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/ command.<type>
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-propertiesCreate / edit a set of six DOF properties for rigid body motion.
delete-propertiesDelete a set of six DOF properties for rigid body motion.
list-propertiesPrint 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.
editEdit 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-radiusSpecify 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-optionsEnter the splash option menu.
orourke-splash-fractionEnable/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-limitingSet 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.