This 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 (described in detail below), the following keywords affect various aspects of the turbulence modeling procedure. Of these, see especially the MAX_WALL_DISTANCE keyword, used to specify the maximum wall distance to be used. For problems with well-behaved boundary layers, appropriate use of this keyword can significantly speed up the wall distance calculation.

• Wall Distance
  • MAX_WALL_DISTANCE - Maximum Wall Distance
• Spalart-Allmaras and Goldberg Keywords
  • FREE_ANUT - Freestream eddy viscosity
• SST Keywords
  • COMPRESSIBLE, PRESSURE - Compressibility correction options
  • FREE_K, FREE_OMEGA - Freestream k and ω
• k-ε Keywords (structured grids only)
  • K-E INITIALIZE - Initialization procedure
  • K-E FREE_K, K-E FREE_MUT - Freestream k and μ_t
  • K-E REINITIALIZE - Reinitialize k, ε, and μ_t
  • K-E LINEARIZATION - Linearization procedure
  • K-E TVD ORDER - TVD accuracy order
  • K-E RELAX - Relaxation iterations
  • K-E MAXIMUM VISCOSITY, K-E REFERENCE VELOCITY - Limiting procedure
  • K-E COMPRESSIBILITY - Compressibility correction options
  • K-E CMU - Variable C_μ option
  • K-E CMUMIN - Minimum C_μ
• Combined RANS/LES Models
  • DES - Spalart DES Model
  • MDES - Shih's Modified DES Model
  • LESB - SST with ε Limiter
  • HYBRID - Nichols-Nelson Hybrid Model
  • PRNS - Partially Resolved Numerical Simulation (unstructured grids only)
  • DETACHED-PRNS - Detached Partially Resolved Numerical Simulation (unstructured grids only)

The choice between inviscid and viscous flow, and the turbulence model to be used, 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.

	{INVISCID | EULER} [NOSLIP]		Inviscid flow. If NOSLIP is specified, no-slip boundary conditions will be applied at adiabatic and viscous walls; otherwise, slip boundary conditions will be applied.
	LAMINAR		Laminar flow.
	CEBECI [SMITH]		Cebeci-Smith algebraic turbulence model. This model is only available for structured grids.
	[BALDWIN] LOMAX		Baldwin-Lomax algebraic turbulence model. This model is only available for structured grids.
	PDT		Combination Baldwin-Lomax and P. D. Thomas algebraic shear layer model. This model is only available for structured grids.
	[BALDWIN] BARTH		Baldwin-Barth one-equation turbulence model. This model is only available for structured grids.
	SPALART [ALLMARAS]		Spalart-Allmaras one-equation turbulence model. Additional keywords may be used with the Spalart-Allmaras model to specify the freestream turbulence level, and to specify use of the Spalart or Shih's Modified Detached Eddy Simulation (DES) turbulence model. For unstructured grids, other keywords may be used to specify use of a PRNS (Partially Resolved Numerical Simulation) or Detached PRNS model. In multi-zone problems, the Spalart-Allmaras model may not be used with different turbulence models in other zones, other than the DES models. However, it may be used with inviscid or laminar flow in other zones.
	POINTWISE		Goldberg pointwise one-equation turbulence model. This model is only available for unstructured grids. An additional keyword may be used with the Goldberg model to specify the freestream turbulence level. In multi-zone problems, the Goldberg pointwise model may not be used with different turbulence models in other zones. However, it may be used with inviscid or laminar flow in other zones.
	SST [COMPRESSIBLE]		Two-equation Shear Stress Transport turbulence model. If COMPRESSIBLE is specified, the compressibility corrections of Suzen and Hoffmann are applied. Additional keywords specific to the SST model are available for specifying compressibility correction options, and for specifying freestream values of k and ω. Other keywords may be used to specify use of a combined SST/LES model using an ε limiter, or the Nichols-Nelson hybrid SST/LES model. And for unstructured grids, the PRNS (Partially Resolved Numerical Simulation) model may be used. The compressibility corrections have been found beneficial for free shear layers in flows where the convective Mach number is above about 0.5). The overall effect is to increase the spreading in mixing layers, jets, etc. In multi-zone problems, the SST model may not be used with different turbulence models in other zones, other than the hybrid SST/LES model. However, it may be used with inviscid or laminar flow in other zones.
	CHIEN [K-E]		Low Reynolds number two-equation k-ε turbulence model of Chien. This model is only available for structured grids. The user should be aware of additional keywords specific to the k-ε models, particulary those used to control initialization. Other keywords may be used to specify use of a Nichols-Nelson hybrid Chien/LES model. In multi-zone problems, the Chien model may not be used with different turbulence models in other zones, other than the Rumsey-Gatski model and/or a hybrid Chien/LES model. It also may not be used with inviscid or laminar flow in other zones.
	RUMSEY-GATSKI [ASM] [K-E]		Low Reynolds number two-equation k-ε 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 k-ε models, particulary those used to control initialization. In multi-zone problems, the Rumsey-Gatski model may not be used with different turbulence models in other zones, other than the Chien model. It also may not be used with inviscid or laminar flow in other zones.

Note that with the exceptions noted above for the Spalart, Goldberg, SST, Chien, and Rumsey-Gatski models, 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. Wind-US 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 three-zone problem with inviscid flow in zone 1 and the Spalart-Allmaras 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 1

   TURBULENCE SPALART
   TURBULENCE INVISCID ZONE 1

   TURBULENCE INVISCID
   TURBULENCE SPALART ZONE 2,3

Additional options that may be specified with the TURBULENCE keyword are:

	ITERATIONS iter		Wind-US organizes the equations to be solved into logical "groups" that are solved together. It also allows multiple iterations of a specific group (i.e., sub-iterations) for each "iteration per cycle". For the one- and two-equation turbulence models, the ITERATIONS option allows the user to request iter sub-iterations of the turbulence model equation group for each iteration per cycle. If NAVIER-STOKES 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.
	RC | ROTATION		For structured grids, this option may be used with the Spalart-Allmaras one-equation model to include a correction for system rotation and streamline curvature.
	F2FIX dmax		For structured grids, this option may be used with the SST two-equation model to specify a maximum distance from the wall, dmax, within which the F2 term may be non-zero. Beyond that distance, the F2 term is set to zero. F2 is a blending function, designed to limit the effects of the shear stress transport term to regions near walls.

Note that for the one- and two-equation turbulence models, the turbulence model equations may be solved without simultaneously solving the Navier-Stokes 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 k-ε variables consistent with the existing mean flow field may be computed by restarting from the SST solution, and solving just the Chien k-ε equations.

   ITERATIONS PER CYCLE 2 ZONE ALL
   NAVIER-STOKES 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 Navier-Stokes sub-iterations and five Chien model sub-iterations for each "iteration per cycle". There will thus be a total of ten iterations of the Chien k-ε equations in each zone prior to completing a cycle and exchanging information between zones.

See Also: ITERATIONS, NAVIER-STOKES ITERATIONS, 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 the algebraic models, and the Spalart-Allmaras, k-ε, and SST 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^−1/5L_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 10,000 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 10,000 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. However, even though the calculation is only done once and the results are saved in the .tda file for later use, there may be a very significant penalty in computational time required at startup for flow problems with many zones and large numbers of grid points.

To significantly reduce this computational time penalty, a user should set DistMax to a lower value. As a general rule of thumb, if a flow problem is expected only to have attached (i.e., non-separated), 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 well-behaved boundary layers, using

   MAX_WALL_DISTANCE DistMax BOUNDARY_LAYER_THICKNESSES

Spalart-Allmaras and Goldberg Models

FREE_ANUT anutinf

When TURBULENCE SPALART or TURBULENCE POINTWISE is specified, indicating use of the Spalart-Allmaras 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.

SST Model

Compressibility Correction Options

COMPRESSIBLE [DISSIPATION] {ON|OFF} [zone_selector] PRESSURE [DILATATION] {ON|OFF} [zone_selector]

If TURBULENCE SST COMPRESSIBLE is specified, indicating that the SST model is to be used with the compressibility corrections of Suzen and Hoffmann, the separate keywords COMPRESSIBLE and PRESSURE may also be specified. The COMPRESSIBLE keyword controls whether or not a compressible dissipation correction is used, and the PRESSURE keyword controls whether or not the pressure dilatation term is included. Both of these are ON by default.

Specifying Freestream k and ω

FREE_K val_k FREE_OM val_om

If TURBULENCE SST is specified, indicating that the 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 k = val_k (ft2/sec2) ω = val_om (1/sec) The turbulent viscosity νt 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 k = 1.5 (0.01 |val_k| U∞) 2 The turbulent viscosity νt is automatically set equal to 0.001 νl, where νl is the laminar viscosity, and the specific dissipation rate is computed as ω = k/νt.
	val_om < 0		The specific dissipation rate ω is set equal to val_om percent of U∞ / Lref, where U∞ is the freestream velocity, and Lref is the reference length from the grid (.cgd) file. Thus ω = 0.01 |val_om| (U∞ / Lref) The turbulent viscosity νt is set to the same percentage of the laminar viscosity. νt = 0.01 |val_om| (νl) The turbulent kinetic energy is then computed as k = ωνt.

The default, and recommended, values are

Note that

• If val_k > 0, a positive value must be specified for val_om.
• If val_k ≤ 0, val_om should not be specified.
• If val_om < 0, any value specified for val_k is ignored.

For structured grids, inflow turbulence levels may be specified for the SST model 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

Chien and Rumsey-Gatski k-ε Models

[The material in this section was originally written by Dennis Yoder of NASA Glenn Research Center.]

Several additional keywords may be used with the Chien and Rumsey-Gatski k-ε 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 k-ε models begin with K-E. Note that all of these apply to structured grids only.

K-E INITIALIZE [FROM] {EXISTING | EQUILIBRIUM | FREESTREAM}

This keyword determines how the turbulent transport variables (k, ε, and μ_t) for the k-ε 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 k-ε 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 k-ε 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 two-equation model, direct conversion of turbulence values is performed. For lower-order 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.

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 K-E INITIALIZE FREESTREAM keyword). The interpretation of the input depends on the signs of val1 and val2.

For the turbulence kinetic energy k_∞,

	k∞ =	3 I2u2∞ / 2		for val1 < 0, and where |val1| = I
		[k∞ / a2∞]dim		for val1 > 0, and where val1 = (k∞)dim (ft/sec)2

and for the turbulent viscosity (μ_t)_∞,

	(μt)∞ =	(μt)∞		for val2 < 0, and where |val2| = (μt)∞
		[(μt)∞ / μ∞]dim		for val2 > 0, and where val2 = [(μt)∞]dim (slug/ft-sec)

where the subscript dim denotes a dimensional value.

If the K-E 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 K-E FREE_MUT keyword is not used, or if val2 =  0, then a default value of val2 = −0.001 is used. 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/ft-s, respectively.

These freestream values are only used when the k-ε model is initialized from uniform conditions. Currently, the model extrapolates to get values at all inflow and outflow boundaries. Thus, K-E FREE_K and K-E FREE_MUT can not be used to specify inflow conditions.

K-E REINITIALIZE

This keyword signals the code to ignore the old k-ε 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.

K-E LINEARIZATION {APPROXIMATE | FULL}

This keyword controls the implicit treatment of the k-ε source terms. The APPROXIMATE formulation results in greater diagonal dominance by neglecting coupling of the k and ε equations. The FULL formulation includes the coupling terms. The default is APPROXIMATE.

K-E [TVD] ORDER {1|2|3}

This keyword sets the spatial order of accuracy of the TVD upwinding used in solving the k-ε equations. The default is first order.

K-E 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.

K-E [MAXIMUM] [TURBULENT] VISCOSITY val1 K-E [TURBULENT] [REFERENCE] VELOCITY val2

The k-ε 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 k or ε falls below its preset minimum value, it is reset to the minimum value. This typically occurs in the freestream.
• If the turbulent kinetic energy exceeds k_max, it is capped at this value. The dissipation rate is taken to be the larger of the current dissipation rate or ε_max.
• If the turbulent viscosity exceeds (μ_t)_max it is capped at this value and the turbulent kinetic energy is recomputed from the turbulent viscosity relation. The turbulent dissipation rate is left unchanged.

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.

K-E COMPRESSIBILITY [CORRECTION] {NONE | OFF | SARKAR | WILCOX | \    USER αk Mt0}

This keyword may be used to specify a compressibility correction, designed to enhance predictions at higher Mach numbers. The equation for the compressibility correction is

The parameters α_k and M_t0 for the various options are defined in the following table.

	Correction Type		αk		Mt0
	NONE | OFF		0.0		0.00
	SARKAR		1.0		0.00
	WILCOX		1.5		0.25

Note that both NONE and OFF disable the compressibility correction, and that values of α_k and M_t0 should only be included when using the USER option. The default is OFF.

Both the Sarkar and Wilcox compressibility corrections are designed to improve the prediction of compressible jet flows by including the compressible portion of the dissipation rate in the transport equation for the turbulent kinetic energy. These corrections use simple algebraic relations between the solenoidal and compressible dissipation rates. 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 core length.

K-E [VARIABLE] CMU {ON|OFF}

It is well known that the baseline k-ε model is poorly suited to adverse pressure gradient flows, such as those found in diffusers. Rodi and Scheuerer [Rodi, W., and Scheuerer, G. (1986) "Scrutinizing the k-ε Turbulence Model Under Adverse Pressure Gradient Conditions," Transactions of the ASME Journal of Fluids Engineering, Vol. 108, pp. 174-179] demonstrated that for these types of flows, the rate of dissipation near solid boundaries is too small relative to the rate of production of turbulent kinetic energy. This causes the model to overpredict skin friction and predict flows to be attached when experimental results show them to be separated.

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 k-ε 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 k-ε model. It has no effect for the Rumsey-Gatski k-ε model.

K-E CMUMIN val

This keyword controls the lower limit of the C_μ coefficient used in the Rumsey-Gatski 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, TEST 51

Combined RANS/LES Models

The idea behind combined RANS/LES (Reynolds-Averaged Navier Stokes / Large Eddy Simulation) turbulence models is to improve predictions of complex flows in a real-world engineering environment, by allowing the use of LES methods with grids typical of those used with traditional Reynolds Averaged Navier Stokes 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 Wind-US. 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 time-accurate mode in one zone, while using a standard RANS model in steady-state mode in the other zones. For example, a three-zone 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
   LESB ZONE 3
   CFL# 1.3
   TIMESTEP SECONDS 5.0E-6 ZONE 3

Spalart DES Model

DES [CDES cdes] [zone_selector]

When TURBULENCE SPALART is specified, the separate keyword DES may also be input 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 Spalart-Allmaras 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 C_des increases the size of the region in which the DES model reduces to the standard Spalart-Allmaras model. Details may be found in papers by Spalart, et. al. [Spalart, P. R., Jou, W. H., Strelets, M., and Allmaras, S. R. (1997) "Comments on the Feasibility of LES for Wings, And on a Hybrid RANS/LES Approach," First AFOSR International Conference On DNS/LES, Aug. 4-8, 1997, Ruston, Louisiana. In Advances in DNS/LES, Liu, C., and Liu, Z., eds., Greyden Press, Columbus, Ohio] and by Shur, et. al. [Shur, M., Spalart, P. R., Strelets, M., and Travin, A. (1999) "Detached-Eddy Simulation of an Airfoil at High Angle of Attack," Fourth International Symposium on Engineering Turbulence Modeling and Measurements, May 24-26, 1999, Corsica].

Shih's Modified DES Model

MDES [CDES cdes] [zone_selector]

The MDES keyword 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. 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.

SST with ε Limiter

LESB [CBLES cb] [zone_selector]

The LESB keyword may be used with the SST model (TURBULENCE SST) to specify use of a combined SST and 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 SST model.

See Also: TEST 15

Nichols-Nelson Hybrid Model

HYBRID [VERSION ver] [CLES cles] [DELTA grid_scale] [zone_selector]

The HYBRID keyword may be used with either the SST or the Chien k-ε model to specify use of the Nichols-Nelson hybrid RANS/LES turbulence model [Nichols, R. H., and Nelson, C. C. (2003) "Applications of RANS/LES Turbulence Models," AIAA Paper 2003-1803].

	ver		A flag indicating the version of the model to be used.     1    The original Nichols-Nelson hybrid model. The μt value from the RANS model is used in the turbulence model equations, and the hybrid μt value is used in the Navier-Stokes equations. 2 The hybrid μt value is used in both the turbulence model and Navier-Stokes equations. 3 The hybrid μt value is used in both the turbulence model and Navier-Stokes equations, but k is treated like a sub-grid kinetic energy, not the full turbulent kinetic energy. (I.e., the model becomes more of an LES subgrid model.) The default value is 1.
	cles		The coefficient cLES used when calculating the LES value of the turbulent viscosity. (μt)LES = cLES ρδk1/2 The default value is 0.0854.
	grid_scale		A flag indicating the method of computing the characteristic grid scale.     1    delta = max(dx,dy,dz) 2 delta = volume1/3 The default value is 1.

Partially Resolved Numerical Simulation (PRNS)

PRNS [RCP Rcp] [zone_selector]

The PRNS keyword may be used with the Spalart-Allmaras and SST models 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 Reynolds-averaged 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 papers by Liu and Shih [Liu, N.-S., and Shih, T.-H. (2006) "Turbulence Modeling for Very Large-Eddy Simulation," AIAA Journal, Vol. 44, No. 4, pp. 687-697] and by Shih, et. al. [Shih, T.-H., Liu, N.-S., and Chen, C.-L. (2006) "A Strategy for Very Large Eddy Simulation of Complex Turbulent Flows," AIAA Paper 2006-175].

Detached PRNS

DETACHED-PRNS [RCP Rcp] [DPRNS dprns] [zone_selector]

This keyword is similar to the PRNS keyword described above, but may only be used with the Spalart-Allmaras 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 "near-wall" region is given by