10. solve/

animate/

Enter the animation menu.

define/

Enter the animation definition menu.

define-monitor

Define new animation.

edit-monitor

Change animation monitor attributes.

playback/

Enter the animation playback menu.

delete

Delete animation sequence.

play

Play the selected animation.

read

Read new animation from file or already-defined animations.

write

Write animation sequence to the file.

dpm-update

Update discrete phase source terms.

dual-time-iterate

Perform unsteady iterations for a specified number of time steps.

execute-commands/

Enter the execute commands menu.

add-edit

Add or edit execute commands.

disable

Disable an execute command.

enable

Enable an execute command.

initialize/

Enter the flow initialization menu.

compute-defaults/

Enter the compute default values menu. You can select the type of zone from which you want to compute these values.

dpm-reset

Reset discrete phase source terms to zero.

fmg-initialization

Initialize using the full-multigrid initialization (FMG).

init-flow-statistics

Initialize unsteady statistics.

initialize-flow

Initialize the flow field with the current default values.

init-instantaneous-vel

Initialize unsteady velocity.

list-defaults

List default values.

repair-wall-distance

Correct wall distance at very high aspect ratio hexahedral/polyhedral cells.

set-defaults/

Set default initial values.

set-fmg-initialization/

Enter the set full-multigrid for initialization menu. Initial values for each variable can be set within this menu.

iterate

Perform a specified number of iterations.

mesh-motion

Perform mesh motion.

monitors/

Set solution monitors.

force/

Enter the force monitors menu.

clear-all-monitors-data

Discard the internal and external file data associated with the force monitors.

clear-drag-monitor-data

Discard the internal and external file data (if any exist) for the drag coefficient.

clear-lift-monitor-data

Discard the internal and external file data (if any exist) for the lift coefficient.

clear-moment-monitor-data

Discard the internal and external file data (if any exist) for the moment coefficient.

drag-coefficient

Set the parameters for monitoring the drag coefficient, including the list of wall zones on which to compute the coefficient, whether to print, plot, and/or write the data, the name of the output file (if appropriate), the plot window, and the force vector associated with the coefficient.

lift-coefficient

Set the parameters for monitoring the lift coefficient, including the list of wall zones on which to compute the coefficient, whether to print, plot, and/or write the data, the name of the output file (if appropriate), the plot window, and the force vector associated with the coefficient.

moment-coefficient

Set the parameters for monitoring the moment coefficient, including the list of wall zones on which to compute the coefficient, whether to print, plot, and/or write the data, the name of the output file (if appropriate), the plot window, the moment center associated with the coefficient, and which component of the moment vector to monitor.

monitor-unsteady-iters?

Specify (for transient calculations) whether the monitors are updated every iteration or every time step.

residual/

Enter the residual monitors menu.

check-convergence?

Choose which currently-monitored residuals should be checked for convergence.

convergence-criteria

Set convergence criteria for residuals that are currently being both monitored and checked.

criterion-type

Set convergence criterion type.

monitor?

Choose which residuals to monitor as printed and/or plotted output.

n-display

Set the number of most recent residuals to display in plots.

n-maximize-norms

Set the number of iterations through which normalization factors will be maximized.

normalization-factors

Set normalization factors for currently-monitored residuals (if normalize? is set to yes).

normalize?

Choose whether to normalize residuals in printed and plotted output.

n-save

Set number of residuals to be saved with data. History is automatically compacted when buffer becomes full.

plot?

Choose whether residuals will be plotted during iteration.

print?

Choose whether residuals will be printed during iteration.

relative-conv-criteria

Set relative convergence criteria for residuals that are currently being both monitored and checked.

re-normalize

Re-normalize residuals by maximum values.

reset?

Choose whether to delete the residual history and reset iteration counter to 1.

scale-by-coefficient?

Choose whether to scale residuals by coefficient sum in printed and plotted output.

window

Specify window in which residuals will be plotted during iteration.

statistic/

Enter the statistic monitors menu.

monitors

Choose which statistics to monitor as printed and/or plotted output.

plot?

Choose whether or not statistics will be plotted during iteration.

print?

Choose whether or not statistics will be printed during iteration.

window

Specify first window in which statistics will be plotted during iteration. Multiple statistics are plotted in separate windows, beginning with this one.

surface/

Contains commands to control surface monitoring.

clear-data

Clear current surface monitor data.

clear-monitors

Remove all defined surface monitors.

curves/

Enter the curves menu.

lines

Set lines parameters for surface monitors.

markers

Set markers parameters for surface monitors.

list-monitors

List defined surface monitors.

set-monitor

Define or modify a surface monitor.

volume/

Contains commands to control volume monitoring.

clear-data

Clear current volume monitor data.

clear-monitors

Remove all defined volume monitors.

list-monitors

List defined volume monitors.

set-monitor

Define or modify a volume monitor.

patch

Patch a value for a flow variable in the domain.

set/

Enter the set solution parameters menu.

adaptive-time-stepping

Set adaptive time stepping parameters.

bc-pressure-extrapolations

Set pressure extrapolations schemes on boundaries.

If you are using the density-based solver, you will be asked the following questions:

extrapolate total quantities on pressure-outlet boundaries?

The default is [no]. If you enter yes, and the flow leaving the pressure outlet is subsonic, then the total pressure and total temperature from the domain's interior are extrapolated to the boundary and used with the imposed static pressure to determine the full thermodynamic state at the boundary.

extrapolate pressure on pressure-inlet boundary?

The default is [no]. If you enter yes, then for cases with very low Mach number flow in the single-precision density-based solver, you can improve convergence by using pressure extrapolation instead of the default velocity extrapolation scheme.

pressure on pressure-outlet b.c. is obtained via an advection

splitting method?

The default is [yes]. If you choose the default, this means that the pressure-outlet boundary condition implementation in the density-based solver has an absorption behavior, as described in this section in the separate User's Guide. To revert to pre- ANSYS FLUENT 6.3 boundary condition implementations, where the pressure on the faces of a pressure-outlet boundary is fixed to the specified value while the flow is subsonic, enter no.

The absorption behavior of the pressure-outlet boundary condition should not be confused with rigorous non-reflecting boundary condition implementation, described in this section in the separate User's Guide.

If you are using the pressure-based solver, you will be asked the following questions:

extrapolate pressure on flow inlets?

The default is [yes].

extrapolate pressure on all boundaries?

The default is [no].

extrapolate velocity on out-flow boundaries?

The default is [no].

correction-tolerance/

Enter the correction tolerance menu.

courant-number

Set the fine-grid Courant number (time step factor). This command is available only for the coupled solvers.

data-sampling

Enable data sampling for unsteady flow statistics.

disable-reconstruction?

Completely disables reconstruction, resulting in totally first-order accuracy.

discretization-scheme/

Enter the discretization scheem menu. This allows you to select the discretization scheme for the convection terms in the solution equations, as well as the pressure-velocity coupling scheme for the pressure-based solver.

pressure

Select which Pressure model is to be used. Five models are available:

Index	Model
10	Standard
11	Linear
12	Second Order
13	Body Force Weighted
14	PRESTO!

flow

Select which Pressure-Velocity Coupling model is to be used. Three models are available:

Index	Model
20	SIMPLE
21	SIMPLEC
22	PISO

mom

Select which Momentum model is to be used. Five models are available:

Index	Model
0	First Order Upwind
1	Second Order Upwind
2	Power Law
4	QUICK
5	Third-Order MUSCL

The Energy and Turbulence models are indexed as in the Momentum model table above.

Contact your ANSYS FLUENT technical support engineer for more details.

equations/

Select the equations to be solved.

expert

Set expert options.

extrapolate-eqn-vars/

Enter the extrapolation menu.

extrapolate-vars?

Applies a predictor algorithm for computing initial conditions at time step n+1.

flow-warnings?

Specify whether or not to print warning messages when reversed flow occurs at inlets and outlets, and when mass flow inlets develop supersonic regions. By default, flow warnings are printed.

flux-type

Set the flux type.

gradient-scheme

Set gradient options.

heterogeneous-stiff-chemistry

Set the heterogeneous stiff-chemistry solver.

limiter-warnings?

Specify whether or not to print warning messages when quantities are being limited. By default, limiter warnings are printed.

limits

Set solver limits for various solution variables, in order to improve the stability of the solution.

mp-mfluid-aniso-drag

Set anisotropic drag parameters for the Eulerian multiphase model.

mp-reference-density

Set the reference density option for the Eulerian multiphase model. The following options are available:

Index	VOF Equation Discretization	Option
0	mass conservative	reference density for a particular phase
		in a cell is treated as the volume averaged
		density of that phase in the whole domain
1	mass conservative	reference density for a particular phase
		in a cell is treated as the density of that
		phase in that cell
2	mass conservative	reference density for any phase in a cell
		is treated as the mixture density of that
		phase in that cell
3	volume conservative	reference density for a particular
		phase in a cell is treated as the density of that
		phase in that cell

max-corrections/

Enter the set max-corrections menu.

max-flow-time

Set the maximm flow time.

multi-grid-amg

Set the parameters that govern the algebraic multigrid procedure.

multi-grid-controls/

Set multigrid parameters and termination criteria.

multi-grid-fas

Set the parameters that control the FAS multigrid solver. This command appears only when the explicit coupled solver is used.

multi-stage

Set the multi-stage coefficients and the dissipation and viscous evaluation stages. This command appears only when the explicit coupled solver is used.

numerics

Set numerics options.

predict-next-time?

Applies a predictor algorithm for computing.

p-v-controls

Set pressure-velocity controls.

p-v-coupling

Select the pressure-velocity coupling scheme.

reactions?

Enable the species reaction sources and set relaxation factor.

relaxation-factor/

Enter the relaxation-factor menu.

relaxation-method

Set the solver relaxation method.

reporting-interval

Set the number of iterations for which convergence monitors are reported. The default is 1 (after every iteration).

residual-smoothing

Set the implicit residual smoothing parameters. This command is available only for the explicit coupled solver.

residual-tolerance/

Enter the residual tolerance menu.

residual-verbosity

Set the amount of residual information to be printed. A value of 0 (the default) prints residuals at the end of each fine grid iteration. A value of 1 prints residuals after every stage of the fine grid iteration. A value of 2 prints residuals after every stage on every grid level.

set-controls-to-default

Set controls to default values.

set-solution-steering

Set solution steering parameters.

slope-limiter-set/

Select a new Fluent solver slope limiter.

solution-steering

Enable solution steering for the density-based solver.

stiff-chemistry

Set solver options for stiff chemistry solutions.

surface-tension

Set surface-tension calculation options.

time-step

Set the magnitude of the (physical) time step $\Delta t$.

under-relaxation/

Enter the under-relaxation menu, which allows you to set the under-relaxation factor for each equation that is being solved in a segregated manner.

undo-timestep

variable-time-stepping

Set variable time-stepping options for VOF explicit schemes.

update-physical-time

Advance the unsteady solution to the next physical time level. Using this command in conjunction with the iterate command allows you to manually advance the solution in time (rather than doing it automatically with the dual-time-iterate command).