animate/
Enter the animation menu.
define/
Enter the animation definition menu.
define-monitor
Define new animation.
edit-monitor
Change animation monitor attributes.
objects/
Enter the object manipulation menu.
clear-history
Clear solution animation object history.
copy
Copy solution animation object.
create
Create new solution animation object.
delete
Delete solution animation object.
edit
Edit solution animation object.
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.
stored-view?
Play the 3D animation sequence using the view stored in the sequence.
write
Write animation sequence to the file.
cell-register-operations/
Enter the cell register operations menu.
add
Create a new cell register operation.
delete
Delete a cell register operation.
edit
Edit an existing cell register operation.
list
List the currently defined cell register operations.
list-properties
List the properties of a report register operation.
cell-registers/
Enter the cell registers menu.
adapt
Adapt the mesh of a cell register.
add
Create a new cell register.
apply-poor-mesh-numerics
Apply poor mesh numerics to the mesh of a cell register.
delete
Delete a cell register.
display
Display a cell register.
edit
Edit an existing cell register.
list
List all of the currently defined cell registers.
list-properties
List the properties of a cell register.
convergence-conditions/
Enter the convergence conditions menu.
condition
Specify whether the solution is considered converged when all of the conditions are met or when one of the conditions is met.
conv-reports/
Enter the convergence reports menu.
add
Create a new convergence condition.
delete
Delete a convergence condition.
edit
Edit a convergence condition.
list
Lists all of the report definition-based convergence conditions.
list-properties
Lists the properties of the specified convergence condition.
frequency
Specify how often convergence checks are performed.
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.
all-zones
Initialize the flow field with the default values.
zone
You can select the type of zone from which you want to compute these values. The types of zones available are:
axis
degassing
exhaust-fan
fan
fluid
inlet-vent
intake-fan
interface
interior
mass-flow-inlet
mass-flow-outlet
network
network-end
outflow
outlet-vent
periodic
porous-jump
pressure-far-field
pressure-inlet
pressure-outlet
radiator
rans-les-interface
recirculation-inlet
recirculation-outlet
shadow
solid
symmetry
velocity-inlet
wall
dpm-reset
Reset discrete phase source terms to zero.
fmg-initialization
Initialize using the full-multigrid initialization (FMG).
hyb-initialization
Initialize using the hybrid initialization method.
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.
open-channel-auto-init
Open channel automatic initialization.
reference-frame
Set reference frame to absolute or relative.
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.
set-hyb-initialization/
Enter the hybrid initialization menu.
general-settings
Enter the general-settings menu.
turbulence-settings
Enter the turbulence-settings menu.
species-settings
Enter the species-settings menu.
show-time-sampled
Display the amount of simulated time covered by the data sampled for unsteady statistics.
vof-patch-smooth-options/
Enter the vof patch/smooth options menu.
execute-smoothing
Perform volumetric smoothing for volume fraction.
set-options
Set options for patching and smoothing volume fraction.
iterate
Perform a specified number of iterations.
Note: This option is still available during transient simulations, since it can be used to add more iterations to the same time step after interrupting iterations within a time step.
mesh-motion
Perform mesh motion.
monitors/
Set solution monitors.
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.
patch
Patch a value for a flow variable in the domain.
report-definitions/
Enter the report definitions menu.
add
Create a report definition.
copy
Create a copy of a report definition.
delete
Delete a report definition.
edit
Edit a report definition.
list
List all defined report definitions.
list-properties
List the properties of a report definition.
rename
Rename a report definition.
report-files/
Enter the report files menu.
add
Create a report file.
clear-data
Clear the data associated with a report file.
delete
Delete a report file.
edit
Edit a report file.
list
List all defined report files.
list-properties
List the properties of a report file.
report-plots/
Enter the report plots menu.
add
Create a report plot.
axes
Define the axes for a report plot.
clear-data
Clear the data associated with a report plot.
curves
Define the curves for a report plot.
delete
Delete a report plot.
edit
Edit a report plot.
list
List all defined report plots.
list-properties
List the properties of a report plot.
set/
Enter the set solution parameters menu.
adaptive-time-stepping
Set adaptive time stepping parameters.
amg-options/
Enter the AMG options menu
amg-gpgpu-options/
contains commands to enable/disable GPGPU acceleration and set solver type and options for individual coupled and scalar equations.
conservative-amg-coarsening?
enable the use of conservative coarsening techniques for coupled equations that can improve parallel performance and/or convergence for some difficult cases.
laplace-coarsening?
enable Laplace coarsening for scalar and/or coupled equations.
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 Calculation Procedure at Pressure Outlet Boundaries of the
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.
Important: The absorption behavior of the pressure-outlet boundary condition should not be confused with rigorous non-reflecting boundary condition implementation, described in Boundary Acoustic Wave Models of the 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].
convergence-acceleration-for-stretched-meshes/
Enable convergence acceleration for stretched meshes to improve the convergence of the implicit density based solver on meshes with high cell stretching.
correction-tolerance/
Enter the correction tolerance menu.
coupled-vof-expert
Set coupled vof expert controls. You will be prompted with the following questions:
Use linearized buoyancy force?
provides the implicit linearization of buoyancy force.
Use blended treatment for buoyancy force?
will turn off buoyancy linearization in certain unstable conditions.
Use false time step linearization?
provides additional stability for buoyancy driven flows in the steady-state pseudo-transient mode by increasing the diagonal dominance using false time step size.
Use smoothed density for pseudo-transient method?
smooths the cell density near the interface, therefore avoiding unphysical acceleration of lighter phase in the vicinity of interface. This option is only available for steady-state pseudo-transient method.
Note: There is an additional entry for the number of density smoothings (default 2), which can be increased in case of very large unphysical velocities across the interface.
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 scheme menu. This allows you to select the discretization scheme for the convection terms in the solution equations.
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! |
mp
Select which convective discretization scheme for volume fraction is to be used. Six models are available:
| Index | Model |
|---|---|
| 0 | First Order |
| 1 | Second Order |
| 28 | Compressive |
| 5 | Modified HRIC |
| 29 | BGM |
| 4 | QUICK |
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.
enable-output-dp-dt?
Control whether the output field variable dp-dt will be available for transient simulation postprocessing. If you select no, pressure fields at the previous time steps will not be stored in memory which reduces memory usage.
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.
warped-face-gradient-correction/
Enter the warped-face gradient correction menu.
enable?
Enable/disable gradient enhancement computations and specify whether Fluent uses fast or memory saving mode.
gradient-scheme
Set gradient options.
heterogeneous-stiff-chemistry
Set the heterogeneous stiff-chemistry solver.
high-order-term-relaxation/
Enter the High Order Term Relaxation menu.
enable?
Enable/Disable High Order Term Relaxation.
options/
High Order Term Relaxation Options.
relaxation-factor
Set the relaxation factor.
variables/
Select the variables.
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.
lock-solid-temperature?
Specify whether you want to lock (or “freeze”) the temperature values for all the cells in solid zones (including those to which you have a hooked an energy source through a UDF) and in walls that have shell conduction enabled, so that the values do not change during further solver iterations.
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 maximum flow time.
max-iterations-per-time-step
Set the number of time steps for a transient simulation.
Note: This option is available when automatic initialization and case modification is enabled.
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.
multiphase-numerics
Set multiphase numerics options.
boiling-parameters/
Enter the menu for the multiphase boiling model parameters.
liquid-vof-factor
When enabled, considers liquid volume fraction effects by multiplying the heat transfer coefficients by the local liquid volume fraction.
thin-film
When enabled, includes multiphase boiling thin film effects using Equation 17–431 in the Fluent Theory Guide.
compressible-flow/
Enter the compressible multiphase flow numerics menu.
alternate-bc-formulation
Enable an alternative formulation for compressible phases at an inlet boundary. This formulation calculates static temperature and pressure using an iterative method based on fundamental thermodynamic relations.
enhanced-numerics
Enable an enhanced numerical treatment that provides better stability at startup and during calculation of compressible flows.
heat-mass-transfer/
Enter the menu for the multiphase heat mass transfer parameters.
area-density/
Enter the menu for the area density
vof-min-seeding
Set the minimum volume fraction for the area density and cavitation. This may be useful, for example, in cases when a species mass transfer model (such as the Symmetric model or Particle model) do not consider evaporation or condensation if the volume fraction of one of the phases is zero. The seeding allows for a phase change to occur in the fluid flow. The default value is 1e-6.
cavitation/
Enter the cavitation heat mass transfer menu.
min-vapor-pressure
Set the minimum vapor pressure limit for the cavitation mass-transfer model. The default value is 1 Pa.
max-vapor-pressure-ratio
Set the maximum limit on the vapor pressure after the turbulence and thermal correction. The default value is five times the vapor pressure, with consideration of turbulent and thermal effects for each cell and phase.
schnerr-cond-coeff
Set the condensation coefficient for the Schnerr-Sauer model ( in Equation 17–500 in the Fluent Theory Guide). The default and recommended value of 0.2.
nita-controls/
Enter the NITA controls menu.
face-pressure-options
Set face pressure options for the pressure calculation. For the predictor step, you can select either PRESTO (default for the Eulerian multiphase model) or Second Order. If you selected PRESTO for the predictor step, then you can select either the PRESTO or Second Order method for the corrector step. If you selected the Second Order method for the predictor step, then ANSYS Fluent will enforce the Second Order method for the corrector step also. When PRESTO is used, the impact of fluxes on the face pressure is inversely proportional to the time step size, which may lead to numerical problems as the time step size decreases. Therefore, the exclusion of transient terms is recommended for very small time steps when using PRESTO.
viscous-flow
Enter the viscous flow multiphase flow numerics menu.
viscosity-averaging
Force harmonic averaging of cell viscosities to calculate face viscosity used in momentum equation. This can improve convergence for highly viscous flow applications (the VOF model only).
nb-gradient-boundary-option?
Switch between the modified treatment of node-based gradients at boundary cells and the legacy treatment (R14.5.7 and earlier).
nita-expert-controls/
Enter the NITA expert control menu.
set-verbosity
Setting this to 1, enables the verbosity for NITA diagnostics. The default value of 0 disables verbosity output for NITA diagnostics.
skewness-neighbor-coupling
enable/disable coupling of the neighbor and skewness corrections.
number-of-iterations
Set the number of iterations for a steady-state simulation without starting the calculation.
number-of-time-steps
Set the number of time steps for a transient simulation without starting the calculation.
numerical-beach-control
Set damping function in flow direction. This command appears only when the VOF model is enabled. Select the damping function to be used:
| Index | Damping Function |
|---|---|
| 0 | Linear |
| 1 | Quadratic |
| 2 | Cubic |
| 3 | Cosine |
numerics
Set numerics options.
open-channel-controls
For flows that do not transition from sub-critical to super-critical, or vice-versa, you can speed-up the solution calculation by updating the frequency of Froude number during run time.
open-channel-wave-options/
Set buffer layer height, verbosity, and open channel wave theory formulation.
set-buffer-layer-ht
Set the buffer layer height.
set-verbosity
Set the open channel wave verbosity.
stokes-wave-variants
Specify which open channel wave theory formulation Fluent uses.
overset/
Specify overset meshing solver options.
high-order-pressure?
Use the pressure gradient of the donor cell in the interpolation of pressure for its receptor cell.
interpolation-method
Select the interpolation method for overset interfaces. Note that the least squares method is recommended for sliding mesh cases.
orphan-cell-treatment?
Enable/disable a numerical treatment that attempts to assign reasonable data values to orphan cells.
p-v-controls
Set pressure-velocity controls.
p-v-coupling
Select which pressure-velocity coupling model is to be used. Four models are available:
| Index | Model |
|---|---|
| 20 | SIMPLE |
| 21 | SIMPLEC |
| 22 | PISO |
| 24 | Coupled |
phase-based-vof-discretization
Set phase based slope limiter for VOF compressive scheme.
poor-mesh-numerics/
Enter the poor mesh numerics menu.
cell-quality-based?
Enable/disable poor mesh numerics on cells with low quality.
enable?
Solution correction on meshes of low quality.
print-poor-elements-count
Print out a listing of the poor cells for each criterion (default, cell quality, and user-defined).
reset-poor-elements?
Reset the list of poor cells included based on quality criteria or user-defined registers.
set-quality-threshold
Set the threshold for quality-based inclusion in the poor mesh numerics. The threshold value is applied to cell orthogonality and the complement of cell skewness.
user-defined-on-register
Include a register for the poor mesh numerics or not.
predict-next-time?
Applies a predictor algorithm for computing.
pseudo-transient-expert/
Enter the pseudo transient expert usage control menu.
pseudo-relaxation-factor/
Enter the pseudo relaxation factor menu.
pseudo-transient
Set the pseudo transient formulation.
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.
second-order-time-options
Enable/disable the variable time step size option for second-order implicit transient formulations.
set-all-species-together
Set all species discretizations and URFs together.
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.
solid-time-step
Enter the solid-time-step menu, which allows you to specify a time step for the solid zone (independent from the fluid zone).
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 .
unsteady-statistics-cff
Unsteady statistics for custom field functions.
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
When enabled, if the truncation error within a time step exceeds the specified tolerance Fluent will automatically undo the current calculation and make another attempt with the time step reduced by 1/2. This will be attempted up to 5 times after which Fluent will accept the result and proceed to the next time step.
variable-time-stepping
Set variable time-stepping options for VOF explicit schemes.
vof-numerics
Set VOF numeric options.
vof-explicit-controls
Set the sub time step calculation method for VOF calculations.
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).