To have further control over the parameters for each individual equation, when solving a pseudo transient case, you can go to the Expert tab, in the Advanced Solution Controls dialog box (Figure 28.20: The Advanced Solution Controls Dialog Box for the Pseudo Transient Method). Note that all equations, except for flow equations (that is pressure and momentum) will be listed. Generally, you will not need to visit this dialog box to enter equation-specific solution parameters. However, it may help in cases where a particular equation is giving convergence problems. Here, ANSYS Fluent allows two options to improve convergence:
Specify a time scale factor for the equation specific time step in lieu of using a uniform global pseudo time step. This scaling factor scales the pseudo time step employed for the flow equations specified in the Run Calculation task page (see Solving Pseudo-Transient Flow).
Use the standard steady-state method by turning off pseudo transient for that particular equation. Here, the corresponding under-relaxation factor to be employed with that equation may be specified. The default values of under-relaxation parameters for all variables are set to values that work well for most of the cases.
The default setting will have the pseudo transient method turned on for all equations with the corresponding time scale factor set to unity, except when one of the combustion models is used. When the pseudo transient method is enabled In combustion cases the species, enthalpy, and combustion variable equations will only use the pseudo transient method if it is manually enabled in the Expert tab. As well, when using the premixed, partially-premixed, or PDF combustion models, the energy equation will only use the pseudo transient method if it is manually enabled in the Expert tab.
By default, all user-defined scalars (UDS) have pseudo transient method disabled. This is because the physical parameters of the UDS and the appropriate time scale are not known to the solver before starting the calculation. You can manually enable pseudo transient method for UDS under the Expert tab in the Advanced Solution Controls Dialog Box.
Solution
→ Controls
Advanced...
Specify the equation-specific steady-state solution method for a particular equation (if needed) by enabling or disabling the pseudo transient method using the On/Off check box next to the equation. The dialog box then allows either specification of a pseudo Time Scale Factor or Under-Relaxation Factor for that particular equation based on the check box setting.
Note: For multiphase flows, the pseudo transient expert options for the volume fraction equation are available only when it is solved in segregated fashion. It is not available when the Coupled with Volume Fractions option is enabled in the Solution Methods task page (see Selecting the Pressure-Velocity Coupling Method for information about this setting).