The Advanced Solution Controls dialog box allows you to set parameters related to the multigrid, multi-stage, and non-iterative solvers.

Controls
tab contains parameters related to the multigrid solver. See Modifying Algebraic Multigrid Parameters and Setting FAS Multigrid Parameters for details about the items below.
contains a drop-down list for each equation that is being solved. From this list you can select the multigrid cycle type (Flexible, V-Cycle, W-Cycle, or F-Cycle). See Specifying the Multigrid Cycle Type for details.
Note that, for the density-based solvers, the Pressure, Momentum, and Energy equations will not appear individually. They will instead be grouped together and called Flow.
Furthermore, for the density-based explicit solver, the Cycle Type choices for the Flow equations will be limited to V-Cycle and W-Cycle, while the choices for Flow for the density-based implicit solver will be limited to V-Cycle and F-Cycle.
specifies the termination criterion for each equation that is being solved using algebraic multigrid. See Setting the Termination and Residual Reduction Parameters for details.
specifies the residual reduction criterion for each equation that is being solved using the Flexible algebraic multigrid cycle. See Setting the Termination and Residual Reduction Parameters for details. (This item will not appear for an equation that is using a V-Cycle, W-Cycle, or F-Cycle.)
contains the drop-down list to choose the stabilization method.
enables bi-conjugate gradient stabilized method.
enables the recursive projection method. RPM stabilization is mainly used in conjunction with the coupled pressure-based solver.
enables the conjugate gradient method. CG stabilization is mainly used in conjunction with the segregated pressure-based solver.
contains parameters related to the algebraic multigrid solver. See Algebraic Multigrid (AMG) in the Theory Guide and Modifying Algebraic Multigrid Parameters for details.
contain parameters that you can set, If you are using the density-based explicit solver or the pressure-based solver with any of the segregated schemes, described in Pressure-Velocity Coupling in the Theory Guide and Choosing the Pressure-Velocity Coupling Method, you will only set Scalar Parameters. If you are using the density-based implicit or the pressure-based coupled scheme, described in Coupled Algorithm, then you can set the Coupled Parameters.
contains parameters that control the V, W, and F cycles. You can set the number of Pre-Sweeps and Post-Sweeps, and the Max Cycles. Normally one post-sweep is performed and no pre-sweeps are done. See Fixed Cycle Parameters for details about using the items below.
sets the number of sweeps to perform before moving to a coarser level.
sets the number of sweeps to perform after coarser level corrections have been applied.
sets the maximum number of V, W, or F cycles to be performed. The multigrid solver will continue to solve the set of equations until either the maximum number of cycles has been performed, or the Termination criteria are satisfied.
contains parameters that control the grouping of equations in the algebraic multigrid algorithm. See Coarsening Parameters for details
is the maximum number of coarse levels that will be built by the multigrid solver. Sets of coarser simultaneous equations are built until the maximum number of levels has been created, or the coarsest level has only 3 equations. Each level has about half as many unknowns as the previous level, so coarsening until there are only a few nodes left will require about as much total coarse-level coefficient storage as was required on the fine mesh. Reducing the maximum coarse levels will reduce the memory requirements, but may require more iterations to achieve a converged solution. Setting Max Coarse Levels to 0 turns off the multigrid solver.
controls the number of equations on each successively
coarser grid level. By default, this parameter is set to 2, indicating
that the number of equations on each level will be 1/2 of the number
on the previous level. In general, the number of equations on each
coarser grid level will be equal to 1/ of the number on the previous
level, where
is the value set for the Coarsen by parameter.
enables the use of conservative coarsening techniques that can improve parallel performance and/or convergence for some difficult cases. This option is only available under Coupled Parameters.
enables the use of Laplace coefficients when grouping cells for coarsening.
consist of two types:
is the simplest smoother type and is recommended when using the pressure-based segregated solver.
is more CPU intensive, but has better smoothing properties for block-coupled systems such as the pressure-based coupled solver and the density-based implicit solver.
contains parameters that control the flexible multigrid cycle.
specifies the number of times to apply the smoothing method each time a relaxation is performed.
sets the maximum number of relaxations to be performed
on the Level 1 grid (fine grid level). This parameter eliminates the
possibility that the Gauss-Seidel solver will get “stuck”
on the fine grid level, unable to reduce the residuals by the fraction
() required by the Termination criteria.
sets the maximum number of relaxations to be performed
on each grid level above Level 1 (that is, the coarse grid levels).
This parameter eliminates the possibility that the Gauss-Seidel solver
will get “stuck” on a coarse grid level, unable to reduce
the residuals on that level by the fraction () required by the Termination criteria. If the iterative solution on a given
grid level is unable to meet the accuracy constraint of the Termination criteria, the correction equation will be
deemed “converged” when this maximum number of relaxations
on that grid level has been performed.
contains additional multigrid parameters.
controls the amount of information that is printed out by the multigrid solver for monitoring purposes. See Setting the Verbosity for details
contains parameters related to the FAS multigrid solver. See Full-Approximation Storage (FAS) Multigrid in the Theory Guide and Setting FAS Multigrid Parameters for details. As noted in the title of this dialog box section, the FAS multigrid solver is used only for the Flow equations (pressure, momentum, and energy).
This section of the dialog box appears only when the density-based explicit solver is used.
contains parameters that control the V, W, and F cycles of the FAS multigrid solver.
sets the number of iterations of the multi-stage solver
to be performed on a given grid level before proceeding to a coarser
grid level (the value of described
in Multigrid Cycles in the Theory Guide). Typically, this is set to 1.
sets the number of multigrid cycles to be performed
on a given grid level before proceeding back up to the finer grid
level (the value of described
in Multigrid Cycles in the Theory Guide). A value of 1 results in V-cycle multigrid, and a value of 2 results
in W-cycle multigrid.
contains parameters that control the grouping of cells in the FAS multigrid algorithm.
sets the maximum number of grid levels to be used in the multigrid process. A value of 0 disables multigrid (no coarse grid levels). If the coarse grids do not already exist, they are created automatically when you start iterating; you cannot create them by clicking the button. See Turning On FAS Multigrid for details.
controls the number of cells in each successively
coarser grid level. By default, this parameter is set to 2, indicating
that the number of cells on each level will be 1/2 of the number on
the previous level. In general, the number of cells on each coarser
grid level will be equal to 1/ of the number on the previous level, where
is the value set for the Coarsen by parameter.
are provided to moderate and stabilize the multigrid corrections.
sets the factor by which to reduce the Courant number for coarse grid levels (that is, every level except the finest). Some reduction of time step (such as the default 0.9) is typically required because the stability limit cannot be determined as precisely on the irregularly shaped coarser grid cells.
sets the factor by which to reduce the magnitude of
the multigrid corrections transferred from one level to the next finer
level. A typical value with is 0.6. If two Pre-Sweeps and two Post-Sweeps are
performed, this value can often be increased to 1.0 (that is, full
correction transfer).
sets the factor by which to reduce the magnitude of the species corrections to stabilize the multigrid calculation. This item appears only when species transport is being modeled.
sets the correction smoothing factor used to interpolate corrections from a coarser grid to a finer grid. For multigrid on structured meshes, corrections can be interpolated up to a finer mesh “smoothly” by using, for example, tri-linear interpolation. For unstructured meshes there is no analogous simple, algebraic procedure that can be used to interpolate without introducing substantial high frequency “noise”. Instead, the corrections are first interpolated, and then subjected to a smoothing pass. The default Correction Smoothing value of 0.5 should be acceptable for all cases; you should not need to change it.
contains additional multigrid parameters.
controls the amount of information that is printed out by the multigrid solver for monitoring purposes.
tab allows you to set parameters that govern the operation of the multi-stage solver. It is available only when the density-based explicit solver is used. See Changing the Multi-Stage Scheme for details about the items below.

Controls
is the number of stages used in the multi-stage scheme.
The default scheme is a 3-stage scheme with coefficients of 0.2075,
0.5915, and 1.0 for the first through third stages, respectively.
Although the dialog box limits the maximum number of stages to five,
you can define a scheme with an arbitrary number of stages with the solve/set/multi-stage text command.
labels the stage to which the parameters in the other columns apply.
sets the multi-stage coefficient for each stage. Coefficients should be greater than zero and less than one. The final stage should always have a coefficient of 1.
sets the stages for which artificial dissipation is evaluated. If a Dissipation box is selected for a particular stage, artificial dissipation will be updated on that stage. If not selected, artificial dissipation will remain “frozen” at the value of the previous stage.
sets the stages for which viscous stresses are evaluated. If a Viscous box is selected for a particular stage, viscous stresses will be updated on that stage. If not selected, viscous stresses will remain “frozen” at the value of the previous stage. Viscous stresses should always be computed on the first stage, and successive evaluations will increase the “robustness” of the solution process, but will also increase the expense (that is, increase the CPU time per iteration). For steady problems, the final solution is independent of the stages on which viscous stresses are updated.
sets the fields to their default values, as assigned by ANSYS Fluent. After execution, the Default button becomes the Reset button.
resets the fields to their most recently saved values (that is, the values before Default was selected). After execution, the Reset button becomes the Default button.
tab contains specialized parameters for limiting spatial discretization, as well as controls for the non-iterative solver.

Controls
contains controls for limiting the spatial discretization. See Selecting Gradient Limiters for more information about limiters.
selects the type of limiter applied to the spatial discretization: Standard, Multidimensional, or Differentiable.
is where the limited value of the reconstruction gradient is determined at the cell face centers. This is the default method.
is where the limited value of the reconstruction gradient is determined along a scaled line between two adjacent cell centroids. On an orthogonal mesh (or when the cell-to-cell direction is parallel to face area direction), this method becomes equivalent to the default cell to face method. For smooth field variation, cell to cell limiting may provide less numerical dissipation on meshes with skewed cells.
enables the limiter filter. The limiter filter is only available with the Standard and Differentiable limiter types.
allows you to select and modify the parameters for each individual equation. See Setting Solution Controls for the Pseudo Transient Method for details.
enables/disables the equation-specific steady state solution method for a particular equation.
allows you to use the standard steady state method by turning off pseudo transient for that particular equation. Specify the corresponding under-relaxation factor to be employed with a particular equation.
allows you to specify a factor that scales the pseudo time step employed for the flow equations specified in the Run Calculation task page. A time scale factor other than 1.0 (default) allows the use of an equation specific time step in lieu of using a uniform global pseudo time step.
contain parameters that control the sub-iterations for the individual equations. See Time-Advancement Algorithm in the Theory Guide for details.
provide control over the maximum number of sub-iterations for each individual equation.
defines the overall accuracy.
controls the solution of the linear equations.
sets the fields to their default values, as assigned by ANSYS Fluent. After execution, the Default button becomes the Reset button.
resets the fields to their most recently saved values (that is, the values before Default was selected). After execution, the Reset button becomes the Default button.