        26.3.1 Choosing the Pressure-Velocity Coupling Method

ANSYS FLUENT provides four segregated types of algorithms: SIMPLE, SIMPLEC, PISO, and (for time-dependant flows using the Non-Iterative Time Advancement option (NITA)) Fractional Step (FSM). These schemes are referred to as the pressure-based segregated algorithm. Steady-state calculations will generally use SIMPLE or SIMPLEC, while PISO is recommended for transient calculations. PISO may also be useful for steady-state and transient calculations on highly skewed meshes. In ANSYS FLUENT, using the Coupled algorithm enables full pressure-velocity coupling, hence it is referred to as the pressure-based coupled algorithm. Pressure-velocity coupling is relevant only for the pressure-based solver.

SIMPLE vs. SIMPLEC

In ANSYS FLUENT, both the standard SIMPLE algorithm and the SIMPLEC (SIMPLE-Consistent) algorithm are available. SIMPLE is the default, but many problems will benefit from using SIMPLEC, particularly because of the increased under-relaxation that can be applied, as described below.

For relatively uncomplicated problems (laminar flows with no additional models activated) in which convergence is limited by the pressure-velocity coupling, you can often obtain a converged solution more quickly using SIMPLEC. With SIMPLEC, the pressure-correction under-relaxation factor is generally set to 1.0, which aids in convergence speed-up. In some problems, however, increasing the pressure-correction under-relaxation to 1.0 can lead to instability due to high mesh skewness. For such cases, you will need to use one or more skewness correction schemes, use a slightly more conservative under-relaxation value (up to 0.7), or use the SIMPLE algorithm. For complicated flows involving turbulence and/or additional physical models, SIMPLEC will improve convergence only if it is being limited by the pressure-velocity coupling. Often it will be one of the additional modeling parameters that limits convergence; in this case, SIMPLE and SIMPLEC will give similar convergence rates.

PISO

The PISO algorithm (see this section in the separate Theory Guide) with neighbor correction is highly recommended for all transient flow calculations, especially when you want to use a large time step. (For problems that use the LES turbulence model, which usually requires small time steps, using PISO may result in an increased computational expense, so SIMPLE or SIMPLEC should be considered instead.) PISO can maintain a stable calculation with a larger time step and an under-relaxation factor of 1.0 for both momentum and pressure. For steady-state problems, PISO with neighbor correction does not provide any noticeable advantage over SIMPLE or SIMPLEC with optimal under-relaxation factors.

PISO with skewness correction is recommended for both steady-state and transient calculations on meshes with a high degree of distortion.

When you use PISO neighbor correction, under-relaxation factors of 1.0 or near 1.0 are recommended for all equations. If you use just the PISO skewness correction for highly-distorted meshes (without neighbor correction), set the under-relaxation factors for momentum and pressure so that they sum to 1 (e.g., 0.3 for pressure and 0.7 for momentum). If you use both PISO methods, follow the under-relaxation recommendations for PISO neighbor correction, above.

For most problems, it is not necessary to disable the default coupling between neighbor and skewness corrections. For highly distorted meshes, however, disabling the default coupling between neighbor and skewness corrections is recommended.

Fractional Step Method

The Fractional Step method (FSM), described in this section in the separate Theory Guide , is available when you choose to use the NITA scheme (i.e., the Non-Iterative Time Advancement option in the Solution Methods task page). With the NITA scheme, the FSM is slightly less computationally expensive compared to the PISO algorithm. Whether you select FSM or PISO depends on the application. For some problems (e.g., simulations that use VOF), FSM could be less stable than PISO.

In most cases, the default values for the solution methods are enough to set a robust convergence of the internal pressure correction sub-iterations due to skewness. Only very complex problems (e.g., moving deforming meshes, sliding interfaces, the VOF model) could require a reduction of relaxation for pressure up to a value of 0.7 or 0.8.

Coupled

Selecting Coupled from the Pressure-Velocity Coupling drop-down list indicates that you are using the pressure-based coupled algorithm, described in this section in the separate Theory Guide. This solver offers some advantages over the pressure-based segregated algorithm. The pressure-based coupled algorithm obtains a more robust and efficient single phase implementation for steady-state flows. It is not available for cases using the Eulerian multiphase, NITA, and periodic mass-flow boundary conditions.

User Inputs

You can specify the pressure-velocity coupling method in the Solution Methods task page (Figure  26.2.1). Solution Methods

Choose SIMPLE, SIMPLEC, PISO, Fractional Step, or Coupled in the Pressure-Velocity Coupling drop-down list.

If you choose PISO, the task page will expand to show the additional parameters for pressure-velocity coupling. By default, the number of iterations for Skewness Correction and Neighbor Correction are set to 1. If you want to use only Skewness Correction, then set the number of iterations for Neighbor Correction to 0. Likewise, if you want to use only Neighbor Correction, then set the number of iterations for Skewness Correction to 0. For most problems, you do not need to change the default iteration values. By default, the Skewness-Neighbor Coupling option is enabled to allow for a more economical, but a less robust variation of the PISO algorithm.

If you choose SIMPLEC under Pressure-Velocity Coupling, you must also set the Skewness Correction, whose default value is 0.

If you choose Coupled, you will have to specify the Courant number in the Solution Controls task page, which is set at 200 by default. You will also specify the Explicit Relaxation Factors for Momentum and Pressure, which are set at 0.75 by default. For more information about these options, refer to this section and this section in the separate Theory Guide.

If high-order momentum discretization is used, you may need to decrease the explicit relaxation to 0.5. For cases with very skewed meshes, the run can be stabilized by further reduction of the explicit relaxation factor to 0.25. If ANSYS FLUENT immediately diverges in the AMG solver, then the CFL number is too high and should be reduced. Reducing the CFL number below 10 is not recommended since it would be better to use the segregated algorithm for the pressure-velocity coupling.

In most transient cases, the CFL number should be set to with an explicit relaxation of 1.0.     Previous: 26.3 Pressure-Based Solver Settings
Up: 26.3 Pressure-Based Solver Settings
Next: 26.3.2 Setting Under-Relaxation Factors
Release 12.0 © ANSYS, Inc. 2009-01-29