[Fluent Inc. Logo] return to home search
next up previous contents index

32.4.1 Solve/Controls/Solution...

The Solve/Controls/Solution... menu item opens the Solution Controls panel.



Solution Controls Panel


The Solution Controls panel allows you to set common solution parameters.

figure

Controls

Equations   contains a list of the equations being solved for the current model. To temporarily disable solution of an equation, deselect it in this list. To re-enable the calculation for an equation, select it. See Section  25.22.2 for details about using this feature in a step-by-step solution process.

Note that, when one of the density-based solvers is used, Energy will not appear as a separate item in the Equations list. For the density-based solvers the energy equation is included in the Flow category (which also includes the pressure and momentum equations).

Under-Relaxation Factors   contains the under-relaxation factors for all equations that are being solved with the pressure-based solver. (See Section  25.9.2 for details.) In the field next to each equation, you can set the under-relaxation factor for that equation.

When one of the density-based solvers is used, Under-Relaxation Factors will appear only for the following variables, when they are included in your model: solid (for conjugate heat transfer models), turbulence variables, and viscosity. The density-based solvers use a segregated method to solve these equations; all the other equations are solved in a coupled manner, so there are no under-relaxation factors for them.

Non-Iterative Solver Controls   contain parameters that control the sub-iterations for the individual equations.
Max. Corrections   provide control over the maximum number of sub-iterations for each individual equation.

Correction Tolerance   defines the overall accuracy.

Residual Tolerance   controls the solution of the linear equations.

Relaxation Factor   defines the explicit relaxation (Section  25.4.4) of variables between sub-iterations and are used to prevent the solution from diverging.

Pressure-Velocity Coupling   contains a drop-down list of the available pressure-velocity coupling schemes: SIMPLE, SIMPLEC, PISO, and Coupled. Fractional Step is available in the drop-down list when the non-iterative time advancement (NITA) scheme is enabled in the Solver panel. See Section  25.9.1, 25.4.3, and 25.9.3 for details about these methods.

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

Skewness Correction   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.

Neighbor Correction   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.

Skewness-Neighbor Coupling   allows for a more economical but a less robust variation of the PISO algorithm.

Courant Number   for the Coupled scheme is used to stabilize the convergence behavior. See Section  25.4.4 for a correlation of the under-relaxation factor and courant number.

Explicit Relaxation Factors   for the Coupled scheme defines the explicit relaxation of variables between sub-iterations for momentum and pressure. See Section  25.4.4 for information.

Solver Parameters   contains solution parameters that are relevant only for the density-based solvers. This section of the panel will not appear if you are using the pressure-based solver.

Courant Number   sets the fine-grid Courant number (time step factor). See Section  25.10.1 for guidelines on setting the Courant number.

Flux Type   consists of three convective flux types: Roe-FDS, AUSM, and Low Diffusion Roe-FDS. Details about each of the flux types can be found in Section  25.5.3.
Roe-FDS   splits the fluxes in a manor that is consistent with their corresponding flux method eigenvalues. It is the default and is recommended for most cases.

AUSM   provides exact resolution of contact and shock discontinuities and it is less susceptible to Carbuncle phenomena.

Low Diffusion Roe-FDS   is used when the LES viscous model is enabled. It reduces the dissipation in LES calculations and is used only for subsonic flows.

Multigrid Levels   specifies the maximum number of coarse levels to be created by the FAS multigrid solver. This item is the same as the Max Coarse Levels under FAS Multigrid Controls in the Multigrid Controls panel, and it appears only when the density-based explicit solver is used.

Residual Smoothing   contains parameters that govern the use of implicit residual smoothing. (See Sections  25.10.3 and 25.5.4 for details.) This section of the panel will appear only when the density-based explicit solver is used.

Iterations   sets the number of iterations of the Jacobi smoother to use. If Iterations is 0, then no implicit residual smoothing is performed.

Smoothing Factor   sets the implicit residual smoothing factor. This item will not appear unless Iterations is set to a non-zero value.

Discretization   contains settings that control the discretization of the convection terms in the solution equations. See Section  25.8 for details.

Pressure   (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.

Flow   (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.

Momentum, Energy, etc.   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 turbulence model is enabled, then you have a choice of selecting Bounded Central Differencing or Central Differencing to solve the convection-diffusion equations.

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).

Volume Fraction   is available when the VOF multiphase model is enabled. The discrtetization schemes that are used when solving volume fraction equations for the VOF explicit scheme are Geo-Reconstruct, CICSAM, Modified HRIC, and QUICK. The discrtetization schemes that are used when solving volume fraction equations for the VOF implicit scheme are First Order Upwind, Second Order Upwind, Modified HRIC, and QUICK. See Section  23.3.2 for detailed information about these VOF-specific interpolation schemes.

Default   sets the fields to their default values, as assigned by FLUENT. After execution, the Default button becomes the Reset button.

Reset   resets the fields to their most recently saved values (i.e., the values before Default was selected). After execution, the Reset button becomes the Default button.


next up previous contents index Previous: 32.4 Solve Menu
Up: 32.4 Solve Menu
Next: 32.4.2 Solve/Controls/Multigrid...
© Fluent Inc. 2006-09-20