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
  • TURBULENCE - Turbulence model selection
• Wall Distance
  • MAX_WALL_DISTANCE - Maximum Wall Distance
• Viscosity Limiter
  • MUT LIMITER - Maximum allowed value of the turbulent viscosity. See Also: K-E MAXIMUM [TURBULENT] VISCOSITY
• Spalart-Allmaras and Goldberg Keywords
  • FREE_ANUT - Freestream eddy viscosity
• SST Keywords
  • COMPRESSIBLE [DISSIPATION], PRESSURE [DILATATION] - Compressibility correction options
  • FREE_K, FREE_OMEGA - Freestream k and ω
  • SST COEF_PTM1 - Transition model production term modification
• k-ε Keywords (structured grids only, except as noted)
  • K-E FREE_K, K-E FREE_MUT - Freestream k and μ_t (Both structured and unstructured)
  • K-E INITIALIZE - Initialization procedure
  • 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 Modified DES Model
  • DDES - Spalart Delayed 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)

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.

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. 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 common options that may be specified with the TURBULENCE keyword are:

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, DEBUG 82, DEBUG 83, TEST 21, TEST 67

Wall Distance

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^−1/5L_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 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., 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

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 Corrections

If TURBULENCE SST {COMPRESSIBLE | TRANSITION} is specified, the 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.

• [Suzen, Y. B., and Hoffmann, K. A. (1998) "Investigation of Supersonic Exhaust Flow by One- and Two-Equation Turbulence Models," AIAA-98-0322]

Specifying Freestream k and ω

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:

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.

These inflow values will be used to initialize the flow. For structured grids, k-ω values on the freestream boundary are only updated when outflow occurs. As long as flow continues entering through the boundary these values will persist. 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 re-establish itself as entering the domain, the boundary values will no longer be those initially specified. This is a current limitation of the structured solver. For unstructured grids, k-ω values on the inflow boundary are updated each cycle with the freestream the values specified.

Inflow turbulence levels may also 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

Production Term Modification

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.

Chien and Rumsey-Gatski k-ε Models

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.

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 FROM FREESTREAM keyword). The interpretation of the input depends on the signs of val1 and val2.

For the turbulence kinetic energy k_∞,

and for the turbulent viscosity (μ_t)_∞,

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 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/ft-s, respectively.

For structured grids, the k-ε models extrapolate to get turbulence values at all inflow and outflow boundaries. Thus, K-E FREE_K and K-E FREE_MUT can be used to initialize the flow, but not to specify inflow conditions.

For unstructured grids, the default setting for K-E FREE_MUT is -5 and -50 for the Goldberg realizable and Shih k-ε 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.

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.

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.

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

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.

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.

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.

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.

The compressibility corrections of Sarkar and Wilcox 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.

• [Sarkar, S., Erlebacher, G. and Hussaini, M. Y. and Kreiss, H. O. (1991) "The Analysis and Modeling of Dilatational Terms in Compressible Turbulence," Journal of Fluid Mechanics, Vol. 227, pp. 473-493]
• [Wilcox, D. C. (1992) "Dilatation-Dissipation Corrections for Advanced Turbulence Models," AIAA Journal, Vol. 30, No. 11, pp. 2639-2646]

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]

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.

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

Realizable and Shih k-ε Models

The specification of the freestream turbulence levels is identical to that described above. However, for unstructured grids, the default setting for K-E FREE_MUT is -5 and -50 for the Goldberg realizable and Shih k-ε models respectively. Also note that these unstructured k-ε solvers will maintain the boundary values, rather than extrapolate like the structured k-ε solvers do.

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
   TURBULENCE SST LESB ZONE 3
   CFL# 1.3
   TIMESTEP SECONDS 5.0E-6 ZONE 3

Spalart DES Model

[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 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 this coefficient increases the size of the region in which the DES model reduces to the standard Spalart-Allmaras model. Details may be found in the following papers:

• [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]
• [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

[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

[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.

• [Spalart, P. R., Deck, S., Shur, M. L., Squires, K. D., Strelets, M., and Travin, A. (2006) "A New Version of Detached-Eddy Simulation, Resistant to Ambiguous Grid Densities," Theoretical and Computational Fluid Dynamics, Vol. 20, pp.181-195.]

SST with ε Limiter

[Note - This option must appear on the same line as the TURBULENCE keyword.]

The LESB keyword option 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.

• [Bush, R. H., and Mani, M. (2001), "A Two-Equation Large Eddy Stress Model for High Sub-Grid Shear," AIAA Paper 2001-2561]

See Also: TEST 15

Nichols-Nelson Hybrid Model

[Note - This option must appear on the same line as the TURBULENCE keyword.]

The HYBRID keyword option 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 2003-0083]

Partially Resolved Numerical Simulation (PRNS)

[Note - This option must appear on the same line as the TURBULENCE keyword.]

The PRNS keyword option may be used with the Spalart-Allmaras 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 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 following papers:

• [Liu, N.-S., and Shih, T.-H. (2006) "Turbulence Modeling for Very Large-Eddy Simulation," AIAA Journal, Vol. 44, No. 4, pp. 687-697]
• [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

[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 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