Chapter 3:  define/

boundary-conditions/

Enter the boundary conditions menu.


Important:  Text User Interface commands that take single or multiple zone names support the use of wildcards. For example, to copy boundary conditions (copy-bc) to all zones of a certain type, use a * in the name of the zone to which you want to copy the conditions.


axis

Set boundary conditions for a zone of this type.

bc-settings/

Enter the boundary conditions settings menu.

mass-flow

Select method for setting the mass flow rate.

pressure-outlet

Set advanced options for pressure outlet boundaries.

copy-bc

Copy boundary conditions to other zones.

degassing

Set boundary conditions for a zone of this type.

exhaust-fan

Set boundary conditions for a zone of this type.

fan

Set boundary conditions for a zone of this type.

fluid

Set boundary conditions for a zone of this type.

inlet-vent

Set boundary conditions for a zone of this type.

intake-fan

Set boundary conditions for a zone of this type.

interface

Set boundary conditions for a zone of this type.

interior

Set boundary conditions for a zone of this type.

list-zones

Print out the types and IDs of all zones in the console window. You can use your mouse to check a zone ID, following the instructions listed under Zone in the Boundary Conditions Task Page section of the User’s Guide.

mass-flow-inlet

Set boundary conditions for a zone of this type.

mass-flow-outlet

Set boundary conditions for a zone of this type.

modify-zones/

Enter the modify zones menu.

activate-cell-zone

Activate cell thread.

append-mesh

Append new mesh.

append-mesh-data

Append new mesh with data.

change-zone-phase

Set the phase (liquid or vapor) for a specific fluid zone.

copy-move-cell-zone

Create a copy of a cell zone that is offset from the original either by a translational distance or a rotational angle. In the copied zone, the bounding face zones are all converted to walls, any existing cell data is initialized to a constant value, and non-conformal interfaces and dynamic zones are not copied; otherwise, the model settings are the same as in the original zone. Note that if you want the copied zone to be connected to existing zones, you must either fuse the boundaries (see Fusing Face Zones in the Fluent User's Guide) or set up a non-conformal interface (see Using a Non-Conformal Mesh in ANSYS Fluent in the Fluent User's Guide).

copy-mrf-to-mesh-motion

Copy motion variable values for origin, axis, and velocities from Frame Motion to Mesh Motion.

copy-mesh-to-mrf-motion

Copy motion variable values for origin, axis, and velocities from Mesh Motion to Frame Motion.

create-all-shell-threads

Mark all finite thickness walls for shell creation. Shell zones will be created at the start of the iterations.

deactivate-cell-zone

Deactivate cell thread.

delete-all-shells

Delete all shell zones and switch off shell conduction on all the walls. These zones can be recreated using the command recreate-all-shells.

delete-cell-zone

Delete a cell thread.

extrude-face-zone-delta

Extrude a face thread a specified distance based on a list of deltas.

extrude-face-zone-para

Extrude a face thread a specified distance based on a distance and a list of parametric locations between 0 and 1, for example, 0 0.2 0.4 0.8 1.0.

fuse-face-zones

Attempt to fuse zones by removing duplicate faces and nodes.

list-zones

List zone IDs, types, kinds, and names.

make-periodic

Attempt to establish periodic/shadow face zone connectivity.

matching-tolerance

Set normalized tolerance used for finding coincident nodes.

merge-zones

Merge zones of same type and condition into one.

mrf-to-sliding-mesh

Change the motion specification from MRF to moving mesh.

orient-face-zone

Orient the face zone.

recreate-all-shells

Recreate shells on all the walls that were deleted using the command delete-all-shells.

replace-zone

Replace cell zone.

sep-cell-zone-mark

Separate cell zone based on cell marking.

sep-cell-zone-region

Separate cell zone based on contiguous regions.

sep-face-zone-angle

Separate face zone based on significant angle.

sep-face-zone-face

Separate each face in zone into unique zone.

sep-face-zone-mark

Separate face zone based on cell marking.

sep-face-zone-region

Separate face zone based on contiguous regions.

slit-periodic

Slit periodic zone into two symmetry zones.

slit-face-zone

Slit two-sided wall into two connected wall zones.

slit-interior-between-diff-solids

Slit the interior zone between solid zones of differing materials to create a coupled wall. You will generally be prompted by Fluent if this is necessary.

zone-name

Give a zone a new name.

zone-type

Set the type for a zone or multiple zones of the same category. You will be prompted for the name / ID of the zone to be changed and the new type for that zone. To change multiple zones, you can enter a list (separated by spaces and contained within a pair of parentheses) or use asterisks (*) as wildcards.

non-reflecting-bc/

Enter the non-reflecting boundary condition menu.

general-nrbc/

Setting for general non-reflecting b.c.

set/

Enter the setup menu for general non-reflecting b.c.’s.

sigma

Set NRBC sigma factor (default value 0.15).

sigma2

Set NRBC sigma2 factor (default value 5.0).

verbosity

Enable/disable nrbc verbosity scheme output.

turbo-specific-nrbc/

Enter the turbo specific nrbc menu.

enable?

Enable/disable non-reflecting b.c.’s.

initialize

Initialize non-reflecting b.c.’s.

set/

Enter the set menu for non-reflecting b.c. parameters.

discretization

Enable use of higher-order reconstruction at boundaries if available.

under-relaxation

Set non-reflecting b.c. under-relaxation factor.

verbosity

Set non-reflecting b.c. verbosity level. 0 : silent, 1 : basic information (default), 2 : detailed information for debugging.

show-status

Show current status of non-reflecting b.c.’s.

open-channel-wave-settings

Open channel wave input analysis.

openchannel-threads

List open channel group IDs, names, types and variables.

outflow

Set boundary conditions for a zone of this type.

outlet-vent

Set boundary conditions for a zone of this type.

periodic

Set boundary conditions for a zone of this type.

phase-shift/

Enter the phase shift settings menu.

multi-disturbances

Set basic phase-shift parameters.

extra-settings

Set other phase-shift parameters.

porous-jump

Set boundary conditions for a zone of this type.

pressure-far-field

Set boundary conditions for a zone of this type.

pressure-inlet

Set boundary conditions for a zone of this type.

pressure-outlet

Set boundary conditions for a zone of this type.

radiator

Set boundary conditions for a zone of this type.

rans-les-interface

Set boundary conditions for a zone of this type.

recirculation-inlet

Set boundary conditions for a zone of this type.

recirculation-outlet

Set boundary conditions for a zone of this type.

set/

Allows you to define one or more settings at single or multiple boundaries/cell zones of a given type at once. Enter q to exit the define/boundary-conditions/set/<type> command.

For a description of the items in this menu, see corresponding define/boundary-conditions/<type>.

shadow

Set boundary conditions for a zone of this type.

solid

Set boundary conditions for a zone of this type.

symmetry

Set boundary conditions for a zone of this type.

target-mass-flow-rate-settings/

Enter the targeted mass flow rate settings menu.

set under-relaxation-factor

The default setting is 0.05.

enable targeted mass flow rate verbosity?

Enable/disable verbosity when using targeted mass flow rate. When enabled, it prints to the console window the required mass flow rate, computed mass flow rate, mean pressure, the new pressure imposed on the outlet, and the change in pressure in SI units.

velocity-inlet

Set boundary conditions for a zone of this type.

wall

Set boundary conditions for a zone of this type.

zone-name

Give a zone a new name.

zone-type

Set the type for a zone or multiple zones of the same category. You will be prompted for the name / ID of the zone to be changed and the new type for that zone. To change multiple zones, you can enter a list (separated by spaces and contained within a pair of parentheses) or use asterisks (*) as wildcards.

custom-field-functions/

Enter the custom field functions menu.

define

Define a custom field function.

delete

Delete a custom field function.

example-cff-definitions

List example custom field functions.

list-valid-cell-function-names

List the names of cell functions that can be used in a custom field function.

load

Load a custom field function.

save

Save a custom field function.

dynamic-mesh/

Enter the dynamic mesh menu.

actions/

Enter the dynamic mesh action menu, where you can initiate manual remeshing (that is, remeshing without running a calculation).

remesh-cell-zone

Manually remesh a cell zone with option to remesh adjacent dynamic face zones.

remesh-cell-zone-cutcell

Manually remesh a cell zone using the CutCell zone remeshing method, in order to generate a predominantly Cartesian mesh.

controls/

Enter the dynamic mesh controls menu. This text command is only available when the define/dynamic-mesh/dynamic-mesh? text command is enabled.

contact-parameters/

Enter the dynamic mesh contact-parameters menu. This text command is only available when you enable contact detection using the prompts of the define/dynamic-mesh/dynamic-mesh? text command.

contact-threshold

Specify threshold distance for contact detection.

contact-udf

Select the UDF to be invoked when contact is detected.

contact-zones

Select face zones involved in contact detection.

flow-control?

Enable/disable flow control.

flow-control-parameters/

Set up and delete flow control zones

create-flow-control-zone

Create a flow control zone.

delete-flow-control-zone

Delete a flow control zone.

implicit-update-parameters/

Enter the dynamic mesh implicit update menu. This text command is only available when you enable implicit mesh updating using the prompts of the define/dynamic-mesh/dynamic-mesh? text command.

motion-relaxation

Specify a value (within the range of 0 to 1) for the motion relaxation, which is applied during the implicit mesh update.

residual-criteria

Specify the relative residual threshold that is used to check the motion convergence during the implicit mesh update.

update-interval

Specify the update interval (that is, the frequency in iterations) at which the mesh is updated within a time step.

in-cylinder-output?

Enable/disable in-cylinder output.

in-cylinder-parameters/

Enter the dynamic mesh in-cylinder menu.

crank-angle-step

Specify crank angle step size.

crank-period

Specify the crank period.

max-crank-angle-step

Specify maximum crank angle step size.

minimum-lift

Specify minimum lift for in-cylinder valves.

modify-lift

Modify lift curve (shift or scale).

piston-data

Specify the crank radius and connecting rod length.

piston-stroke-cutoff

Specify the cut off point for in-cylinder piston.

position-starting-mesh

Move mesh from top dead center to starting crank angle.

print-plot-lift

Print or plot valve lift curve.

starting-crank-angle

Specify the initial value for the crank angle.

layering?

Enable/disable dynamic-layering in quad/hex cell zones.

layering-parameters/

Enter the dynamic mesh layering menu.

collapse-factor

Set the factor determining when to collapse dynamic layers.

constant-height?

Enable/disable layering based on constant height, else layering based on constant ratio.

split-factor

Set the factor determining when to split dynamic layers.

remeshing?

Enable/disable local remeshing in tri/tet and mixed cell zones.

remeshing-parameters/

Enter the dynamic mesh remeshing menu to set parameters for all remeshing methods except the Cutcell zone remeshing method.

cell-skew-max

Set the cell skewness threshold above which cells will be remeshed.

face-skew-max

Set the face skewness threshold above which faces will be remeshed.

length-max

Set the length threshold above which cells will be remeshed.

length-min

Set the length threshold below which cells will be remeshed.

must-improve-skewness?

Enable/disable cavity replacement only if remeshing improves the skewness.

parallel-remeshing?

Disable/enable parallel remeshing.

remeshing-after-moving?

Enable a second round of remeshing based on the skewness parameters after the boundary has moved.

remeshing-methods

Enable/disable remeshing methods.

size-remesh-interval

Set the interval (in time steps) when remeshing based on size is done.

sizing-funct-defaults

Set sizing function defaults.

sizing-funct-rate

Determine how far from the boundary the increase/decrease happens.

sizing-funct-resolution

Set the sizing function resolution with respect to shortest boundary.

sizing-funct-variation

Set the maximum sizing function increase/decrease in the interior.

sizing-function?

Enable/disable sizing function to control size based remeshing.

six-dof-parameters/

Enter the dynamic mesh six degrees of freedom (DOF) solver menu.

create-properties

Create / edit a set of six DOF properties for rigid body motion.

delete-properties

Delete a set of six DOF properties for rigid body motion.

list-properties

Print summaries of the existing sets of six DOF properties for rigid body motion.

motion-history-file-name

Specify the name and location of the six DOF motion history file.

motion-history?

Enable/disable writing position/orientation of six DOF zones to file.

second-order?

Enable/Disable the second order six degrees of freedom solver.

x-component-of-gravity

Specify x-component of gravity.

y-component-of-gravity

Specify y-component of gravity.

z-component-of-gravity

Specify z-component of gravity.

smoothing?

Enable/disable smoothing in cell zones.

smoothing-parameters/

Enter the dynamic mesh smoothing menu.

bnd-node-relaxation

The boundary node relaxation is used by spring smoothing. The boundary node relaxation allows you to relax the update of the node positions at deforming boundaries. A value of 0 prevents deforming boundary nodes from moving and a value of 1 indicates no under-relaxation.

bnd-stiffness-factor

Set the stiffness factor for springs connected to boundary nodes.

boundary-distance-method

Set the method used to evaluate the boundary distance for the diffusion coefficient calculation, when diffusion-based smoothing is enabled.

constant-factor

Set the spring constant relaxation factor.

convergence-tolerance

Set the convergence tolerance for spring-based solver.

diffusion-coeff-function

Specify whether the diffusion coefficient for diffusion-based smoothing is based on the boundary distance or the cell volume.

diffusion-coeff-parameter

Set the diffusion coefficient parameter used for diffusion-based smoothing.

diffusion-fvm?

Answering yes at the prompt changes the diffusion-based smoothing method to the cell-based finite volume approach that was the default in releases prior to Fluent 15.0. Answering no at the prompt changes the diffusion-based smoothing method to the default node-based finite element method.

max-iter

Set the maximum number of iterations for spring-based solver.

relative-convergence-tolerance

Set the relative residual convergence tolerance for Diffusion smoothing.

skew-smooth-cell-skew-max

Set the skewness threshold, above which cells will be smoothed using the skewness method.

skew-smooth-face-skew-max

Set the skewness threshold, above which faces will be smoothed using the skewness method.

skew-smooth-niter

Set the number of skewness-based smoothing cycles.

smooth-from-reference-position?

Enable / disable smoothing from a reference position. Such smoothing may produce greater mesh quality consistency for cases with periodic or quasi-periodic motion, and is only available when the smoothing method is based on diffusion or the linearly elastic solid model.

smoothing-method

Specify the smoothing method (spring, diffusion, or linearly elastic solid) used by the dynamic mesh model.

spring-on-all-elements?

Enable/disable spring-based smoothing for all cell shapes.

spring-on-simplex-shapes?

Enable/disable spring-based smoothing for triangular / tetrahedral cells in mixed element zones.

poisson-ratio

Set the Poisson’s ratio used by the linearly elastic solid model.

verbosity

Setting this to 1 will cause smoothing residuals to be printed to the text console. The default value of 0 suppresses this output.

dynamic-mesh?

Enable/disable the dynamic mesh solver.

events/

Enter the dynamic mesh events menu.

export-event-file

Export dynamic mesh events to file.

import-event-file

Import dynamic mesh event file.

steady-pseudo-time-control

Enable/disable the pseudo time step control in the graphical user interface.

transient-settings/

Enter the transient dynamic mesh settings menu. This text command is only available when you enable dynamic mesh using the prompts of the define/dynamic-mesh/dynamic-mesh? text command. Solver time must also be set to Transient.

allow-second-order?

Enable/disable second order transient scheme for dynamic mesh cases.

verbosity

Enable/disable transient scheme verbosity for dynamic mesh cases.

zones/

Enter the dynamic mesh zones menu.

create

Create or edit a dynamic zone.

delete

Delete a dynamic zone.

insert-boundary-layer

Insert a new cell zone.

insert-interior-layer

Insert a new layer cell zone at a specified location.

list

List the dynamic zones.

remove-boundary-layer

Remove a cell zone.

remove-interior-layer

Remove an interior layer cell zone.

enable-mesh-morpher-optimizer?

Enable the mesh morpher/optimizer. When the mesh morpher/optimizer is enabled, the define/mesh-morpher-optimizer text command becomes available.

injections/

Enter the injections menu.

For a description of the items in this menu, see define/models/dpm/injections.

materials/

Enter the materials menu.

change-create

Change the properties of a locally-stored material or create a new material.

copy

Copy a material from the database.

copy-by-formula

Copy a material from the database by formula.

data-base/

Enter the material database menu.

database-type

Set the database type.

edit

Edit material.

list-materials

List all materials in the database.

list-properties

List the properties of a material in the database.

new

Define new material.

save

Save user-defined database.

delete

Delete a material from local storage.

list-materials

List all locally-stored materials.

list-properties

List the properties of a locally-stored material.

mesh-interfaces/

Enter the mesh-interfaces menu.

auto-pairing

Create mesh interfaces for some or all of the interface zones. This text command automatically "pairs" the zones, so that you do not have to manually assign the zones to the two sides of each interface as part of the creation process. Note that not all of the interface options are available at the time of creation: some can be enabled afterward using the define/mesh-interfaces/edit text command; for the periodic and periodic repeats options, you must instead create the interface using the define/mesh-interfaces/make-periodic and define/mesh-interfaces/create text commands, respectively.

create

Create a mesh interface.

delete

Delete a mesh interface.

draw

Draw specified sliding interface zone.

edit

Edit attributes of mesh interfaces, including the interface options and (for a single interface) the name and the list of interface zones assigned to the interface.

enforce-continuity-after-bc?

Enable/disable continuity across the boundary condition interface for contour plots in postprocessing.

enforce-coupled-wall-between-solids?

Enable/disable automatic definition of solid-solid interfaces as coupled walls. By default this option is disabled and ANSYS Fluent creates interior boundaries at solid-solid interfaces.

improve-quality

Checks the quality of all mapped interfaces. If Fluent finds any mapped interfaces that require improvement it will list them and ask you if you would like to increase the tolerance to improve the interfaces.

list

List all mesh interfaces.

make-periodic

Make interface zones periodic.

mapped-interface-options/

Enter the mapped-interface menu. Options are available to convert a non-conformal interface to a mapped interface.

convert-to-mapped-interface

Convert non-conformal mesh interface to mapped mesh interfaces. Answering yes to Convert all mesh interfaces to mapped mesh interfaces? will enforce the mapping such that it specifies all interfaces as mapped interfaces; the mapped interfaces are created regardless of mesh quality. Answering yes to Convert poorly matching mesh interfaces to mapped mesh interfaces? will automate the mapping such that all interfaces that penetrate each other are automatically defined as mapped interfaces. Note that in all cases, only interfaces for which at least one side of the interface consists of only solid zones will be converted.

tolerance

Specify the mapped interface tolerance. After changing the tolerance, the existing mapped interface will be updated.

solution-controls

Specify the mapped frequency and under-relaxation factor for mapped interfaces.

mapped-interface-solution-controls

Set the mapping frequency and under-relaxation factor.

mapped-interface-tolerance

Specify the tolerance for creating mapped interfaces.

reset

Delete all sliding-interfaces.

use-virtual-polygon-approach

Use new virtual polygon approach for interfaces.


Important:  Note that case files created after ANSYS Fluent 6.1 will not show the virtual-polygon option, since it is the default.


mesh-morpher-optimizer/

Enter the mesh morpher/optimizer menu in order to deform the mesh as part of a shape optimization problem. This text command is only available when the define/enable-mesh-morpher-optimizer? text command has been enabled.

deformation-settings/

Enter the deformation menu. This text command is only available if you have created a deformation region using the define/mesh-morpher-optimizer/region/create or the define/mesh-morpher-optimizer/region/define-bounding-box text command.

check-mesh

Display a mesh check report in the console for the mesh displayed in the graphics window. The mesh check report provides volume statistics, mesh topology and periodic boundary information, verification of simplex counters, and verification of node position with reference to the axis for axisymmetric cases. This text command is only available if the define/mesh-morpher-optimizer/optimizer? text command is disabled.

deform-mesh

Modify the mesh and update the mesh display in the graphics window based on the parameter and deformation settings. This text command is only available if the define/mesh-morpher-optimizer/optimizer? text command is disabled.

motion-settings

Enter the motion settings menu, where you can create, modify, and delete the motions applied to the control points. This text command is only available if the define/mesh-morpher-optimizer/set-control-point-distribution text command is set to unstructured.

create

Create a new motion, by specifying the parameter, type of motion (translation, rotation, or radial motion), directional settings, name, and control points. Note that for translations, the values you enter for the direction components are multiplied with the value of the parameter to define the displacement applied to the control points.

delete

Delete an existing motion.

modify

Modify the settings for an existing motion.

read-from-file

Define the settings for all the motions by reading an ASCII text file.

write-to-file

Write the settings for all the motions to an ASCII text file.

read-motion-settings-from-file

Define all of the motion settings by reading an ASCII text file. This text command is only available if the define/mesh-morpher-optimizer/set-control-point-distribution text command is set to regular.

reset-all-deformations

Undo any deformations made to the mesh and update the mesh display in the graphics window.

set-constraints

Define the constraints on a boundary zone, in order to limit the freedom of a particular zone that falls within the deformation region(s) during the morphing of the mesh.

set-constraints-multiple

Define the constraints on multiple boundary zones, in order to limit the freedom of particular zones that fall within the deformation region(s) during the morphing of the mesh.

set-parameters

Assign translation direction components and a single parameter to a single control point in a region. Note that the values you enter for the direction components are multiplied with the value of the parameter to define the displacement applied to the control point. This text command is only available if the define/mesh-morpher-optimizer/set-control-point-distribution text command is set to regular.

set-parameters-multiple

Assign translation direction components and multiple parameters to multiple control points in a region. Note that the values you enter for the direction components are multiplied with the value of the parameter to define the displacement applied to the control point. This text command is only available if the define/mesh-morpher-optimizer/set-control-point-distribution text command is set to regular.

write-motion-settings-to-file

Write the motion settings to an ASCII text file. This text command is only available if the define/mesh-morpher-optimizer/set-control-point-distribution text command is set to regular.

morpher-summary

Display a summary of the mesh morpher/optimizer settings in the console. This text command is only available if you have created a deformation region using the define/mesh-morpher-optimizer/region/create or the define/mesh-morpher-optimizer/region/define-bounding-box text command.

optimizer-parameters/

Enter the optimizer menu. This text command is only available when you have created a deformation region using the define/mesh-morpher-optimizer/region/create or the define/mesh-morpher-optimizer/region/define-bounding-box text command and have enabled the define/mesh-morpher-optimizer/optimizer? text command.

convergence-criteria

Define the convergence criteria for the optimizer.

custom-calculator

Enter the custom calculator menu, in order to define the objective function as a function of output parameters. This menu is not available when the NEWUOA optimizer is selected using the define/mesh-morpher-optimizer/optimizer-parameters/optimizer-type text command.

define

Define the custom objective function that will be minimized by the optimizer.

delete

Delete the saved custom objective function.

example-obj-fn-definitions

Print examples of custom objective function definitions in the console.

list-output-parameters

Print a list of the output parameters that can be used to define the custom objective function.

disable-mesh-check

Specify whether you want to disable the general mesh check that is part of the optimization process. This check is conducted immediately after the mesh is deformed in every design stage, and determines whether a solution is calculated. Disabling this check allows you to use mesh repair commands (which can be set up using the define/mesh-morpher-optimizer/optimizer-parameters/initial-commands text command) at the start of a design stage, so that an accurate solution can be calculated.

end-commands

Specify the commands (text commands or command macros) that will be executed after the solution has run and converged for a design stage. This text command is not available when the NEWUOA optimizer is selected using the define/mesh-morpher-optimizer/optimizer-parameters/optimizer-type text command.

initial-commands

Specify the commands (text commands or command macros) that will be executed after the design has been modified, but before ANSYS Fluent has started to run the calculation for that design stage. This text command is not available when the NEWUOA optimizer is selected using the define/mesh-morpher-optimizer/optimizer-parameters/optimizer-type text command.

initialization

Specify how the solution variables should be treated after the mesh is deformed, that is, whether they should be initialized to the values defined in the Solution Initialization task page, remain the values obtained in the previous design iteration, or be read from a data file that you specify.

iterations-per-design

Define the maximum number of iterations ANSYS Fluent will perform for each design change.

maximum-designs

Define the maximum number of design stages the optimizer will undergo to reach the specified objective function.

mesh-quality-check

Specify if orthogonal quality should be used to determine whether a solution is calculated for a mesh, and define the minimum orthogonal quality value allowed (values may range from 0–1, where 0 represents the worst quality).

monitor/

Enter the monitor menu in order to plot and/or record optimization history data, that is, how the value of the objective function varies with each design stage produced by the mesh morpher/optimizer. This text menu is not available when the NEWUOA optimizer is selected using the define/mesh-morpher-optimizer/optimizer-parameters/optimizer-type text command.

clear-opt-hist

Discard the optimization history data, including the associated files.

plot-hist

Display an XY plot of the optimization history data generated during the last calculation. Note that no plot will be displayed if the data was discarded using the define/mesh-morpher-optimizer/optimizer-parameters/monitor/clear-optimization-monitor-data text command.

plot?

Enable the plotting of the optimization history data in the graphics window.

write?

Enable the saving of the optimization history data to a file.

newuoa-initial-parameter-variation

Define how much the parameters will be allowed to vary during the initial calculations. This text command is only available when the NEWUOA optimizer is selected using the define/mesh-morpher-optimizer/optimizer-parameters/optimizer-type text command.

objective-function-definition

Specify whether the format of the objective function is a user-defined function, a Scheme source file, or a custom function based on output parameters. The custom function is defined using the text commands in the define/mesh-morpher-optimizer/optimizer-parameters/custom-calculator menu. The objective-function-definition text command is not available when the NEWUOA optimizer is selected using the define/mesh-morpher-optimizer/optimizer-parameters/optimizer-type text command.

optimize

Initiate the optimization process. This text command is only available if the define/mesh-morpher-optimizer/optimizer? text command is enabled.

optimizer-type

Specify which optimizer is to be used. You can select one of the six built-in optimizers (1–5 and 7), or specify that you will use Design Exploration in ANSYS Workbench (6). Note that 6 is only available if you have launched your ANSYS Fluent session from ANSYS Workbench. For information about how the built-in optimizers function or how to use Design Exploration, see Design Analysis and Optimization in the User's Guide or Working With Input and Output Parameters in Workbench in the ANSYS Fluent in Workbench User's Guide, respectively.

save-case-data-files

Set up the automatic saving of intermediate case and data files during the optimization run, by specifying: the frequency (in design iterations) with which file sets are saved; the maximum number of file sets retained (after the maximum limit has been saved, the earliest file set will be overwritten with the latest); and the root name assigned to the files (which will have the design iteration number appended to it).

optimizer?

Enable the use of a built-in optimizer. This text command is only available if you have created a deformation region using the define/mesh-morpher-optimizer/region/create or the define/mesh-morpher-optimizer/region/define-bounding-box text command.

parameter-settings/

Enter the parameters menu.

number-of-parameters

Define the number of parameters that will be used to define the deformation.

parameter-bounds

Define the minimum and maximum values allowed by the built-in optimizer for the parameters. This text command is only available if the define/mesh-morpher-optimizer/optimizer? text command is enabled.

parameter-value

Define the value of a parameter. This value represents a magnitude that will then be used along with other direction settings to define motions that produce an overall displacement for a given control point. The value will specify a length in meters for translations and radial motions, and will specify an angle in degrees for rotations; the units here will be used regardless of what units you are using in the case. Note that you can enter a numeric value or define an input parameter (if you have enabled the definition of input parameters using the define/parameters/enable-in-TUI? text command). The parameter-value text command is only available in the following situations:

  • if the define/mesh-morpher-optimizer/optimizer? text command is disabled

  • if the define/mesh-morpher-optimizer/optimizer? text command is enabled and 6 is selected for the optimizer type via the define/mesh-morpher-optimizer/optimizer-type text command

region/

Enter the region menu in order to define the regions of the domain where the mesh will be deformed in order to optimize the shape.

control points

Enter the control points menu in order to create, modify, and/or delete control points. This text command is only available if the define/mesh-morpher-optimizer/set-control-point-distribution text command is set to unstructured.

create

Create a new control point by defining the coordinates of a point within an existing deformation region.

delete

Delete existing control points.

distribute-points-on-zone

Create an approximate number of control points on the mesh nodes of a particular boundary zone, with a distribution that is based on the distribution of the cell faces in that zone.

modify

Modify the coordinates of existing control points.

read-from-file

Define all of the control points by reading an ASCII text file.

write-to-file

Write the control point coordinates to an ASCII text file.

create

Create a new deformation region by specifying the name, number of control points (for a regular distribution), dimensions, origin coordinates, the components of the direction vectors, and whether to smooth the transitions of the mesh at the region boundaries (for an unstructured distribution). The region will be a “box”, that is, a rectangle for 2D cases or a rectangular hexahedron for 3D cases. After you have created a deformation region, additional menus will be available in the define/mesh-morpher-optimizer menu.

define-bounding-box

Create a new deformation region by specifying the name, the bounding zones that best represent the extents of the deformation region, the number of control points (for a regular distribution), and whether to smooth the transitions of the mesh at the region boundaries (for an unstructured distribution). The region will be a “box”, that is, a rectangle for 2D cases or a rectangular hexahedron for 3D cases. After you have created a deformation region, additional menus will be available in the define/mesh-morpher-optimizer menu.

delete

Delete a deformation region.

scaling-enlarge

Set the scaling factor applied to the bounding box when you click the Enlarge button in the Regions tab of the Mesh Morpher/Optimizer dialog box.

scaling-reduce

Set the scaling factor applied to the bounding box when you click the Reduce button in the Regions tab of the Mesh Morpher/Optimizer dialog box.

set-control-point-distribution

Specify whether the control point distribution is regular (that is, spread in a regular distribution throughout the entire deformation region) or unstructured (that is, distributed at specified locations).

mixing-planes/

Enter the mixing planes menu.

create

Create a mixing plane.

delete

Delete a mixing plane.

list

List defined mixing plane(s).

set/

Set global parameters relevant to mixing planes.

averaging-method

Set the mixing plane profile averaging method.

under-relaxation

Set mixing plane under-relaxation factor.

fix-pressure-level

Set fixed pressure level using value based on define/reference-pressure-location.

conserve-swirl/

Enter the menu to set swirl conservation in mixing plane menu.

enable?

Enable/disable swirl conservation in mixing plane.

verbosity?

Enable/disable verbosity in swirl conservation calculations.

report-swirl-integration

Report swirl integration (Torque) on inflow and outflow zones.

conserve-total-enthalpy/

Enter the menu to set total enthalpy conservation in mixing plane menu.

enable?

Enable/disable total enthalpy conservation in mixing plane.

verbosity?

Enable/disable verbosity in total-enthalpy conservation calculations.

models/

Enter the models menu to configure the solver.

acoustics/

Enter the acoustics menu.

auto-prune

Enable/disable auto prune of the receiver signal(s) during read-and-compute.

broad-band-noise?

Enable/disable the broadband noise model.

convective-effects?

Enable/disable the convective effects option.

compute-write

Compute sound pressure.

cylindrical-export?

Enable/disable the export of data in cylindrical coordinates.

display-flow-time?

Enable/disable the display of flow time during read-and-compute.

export-source-data-cgns?

Enable/disable the export of acoustic source data in CGNS format.

export-volumetric-sources?

Enable/disable the export of fluid zones.

export-volumetric-sources-cgns?

Enable/disable the export of fluid zones.

ffowcs-williams?

Enable/disable the Ffowcs-Williams-and-Hawkings model.

moving-receiver?

Enable/disable the moving receiver option.

off?

Enable/disable the acoustics model.

read-compute-write

Read acoustic source data files and compute sound pressure.

receivers

Set acoustic receivers.

sources

Set acoustic sources.

sources-fft/

Enter the acoustic sources fast Fourier transform (FFT) menu, to compute Fourier spectra from acoustic source data (ASD) files, create postprocessing variables for the pressure signals, and write CGNS files of the spectrum data.

read-asd-files

Read ASD files to perform FFT of the pressure history field.

compute-fft-fields

Compute FFT of the read pressure histories. The computed spectra replace the pressure histories in memory.

clean-up-storage-area

De-allocate memory used to store the pressure histories and their Fourier spectra, as well as any created surface variables for the visualization.

write-cgns-files

Write surface pressure spectra in CGNS format, which can be used for one-way coupling with ANSYS Mechanical in the frequency domain.

fft-surface-variables/

Enter the menu to create surface variables from the computed Fourier spectra for visualization.

create-constant-width-bands

Select up to 20 constant width bands and create surface pressure level (SPL) variables for them.

create-octave-bands

Create surface pressure level (SPL) variables for 17 technical octaves.

create-third-bands

Create surface pressure level (SPL) variables for 54 technical thirds.

create-set-of-modes

Select up to 20 individual Fourier modes and create variable pairs for them, containing the real and the imaginary parts of the complex Fourier amplitudes.

remove-variables

Remove all variables created in this menu.

write-acoustic-signals

Write on-the-fly sound pressure.

write-centroid-info

Write centroid info.

addon-module

Load addon module.

axisymmetric?

Specify whether or not the domain is axisymmetric.

crevice-model?

Enable/disable the crevice model.

crevice-model-controls/

Enter the crevice model controls menu.

dpm/

Enter the dispersed phase model menu.

clear-particles-from-domain

Remove/keep all particles currently in the domain.

collisions/

Enter the DEM collisions menu.

collision-mesh

Input for the collision mesh.

collision-pair-settings/

Supply settings for collisions to a pair of collision partners. You will be prompted to specify the Impact collision partner and the Target collision partner.

contact-force-normal

Sets the normal contact force law for this pair of collision partners.

contact-force-tangential

Sets the tangential contact force law for this pair of collision partners.

list-pair-settings

Lists the current settings for this pair of collision partners.

collision-partners/

Manage collision partners.

copy

Copy a collision partner.

create

Create a collision partner.

delete

Delete a collision partner.

list

Lists all known collision partners.

rename

Rename a collision partner.

dem-collisions?

Enable/disable the DEM collision model.

list-all-pair-settings

For each pair of collision partners, lists the collision laws and their parameters.

max-particle-velocity

Set the maximum particle velocity that may arise from collisions.

fill-injection-material-sources

Initialize the DPM sources corresponding to each material.

injections/

Enter the injections menu.

create-injection

Create an injection.

delete-injection

Delete an injection.

injection-properties/

Enter the menu to set or display properties for one or more injections.

list/

Enter the menu to display the current properties for one or more injections.

list-picked-injections

List the injections that have been selected for display using pick-injections-to-list.

list-picked-properties-to-list

List the properties that have been selected for display using pick-properties-to-list.

list-property-values

List the settings for the properties selected with pick-properties-to-list. This text command is only available when a single injection has been selected with pick-injections-to-list. This option is available if at least two injections have been selected.

list-uniform-values

List the settings for properties selected with pick-properties-to-list that have uniform values for all of the injections selected with pick-injections-to-list. This option is available if at least two injections have been selected.

list-values-per-injection

For each injection selected with pick-injections-to-list, list the values for properties selected with pick-properties-to-list. This option is available if at least two injections ave been selected.

list-values-per-property

For each property selected with pick-properties-to-list, list the values for the injections selected with pick-injections-to-list. This option is available if at least two injections have been selected.

pick-injections-to-list

Select the injection or injections for which property values will be displayed. The use of asterisks (*) as wildcards is supported.

pick-properties-to-list

Select the property or properties for which values will be displayed. The use of asterisks (*) as wildcards is supported.

set/

Enter the menu to set physical models such as drag and breakup for one or more injections.

list-picked-injections

List the injections selected for setting with pick-injections-to-set.

location/

Enters the injection location settings menu. This command is only available when you select the injection(s) using the prompts of the define/models/dpm/injections/properties/set/pick-injections-to-set text command.

spatial-staggering/

Enters the injection spatial-staggering settings menu.

stagger-atomizer-positions?

Enable spatial staggering of the atomizer injection. This option is available only if at least one atomizer injection has been selected using define/injections/properties/set/pick-injections-to-set.

stagger-radius

Specify the stagger radius of the region from which particles are released. This option is available only if at least one standard injection has been selected using define/injections/properties/set/pick-injections-to-set.

stagger-std-inj-positions?

Enable injection-specific spatial staggering of the particles. This option is available only if at least one standard injection has been selected using define/injections/properties/set/pick-injections-to-set.

physical-models

Enter the menu to set physical models such as drag and breakup for the selected injections. This command is only available when you select the injection(s) using the prompts of the define/models/dpm/injections/properties/set/pick-injections-to-set text command.

brownian-motion

Enable Brownian motion effects for the currently selected injection(s).

drag-parameters

Set the drag law and corresponding parameters for the currently selected injection(s).

particle-rotation

Enter the menu to set-up rotation related models.

enable-rotation

Enable/disable solution of ODE for the angular acceleration of particles.

magnus-lift-law

Set the law for the rotational lift coefficient used in the formulation of Magnus lift force.

rotational-drag-law

Set the law for the rotational drag coefficient.

rough-wall-model

Enable/disable the rough wall model.

spray-secondary-breakup

Enter the menu for setting the breakup model and parameters for the currently selected injection(s). Available commands are as those described under define/models/dpm/spray-model/ with the addition of the following.

pick-injections-to-set

Select the injection or injections for which properties will be set. The use of asterisks (*) as wildcards is supported.

list-particles

List particle streams in an injection.

modify-all-injections

Enter the menu to set properties for all injections.

injection-type

Define injection type.

number-of-tries

Set the number of stochastic tries.

random-eddy-lifetime?

Turn enable/disable a random eddy lifetime.

stochastic-tracking?

Turn enable/disable stochastic tracking.

time-scale-constant

Set the time scale constant.

rename-injection

Rename an injection.

set-injection-properties

Set injection properties.


Important:  Drag and breakup model parameters for each injection are set instead in /define/models/dpm/injections/injection-properties.


interaction/

Set parameters for coupled discrete phase calculations.

coupled-calculations?

Select whether or not to couple continuous and discrete phase calculations.

implicit-momentum-coupling?

Enable/disable implicit treatment for the DPM momentum source terms.

implicit-source-term-coupling?

Enable/disable implicit treatment for all DPM source terms.

linearized-dpm-source-terms?

Enable/disable linearization of source terms for the discrete phase.

dpm-iteration-interval

Set the frequency with which the particle trajectory calculations are introduced.

reset-sources-at-timestep?

Enable/disable flush of DPM source terms at beginning of every time step.

underrelaxation-factor

Set the under-relaxation factor for the discrete phase sources.

update-dpm-sources-every-flow-iteration?

Enable/disable the update of DPM source terms every flow iteration (if this option is not enabled, the terms will be updated every DPM iteration).

numerics/

Enter the numerics menu to set numerical solution parameters.

automated-scheme-selection?

Enable/disable the adaptation of integration step length based on a maximum error.

average-DDPM-variables?

Enable/disable mesh node averaging of DDPM quantities.

average-each-step?

Enable/disable mesh node averaging during integration time step.

average-kernel

Specify the averaging kernel to use for mesh node averaging.

average-source-terms?

Enable/disable mesh node averaging of DPM source terms.

coupled-heat-mass-update

Enable/disable coupled heat and mass update.

drag-law

Set the drag law.

enable-node-based-averaging?

Enable/disable mesh node averaging of DPM quantities.

error-control?

Adapt integration step length based on a maximum error.

gaussian-factor

Specify the Gaussian constant when using the gaussian kernel for mesh node averaging.

minimum-liquid-fraction

A droplet evaporates completely when the remaining mass is below this fraction of the initial droplet mass.

tracking-parameters

Set parameters for the (initial) tracking step length.

tracking-scheme

Specify a tracking scheme.

underrelax-film-height

Set the under-relaxation factor for the film height calculation. The recommended values range between 0.5 (default) and 0.9.

vaporization-limiting-factors

Set the Vaporization Fractional Change Limits.

options/

Enter the options menu to set optional models.

allow-supercritical-pressure-vaporization?

Enforce the switching from vaporization to boiling even if the boiling point is not calculated from the vapor pressure data. If the pressure in your model is above critical you must retain the default setting (yes). This options is available only if when Pressure Dependent Boiling is enabled in the Physical Models tab of the Discrete Phase Models dialog box. For more details, see Enabling Pressure Dependent Boiling in the Fluent User's Guide.

brownian-motion

Enable/disable Brownian motion of particles.

enable-contour-plots

Enable computation of mean and/or RMS values of additional discrete phase variables for postprocessing.

ensemble-average

Ensemble average cloud properties.

erosion-accretion

Enable/disable erosion/accretion.

film-separation-angle

Set the angle between faces that causes film particles to separate from the wall.

init-erosion-accretion-rate

Initialize the erosion/accretion rates with zero.

maximum-udf-species

Specify the maximum number of species that will be accessible from discrete phase model UDFs. Only species with indices up to this value are accessible in discrete phase model UDFs.

particle-radiation

Enable/disable particle radiation.

stagger-spatially-atomizer-injections?

Enable/disable spatial staggering for atomizer and solid-cone injections.

stagger-spatially-standard-injections?

Enable/disable spatial staggering for standard (non-atomizer and non-solid-cone) injections.

stagger-temporally?

Enable/disable temporal staggering.

staggering-factor

Control the percentage of every particle's initial time step that will be sampled.

pressure-gradient-force

Enable/disable inclusion of pressure gradient effects in the particle force balance.

saffman-lift-force

Enable/disable Saffman lift force.

stagger-radius

Specify the region over which to spatially stagger particles when particle-staggering is enabled for non-atomizer injections.

step-report-sig-figures

Set significant figures in the step-by-step report.

thermophoretic-force

Enable/disable thermophoretic force.

track-in-absolute-frame

Enable/disable tracking in absolute frame.

two-way-coupling

Enable/disable calculation of DPM sources in TKE equation.

uniform-mass-distribution-for-injections?

Specify a uniform distribution of mass over the cross-section of solid cone and atomizer injections. This can become important when the mesh is smaller than the diameter (or another characteristic size) of the injection.

vaporization-heat-transfer-averaging

Enables averaging of the Spalding heat transfer term for the convection/diffusion-controlled model.

vaporization-options

Set Vaporization options.

virtual-mass-force

Enable/disable inclusion of the virtual mass force in the particle force balance.

parallel/

Enter the parallel menu to set parameters for parallel DPM calculations.

enable-workpile?

Turn on/off particle workpile algorithm. This option is only available when the define/models/dpm/parallel/use-shared-memory option is selected.

hybrid-2domain?

enables or disables the use of a second domain for DPM particle tracking.

n-threads

Set the number of processors to use for DPM. This option is only available when the define/models/dpm/parallel/enable-workpile? option is enabled.

report

Print particle workpile statistics. This option is only available when the define/models/dpm/parallel/enable-workpile? option is enabled.

use-hybrid

Specify that the calculations are performed using multicore cluster computing or shared-memory machines. This option works in conjunction with openmpi for a dynamic load balancing without migration of cells.

use-message-passing

Specify that the calculations are performed using cluster computing or shared-memory machines. With this option, the compute node processes themselves perform the particle work on their local partitions and particle migration to other compute nodes is implemented using message passing primitives.

use-shared-memory

Specify that the calculations are performed on shared-memory multiprocessor machines.

splash-options

Enter the splash option menu.

orourke-splash-fraction

Enable/disable the O’Rourke formulation (default for the Lagrangian Wall Film (LWF) model). If the O’Rourke formulation is disabled, the Stanton formulation (default for the Eulerian Wall Film (EWF) model) is used in a simulation.

splash-pdf-limiting

Set the splash pdf limiting method. Available methods are: the splash pdf tail limiting (default for the LWF model) and the splash pdf peak limiting (default for the EWF model). For the splash pdf peak limiting, you will be prompted to specify the peak limiting value.

spray-model/

Enter the spray model menu. This command is available only if the breakup model enabled globally.

breakup-model-summary

Current spray model settings.

consider-children-in-the-same-tracking-step?

Enable/disable collecting and tracking new generated child droplets within the same time step.

droplet-coalescence?

Enable/disable droplet coalescence when using the stochastic collision model. This option is available if all injections have been selected and the DEM model is disabled.

droplet-collision?

Enable/disable droplet collision model.

enable-breakup?

Enable/disable breakup globally, but do not alter injection settings other than enable/disable.

khrt-model

Enable KHRT breakup model.

no-breakup

Disable the currently enabled breakup model. This option is available only if the breakup model is enabled globally and for the selected injections, and not all injections have been selected.

set-breakup

Enable/disable breakup model globally and uniformly specify injection breakup parameters.

ssd-model

Enable SSD breakup model.

tab-model

Enable TAB breakup model.

tab-number-of-breakup-parcels

Set the number of parcels to break up a droplet in the TAB model.

tab-randomize-breakup-parcel-diameter?

Enable sampling of diameter for each TAB breakup parcel from a Rosin-Rammler distribution using a random number.

wave-allow-rayleigh-growth?

Allow treatment of the Rayleigh regime, in which a cylindrical liquid jet breaks into droplets of larger diameter. This option is available only if the WAVE model is enabled.

wave-mass-cutoff

Set the minimum percentage of parent parcel mass shed before new parcel creation. This option is available only if the WAVE model is enabled.

wave-model

Enable WAVE breakup model.

wave-spray-angle-constant

Set the spray-angle constant to compute orthogonal velocity components of child droplets after breakup. This option is available only if the WAVE model is enabled.

unsteady-tracking

Enable/disable unsteady particle tracking.

user-defined

Set DPM user-defined functions.

electric-potential?

Enable/disable the electric-potential model.

energy?

Enable/disable the energy model.

eulerian-wallfilm/

Enter the Eulerian wall film model menu.

enable-wallfilm-model?

Enable/disable Eulerian Wall Film Model.

initialize-wallfilm-model

Initialize Eulerian Wall Film Model.

solve-wallfilm-equation?

Activate Eulerian Wall Film Equations.

model-options

Set Eulerian Wall Film Model Options.

film-material

Set Film Material and Properties.

solution-options

Set Eulerian Wall Film Model Solution Options.

frozen-flux?

Enable/disable frozen flux formulation for transient flows.

heat-exchanger/

Enter the heat exchanger menu.

dual-cell-model/

Enter the dual cell model menu.

add-heat-exchanger

Add heat-exchanger.

alternative-formulation?

Enable/disable alternative formulation for heat transfer calculations.

delete-heat-exchanger

Delete heat-exchanger.

heat-exchanger?

Enable/disable the dual cell heat-exchanger model.

modify-heat-exchanger

Modify heat-exchanger.

plot-NTU

Plot NTU vs. primary mass flow rate for each auxiliary mass flow rate.

write-NTU

Write NTU vs. primary mass flow rate for each auxiliary mass flow rate.

macro-model/

Enter the heat macro-model menu.

delete-heat-exchanger-group

Delete heat-exchanger group.

heat-exchanger?

Enable/disable heat-exchanger model.

heat-exchanger-group

Define heat-exchanger group.

heat-exchanger-macro-report

Report the computed values of heat rejection, outlet temperature, and inlet temperature for the macroscopic cells (macros) in a heat exchanger.

heat-exchanger-model

Define heat-exchanger core model.

heat-exchanger-report

Report the computed values of total heat rejection, outlet temperature, and inlet temperature for a specified heat-exchanger core.

heat-exchanger-zone

Specify the zone that represents the heat exchanger, the dimensions of the heat exchanger, the macro grid, and the coolant direction and properties.

plot-NTU

Plot NTU vs. primary mass flow rate for each auxiliary mass flow rate.

write-NTU

Write NTU vs. primary mass flow rate for each auxiliary mass flow rate.

multiphase/

Enter the multiphase model menu.

body-force-formulation

Specify body force formulation.

boiling-model-options

Specify the boiling model options. You can choose the RPI boiling model, Non-equilibrium boiling, or Critical heat flux.

coupled-level-set

Enable coupled level set interface tracking method.

eulerian-parameters

Specify Eulerian parameters.

expert-options

Specify the volume fraction sub-time step calculation method and whether to solve vof every iteration.

interface-modeling-options

Specify interface modeling options.

mixture-parameters

Specify mixture parameters.

model

Specify multiphase model.

number-of-phases

Specify the number of phases.

vof-sub-models

Enable the Open Channel sub-model and/or the Open Channel Wave Boundary Condition sub-model.

volume-fraction-parameters

Specify volume fraction parameters.

wet-steam/

Enter the wet steam model menu.

compile-user-defined-wetsteam-functions

Compile user-defined wet steam library.

enable?

Enable/disable the wet steam model.

load-unload-user-defined-wetsteam-library

Load or unload user-defined wet steam library.

set/

Enter the set menu for setting wet steam model options.

max-liquid-mass-fraction

Set the maximum limit on the condensed liquid-phase mass-fraction to prevent divergence.

noniterative-time-advance?

Enable/disable noniterative time advancement scheme.

nox?

Enable/disable the NOx model.

nox-parameters/

Enter the NOx parameters menu.

inlet-diffusion?

Enable/disable inclusion of diffusion at inlets.

nox-chemistry

Select NOx chemistry model.

nox-expert

Select additional NOx equations.

nox-turbulence-interaction

Set NOx turbulence interaction model.

radiation/

Enter the radiation models menu.

blending-factor

Set numeric option for Discrete Ordinate model. Make sure that Second Order Upwind is selected for the Discrete Ordinates spatial discretization for the blending-factor option to appear in the text command list.

coarsen-radiation-mesh?

Enable/disable mesh coarsening for the Monte Carlo radiation model.

discrete-ordinates?

Enable/disable discrete ordinates radiation model.

discrete-transfer?

Enable/disable discrete transfer radiation model.

do-acceleration?

Enable/disable the acceleration of the discrete ordinates (DO) radiation model calculations. Note that this text command is only available when running on Linux in parallel.

do-coupling?

Enable/disable DO/energy coupling.

do-irradiation?

Enable/disable the DO irradiation model.

dtrm-parameters/

Enter the dtrm parameters menu.

check-ray-file

Read DTRM rays file.

controls

Set dtrm solution controls.

make-globs

Make globs (coarser mesh) for radiation.

ray-trace

Create DTRM rays for radiation.

fast-second-order-discrete-ordinate?

Enable/disable the fast-second-order option for Discrete Ordinate Model.

mc-model-parameters

Specify Monte Carlo model parameters. This text command is available only when the Monte Carlo model is enabled.

mc-under-relaxation

Set the under-relaxation factor for Monte Carlo radiation sources used in the energy equation.

method-partially-specular-wall

Set the method for partially specular wall with discrete ordinate model.

montecarlo?

Enable/disable the Monte Carlo radiation model.

non-gray-model-parameters

Set parameters for non-gray model.

p1?

Enable/disable P1 radiation model.

radiation-iteration-parameters

Set iteration parameters for radiation models.

radiation-model-parameters

Set parameters for radiation models.

rosseland?

Enable/disable Rosseland radiation model.

s2s?

Enable/disable S2S radiation model.

s2s-parameters/

Enter the S2S parameters menu.

compute-fpsc-values

Compute only fpsc values based on current settings

compute-vf-only

Compute/write view factors only.

compute-write-vf

Compute/write surface clusters and view factors for S2S radiation model.

non-participating-boundary-zones-temperature

Set temperature for the non-participating boundary zones.

print-thread-clusters

Print the following for all boundary threads: thread-id, number of faces, faces per surface cluster, and the number of surface clusters.

print-zonewise-radiation

Print the zonewise incoming radiation, viewfactors, and average temperature.

read-vf-file

Read S2S file.

set-global-faces-per-surface-cluster

Set global value of faces per surface cluster for all boundary zones.

set-vf-parameters

Set the parameters needed for the viewfactor calculations.

split-angle

Set split angle for the clustering algorithm.

use-new-cluster-algorithm

Use the new surface clustering algorithm.

use-old-cluster-algorithm

Use the old surface clustering algorithm.

solar?

Enable/disable solar model.

solar-calculator

Calculate sun direction and intensity.

solar-parameters/

Enter the solar parameters menu.

autoread-solar-data

Set autoread solar data parameters.

autosave-solar-data

Set autosave solar data parameters.

ground-reflectivity

Set ground reflectivity parameters.

illumination-parameters

Set illumination parameters.

iteration-parameters

Set update parameters.

quad-tree-parameters

Set quad-tree refinement parameters.

scattering-fraction

Set scattering fraction parameters.

solar-thread-control

Set the number of threads to run the solar flux calculation. This item appears only when running in parallel with nodes located on a separate machine from the one running the host process and Solar Ray Tracing is enabled.

sol-adjacent-fluidcells

Set solar load on for adjacent fluid cells.

sol-camera-pos

Set camera position based on sun direction vector.

sol-on-demand

Set solar load on demand.

sun-direction-vector

Set sun direction vector.

use-direction-from-sol-calc

Set direction computed from solar calculator.

solution-method-for-do-coupling

Enable/disable the solution method for DO/energy coupling.

wsggm-cell-based

Enable/disable WSGGM cell based method. Note that when enabled, the wsggm-cell-based option will become available in the Absorption Coefficient drop-down list in the Create/Edit Materials dialog box.

shell-conduction/

Enter the shell conduction models menu.

enhanced-encapsulation?

Enable/disable an enhanced routine for the encapsulation of coupled walls during mesh partitioning that is enabled by default when shell conduction and/or the surface to surface (S2S) radiation model is used.

multi-layer-shell?

Enable/disable the ability to define multi-layer shell conduction for walls. Note that the warped-face gradient correction (WFGC) is not supported when multi-layer shells are disabled.

read-csv

Define the shell conduction settings by reading a CSV file.

settings

Enable shell conduction and define the settings for any wall or group of walls by manually entering the number and properties of the layers.

write-csv

Write your saved shell conduction settings to a CSV file.

solidification-melting?

Enable/disable the solidification and melting model.

solver/

Enter the menu to select the solver.

density-based-explicit

Enable/disable the density-based-explicit solver.

density-based-implicit

Enable/disable the density-based-implicit solver.

pressure-based

Enable/disable the pressure-based solver.

soot?

Enable/disable the soot model.

soot-parameters/

Enter the soot parameters menu.

inlet-diffusion?

Enable/disable inclusion of diffusion at inlets.

modify-schmidt-number?

Change the turbulent Schmidt number for soot/nuclei equations.

soot-model-parameters

Select soot model parameters.

soot-process-parameters

Select soot process parameters.

soot-radiation-interaction

Enable/disable the soot-radiation interaction model.

soot-turbulence-interaction

Set soot-turbulence interaction model.

sox?

Enable/disable the SOx model.

sox-parameters/

Enter the SOx parameters menu.

inlet-diffusion?

Enable/disable inclusion of diffusion at inlets.

s-atom-balance?

Enable/disable S-atom mass balance calculation.

sox-chemistry

Select the SOx chemistry model.

sox-turbulence-interaction

Set the SOx /turbulence interaction model.

species/

Enter the species models menu.

CHEMKIN-CFD?

Enable/disable the ANSYS CHEMKIN-CFD solver.

CHEMKIN-CFD-parameters/

Enter the expert CHEMKIN-CFD parameters menu.

add-cell-monitor

Monitor cell for debug output.

advanced-options

Set advanced parameter options.

basic-options

Set basic parameter options.

delete-cell-monitors

Delete cell monitors.

list-cell-monitors

List cell monitors.

clear-isat-table

Kill ISAT table.

coal-calculator

Set up coal modeling inputs.

decoupled-detailed-chemistry?

Enable/disable the Decoupled Detailed Chemistry model.

diffusion-energy-source?

Enable/disable diffusion energy source.

electro-chemical-surface-reactions?

Enable/disable electrochemical surface reactions.

epdf-energy?

Enable/disable EPDF energy option.

flamelet-expert

Set flamelet expert parameters.

full-tabulation?

Enable/disable building of a full 2-mixture fraction table

heat-of-surface-reactions?

Enable/disable heat of surface reactions.

ignition-model?

Enable/disable the ignition model.

ignition-model-controls

Set ignition model parameters.

import-flamelet-for-restart

Import Flamelet File for Restart.

inert-transport-controls

Set inert transport model parameters.

inert-transport-model?

Enable/disable the inert transport model.

inlet-diffusion?

Enable/disable inclusion of diffusion at inlets.

integration-parameters

Set chemistry ODE integrator parameters. Enable/disable stiff chemistry acceleration methods and set their parameters.

init-unsteady-flamelet-prob

Initialize Unsteady Flamelet Probability.

liquid-energy-diffusion?

Enable/disable energy diffusion for liquid regime.

liquid-micro-mixing?

Enable/disable liquid micro mixing.

mass-deposition-source?

Enable/disable mass deposition source due to surface reactions.

mixing-model

Set PDF Transport mixing model.

multicomponent-diffusion?

Enable/disable multicomponent diffusion.

non-premixed-combustion?

Enable/disable non-premixed combustion model.

non-premixed-combustion-expert

Set PDF expert parameters.

non-premixed-combustion-parameters

Set PDF parameters.

off?

Enable/disable solution of species models.

partially-premixed-combustion?

Enable/disable partially premixed combustion model.

partially-premixed-combustion-expert

Set PDF expert parameters.

partially-premixed-combustion-parameters

Set PDF parameters.

partially-premixed-properties

Set/change partially-premixed mixture properties. This command is only available when partially-premixed-combustion? is enabled.

re-cacl-par-premix-props

Re-calculate partially-premixed properties. This command is only available when partially-premixed-combustion? is enabled.

particle-surface-reactions?

Enable/disable particle surface reactions.

pdf-transport?

Enable/disable the composition PDF transport combustion model.

pdf-transport-expert?

Enable/disable PDF Transport expert user.

premixed-model

Set premixed combustion model.

premixed-combustion?

Enable/disable premixed combustion model.

reaction-diffusion-balance?

Enable/disable reaction diffusion balance at reacting surface for surface reactions.

reacting-channel-model?

Enable/disable the Reacting Channel Model.

reacting-channel-model-options

Set Reacting Channel Model parameters.

reactor-network-model?

Enable/disable the Reactor Network Model.

relax-to-equil?

Enable/disable the Relaxation to Chemical Equilibrium model.

save-gradients?

Enable/disable storage of species mass fraction gradients.

set-premixed-combustion

Set premixed combustion parameters.

set-turb-chem-interaction

Set EDC model constants.

spark-model

Switch between the R15 and R14.5 spark models and set spark model parameters.

species-migration?

Include species migration in electric field. This command is available only when the electrochemical surface reactions are enabled.

species-transport-expert

Set the convergence acceleration expert parameters. This command is only available when the species transport model is enabled.

use convergence acceleration method?

Answering yes at the prompt, uses a combination of different convergence acceleration techniques. If you enter no (default), additional options will be displayed in the console.

Use species clipping?

Enable/disable the explicit clipping of species between 0 and 1.

Linearize higher order convection sources?

Enable/disable linearization of higher order convection sources.

Linearize secondary diffusion sources?

Enable/disable linearization of species secondary diffusion sources.

Enable mesh quality based first-second order species blending?

Enable/disable skewness-based blending of first and second order convection.

Minimum cell quality threshold for blending

Specify the minimum cell orthogonal quality for blending.

species-transport?

Enable/disable the species transport model.

stiff-chemistry?

Enable/disable stiff chemistry option.

surf-reaction-aggressiveness-factor?

Set the surface reaction aggressiveness factor.

surf-reaction-netm-params

Set the surface reaction parameters for the Non-Equilibrium Thermal Model.

thermal-diffusion?

Enable/disable thermal diffusion.

thickened-flame-model?

Enable/disable the Relaxation to Chemical Equilibrium model

volumetric-reactions?

Enable/disable volumetric reactions.

wall-surface-reactions?

Enable/disable wall surface reactions.

steady?

Enable/disable the steady solution model.

swirl?

Enable/disable axisymmetric swirl velocity.

unsteady-1st-order?

Enable/disable first-order unsteady solution model.

unsteady-2nd-order-bounded?

Enable/disable bounded second-order unsteady formulation.

unsteady-2nd-order?

Enable/disable the second-order unsteady solution model.

unsteady-global-time?

Enable/disable the unsteady global-time-step solution model.

viscous/

Enter the viscous model menu.

add-intermittency-transition-model?

Enable/disable the Intermittency Transition model to account for transitional effects. This text command is only available for the BSL -, SST -, Scale-Adaptive Simulation with BSL / SST, and Detached Eddy Simulation with BSL / SST models.

buoyancy-effects?

Enable/disable effects of buoyancy on turbulence.

curvature-correction?

Enable/disable the curvature correction.

des-limiter-option

Select the DES limiter option (none, F1, F2, Delayed DES, or Improved Delayed DES).

detached-eddy-simulation?

Enable/disable detached eddy simulation.

inviscid?

Enable/disable inviscid flow model.

ke-easm?

Enable/disable the EASM - turbulence model.

ke-realizable?

Enable/disable the realizable - turbulence model.

ke-rng?

Enable/disable the RNG - turbulence model.

ke-standard?

Enable/disable the standard - turbulence model.

k-kl-w?

Enable/disable the k-kl- turbulence model.

kw-easm?

Enable/disable the EASM - turbulence model.

kw-low-re-correction?

Enable/disable the - low Re option.

kw-shear-correction?

Enable/disable the - shear-flow correction option. This text command is only available for the standard - model and the stress-omega RSM model.

kw-bsl?

Enable/disable the baseline (BSL) - turbulence model.

kw-sst?

Enable/disable the SST - turbulence model.

kw-standard?

Enable/disable the standard - turbulence model.

laminar?

Enable/disable laminar flow model.

large-eddy-simulation?

Enable/disable large eddy simulation.

les-dynamic-energy-flux?

Enable/disable the dynamic sub-grid scale turbulent Prandtl Number.

les-dynamic-scalar-flux?

Enable/disable the dynamic sub-grid scale turbulent Schmidt Number.

les-subgrid-dynamic-fvar?

Enable/disable the dynamic subgrid-scale mixture fraction variance model.

les-subgrid-smagorinsky?

Enable/disable the Smagorinsky-Lilly subgrid-scale model.

les-subgrid-tke?

Enable/disable kinetic energy transport subgrid-scale model.

les-subgrid-wale?

Enable/disable WALE subgrid-scale model.

les-subgrid-wmles-s_minus_omega?

Enable/disable the WMLES - subgrid-scale model.

les-subgrid-wmles?

Enable/disable the WMLES subgrid-scale model.

mixing-length?

Enable/disable mixing-length (algebraic) turbulence model.

multiphase-turbulence/

Enter the multiphase turbulence menu.

multiphase-options

Enable/disable multiphase options.

rsm-multiphase-models

Select Reynolds Stress multiphase model.

turbulence-multiphase-models

Select - multiphase model.

near-wall-treatment/

Enter the near wall treatment menu.

enhanced-wall-treatment?

Enable/disable enhanced wall functions.

menter-lechner?

Enable/disable the Menter-Lechner near-wall treatment.

non-equilibrium-wall-fn?

Enable/disable non-equilibrium wall functions.

scalable-wall-functions?

Enable/disable scalable wall functions.

standard-wall-fn?

Enable/disable standard wall functions.

user-defined-wall-functions?

Enable/disable user-defined wall functions.

werner-wengle-wall-fn?

Enable/disable Werner-Wengle wall functions.

wf-pressure-gradient-effects?

Enable/disable wall function pressure- gradient effects.

wf-thermal-effects?

Enable/disable wall function thermal effects.

reynolds-stress-model?

Enable/disable the Reynolds-stress turbulence model.

rng-differential-visc?

Enable/disable the differential-viscosity model.

rng-swirl-model?

Enable/disable swirl corrections for rng-model.

rsm-bsl-based?

Enable/disable the stress-BSL Reynolds stress model.

rsm-linear-pressure-strain?

Enable/disable the linear pressure-strain model in RSM.

rsm-omega-based?

Enable/disable the stress-omega Reynolds stress model.

rsm-solve-tke?

Enable/disable the solution of T.K.E. in RSM model.

rsm-ssg-pressure-strain?

Enable/disable quadratic pressure-strain model in RSM.

rsm-wall-echo?

Enable/disable wall-echo effects in RSM model.

sa-alternate-prod?

Enable/disable strain/vorticity production in Spalart-Allmaras model.

sa-damping?

Enable/disable full low-Reynolds number form of Spalart-Allmaras model.


Note:  This option is only available if your response was no to sa-enhanced-wall-treatment?.


sa-enhanced-wall-treatment?

Enable/disable the enhanced wall treatment for the Spalart-Allmaras model. If disabled, no smooth blending between the viscous sublayer and the log-law formulation is employed, as was done in versions previous to Fluent 14.

sas?

Enable/disable Scale-Adaptive Simulation (SAS) in combination with the SST - turbulence model.

spalart-allmaras?

Enable/disable Spalart-Allmaras turbulence model.

transition-sst?

Enable/disable the transition SST turbulence model.

trans-sst-roughness-correlation?

Enable/disable the Transition-SST roughness correlation option.

turb-compressibility?

Enable/disable the compressibility correction option.

turbulence-expert/

Enter the turbulence expert menu.

curvature-correction-coefficient

Set the strength of the curvature correction term. The default value is 1. This is available after the curvature-correction? option is enabled.

kato-launder-model?

Enable/disable Kato-Launder modification.

kw-add-des?

Enable/disable Detached Eddy Simulation (DES) in combination with the currently selected BSL - model or transition SST model. This text command is only available for transient cases.

kw-add-sas?

Enable/disable Scale-Adaptive Simulation (SAS) in combination with the currently selected -based URANS turbulence model. This text command is only available for transient cases.

kw-vorticity-based-production?

Enable/disable vorticity-based production.

low-re-ke?

Enable/disable the low-Re - turbulence model.

low-re-ke-index

Specify which low-Reynolds-number - model is to be used. Six models are available:

Index Model

0

Abid

1

Lam-Bremhorst

2

Launder-Sharma

3

Yang-Shih

4

Abe-Kondoh-Nagano

5

Chang-Hsieh-Chen

Contact your ANSYS, Inc. technical support engineer for more details.

production-limiter?

Enable/disable Production Limiter modification.

non-newtonian-modification?

Enable/disable non-Newtonian modification for Lam-Bremhorst model.

restore-sst-v61?

Enable/disable SST formulation of v6.1.

rke-cmu-rotation-term?

Modify the definition for the realizable - model.


Important:  Note that the use of the realizable - model with multiple reference frames is not recommended. This text command is provided for expert users who want to experiment with this combination of models. Others should use it only on the advice of a technical support engineer.


sbes-sdes-hybrid-model

Select the hybrid model, to specify whether you want to apply the Shielded Detached Eddy Simulation (SDES) model, Stress-Blended Eddy Simulation (SBES), or SBES with a user-defined function.

sbes-sgs-option

Select the subgrid-scale model for the LES portion of your Stress-Blended Eddy Simulation (SBES).

thermal-p-function?

Enable/disable Jayatilleke P function.

turb-add-sbes-sdes?

Enable/disable the Stress-Blended Eddy Simulation (SBES) model or Shielded Detached Eddy Simulation (SDES) model.

turb-non-newtonian?

Enable/disable turbulence for non-Newtonian fluids.

turbulence-damping?

Enable/disable turbulence damping and set turbulence damping parameters.

turb-pk-compressible?

Enable/disable turbulent production due to compressible divergence.

user-defined

Select user-defined functions to define the turbulent viscosity and the turbulent Prandtl and Schmidt numbers.

user-defined-transition

Set user-defined transition correlations.

v2f?

Enable/disable V2F turbulence model.

zero-equation-hvac?

Enable/disable zero-equation HVAC turbulence model.

operating-conditions/

Enter the define operating conditions menu.

gravity

Set gravitational acceleration.

gravity-mrf-rotation

Enable/disable rotation of gravity vector in moving reference frame simulations. If enabled, the gravity vector will rotate with respect to the moving reference frame such that the direction of gravity in global coordinates remains fixed.

operating-density?

Enable/disable use of a specified operating density.

operating-pressure

Set the operating pressure.

operating-temperature

Set the operating temperature for Boussinesq.

reference-pressure-location

Set the location of the cell whose pressure value is used to adjust the gauge pressure field for incompressible flows that do not involve any pressure boundaries.

set-phase

Select phase for real gas EOS subcritical condition.

used-ref-pressure-location

See the actual coordinates of the reference pressure used.

use-inlet-temperature-for-operating-density

Use inlet temperature to calculate operating density.

overset-interfaces/

Enter the overset interfaces menu.

check

Checks the integrity of the overset interfaces. Reports orphan cells and errors in the domain connectivity.

clear

Clears the domain connectivity of an overset interface. This text command is only available when define/overset-interfaces/options/expert is set to yes.

clear-all

Clears the domain connectivity of all overset interfaces. This text command is only available when define/overset-interfaces/options/expert is set to yes.

create

Creates an overset interface.

debug-hole-cut

Debugging tool to troubleshoot hole cutting of overset interfaces. This text command is only available when define/overset-interfaces/options/expert is set to yes.

delete

Deletes an overset interface.

delete-all

Deletes all overset interfaces in the domain.

grid-priorities

Allows you to specify grid priorities on background and component meshes, used in the overlap minimization of an overset interface.

intersect

Executes the hole cutting of an overset interface and establishes the domain connectivity. This text command is only available when define/overset-interfaces/options/expert is set to yes.

intersect-all

Executes hole cutting for all overset interfaces in the domain. This text command is only available when define/overset-interfaces/options/expert is set to yes.

list

Lists information about the overset interfaces. The output depends on the overset verbosity setting.

mark-cell-change

Marks cells that have undergone a specified overset cell type change (from solve, receptor, or dead to any other type) in the last time step. Adaption registers are automatically filled based on these markings. This text command is only available for unsteady simulations and if define/overset-interfaces/options/expert is set to yes.

mark-cells

Marks the specified overset cells (solve, receptor, donor, orphan, or dead) and fills adaption registers based on the markings. Display the registers via the text command adapt/display-register.

options/

Enters the overset interface options menu.

auto-create?

Enables the automatic creation of a default overset interface during initialization or mesh motion update.

donor-priority-method

Allows you to specify whether the cell donor priority used in the overlap minimization of an overset interface is inversely proportional to either the cell size or the distance to the nearest boundary.

expert

Enables / disables overset-related expert tools.

extended-donor-search?

Enables / disables modified donor search parameters. When enabled, more conservative overset parameters are used for the creation of the overset interface (at the cost of increased processing time). This text command is only available when define/overset-interfaces/options/expert is set to yes.

minimize-overlap?

Allows you to disable overlap minimization during hole cutting.

node-connected-donors?

Allows you to switch between face or node connected donor cells. This text command is only available when define/overset-interfaces/options/expert is set to yes.

overlap-boundaries?

Allows you to disable detection of overlap boundaries during hole cutting.

render-receptor-cells?

Allows you to enable visualization of receptor cells in contour and mesh displays.

solve-island-removal

Sets the method used to control the removal of isolated patches of solve cells. This text command is only available when define/overset-interfaces/options/expert is set to yes.

transient-caching

Sets the options to control caching of entities in transient overset simulations. This text command is only available when define/overset-interfaces/options/expert is set to yes.

update-before-case-write?

Enables / disables the updating of the overset interfaces before writing a case file in the hierarchical data format (HDF). This text command is only available when define/overset-interfaces/options/expert is set to yes.

verbosity

Specify the level of detail printed in the console about overset interfaces.

parameters/

Enter the parameters menu.

enable-in-TUI?

Enable/disable parameters in the text user interface.

input-parameters/

Enter the input-parameters menu.

delete

Delete an input parameter.

edit

Edit an input parameter.

output-parameters/

Enter the output-parameters menu.

create

Create an output parameter.

delete

Delete an output parameter.

edit

Edit an output parameter.

print-all-to-console

Display all parameter values in the console.

print-to-console

Display parameter value in the console.

write-all-to-file

Write all parameter values to file.

write-to-file

Write parameter value to file.

periodic-conditions/

Enter the periodic conditions menu.

massflow-rate-specification?

Enable/disable specification of mass flow rate at the periodic boundary.

pressure-gradient-specification?

Enable/disable specification of pressure gradient at the periodic boundary.

phases/

Enter the phases menu.

domain/

Enter the domain menu.

iac-expert/

Enter the IAC expert setting menu.

hibiki-ishii-model

Set Hibiki-Ishii model coefficients.

ishii-kim-model

Set Ishii-Kim model coefficients.

yao-morel-model

set Yao-Morel model coefficients.

interaction-domain

Set models and properties for a domain of this type.

phase-domain

Set models and properties for a domain of this type.

profiles/

Enter the boundary profiles menu.

delete

Delete a profile.

delete-all

Delete all boundary-profiles.

interpolation-method

Choose the method for interpolation of profiles.

list-profiles

List all profiles.

list-profile-fields

List the fields of a particular profile.

morphing?

Enable/disable profile morphing options in Orient Profile panel.

update-interval

Set interval between updates of dynamic profiles.

solution-strategy/

Enter the automatic initialization and case modification strategy menu.

automatic-case-modification/

Enter the automatic case modification menu.

before-init-modification

Specify modification to be performed before initialization.

modifications

Specify modifications to be performed during solution.

original-settings

Specify modification to be performed after initialization to restore to original settings.

automatic-initialization

Define how the case is to be automatically initialized.

continue-strategy-execution

Continue execution of the currently defined automatic initialization and case modification strategy.

enable-strategy?

Enable/disable automatic initialization and case modification.

execute-strategy

Execute the currently defined automatic initialization and case modification strategy.

turbo/

Enter the turbo menu.

define-topology

Define a turbo topology.

mesh-method

Set turbo structured mesh generation method.

search-method

Set search method for a topology.

projection-method

Set 2D projection method.

units

Set unit conversion factors.

user-defined/

Enter the user-defined functions and scalars menu.

1D-coupling

Load 1D library.

compiled-functions

Open user-defined function library.

execute-on-demand

Execute UDFs on demand.

fan-model

Configure user-defined fan model.

function-hooks

Hook up user-defined functions.

interpreted-functions

Load interpreted user-defined functions.

real-gas-models

Enter the real-gas menu to enable/configure real gas model.

nist-multispecies-real-gas-model

Load the NIST real-gas library.

nist-real-gas-model

Load the NIST real-gas library.

nist-settings

Specify the name and the location for the REFPROP library and fluid files.

set-phase

Select the phase for NIST real gas model.

user-defined-multispecies-real-gas-model

Load a user-defined multispecies real-gas library.

user-defined-real-gas-model

Load the user-defined real-gas library.

use-contributed-cpp?

Enable/disable use of the cpp utility included with the ANSYS Fluent installation.

user-defined-memory

Allocate user-defined memory.

user-defined-scalars

Define user-defined scalars.


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