26.3.3 Setting Solution Controls for the Non-Iterative Solver

You can use the non-iterative solver (see this section in the separate Theory Guide) for transient problems in order to increase the speed and efficiency of the calculations.

The settings for the non-iterative solver should provide control over the maximum number of sub-iterations for each individual equation. The criteria for convergence include the Correction Tolerance (defined by the overall accuracy), Residual Tolerance (controlling the solution of the linear equations), and the individual Relaxation Factor. The default control settings are optimally designed in order to get a second-order accurate solution. These controls are accessible via the Expert tab, in the Advanced Solution Controls dialog box (Figure  26.3.2).

To use ANSYS FLUENT's non-iterative transient solver in order to boost the efficiency of transient simulations:

1.   Go to the Solution Methods task Page.

Solution Methods

2.   Enable Non-Iterative Time-Advancement.

3.   Under Pressure-Velocity Coupling, you can choose either the Fractional Step or PISO scheme. Under Non-Iterative Solver Controls (Figure  26.3.2), you will see parameters that control the sub-iterations for individual equations (see below). When you select the PISO scheme, you can set the value for the Neighbor Correction. Skewness correction is performed automatically.

User Inputs

You can modify the non-iterative solution controls in the Advanced Solution Controls dialog box (Figure  26.3.2).

Solution Controls Advanced...

Figure 26.3.2: The Advanced Solution Controls Dialog Box for the Pressure-Based Segregated Non-Iterative Solver

Under Non-Iterative Solver Controls, there are several parameters that control the sub-iterations for the individual equations.

The sub-iterations for an equation stop when the total number of sub-iterations exceeds the value specified for Max. Corrections, regardless of whether or not the convergence criteria (described below) are met.

The sub-iterations for an equation end when the ratio of the residuals at the current sub-iteration and the first sub-iteration is less than the value specified in the Correction Tolerance field. You can monitor the details of the sub-iteration convergence by looking at the AMG solver performance (i.e., setting the Verbosity field in the Multigrid tab in the Advanced Solution Controls dialog box to 1). Be sure to pay attention to the residuals for the current sub-iteration (i.e., the residual for the 0-th AMG cycle at the current sub-iteration) and the initial residual of the time step (i.e., the residual for the 0-th AMG cycle of the first sub-iteration). The ratio of these two residuals is what is controlled by the Correction Tolerance field. These two residuals are also the residuals plotted when using the Residual Monitor panel and reported in the ANSYS FLUENT console at the end of a time step. Note that the residuals reported at the end of a time step can be scaled or unscaled, depending on the settings in the Residual Monitor dialog box. The residuals reported when monitoring the AMG solver performance are always unscaled.

For each interim sub-iteration, the AMG cycles continue until the usual AMG termination criteria (0.1 by default, and set in the Multigrid tab) are met. However, for the last sub-iteration (i.e., either when the maximum number of sub-iterations are reached or when the correction tolerance is satisfied), the AMG cycles continue until the ratio of the residual at the current cycle to the initial residual (the residual for the 0-th AMG cycle of the first sub-iteration of the time step) drops below the value specified for Residual Tolerance. You may want to adjust the Residual Tolerance, depending on the time step selected. The default Residual Tolerance should be well suited for moderate time steps (i.e., for cell CFL numbers of 1 to 10). Note that you can display the cell CFL numbers for unsteady problems by selecting Cell Courant Number in the Velocity... category of all postprocessing dialog boxes. For very small time steps (cell CFL $<<$1), the diagonal dominance of the system is very high and the convergence should be driven further by reducing the Residual Tolerance value. For larger time steps (cell CFL $>>$1), it may be possible that the residual tolerance cannot be reached due to round-off errors, and unless the Residual Tolerance value is increased, AMG cycles can be wasted. Again, this can be monitored by monitoring the AMG solver performance.

The Relaxation Factor field defines the explicit relaxation (see this section in the separate Theory Guide) of variables between sub-iterations. The relaxation factors can be used to prevent the solution from diverging. They should be left at their default values of 1, unless divergence is detected. If the solution diverges, you should first try to stabilize the solution by lowering the relaxation factors for pressure to 0.7- 0.8, and by reducing the time step.

The following is a list of models that are compatible with the non-iterative solver:

• Inviscid flow (excluding ideal gas)

• Laminar flow

• All models of turbulence (including LES and DES), except RSM

• S2S radiation model

• Heat transfer

• Non-reacting species transport

• General compressible flows (most subsonic and some transonic applications)

• VOF multiphase model (most applications)

• Phase change (solidification and melting)

• Porous media model (isotropic resistance)

The following is a list of models that are compatible with the non-iterative solver, but may result in some instabilities and inaccuracies for certain flow conditions:

• MDM

• Non-Newtonian fluids

• General compressible flows (aerospace supersonic applications)

• Floating operating pressure

• Reacting species and any type of combustion including PDF

The following is a list of models that are not compatible with the non-iterative solver:

• Eulerian multiphase (all non-VOF models)

• Radiation models (except S2S)

• DPM, spark, and crevice models

• UDS transport

• Porous jump

• Porous media model (anisotropic resistance)

• RSM turbulence model

The PRESTO! pressure interpolation scheme, when used with the non-iterative time-advancement solver, is less stable than in the case of the iterative time-advancement solver. As a consequence, smaller time steps may be required.

As mentioned above, the default control settings are optimally designed to obtain a second-order solution. In order to save CPU time, in cases where transient accuracy is not a main concern (i.e., first-order integration in time and space), or when NITA is used to converge toward a steady state solution, you may want to set the Max. Corrections value to 1 in the Advanced Solution Controls dialog box ( Expert tab) for all transport equations except pressure.