(for the pressure-based solver only) provides a drop-down list of the available pressure-velocity coupling schemes: SIMPLE, SIMPLEC, PISO, and Coupled. When the non-iterative time advancement (NITA) scheme is enabled in the Solution Methods task page, Fractional Step is available for single phase flows, and Phase Coupled SIMPLE is available for Eulerian multiphase flows. See Pressure-Velocity Coupling in the Fluent Theory Guide, and Choosing the Pressure-Velocity Coupling Method, Setting Solution Controls for the Non-Iterative Solver, and Selecting the Pressure-Velocity Coupling Method for details about these methods.

enables the SIMPLEC and PISO skewness correction for highly skewed meshes if the value (number of iterations) is greater than 0. The default value is 0 for SIMPLEC and 1 for PISO.

enables the PISO neighbor correction, which is recommended for transient calculations, if the value (number of iterations) is greater than 0. The default value is 1.

allows for a more economical but a less robust variation of the PISO algorithm.

couples velocity corrections, shared pressure corrections, and the correction for volume fraction simultaneously. This option is available in the interface after you have selected Coupled from the Scheme drop-down list for Pressure-Velocity Coupling.

solves all primary and secondary volume fraction equations and scales the resulting volume fractions to satisfy the requirement that they sum to 1. If this is disabled, only the secondary phase volume fractions are solved directly and the primary phase volume fraction is set such that the volume fractions sum to 1.

(for the pressure-based solver) provides a drop-down list of the mass flux types: Rhie-Chow: distance based and Rhie-Chow: momentum based. Details about each of the flux types can be found in Discretization of the Continuity Equation in the Theory Guide. You cannot change the selection if Auto Select is enabled. For multiphase models other than the wet steam model, this list is not available and the Rhie-Chow: momentum based flux option is used.

enables the automatic selection of the Flux Type, so that the most robust formulation is used for the flow models and mesh attributes of your case (for details, see Mass Flux Types). This option is enabled by default.

contains a drop-down list of the options for setting the method of computing the gradient in Equation 23–30 in the Theory Guide: Green-Gauss Cell Based; Green-Gauss Node-Based, and Least Squares Cell Based. See Evaluation of Gradients and Derivatives in the Theory Guide for details.

(for the pressure-based solver only) contains a drop-down list of the discretization schemes available for the pressure equation: Standard, PRESTO!, Linear, Second Order, Body Force Weighted, and Modified Body Force Weighted.

This item appears only when the pressure-based solver is used.

(for the density-based solvers only) contains a drop-down list of the discretization schemes available for the pressure, momentum, and (if relevant) energy equations: First Order Upwind, Second Order Upwind, Third-Order MUSCL, and (if the LES, DES, SAS, SDES, or SBES turbulence model is enabled) Bounded Central Differencing.

This item appears only when one of the density-based solvers is used.

are the names of the other convection-diffusion equations being solved. In the drop-down list next to each equation, you can select the First Order Upwind, Second Order Upwind, QUICK, or Third-Order MUSCL discretization scheme for that equation.

If the LES, DES, SAS, SDES, or SBES turbulence model is enabled, then you have a choice of selecting Bounded Central Differencing or Central Differencing for Momentum. If Bounded Central Differencing is selected, an entry field BCD Scheme Boundedness appears under the Spatial Discretization group box.

If one of the density-based solvers is used, Momentum and Energy will not appear. For the density-based solvers, the discretization scheme for these equations is selected in the Flow drop-down list (described above).

specifies the boundedness strength of the BCD scheme as a constant or an expression. In the latter case, the field variable BCD Scheme Boundedness is created in the Derivatives category and can be visualized.

is available when the VOF multiphase model is enabled. The discretization schemes that are used when solving volume fraction equations for the VOF explicit scheme are Geo-Reconstruct, Compressive, CICSAM, Modified HRIC, and QUICK. The discretization schemes that are used when solving volume fraction equations for the VOF implicit scheme are First Order Upwind, Second Order Upwind, Compressive, Modified HRIC, BGM (steady state only), and QUICK. See Interpolation Near the Interface in the Theory Guide for detailed information about these VOF-specific interpolation schemes.