Chapter 11:  solve/

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 conservativereference density for a particular phase in a cell is treated as the density of that phase in that cell
2 mass conservativereference 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).


Release 18.2 - © ANSYS, Inc. All rights reserved.