable C_{μ} formulation, which is derived from algebraic stress modeling, is designed to help remedy this problem by reducing the turbulent viscosity in regions of the flowfield where the production of turbulent kinetic energy is significantly larger than the rate of dissipation. The specific formulation used is:
The variable C_{μ} option can provide added stability to the kε model, such as in the case of an airfoil, where the sudden deceleration of the flow near the leading edge would otherwise result in a significant rate of production. In regions of the flow where the turbulence is in equilibrium, i.e., where the production and dissipation are balanced, the turbulent viscosity remains unchanged.
The above keyword may be used to turn this option on or off
(the default is OFF) for the Chien kε model.
KE CMUMIN val 
This keyword controls the lower limit of the C_{μ} coefficient used in the RumseyGatski model. As part of the algebraic Reynolds stress formulation C_{μ} varies throughout the flowfield with typical values in the range [0.07, 0.19]. The default value for this limiter is 0.0005, as recommended by Rumsey.
See Also: TEST 29
Realizable and Shih kε Models
KE FREE_K val1 KE FREE_MUT val2 
The specification of the freestream turbulence levels is identical to that described above. However, for unstructured grids, the default setting for KE FREE_MUT is 5 and 50 for the Goldberg realizable and Shih kε models respectively. Also note that these unstructured kε solvers will maintain the boundary values, rather than extrapolate like the structured kε solvers do.
Combined RANS/LES Models
The idea behind combined RANS/LES (Reynoldsaveraged NavierStokes / large eddy simulation) turbulence models is to improve predictions of complex flows in a realworld engineering environment, by allowing the use of LES methods with grids typical of those used with traditional Reynoldsaveraged NavierStokes models. The combined model reduces to the standard RANS model in high mean shear regions (e.g., near viscous walls), where the grid is refined and has a large aspect ratio unsuitable for LES models. As the grid is traversed away from high mean shear regions, it typically becomes coarser and more isotropic, and the combined model smoothly transitions to an LES model.
Several combined RANS/LES models are available in WindUS. The combined models may only be used for unsteady flows (i.e., the time step is a constant). They are zonal, however, so you can use a combined model in timeaccurate mode in one zone, while using a standard RANS model in steadystate mode in the other zones. For example, a threezone problem could use the standard SST model with a specified CFL number in zones 1 and 2, and the combined SST/LES model (implemented using an ε limiter) with a specified time step in zone 3, using the following keywords:
TURBULENCE SST TURBULENCE SST LESB ZONE 3 CFL# 1.3 TIMESTEP SECONDS 5.0E6 ZONE 3This capability can accelerate the solution convergence tremendously, especially for large configurations (10 to 20 million grid points) that would be impossible to run in timeaccurate mode throughout the flow field.
Spalart DES Model
DES [CDES cdes] 
[Note  This option must appear on the same line as the TURBULENCE keyword.]
When TURBULENCE SPALART is specified, the optional keyword DES may also be added to the line to use the Spalart detached eddy simulation (DES) turbulence model. It is intended to improve the results for unsteady and massively separated flows. The DES model reduces to the standard SpalartAllmaras model near viscous walls, where the grid is refined and has a large aspect ratio, but acts like a large eddy simulation (LES) model away from the boundary, where the grid is coarser and has an aspect ratio of order one.
The input parameter cdes specifies the value of the coefficient C_{des} in the model. The default value is 0.65. Increasing this coefficient increases the size of the region in which the DES model reduces to the standard SpalartAllmaras model. Details may be found in the following papers:
Shih's Modified DES Model
MDES [CDES cdes] 
[Note  This option must appear on the same line as the TURBULENCE keyword.]
The MDES keyword option is similar to the DES keyword described above, and may be specified in conjunction with TURBULENCE SPALART to use Shih's modified version of the DES model. The main difference between the approaches is that this one uses a length scale based on the cubed root of the cell volume instead of the largest cell edge. As in the standard DES model, the input parameter cdes specifies the value of the coefficient C_{des}, and the default value is 0.65.
Spalart's Delayed DES Model
DDES [CDES cdes] 
[Note  This option must appear on the same line as the TURBULENCE keyword.]
The DDES keyword option is also similar to the DES keyword described above, and may be specified in conjunction with TURBULENCE SPALART to use Spalart's delayed DES model. This method is intended to be somewhat less grid sensitive than the original DES approach. As in the standard DES model, the input parameter cdes specifies the value of the coefficient C_{des}, and the default value is 0.65. The DDES option is only available for use on unstructured grids.
BSL or SST with ε Limiter
LESB [CBLES cb] 
[Note  This option must appear on the same line as the TURBULENCE keyword.]
The LESB keyword option may be used with the BSL or SST models (TURBULENCE SST) to specify use of a combined RANS/LES turbulence model, using an ε limiter.
The input parameter cb specifies the value of the coefficient C_{B} in the model. The default value is 10.0. Increasing C_{B} increases the size of the region in which the combined model reduces to the standard BSL or SST model.
See Also: TEST 15
NicholsNelson Hybrid Model
HYBRID [VERSION ver] [CLES cles] [DELTA grid_scale] 
[Note  This option must appear on the same line as the TURBULENCE keyword.]
The HYBRID keyword option may be used with either the BSL, SST, or structured grid kε models to specify use of the NicholsNelson hybrid RANS/LES turbulence model.
ver  A flag indicating the version of the model to be used.
The default value is 1.  

cles  The coefficient c_{LES} used when calculating
the LES value of the turbulent viscosity.
The default value is 0.0854.  
grid_scale  A flag indicating the method of computing the characteristic grid
scale.
The default value is 1. 
Partially Resolved Numerical Simulation (PRNS)
PRNS [RCP Rcp] 
[Note  This option must appear on the same line as the TURBULENCE keyword.]
The PRNS keyword option may be used with the SpalartAllmaras model (TURBULENCE SPALART) to specify use of the PRNS (Partially Resolved Numerical Simulation) model, and is only applicable to unstructured grids. The input value Rcp is the resolution control parameter, the ratio of the temporal filter width to the turbulent integral time scale. A value of Rcp = 1.0 corresponds to a Reynoldsaveraged solution (i.e., no turbulent eddy resolution), while lower values result in smaller turbulent eddies being resolved. The default value is 0.4, intended to correspond to a very large eddy simulation.
Note that lowering Rcp means that more grid points are required to resolve the smaller eddies. In their original paper describing the PRNS model, Liu and Shih suggest that the number of grid points for a PRNS solution N_{PRNS} may be estimated using the formula
For more details on the PRNS model see the following papers:
Detached PRNS
DETACHEDPRNS [RCP Rcp] [DPRNS dprns] 
[Note  This option must appear on the same line as the TURBULENCE keyword.]
This keyword is similar to the PRNS keyword described above, but may only be used with the SpalartAllmaras model. It specifies use of the detached PRNS model, and is also only applicable to unstructured grids. The input value Rcp is again the resolution control parameter, with a default value of 0.4.
Unlike the standard PRNS model, the detached PRNS model doesn't scale the production term and turbulent viscosity near viscous walls. The size of this "nearwall" region is given by
Last updated 14 Nov 2016