The Solution Methods task page allows you to specify various parameters associated with the solution method to be used in the calculation.

Controls
provides a drop-down list of the available types of solver formulations: Implicit and Explicit.
This item appears only when the density-based solver is used.
provides a drop-down list of the convective flux types: Roe-FDS, AUSM, and Low Diffusion Roe-FDS. Details about each of the flux types can be found in Convective Fluxes in the Theory Guide.
contains settings for pressure-velocity coupling schemes.
(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.
contains settings that control the spatial discretization of the convection terms in the solution equations. See Choosing the Spatial Discretization Scheme for details.
contains a drop-down list of the options for setting the method of computing the gradient in Equation 21–33 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, and 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, and Third-Order MUSCL.
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, Power Law, 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 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).
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.
contains options for setting different time-dependent solution formulations. This option appears only when Transient is enabled under Time in the General task page. Available options include: Explicit (available only for the Density Based Explicit solver); First Order Implicit; Second Order Implicit; and Bounded Second Order Implicit. See Performing Time-Dependent Calculations for details.
enables non-iterative time-advancement (NITA) scheme. See Time-Advancement Algorithm in the Theory Guide for details.
enables an option to discretize the convective part of Equation 21–67 in the Theory Guide using the mass flux at the cell faces from the previous time level n. This option is available only for a Transient solution. See The Frozen Flux Formulation in the Theory Guide for details.
enables an option to apply the pseudo transient under-relaxation method, which is a form of implicit under-relaxation (see Pseudo Transient Under-Relaxation). This option is available for the pressure-based solver when Coupled is selected as the Pressure-Velocity Coupling scheme and for the density-based implicit solver. Note that this method can only be used when running a steady-state simulation.
enables an adjustment to the gradient discretization method that improves the gradient accuracy for meshes containing high aspect ratios, cells with non-flat faces, and highly deformed cells. By default, the fast, or more computationally efficient mode of the warped-face gradient correction is used. For additional information about the warped-face gradient correction, see Warped-Face Gradient Correction.
Enable convergence acceleration for stretched meshes to improve the convergence of the implicit density based solver on meshes with high cell stretching (see Convergence Acceleration for Stretched Meshes (CASM)).
enables the relaxation of high order terms to aid in the solution behavior of flow simulations when higher order spatial discretization is used.
Opens the Relaxation Options Dialog Box.
enables an option to use the same discretization scheme for all the species rather than setting each of the species individually. Notice that you will no longer see your list of individual species, instead a Species field will appear with the scheme of your choice. Note that this option is available when species transport is enabled.
sets the fields to their default values, as assigned by ANSYS Fluent.
reports statistics on the number and type of cells that ANSYS Fluent has identified as having poor quality.