define/boundary-conditions/Enters 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 an asterisk (*) in the name of the zone to which you want to copy the conditions.define/boundary-conditions/axisSets boundary conditions for a zone of this type.
define/boundary-conditions/bc-settings/Enters the boundary conditions settings menu.
define/boundary-conditions/bc-settings/degassing-verbositySets the verbosity level of the total mass flow rate at the degassing boundary. If set to 1 (the default), the information will be reported in the console. Changing it to 0 disables the reporting. This item is available only when a degassing boundary condition is being used in the simulation.
define/boundary-conditions/bc-settings/mass-flowSelects method for setting the mass flow rate.
define/boundary-conditions/bc-settings/pressure-outletSets advanced options for pressure outlet boundaries.
define/boundary-conditions/bc-settings/pressure-far-fieldSets advanced options for pressure far field boundaries.
define/boundary-conditions/bc-settings/pressure-far-field/riemann-invariants-tangency-correction?Enables/disables the Riemann-invariant tangency correction as described in Tangency Correction.
define/boundary-conditions/bc-settings/pressure-far-field/type?Enables/disables the flux-based treatment of the far-field boundary condition as described in Flux-based Pressure Far-Field.
define/boundary-conditions/copy-bcCopies boundary conditions to other zones.
define/boundary-conditions/degassingSets boundary conditions for a zone of this type.
define/boundary-conditions/detect-boundary-advectionReviews the boundary walls adjacent to solid zones that involve solid motion, and automatically enables the modeling of boundary advection where needed, in order to account for the heat that advects into or out of the domain due to the solid motion. Boundary advection is enabled for a wall when the average angle of the velocity of the solid is greater than 2 degrees at the wall. This text command is only available when the energy equation is enabled and solid motion is enabled for a solid zone with a nonzero velocity.
define/boundary-conditions/exhaust-fanSets boundary conditions for a zone of this type.
define/boundary-conditions/fanSets boundary conditions for a zone of this type.
define/boundary-conditions/fluidSets boundary conditions for a zone of this type.
define/boundary-conditions/impedance-data-fitting/Enters the impedance data fitting menu, which provides text commands that can be helpful when you are using the impedance boundary condition (IBC).
define/boundary-conditions/impedance-data-fitting/absorption-dataReads an input file with experimental absorption coefficient data in the frequency domain and then computes the terms needed for an approximation of the reflection coefficient as a series of poles / residues in the time domain. The resulting terms are printed in the console, and can be written to a pole / residue file (which can be imported and the impedance parameters applied to a boundary condition using the
define/boundary-conditions/impedance-data-fitting/import-parameterstext command). You can also write a file with fitted frequency / impedance data, which can be compared to the input data to evaluate how well it fits.define/boundary-conditions/impedance-data-fitting/convergence-toleranceSets the convergence tolerance, which is an accuracy that is used for completing the iterative fitting procedure in the calculations performed from the
define/boundary-conditions/impedance-data-fitting/text command menu. By default, the tolerance is set to 1e-6.define/boundary-conditions/impedance-data-fitting/impedance-dataReads an input file with experimental specific impedance data in the frequency domain and then computes the terms needed for an approximation of the reflection coefficient as a series of poles / residues in the time domain. The resulting terms are printed in the console, and can be written to a pole / residue file (which can be imported and the impedance parameters applied to a boundary condition using the
define/boundary-conditions/impedance-data-fitting/import-parameterstext command). You can also write a file with fitted frequency / impedance data, which can be compared to the input data to evaluate how well it fits.define/boundary-conditions/impedance-data-fitting/import-parametersReads a pole / residue file with impedance parameters in the time domain and applies them to a specified boundary condition.
define/boundary-conditions/impedance-data-fitting/iterationsSets the number of internal iterations used for the calculations performed from the
define/boundary-conditions/impedance-data-fitting/text command menu. By default, the number of iterations is set to 20.define/boundary-conditions/impedance-data-fitting/reflection-dataReads an input file with experimental reflection coefficient data in the frequency domain and then computes the terms needed for an approximation of the reflection coefficient as a series of poles / residues in the time domain. The resulting terms are printed in the console, and can be written to a pole / residue file (which can be imported and the impedance parameters applied to a boundary condition using the
define/boundary-conditions/impedance-data-fitting/import-parameterstext command). You can also write a file with fitted frequency / impedance data, which can be compared to the input data to evaluate how well it fits.define/boundary-conditions/impedance-data-fitting/residue-toleranceSets the residue tolerance, which is the minimum value of residues that are kept in the fitting performed from the
define/boundary-conditions/impedance-data-fitting/text command menu. This residue check helps to eliminate parasitic poles. By default, the tolerance is set to 1e-6.define/boundary-conditions/impedance-data-fitting/verbositySets the verbosity of the progress messages during the fitting performed from the
define/boundary-conditions/impedance-data-fitting/text command menu. Setting this to1results in messages being printed in the console as the fitting calculation progresses. The default value of0suppresses this output.
define/boundary-conditions/inlet-ventSets boundary conditions for a zone of this type.
define/boundary-conditions/intake-fanSets boundary conditions for a zone of this type.
define/boundary-conditions/interfaceSets boundary conditions for a zone of this type.
define/boundary-conditions/interiorSets boundary conditions for a zone of this type.
define/boundary-conditions/knudsen-number-calculatorComputes the Knudsen number based on a characteristic physical length and the area-averaged flow quantities along an incoming-flow boundary. You can use this information to determine flow regime for selecting the appropriate wall boundary treatment. For details, see Partial Slip for Rarefied Gases in the Fluent User's Guide.
define/boundary-conditions/list-zonesPrints 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.
define/boundary-conditions/mass-flow-inletSets boundary conditions for a zone of this type.
define/boundary-conditions/mass-flow-outletSets boundary conditions for a zone of this type.
define/boundary-conditions/modify-zones/Enters the modify zones menu.
define/boundary-conditions/modify-zones/activate-cell-zoneActivates cell thread.
define/boundary-conditions/modify-zones/append-meshAppends new mesh.
define/boundary-conditions/modify-zones/append-mesh-dataAppends new mesh with data.
define/boundary-conditions/modify-zones/change-zone-stateSets the state (liquid or vapor) for a specific fluid zone.
define/boundary-conditions/modify-zones/convert-all-solid-mrf-to-solid-motionConverts all solid zones using frame motion to instead use solid motion, copying the motion variable values for origin, axis, and velocities.
define/boundary-conditions/modify-zones/copy-move-cell-zoneCreates 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).
define/boundary-conditions/modify-zones/copy-mrf-to-mesh-motionCopies motion variable values for origin, axis, and velocities from Frame Motion to Mesh Motion.
define/boundary-conditions/modify-zones/copy-mesh-to-mrf-motionCopies motion variable values for origin, axis, and velocities from Mesh Motion to Frame Motion.
define/boundary-conditions/modify-zones/create-all-shell-threadsMarks all finite thickness walls for shell creation. Shell zones will be created at the start of the iterations.
define/boundary-conditions/modify-zones/create-periodic-interfaceCreates a conformal or non-conformal periodic interface.
define/boundary-conditions/modify-zones/deactivate-cell-zoneDeactivates cell thread.
define/boundary-conditions/modify-zones/delete-all-shellsDeletes all shell zones and switches off shell conduction on all the walls. These zones can be recreated using the command
recreate-all-shells.define/boundary-conditions/modify-zones/delete-cell-by-markDeletes cells that are marked by a specified cell register, creating one boundary zone of type symmetry for each cell zone at the faces that the deleted cells shared with their neighboring cells. This text command is not supported with overset meshes or shell conduction walls.
define/boundary-conditions/modify-zones/delete-cell-zoneDeletes a cell thread.
define/boundary-conditions/modify-zones/extrude-face-zone-deltaExtrudes a face thread a specified distance based on a list of deltas.
define/boundary-conditions/modify-zones/extrude-face-zone-paraExtrudes 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.
define/boundary-conditions/modify-zones/fuse-face-zonesAttempts to fuse zones by removing duplicate faces and nodes.
define/boundary-conditions/modify-zones/list-zonesLists zone IDs, types, kinds, and names.
define/boundary-conditions/modify-zones/make-periodicAttempts to establish periodic/shadow face zone connectivity.
define/boundary-conditions/modify-zones/matching-toleranceSets normalized tolerance used for finding coincident nodes.
define/boundary-conditions/modify-zones/merge-zonesMerges zones of same type and condition into one.
define/boundary-conditions/modify-zones/mrf-to-sliding-meshChanges the motion specification from MRF to moving mesh.
define/boundary-conditions/modify-zones/orient-face-zoneOrients the face zone.
define/boundary-conditions/modify-zones/recreate-all-shellsRecreates shells on all the walls that were deleted using the command
delete-all-shells.define/boundary-conditions/modify-zones/replace-zoneReplaces cell zone.
define/boundary-conditions/modify-zones/rotate-zoneRotates individual cell zones.
define/boundary-conditions/modify-zones/scale-zoneScales individual cell zones.
define/boundary-conditions/modify-zones/sep-cell-zone-markSeparates cell zone based on cell marking.
define/boundary-conditions/modify-zones/sep-cell-zone-regionSeparates cell zone based on contiguous regions.
define/boundary-conditions/modify-zones/sep-face-zone-angleSeparates face zone based on significant angle.
define/boundary-conditions/modify-zones/sep-face-zone-faceSeparates each face in zone into unique zone.
define/boundary-conditions/modify-zones/sep-face-zone-markSeparates face zone based on cell marking.
define/boundary-conditions/modify-zones/sep-face-zone-regionSeparates face zone based on contiguous regions.
define/boundary-conditions/modify-zones/slit-periodicSlits periodic zone into two symmetry zones.
define/boundary-conditions/modify-zones/slit-face-zoneSlits two-sided wall into two connected wall zones.
define/boundary-conditions/modify-zones/slit-interior-between-diff-solidsSlits 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.
define/boundary-conditions/modify-zones/translate-zoneTranslates individual cell zones.
define/boundary-conditions/modify-zones/zone-nameGives a zone a new name.
define/boundary-conditions/modify-zones/zone-typeSets 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.
define/boundary-conditions/non-overlapping-zone-nameDisplays the name of the non-overlapping zone associated with a specified interface zone. This text command is only available after a mesh interface has been created.
define/boundary-conditions/non-reflecting-bc/Enters the non-reflecting boundary condition menu.
define/boundary-conditions/non-reflecting-bc/general-nrbc/Setting for general non-reflecting b.c.
define/boundary-conditions/non-reflecting-bc/general-nrbc/set/Enters the setup menu for general non-reflecting b.c.’s.
define/boundary-conditions/non-reflecting-bc/general-nrbc/set/sigmaSets NRBC sigma factor (default value 0.15).
define/boundary-conditions/non-reflecting-bc/general-nrbc/set/sigma2Sets NRBC sigma2 factor (default value 5.0).
define/boundary-conditions/non-reflecting-bc/general-nrbc/set/verbosityEnables/disables nrbc verbosity scheme output.
define/boundary-conditions/non-reflecting-bc/turbo-specific-nrbc/Enters the turbo specific nrbc menu.
define/boundary-conditions/non-reflecting-bc/turbo-specific-nrbc/enable?Enables/disables non-reflecting b.c.’s.
define/boundary-conditions/non-reflecting-bc/turbo-specific-nrbc/initializeInitializes non-reflecting b.c.’s.
define/boundary-conditions/non-reflecting-bc/turbo-specific-nrbc/set/Enters the set menu for non-reflecting b.c. parameters.
define/boundary-conditions/non-reflecting-bc/turbo-specific-nrbc/set/discretizationEnables use of higher-order reconstruction at boundaries if available.
define/boundary-conditions/non-reflecting-bc/turbo-specific-nrbc/set/under-relaxationSets non-reflecting b.c. under-relaxation factor.
define/boundary-conditions/non-reflecting-bc/turbo-specific-nrbc/set/verbositySets non-reflecting b.c. verbosity level. 0 : silent, 1 : basic information (default), 2 : detailed information for debugging.
define/boundary-conditions/non-reflecting-bc/turbo-specific-nrbc/show-statusShows current status of non-reflecting b.c.’s.
define/boundary-conditions/open-channel-wave-settingsOpens channel wave input analysis.
define/boundary-conditions/openchannel-threadsLists open channel group IDs, names, types and variables.
define/boundary-conditions/outflowSets boundary conditions for a zone of this type.
define/boundary-conditions/outlet-ventSets boundary conditions for a zone of this type.
define/boundary-conditions/perforated-walls/Enters the perforated walls menu.
define/boundary-conditions/perforated-walls/model-setupSets up the perforated wall model for each effusion surface.
define/boundary-conditions/perforated-walls/read-input-fileReads an input file for perforated walls.
define/boundary-conditions/periodicSets boundary conditions for a zone of this type.
define/boundary-conditions/phase-shift/Enters the phase shift settings menu.
define/boundary-conditions/phase-shift/multi-disturbancesSets basic phase-shift parameters.
define/boundary-conditions/phase-shift/extra-settingsSets other phase-shift parameters.
define/boundary-conditions/physical-velocity-porous-formulation?Enables the physical velocity (rather than superficial velocity) porous formulation. This text command is only available when you have enabled the porous zone option for a cell zone while using the pressure-based solver.
define/boundary-conditions/porous-jumpSets boundary conditions for a zone of this type.
define/boundary-conditions/pressure-far-fieldSets boundary conditions for a zone of this type.
define/boundary-conditions/pressure-inletSets boundary conditions for a zone of this type.
define/boundary-conditions/pressure-outletSets boundary conditions for a zone of this type.
define/boundary-conditions/radiatorSets boundary conditions for a zone of this type.
define/boundary-conditions/rans-les-interfaceSets boundary conditions for a zone of this type.
define/boundary-conditions/recirculation-inletSets boundary conditions for a zone of this type.
define/boundary-conditions/recirculation-outletSets boundary conditions for a zone of this type.
define/boundary-conditions/rename-zone/Enter the menu for renaming cell and face zones based on adjacency, adding suffixes or prefixes to names, and renaming zones based on the Fluent naming conventions.
define/boundary-conditions/rename-zone/add-suffix-or-prefixAdd a suffix or prefix to one or more zones.
define/boundary-conditions/rename-zone/rename-by-adjacencyAppend the name of the adjacent cell zone to the specified face zone. For example, if fluid is the adjacent cell zone, and you select a face zone named interior, the resulting name of the face zone would be interior-fluid.
define/boundary-conditions/rename-zone/rename-to-defaultRename a zone to use the Fluent naming convention.
define/boundary-conditions/set/Allows you to define one or more settings at single or multiple boundaries/cell zones of a given type at once. Enter
qto exit thedefine/boundary-conditions/set/command.<type>For a description of the items in this menu, see corresponding
define/boundary-conditions/.<type>define/boundary-conditions/shadowSets boundary conditions for a zone of this type.
define/boundary-conditions/solidSets boundary conditions for a zone of this type.
define/boundary-conditions/symmetrySets boundary conditions for a zone of this type.
define/boundary-conditions/target-mass-flow-rate-settings/Allows you to define the targeted mass flow rate settings through the following prompts:
set under-relaxation-factorThe default setting is 0.05.
enable targeted mass flow rate verbosity?Enables/disables verbosity when using targeted mass flow rate. When enabled, it prints to the console 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.
define/boundary-conditions/velocity-inletSets boundary conditions for a zone of this type.
define/boundary-conditions/wallSets boundary conditions for a zone of this type.
define/boundary-conditions/zone-nameGives a zone a new name.
define/boundary-conditions/zone-typeSets 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.
define/curvilinear-coordinate-system/Enters the curvilinear coordinate system menu.
define/curvilinear-coordinate-system/calculation-settingsSpecifies settings for the diffusion-based direction calculations.
define/curvilinear-coordinate-system/deleteDeletes a curvilinear coordinate system.
define/curvilinear-coordinate-system/editEdits a previously defined curvilinear coordinate system.
define/curvilinear-coordinate-system/newCreates a new curvilinear coordinate system.
define/custom-field-functions/Enters the custom field functions menu.
define/custom-field-functions/defineDefines a custom field function.
define/custom-field-functions/deleteDeletes a custom field function.
define/custom-field-functions/example-cff-definitionsLists example custom field functions.
define/custom-field-functions/list-valid-cell-function-namesLists the names of cell functions that can be used in a custom field function.
define/custom-field-functions/loadLoads a custom field function.
define/custom-field-functions/saveSaves a custom field function.
define/dynamic-mesh/Enters the dynamic mesh menu.
define/dynamic-mesh/actions/Enters the dynamic mesh action menu, where you can initiate manual remeshing (that is, remeshing without running a calculation).
define/dynamic-mesh/actions/remesh-cell-zoneManually remeshes a cell zone with option to remesh adjacent dynamic face zones.
define/dynamic-mesh/controls/Enters the dynamic mesh controls menu. This text command is only available when the
define/dynamic-mesh/dynamic-mesh?text command is enabled.define/dynamic-mesh/controls/contact-parameters/Enters 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.define/dynamic-mesh/controls/contact-parameters/contact-face-zonesSelects face zones involved in contact detection.
define/dynamic-mesh/controls/contact-parameters/contact-methodSelects the method used for flow control in the contact region. Enter
0for the contact zones method (which restricts the flow using additional cell zones with porous zone properties) or1for the contact marks method (which blocks the flow using zero-mass-flux boundaries).
define/dynamic-mesh/controls/contact-parameters/contact-thresholdSpecifies threshold distance for contact detection.
define/dynamic-mesh/controls/contact-parameters/contact-udfSelects the UDF to be invoked when contact is detected.
define/dynamic-mesh/controls/contact-parameters/flow-control-parameters/Enters the flow control parameters menu, which provides settings related to controlling the flow in the contact region.
define/dynamic-mesh/controls/contact-parameters/flow-control-parameters/create-flow-control-zoneCreates a flow control zone as part of the contact zones method.
define/dynamic-mesh/controls/contact-parameters/flow-control-parameters/delete-flow-control-zoneDeletes a flow control zone as part of the contact zones method.
define/dynamic-mesh/controls/contact-parameters/flow-control-parameters/solution-stabilization?Enables/disables the performance of additional iterations per time step and the application of solution controls to improve the stability of the solver as part of the contact marks method.
define/dynamic-mesh/controls/contact-parameters/flow-control?Enables/disables flow control in the contact region.
define/dynamic-mesh/controls/contact-parameters/render-contact-cells?Enables/disables the availability of a field variable (contact-cell-mark) that can be used to display contours of cells marked for flow blocking as part of the contact marks method, and allows you to postprocess other field variables on those cells.
define/dynamic-mesh/controls/contact-parameters/update-contact-marksUpdates which cells are marked in order to block flow in the contact region as part of the contact marks method.
define/dynamic-mesh/controls/contact-parameters/verbositySets the level of detail printed in the console regarding contact detection.
define/dynamic-mesh/controls/implicit-update-parameters/Enters 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.define/dynamic-mesh/controls/implicit-update-parameters/motion-relaxationSpecifies a value (within the range of 0 to 1) for the motion relaxation, which is applied during the implicit mesh update.
define/dynamic-mesh/controls/implicit-update-parameters/residual-criteriaSpecifies the relative residual threshold that is used to check the motion convergence during the implicit mesh update.
define/dynamic-mesh/controls/implicit-update-parameters/update-intervalSpecifies the update interval (that is, the frequency in iterations) at which the mesh is updated within a time step.
define/dynamic-mesh/controls/in-cylinder-output?Enables/disables in-cylinder output.
define/dynamic-mesh/controls/in-cylinder-parameters/Enters the dynamic mesh in-cylinder menu.
define/dynamic-mesh/controls/in-cylinder-parameters/crank-angle-stepSpecifies crank angle step size.
define/dynamic-mesh/controls/in-cylinder-parameters/crank-periodSpecifies the crank period.
define/dynamic-mesh/controls/in-cylinder-parameters/max-crank-angle-stepSpecifies maximum crank angle step size.
define/dynamic-mesh/controls/in-cylinder-parameters/minimum-liftSpecifies minimum lift for in-cylinder valves.
define/dynamic-mesh/controls/in-cylinder-parameters/modify-liftModifies lift curve (shift or scale).
define/dynamic-mesh/controls/in-cylinder-parameters/piston-dataSpecifies the crank radius and connecting rod length.
define/dynamic-mesh/controls/in-cylinder-parameters/piston-stroke-cutoffSpecifies the cut off point for in-cylinder piston.
define/dynamic-mesh/controls/in-cylinder-parameters/position-starting-meshMoves mesh from top dead center to starting crank angle.
define/dynamic-mesh/controls/in-cylinder-parameters/print-plot-liftPrints or plot valve lift curve.
define/dynamic-mesh/controls/in-cylinder-parameters/starting-crank-angleSpecifies the initial value for the crank angle.
define/dynamic-mesh/controls/layering?Enables/disables dynamic layering in prismatic cell zones (quadrilaterals in 2D, or polyhedrals, hexahedrals, or wedges in 3D).
define/dynamic-mesh/controls/layering-parameters/Enters the dynamic mesh layering menu.
define/dynamic-mesh/controls/layering-parameters/collapse-factorSets the factor determining when to collapse dynamic layers.
define/dynamic-mesh/controls/layering-parameters/constant-height?Enables/disables layering based on constant height, else layering based on constant ratio.
define/dynamic-mesh/controls/layering-parameters/split-factorSets the factor determining when to split dynamic layers.
define/dynamic-mesh/controls/periodic-displacement-parameters/Enters the periodic displacement parameters menu.
define/dynamic-mesh/controls/periodic-displacement-parameters/create-propertiesSets the properties for periodic displacement.
define/dynamic-mesh/controls/periodic-displacement-parameters/list-propertiesLists the properties for periodic displacement.
define/dynamic-mesh/controls/remeshing?Enables/disables local remeshing in tri/tet and mixed cell zones.
define/dynamic-mesh/controls/remeshing-parameters/Enters the dynamic mesh remeshing menu to set parameters for all remeshing methods.
define/dynamic-mesh/controls/remeshing-parameters/cell-skew-maxSets the cell skewness threshold above which cells will be remeshed.
define/dynamic-mesh/controls/remeshing-parameters/face-skew-maxSets the face skewness threshold above which faces will be remeshed.
define/dynamic-mesh/controls/remeshing-parameters/length-maxSets the length threshold above which cells will be remeshed.
define/dynamic-mesh/controls/remeshing-parameters/length-minSets the length threshold below which cells will be remeshed.
define/dynamic-mesh/controls/remeshing-parameters/parallel-remeshing?Disables/enables parallel remeshing as part of methods-based remeshing..
define/dynamic-mesh/controls/remeshing-parameters/prism-controls/Enters the dynamic mesh prism controls menu, which provides text commands that can be useful when you want to modify the algorithm that attempts to retain the size distribution during unified remeshing. Each prism control definition is applied to one or more boundary zones, and then affects the height distribution and number of layers of the wedge cells in the adjacent boundary layers.
define/dynamic-mesh/controls/remeshing-parameters/prism-controls/addAdds a new prism controls definition.
After being prompted for a name, you can enter the following to complete the definition:
first-aspect-ratioSets the aspect ratio for the individual wedge cells in the first layer of cells adjacent to the specified
zones. It is defined as the ratio of the local wedge base length (as averaged at the nodes) to the local wedge layer height. It is used whenaspect-ratiois selected for theoffset-type.first-heightSets the height of the first layer of wedge cells in the boundary layer adjacent to the specified
zones. It is used whenuniformis selected for theoffset-type(which is the default).growth-methodSpecifies the method used to determine the increase in height of the wedge cell layers beyond the first layer. The only available option is
geometric, so that the height of each layer is the height of the previous layer multiplied by therate.nameSpecifies the name of the prism controls definition.
nlayersSets the number of layers of wedge cells in the boundary layer adjacent to the specified
zones.offset-typeAllows you to select from the following types, in order to determine how the first layer of wedge cells (adjacent to the
zones) are generated during remeshing:uniformSpecifies that every new node (child) of the first layer of wedge cells is the same distance away from its parent node (that is, the corresponding node on the boundary zone, from which the direction vector is pointing). This distance is defined by the
first-height. Theuniformtype is selected by default.aspect-ratioSpecifies that the first layer of wedge cells that are extruded from the
zonesare defined using an aspect ratio, that is, the ratio of the local wedge base length (as averaged at the nodes) to the local wedge layer height. This aspect ratio is defined by thefirst-aspect-ratio. Note that for a uniform mesh, the heights of the cells in the first layer will be roughly the same, while for a varying mesh, these heights will vary.smooth-transitionSpecifies that the last layer of wedge cells that are extruded from the
zonesare defined using a transition rate, that is, the ratio of the local wedge cell height (as averaged at the nodes) to the height of the local tetrahedral cell that will be generated adjacent to the last layer. This transition rate / ratio is defined by thetransition-rate. This offset type allows you to easily provide a smooth transition for the cell volumes from the wedge cell layers to the cells deeper within the mesh. After the height of the last wedge cell layer is calculated, the height of the first layer is automatically computed according to your specified growthrateandnlayers. Note that for a uniform mesh, the heights of the cells in the first layer will be roughly the same, while for a varying mesh, these heights will vary.
rateSets the coefficient for the
growth-methodused to determine the increase in height of the wedge cell layers beyond the first layer.transition-rateSets the ratio of the local wedge cell height (as averaged at the nodes) in the last wedge cell layer to the height of the local tetrahedral cell that will be generated adjacent to the last layer (deeper within the mesh). It is used when
smooth-transitionis selected for theoffset-type.zonesSpecifies all of the boundary zones on which this prism controls definition is applied.
Enter
qwhen the definition is complete to return to the text command menu.define/dynamic-mesh/controls/remeshing-parameters/prism-controls/deleteDeletes an existing prism controls definition.
define/dynamic-mesh/controls/remeshing-parameters/prism-controls/editEdits an existing prism controls definition. You can revise the fields listed previously for the
define/dynamic-mesh/controls/remeshing-parameters/prism-controls/addtext command.define/dynamic-mesh/controls/remeshing-parameters/prism-controls/listPrints a list of the existing prism controls definitions in the console.
define/dynamic-mesh/controls/remeshing-parameters/prism-controls/list-propertiesPrints the properties of an existing prism controls definition of your choice in the console.
define/dynamic-mesh/controls/remeshing-parameters/prism-layer-parameters/Enters the dynamic mesh prism layer parameters menu, where you can define the parameters of the prism layers as part of methods-based remeshing.
define/dynamic-mesh/controls/remeshing-parameters/prism-layer-parameters/first-heightSets the first cell height in the prism layer.
define/dynamic-mesh/controls/remeshing-parameters/prism-layer-parameters/growth-rateSets the geometric growth rate of the prism layer.
define/dynamic-mesh/controls/remeshing-parameters/prism-layer-parameters/number-of-layersSets the number of elements in the prism layer.
define/dynamic-mesh/controls/remeshing-parameters/remeshing-after-moving?Enables a second round of remeshing based on the skewness parameters after the boundary has moved as part of methods-based remeshing.
define/dynamic-mesh/controls/remeshing-parameters/remeshing-methodsEnables/disables individual remeshing options as part of methods-based remeshing.
define/dynamic-mesh/controls/remeshing-parameters/retain-size-distribution?Enables/disables the use of local size criteria when marking cells for unified remeshing (in an attempt to maintain the initial mesh size distribution even as the mesh moves), rather than marking cells based on the minimum and maximum length scale values of the cell zone in the initial mesh. Either marking can be overridden if more restrictive values are specified using the
define/dynamic-mesh/controls/remeshing-parameters/length-minanddefine/dynamic-mesh/controls/remeshing-parameters/length-maxtext commands.define/dynamic-mesh/controls/remeshing-parameters/size-remesh-intervalSets the interval (in time steps) when remeshing based on size is done for methods-based remeshing.
define/dynamic-mesh/controls/remeshing-parameters/sizing-controls/Enters the dynamic mesh sizing controls menu, which provides text commands that can be useful when you want to modify the algorithm that attempts to retain the size distribution during unified remeshing. Each sizing control definition is applied to one or more boundary zones, and then affects the size of the cells throughout the mesh based on their distance from those boundary zone(s) and your settings in the definition.
define/dynamic-mesh/controls/remeshing-parameters/sizing-controls/addAdds a new sizing controls definition.
After being prompted for a name, you can enter the following to complete the definition:
growth-rateSets the growth rate of the sizing controls definition.
intervalSets the interval (in time steps) at which the evaluation of the sizing of the cells that result from the sizing control definition is updated. This setting is only relevant when
autois selected for themotionsetting. By default, theintervalis set to10time steps. This setting does not typically need to be adjusted: you could decrease it if you are using large time steps (which is not recommended), and you could increase it if it negatively impacts the calculation speed.max-lengthSets a maximum length threshold that is used when the
typeis set toautoorsoft.min-lengthSets a maximum length threshold that is used when the
typeis set toauto.motionDetermines whether the evaluation of the sizing of the cells that result from the size control definition is updated when zones move:
autospecifies that Fluent updates the evaluation during motion; andstaticspecifies that the evaluation is not updated during motion.nameSpecifies the name of the sizing controls definition.
typeSpecifies how the sizing is affected by the selected boundary zones:
autospecifies that the default size distribution (rather than the initial size distribution in your selected boundary zones) is used, along with your specifiedmax-lengthandmin-lengthvalues;softspecifies that the maximum length scale of your selected boundary zones is used, along with your specifiedmin-lengthvalue; andmeshedspecifies that the maximum and minimum length scales of your selected boundary zones are used, in order to respect their initial size distribution. This setting is only relevant if you have more than one sizing controls definition.zonesSpecifies all of the boundary zones on which the sizing controls definition is applied.
Enter
qwhen the definition is complete to return to the text command menu.define/dynamic-mesh/controls/remeshing-parameters/sizing-controls/deleteDeletes an existing sizing controls definition.
define/dynamic-mesh/controls/remeshing-parameters/sizing-controls/editEdits an existing sizing controls definition. You can revise the fields listed previously for the
define/dynamic-mesh/controls/remeshing-parameters/sizing-controls/addtext command.define/dynamic-mesh/controls/remeshing-parameters/sizing-controls/listPrints a list of the existing sizing controls definitions in the console.
define/dynamic-mesh/controls/remeshing-parameters/sizing-controls/list-propertiesPrints the properties of an existing sizing controls definition of your choice in the console.
define/dynamic-mesh/controls/remeshing-parameters/sizing-funct-defaultsSets sizing function defaults.
define/dynamic-mesh/controls/remeshing-parameters/sizing-funct-rateDetermines how far from the boundary the increase/decrease happens.
define/dynamic-mesh/controls/remeshing-parameters/sizing-funct-resolutionSets the sizing function resolution with respect to shortest boundary.
define/dynamic-mesh/controls/remeshing-parameters/sizing-funct-variationSets the maximum sizing function increase/decrease in the interior.
define/dynamic-mesh/controls/remeshing-parameters/sizing-function?Enables/disables the sizing function as part of methods-based remeshing.
define/dynamic-mesh/controls/remeshing-parameters/unified-remeshing?Enables/disables unified remeshing, which specifies that an algorithm is used that combines aspects of a variety of remeshing methods. It is applied to triangular or tetrahedral cells and can produce wedge cells in 3D boundary layer meshes. Unified remeshing simplifies the remeshing setup and can provide increased robustness compared to methods-based remeshing, especially for parallel simulations.
define/dynamic-mesh/controls/remeshing-parameters/zone-remeshingEnables/disables the cell zone remeshing method as part of methods-based remeshing.
define/dynamic-mesh/controls/six-dof-parameters/Enters the dynamic mesh six degrees of freedom (DOF) solver menu.
define/dynamic-mesh/controls/six-dof-parameters/create-propertiesCreates/edits a set of six DOF properties for rigid body motion.
define/dynamic-mesh/controls/six-dof-parameters/delete-propertiesDeletes a set of six DOF properties for rigid body motion.
define/dynamic-mesh/controls/six-dof-parameters/list-propertiesPrints summaries of the existing sets of six DOF properties for rigid body motion.
define/dynamic-mesh/controls/six-dof-parameters/motion-history-file-nameSpecifies the name and location of the six DOF motion history file.
define/dynamic-mesh/controls/six-dof-parameters/motion-history?Enables/disables writing position/orientation of six DOF zones to file.
define/dynamic-mesh/controls/six-dof-parameters/second-order?Enables/disables the second order six degrees of freedom solver.
define/dynamic-mesh/controls/six-dof-parameters/x-component-of-gravitySpecifies x-component of gravity.
define/dynamic-mesh/controls/six-dof-parameters/y-component-of-gravitySpecifies y-component of gravity.
define/dynamic-mesh/controls/six-dof-parameters/z-component-of-gravitySpecifies z-component of gravity.
define/dynamic-mesh/controls/smoothing?Enables/disables smoothing in cell zones.
define/dynamic-mesh/controls/smoothing-parameters/Enters the dynamic mesh smoothing-parameters menu.
define/dynamic-mesh/controls/smoothing-parameters/amg-stabilizationSets the algebraic multigrid (AMG) stabilization method for mesh smoothing calculations that use finite element discretization. This text command is available for diffusion-based smoothing and linearly elastic solid smoothing.
define/dynamic-mesh/controls/smoothing-parameters/bnd-node-relaxationThe 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.
define/dynamic-mesh/controls/smoothing-parameters/bnd-stiffness-factorSets the stiffness factor for springs connected to boundary nodes.
define/dynamic-mesh/controls/smoothing-parameters/boundary-distance-methodSets the method used to evaluate the boundary distance for the diffusion coefficient calculation, when diffusion-based smoothing is enabled.
define/dynamic-mesh/controls/smoothing-parameters/constant-factorSets the spring constant relaxation factor.
define/dynamic-mesh/controls/smoothing-parameters/convergence-toleranceSets the convergence tolerance for spring-based solver.
define/dynamic-mesh/controls/smoothing-parameters/diffusion-coeff-functionSpecifies whether the diffusion coefficient for diffusion-based smoothing is based on the boundary distance or the cell volume.
define/dynamic-mesh/controls/smoothing-parameters/diffusion-coeff-parameterSets the diffusion coefficient parameter used for diffusion-based smoothing.
define/dynamic-mesh/controls/smoothing-parameters/diffusion-fvm?Answering
yesat 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. Answeringnoat the prompt changes the diffusion-based smoothing method to the default node-based finite element method.define/dynamic-mesh/controls/smoothing-parameters/local-smoothing?Enables/disables local smoothing, when the smoothing method is based on a radial basis function interpolation. Local smoothing limits the amount of the domain that is smoothed to only those cells that are close to the moving boundary zone(s), to ensure that the mesh away from the moving boundary remains undisturbed by the smoothing, and to decrease the computational time required for smoothing.
define/dynamic-mesh/controls/smoothing-parameters/number-local-layersSets the number of layers of cells adjacent to the moving boundary zone that are smoothed as part of local smoothing with the radial basis function method. If Fluent detects boundary layers on the moving boundary zone, they are smoothed before and independently of the local smoothing region, ensuring that they retain their shape as much as possible. The portion of the mesh smoothed by the local smoothing is then evaluated starting from the edge of the boundary layers.
define/dynamic-mesh/controls/smoothing-parameters/max-iterSets the maximum number of iterations for the smoothing calculations when the spring-based, diffusion-based, or linearly elastic solid method is used.
define/dynamic-mesh/controls/smoothing-parameters/relative-convergence-toleranceSets the relative residual convergence tolerance for smoothing based on diffusion, the linearly elastic solid model, or a radial basis function interpolation.
define/dynamic-mesh/controls/smoothing-parameters/skew-smooth-all-deforming-boundaries?Enables/disables skewness smoothing for all deforming dynamic boundary zones. This is enabled by default. If disabled, skewness smoothing is only applied to the deforming dynamic boundary zones that have smoothing explicitly enabled or use local face remeshing.
define/dynamic-mesh/controls/smoothing-parameters/skew-smooth-cell-skew-maxSets the skewness threshold, above which cells will be smoothed using the skewness method.
define/dynamic-mesh/controls/smoothing-parameters/skew-smooth-face-skew-maxSets the skewness threshold, above which faces will be smoothed using the skewness method.
define/dynamic-mesh/controls/smoothing-parameters/skew-smooth-niterSets the number of skewness-based smoothing cycles.
define/dynamic-mesh/controls/smoothing-parameters/smooth-boundary-layers-with-adjacent-zone?Enables/disables the smoothing of the boundary layers adjacent to a moving boundary zone before and independently of the bulk of the mesh, ensuring that they retain their shape as much as possible. This text command is only available with the radial basis function smoothing method, when the following text command is disabled:
define/dynamic-mesh/controls/smoothing-parameters/local-smoothing?.define/dynamic-mesh/controls/smoothing-parameters/smooth-from-reference-position?Enables/disables smoothing from a reference position. Such smoothing may produce greater mesh quality consistency for stationary or moving meshes with periodic or quasi-periodic motion, and is only available when the smoothing method is based on diffusion, the linearly elastic solid model, or a radial basis function interpolation.
define/dynamic-mesh/controls/smoothing-parameters/smoothing-methodSpecifies the smoothing method used by the dynamic mesh model. The available options are:
spring: spring-based smoothingdiffusion: diffusion-based smoothinglinelast: linearly elastic solid smoothingradial: radial basis function smoothing
define/dynamic-mesh/controls/smoothing-parameters/spring-on-all-elements?Enables/disables spring-based smoothing for all cell shapes; if disabled, the spring-based smoothing is applied based on the setting of the
define/dynamic-mesh/controls/smoothing-parameters/spring-on-simplex-shapes?text command.define/dynamic-mesh/controls/smoothing-parameters/spring-on-simplex-shapes?Enables/disables spring-based smoothing for triangular / tetrahedral cells in mixed element zones; if disabled, the spring-based smoothing is applied to triangular / tetrahedral cells in triangular / tetrahedral element zones.
define/dynamic-mesh/controls/smoothing-parameters/poisson-ratioSets the Poisson’s ratio used for smoothing based on the linearly elastic solid model.
define/dynamic-mesh/controls/smoothing-parameters/verbositySpecifies the level of detail printed to the console during the calculation. Setting this to
1(for radial basis function smoothing) ensures that the absolute tolerance computed (based on your specified relative tolerance) is printed, or (for all other smoothing methods) ensures that smoothing residuals are printed; alternatively, the default value of0suppresses such output.
define/dynamic-mesh/controls/steady-pseudo-time-control?Enables/disables the pseudo time step control in the graphical user interface.
define/dynamic-mesh/dynamic-mesh?Enables/disables the dynamic mesh solver.
define/dynamic-mesh/events/Enters the dynamic mesh events menu.
define/dynamic-mesh/events/export-event-fileExports dynamic mesh events to file.
define/dynamic-mesh/events/import-event-fileImports dynamic mesh event file.
define/dynamic-mesh/transient-settings/Enters 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.define/dynamic-mesh/transient-settings/allow-second-order?Enables/disables second order transient scheme for dynamic mesh cases.
define/dynamic-mesh/transient-settings/verbosityEnables/disables transient scheme verbosity for dynamic mesh cases.
define/dynamic-mesh/zones/Enters the dynamic mesh zones menu.
define/dynamic-mesh/zones/createCreates or edit a dynamic zone.
define/dynamic-mesh/zones/deleteDeletes a dynamic zone.
define/dynamic-mesh/zones/insert-boundary-layerInserts a new cell zone.
define/dynamic-mesh/zones/insert-interior-layerInserts a new layer cell zone at a specified location.
define/dynamic-mesh/zones/listLists the dynamic zones.
define/dynamic-mesh/zones/remove-boundary-layerRemoves a cell zone.
define/dynamic-mesh/zones/remove-interior-layerRemoves an interior layer cell zone.
define/enable-mesh-morpher-optimizer?Enables the mesh morpher/optimizer. When the mesh morpher/optimizer is enabled, the
define/mesh-morpher-optimizertext command becomes available.define/gap-model/Enters the gap model menu, where you can define one or more gap regions where the flow is blocked or decelerated when face zones move within a specified proximity threshold of each other.
define/gap-model/advanced-options/Enters the advanced options menu for the gap model.
define/gap-model/advanced-options/check-cfl-condition?Enables/disables the printing of warnings if the time step size is too large based on a Courant (CFL) number automatically determined for your specified solution stability level.
define/gap-model/advanced-options/enhanced-data-interpolation?Enables/disables the use of enhanced data interpolation when updating information in gap regions. This text command is only available if you have enabled the
define/gap-model/advanced-options/expert?text command.define/gap-model/advanced-options/expert?Enables/disables access to expert-level text commands for the gap model.
define/gap-model/advanced-options/extend-gap-regions?Enables/disables the extending of the gap regions by including additional cells in the vicinity of the gap interfaces during marking. This is useful when the default shape of the marked cells is negatively affecting solution stability or convergence behavior.
define/gap-model/advanced-options/fill-data-in-gap-regions?Enables/disables the interpolation of solution data throughout the gap regions. This text command is only available if you have enabled the
define/gap-model/advanced-options/expert?text command.define/gap-model/advanced-options/precise-gap-marking?Enables/disables the use of a more accurate search algorithm for marking cells in gap regions. Note that it can be costly, particularly for 3D cases or those with a large number of cells inside the gap regions. This text command is only available if you have enabled the
define/gap-model/advanced-options/expert?text command.define/gap-model/advanced-options/reduce-gap-regions?Enables/disables a more restrictive algorithm for marking cells in gap regions. This text command is only available if you have enabled the
define/gap-model/advanced-options/expert?text command.define/gap-model/advanced-options/render-flow-modeling-gaps?Enables/disables the rendering of the solution in the cells of flow-modeling gap regions during postprocessing. This text command is only available if you have enabled the
define/gap-model/advanced-options/expert?text command.define/gap-model/advanced-options/render-gap-interface?Enables/disables the rendering of the mesh surfaces inside the gap regions when displaying the mesh with contours. Note that the solution is still not rendered inside the flow-blocking gap regions.
define/gap-model/advanced-options/revert-controls-to-defaultReverts the global gap stabilization level and any related solver settings to the default.
define/gap-model/advanced-options/solution-stabilizationSets the global solution stabilization level for the gap regions.
define/gap-model/advanced-options/sponge-layerAllows you to edit the solution stabilization settings for flow-modeling gap regions that have sponge-layer local stabilization enabled.
You can set the viscosity variation factor, which determines how much the viscosity linearly varies within the gap region as you approach the center. The default value of
0produces maximum variability, which is appropriate when the gap size is larger and/or the viscosity within the gap region is very high compared to the flow domain. You can enter values closer to1(so that the viscosity is more fixed / constant throughout) when the gap is smaller and/or the viscosity variation is lower. Minimizing the variability restricts the flow better, but can lead to solution instability.You can set minimum limit for the velocity in the sponge layers. Viscosity scaling is disabled if the average velocity inside the gap region is less than this minimum.
You can set the maximum limit for the viscosity change ratio in the sponge layers. The local stabilization method measures the variation of maximum viscosity to minimum viscosity inside the gap region, and constrains this ratio to be bounded between 0 and the value you enter.
define/gap-model/advanced-options/verbositySets the verbosity for messages printed in the console related to the gap model.
define/gap-model/createCreates a single gap region, so that when selected face zones move within a specified proximity threshold of each other, flow blockage / deceleration is applied to the cells that lie within the threshold.
define/gap-model/deleteDeletes an existing gap region.
define/gap-model/delete-allDeletes all of the existing gap regions.
define/gap-model/editEdits an existing gap region.
define/gap-model/enable?Enables/disables the gap model.
define/gap-model/list-gap-cell-zonesLists the names of the cell zones that can be excluded for individual gap regions (so that such cells are not marked for flow blockage / deceleration).
define/gap-model/list-gap-face-zonesLists the names of the face zones that can be used for creating gap regions.
define/gap-model/list-gap-regionsLists the properties of the gap regions.
define/injections/Enters the injections menu.
For a description of the items in this menu, see
define/models/dpm/injections.define/materials/Enters the materials menu.
define/materials/change-createChanges the properties of a locally-stored material or create a new material.
Note: Generally, the properties you enter at the prompts will be filtered according to your case and model settings. However, some of the listed properties may not match the selection choice in the Graphics User Interface. Typically, those excessive properties in the Text User Interface will not be used in your simulation.
define/materials/copyCopies a material from the database.
define/materials/copy-by-formulaCopies a material from the database by formula.
define/materials/data-base/Enters the material database menu.
define/materials/data-base/database-typeSets the database type (
fluent-database,granta-mds, oruser-defined).define/materials/data-base/editEdits material.
define/materials/data-base/list-materialsLists all materials in the database.
define/materials/data-base/list-propertiesLists the properties of a material in the database.
define/materials/data-base/newDefines new material.
define/materials/data-base/saveSaves user-defined database.
define/materials/deleteDeletes a material from local storage.
define/materials/list-materialsLists all locally-stored materials.
define/materials/list-propertiesLists the properties of a locally-stored material.
define/mesh-interfaces/Enters the mesh-interfaces menu.
define/mesh-interfaces/auto-options/Enters the auto-options menu. This menu is only available when the
define/mesh-interfaces/one-to-one-pairing?text command is enabled.define/mesh-interfaces/auto-options/naming-optionSpecifies whether the name of each new one-to-one mesh interface (as well as existing mesh interfaces, if you so desire) has no additional suffix, or a suffix that includes the names of the associated boundary zones, the IDs of the associated boundary zones, or the names of the adjacent cell zones.
define/mesh-interfaces/auto-options/pairing-between-different-cell-zones-only?Specifies whether the one-to-one mesh interfaces are only created between different cell zones.
define/mesh-interfaces/auto-options/set-default-name-prefixSpecifies the default interface name prefix used for one-to-one mesh interfaces.
define/mesh-interfaces/auto-options/set-minimum-area-percentageSets the minimum area percentage of overlap for one-to-one mesh interface creation. If zones are paired using the automatic method, after the mesh interfaces are created, a check will be done: if the area that two zones overlap divided by the area of the zone is less than this value for both zones in any mesh interface, then that mesh interface will be deleted. This can help you avoid unnecessary or unintentional mesh interfaces. By default the minimum area percentage is set to 0, so no pairings are deleted. When you are setting up a sliding mesh simulation in which the zones begin with little or no overlap and then slide into a position that includes more overlap, you should make sure the minimum area percentage is set such that it does not delete your intended mesh interface.
define/mesh-interfaces/auto-options/set-one-to-one-pairing-toleranceEnables/disables the use of adjustable tolerances to determine which of the selected boundary zones can be paired up to make mesh interfaces. You can specify a
Length factor, and the product of thisLength factorand the largest mesh length scale of the interface boundaries is used in the evaluation of the tolerances. You can reduce theLength factorif the resulting interface areas are too large or if boundary zones that you do not want paired are paired. An increase in theLength factoris recommended if any expected interfaces are not created, or if the intersection areas are smaller than expected.
define/mesh-interfaces/auto-pairingAutomatically "pairs" some or all of the interface zones, in order to create mesh interfaces. This text command is only available when the
define/mesh-interfaces/one-to-one-pairing?text command is disabled.define/mesh-interfaces/coupled-interfaces-inherit-bcs?Allows you to specify that the boundary conditions of the original zones are copied to the resulting coupled wall pair when a mesh interface is created at a solid-to-solid zone interface of different materials or a fluid-to-solid zone interface. This text command is only available when the
define/mesh-interfaces/one-to-one-pairing?text command is enabled.define/mesh-interfaces/createCreates mesh interfaces.
define/mesh-interfaces/create-manuallyCreates mesh interfaces by pairing all of the possible combinations between two specified groups of boundary zones, even if the zones do not currently overlap. This can be useful for setting up sliding mesh simulations. This text command is only available when the
define/mesh-interfaces/one-to-one-pairing?text command is enabled.define/mesh-interfaces/deleteDeletes a mesh interface.
define/mesh-interfaces/delete-allDeletes all mesh interfaces.
define/mesh-interfaces/delete-interfaces-with-small-overlapDeletes one-to-one mesh interfaces that have a small area of overlap. You define the area percentage that is used for deletion: if the area that the two zones overlap divided by the area of the zone is less than this value for both zones in any mesh interface, then that mesh interface will be deleted.
define/mesh-interfaces/displayDisplays the specified mesh interface zone.
define/mesh-interfaces/editEdits attributes of existing mesh interfaces. For one-to-one interfaces, you can edit the name; for many-to-many interfaces, you can edit the interface options and (for a single interface) the name and the list of interface zones assigned to the interface.
define/mesh-interfaces/enable-visualization-of-interfaces?Enables/disables the filling of node coordinates on the zones of mesh interfaces, so that they can be displayed in the graphics window.
define/mesh-interfaces/enforce-continuity-after-bc?Enables/disables continuity across the boundary condition interface for contour plots in postprocessing.
define/mesh-interfaces/enforce-coupled-wall-between-solids?Enables/disables 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.
define/mesh-interfaces/improve-qualityChecks 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.
define/mesh-interfaces/listPrints information about the mesh interface(s) in the console.
define/mesh-interfaces/mapped-interface-options/Enters the mapped-interface menu. Options are available to convert a non-conformal interface to a mapped interface. This menu is only available when the
define/mesh-interfaces/one-to-one-pairing?text command is disabled.define/mesh-interfaces/mapped-interface-options/convert-to-mapped-interfaceConverts non-conformal mesh interface to mapped mesh interfaces. Answering
yestoConvert 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. AnsweringyestoConvert 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.define/mesh-interfaces/mapped-interface-options/solution-controlsSpecifies the mapped frequency and under-relaxation factor for mapped interfaces.
define/mesh-interfaces/mapped-interface-options/toleranceSpecifies the mapped interface tolerance. After changing the tolerance, the existing mapped interface will be updated.
define/mesh-interfaces/non-conformal-interface-numerics/Enters the non-conformal-interface-numerics menu.
define/mesh-interfaces/non-conformal-interface-numerics/change-numerics?Provides options to improve numerics for non-conformal interfaces in some cases.
Enforce watertight cells for fluid-solid and solid-solid interfaces?: Answeringyesensures cells adjacent to a non-conformal fluid-solid or solid-solid interface are watertight when performing the coupled wall discretization.Use enhanced gradient computations for fluid-solid and solid-solid interfaces?: Answeringyesenables improvements to the calculation of gradients.Recreate non-conformal interfaces?: If you change the response to either of the previous two questions then interfaces should be recreated.
define/mesh-interfaces/one-to-one-pairing?Enables/disables the use of the one-to-one interface creation method. This method is enabled by default, such that a single zone is assigned to each side of all of the mesh interfaces when they are created; otherwise the mesh interfaces may have multiple zones on one or both sides. Any mesh interfaces that exist when the use of this method is changed will either be deleted or modified to be compatible with this method.
define/mesh-interfaces/remove-left-handed-interface-faces?Removes left-handed faces (which can cause the mesh to be invalid) during mesh interface creation.
define/mesh-interfaces/transfer-motion-across-interfaces?Enables/disables the automatic transfer of motion across a mesh interface when only one side is moving as a result of user-defined or system coupling motion. You can specify the method by which the motion is transferred:
transfer-displacements(the default) interpolates nodal displacement from the active side of the interface to the passive side, and is recommended when there are gaps and/or penetrations in the mesh interface that must be maintained;project-nodesprojects the passive nodes onto the faces of active side, and is recommended when the active side includes significant tangential motion (as only the normal displacement is effectively transferred in this method).define/mesh-interfaces/turbo-createCreates a general turbo interface. This text command is only available if the
define/turbo-model/enable-turbo-model?text command is enabled.define/mesh-interfaces/use-virtual-polygon-approachUses 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.
define/mesh-interfaces/verbositySets the mesh interface verbosity.
define/mesh-morpher-optimizer/Enters 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.define/mesh-morpher-optimizer/deformation-settings/Enters the deformation menu. This text command is only available if you have created a deformation region using the
define/mesh-morpher-optimizer/region/createor thedefine/mesh-morpher-optimizer/region/define-bounding-boxtext command.define/mesh-morpher-optimizer/deformation-settings/check-meshDisplays 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.define/mesh-morpher-optimizer/deformation-settings/deform-meshModifies the mesh and updates 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.define/mesh-morpher-optimizer/deformation-settings/motion-settings/Enters 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-distributiontext command is set to unstructured.define/mesh-morpher-optimizer/deformation-settings/motion-settings/createCreates 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.
define/mesh-morpher-optimizer/deformation-settings/motion-settings/deleteDeletes an existing motion.
define/mesh-morpher-optimizer/deformation-settings/motion-settings/modifyModifies the settings for an existing motion.
define/mesh-morpher-optimizer/deformation-settings/motion-settings/read-from-fileDefines the settings for all the motions by reading an ASCII text file.
define/mesh-morpher-optimizer/deformation-settings/motion-settings/write-to-fileWrites the settings for all the motions to an ASCII text file.
define/mesh-morpher-optimizer/deformation-settings/read-motion-settings-from-fileDefines 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-distributiontext command is set to regular.define/mesh-morpher-optimizer/deformation-settings/reset-all-deformationsUndoes any deformations made to the mesh and updates the mesh display in the graphics window.
define/mesh-morpher-optimizer/deformation-settings/set-constraintsDefines 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.
define/mesh-morpher-optimizer/deformation-settings/set-constraints-multipleDefines 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.
define/mesh-morpher-optimizer/deformation-settings/set-parametersAssigns 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-distributiontext command is set to regular.define/mesh-morpher-optimizer/deformation-settings/set-parameters-multipleAssigns 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-distributiontext command is set to regular.define/mesh-morpher-optimizer/deformation-settings/write-motion-settings-to-fileWrites the motion settings to an ASCII text file. This text command is only available if the
define/mesh-morpher-optimizer/set-control-point-distributiontext command is set to regular.
define/mesh-morpher-optimizer/morpher-summaryDisplays 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/createor thedefine/mesh-morpher-optimizer/region/define-bounding-boxtext command.define/mesh-morpher-optimizer/optimizer-parameters/Enters the optimizer menu. This text command is only available when you have created a deformation region using the
define/mesh-morpher-optimizer/region/createor thedefine/mesh-morpher-optimizer/region/define-bounding-boxtext command and have enabled thedefine/mesh-morpher-optimizer/optimizer?text command.define/mesh-morpher-optimizer/optimizer-parameters/convergence-criteriaDefines the convergence criteria for the optimizer.
define/mesh-morpher-optimizer/optimizer-parameters/custom-calculator/Enters 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-typetext command.define/mesh-morpher-optimizer/optimizer-parameters/custom-calculator/defineDefines the custom objective function that will be minimized by the optimizer.
define/mesh-morpher-optimizer/optimizer-parameters/custom-calculator/deleteDeletes the saved custom objective function.
define/mesh-morpher-optimizer/optimizer-parameters/custom-calculator/example-obj-fn-definitionsPrints examples of custom objective function definitions in the console.
define/mesh-morpher-optimizer/optimizer-parameters/custom-calculator/list-output-parametersPrints a list of the output parameters that can be used to define the custom objective function.
define/mesh-morpher-optimizer/optimizer-parameters/disable-mesh-checkSpecifies 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-commandstext command) at the start of a design stage, so that an accurate solution can be calculated.define/mesh-morpher-optimizer/optimizer-parameters/end-commandsSpecifies 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-typetext command.define/mesh-morpher-optimizer/optimizer-parameters/initial-commandsSpecifies 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-typetext command.define/mesh-morpher-optimizer/optimizer-parameters/initializationSpecifies how the solution variables should be treated after the mesh is deformed, that is, whether they should be initialized to the values defined in theSolution Initialization task page, remain the values obtained in the previous design iteration, or be read from a data file that you specify.
define/mesh-morpher-optimizer/optimizer-parameters/iterations-per-designDefines the maximum number of iterations Ansys Fluent will perform for each design change.
define/mesh-morpher-optimizer/optimizer-parameters/maximum-designsDefines the maximum number of design stages the optimizer will undergo to reach the specified objective function.
define/mesh-morpher-optimizer/optimizer-parameters/mesh-quality-checkSpecifies if orthogonal quality should be used to determine whether a solution is calculated for a mesh, and defines the minimum orthogonal quality value allowed (values may range from
0–1, where0represents the worst quality).define/mesh-morpher-optimizer/optimizer-parameters/monitor/Enters 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-typetext command.define/mesh-morpher-optimizer/optimizer-parameters/monitor/clear-opt-histDiscards the optimization history data, including the associated files.
define/mesh-morpher-optimizer/optimizer-parameters/monitor/plot-histDisplays 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-datatext command.define/mesh-morpher-optimizer/optimizer-parameters/monitor/plot?Enables the plotting of the optimization history data in the graphics window.
define/mesh-morpher-optimizer/optimizer-parameters/monitor/write?Enables the saving of the optimization history data to a file.
define/mesh-morpher-optimizer/optimizer-parameters/newuoa-initial-parameter-variationDefines 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-typetext command.define/mesh-morpher-optimizer/optimizer-parameters/objective-function-definitionSpecifies 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-calculatormenu. Theobjective-function-definitiontext command is not available when the NEWUOA optimizer is selected using thedefine/mesh-morpher-optimizer/optimizer-parameters/optimizer-typetext command.define/mesh-morpher-optimizer/optimizer-parameters/optimizeInitiates the optimization process. This text command is only available if the
define/mesh-morpher-optimizer/optimizer?text command is enabled.define/mesh-morpher-optimizer/optimizer-parameters/optimizer-typeSpecifies which optimizer is to be used. You can select one of the six built-in optimizers (
1–5and7), or specify that you will use Design Exploration in Ansys Workbench (6). Note that6is 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.define/mesh-morpher-optimizer/optimizer-parameters/save-case-data-filesSets 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).
define/mesh-morpher-optimizer/optimizer?Enables 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/createor thedefine/mesh-morpher-optimizer/region/define-bounding-boxtext command.define/mesh-morpher-optimizer/parameter-settings/Enters the parameters menu.
define/mesh-morpher-optimizer/parameter-settings/number-of-parametersDefines the number of parameters that will be used to define the deformation.
define/mesh-morpher-optimizer/parameter-settings/parameter-boundsDefines 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.define/mesh-morpher-optimizer/parameter-settings/parameter-valueDefines 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). Theparameter-valuetext command is only available in the following situations:if the
define/mesh-morpher-optimizer/optimizer?text command is disabledif the
define/mesh-morpher-optimizer/optimizer?text command is enabled and6is selected for the optimizer type via thedefine/mesh-morpher-optimizer/optimizer-typetext command
define/mesh-morpher-optimizer/region/Enters the region menu in order to define the regions of the domain where the mesh will be deformed in order to optimize the shape.
define/mesh-morpher-optimizer/region/controlpoints/Enters 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-distributiontext command is set to unstructured.define/mesh-morpher-optimizer/region/controlpoints/createCreates a new control point by defining the coordinates of a point within an existing deformation region.
define/mesh-morpher-optimizer/region/controlpoints/deleteDeletes existing control points.
define/mesh-morpher-optimizer/region/controlpoints/distribute-points-on-zoneCreates 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.
define/mesh-morpher-optimizer/region/controlpoints/modifyModifies the coordinates of existing control points.
define/mesh-morpher-optimizer/region/controlpoints/read-from-fileDefines all of the control points by reading an ASCII text file.
define/mesh-morpher-optimizer/region/controlpoints/write-to-fileWrites the control point coordinates to an ASCII text file.
define/mesh-morpher-optimizer/region/createCreates 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-optimizermenu.define/mesh-morpher-optimizer/region/define-bounding-boxCreates 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-optimizermenu.define/mesh-morpher-optimizer/region/deleteDeletes a deformation region.
define/mesh-morpher-optimizer/region/scaling-enlargeSets 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.
define/mesh-morpher-optimizer/region/scaling-reduceSets 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.
define/mesh-morpher-optimizer/set-control-point-distributionSpecifies 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).
define/models/Enters the models menu to configure the solver.
define/models/ablation?Enables/disables the ablation model.
define/models/acoustics/Enters the acoustics menu.
define/models/acoustics/auto-pruneEnables/disables auto prune of the receiver signal(s) during read-and-compute.
define/models/acoustics/broad-band-noise?Enables/disables the broadband noise model.
define/models/acoustics/convective-effects?Enables/disables the convective effects option.
define/models/acoustics/compute-writeComputes sound pressure.
define/models/acoustics/cylindrical-export?Enables/disables the export of data in cylindrical coordinates.
define/models/acoustics/display-flow-time?Enables/disables the display of flow time during read-and-compute.
define/models/acoustics/export-source-data-cgns?Enables/disables the export of acoustic source data in CGNS format.
define/models/acoustics/export-volumetric-sources?Enables/disables the export of fluid zones.
define/models/acoustics/export-volumetric-sources-cgns?Enables/disables the export of fluid zones.
define/models/acoustics/export-source-data?Enables/disables the export of acoustic source data in ASD format during the wave equation model run.
define/models/acoustics/far-field-parameters/Enters the menu to specify the far-field density and speed of sound. Note that this menu is currently available only with the acoustics wave equation model.
define/models/acoustics/far-field-parameters/far-field-densitySpecifies the far-field density value for the acoustics wave equation model.
define/models/acoustics/far-field-parameters/far-field-sound-speedSpecifies the far-field speed of sound value for the acoustics wave equation model.
define/models/acoustics/ffowcs-williams?Enables/disables the Ffowcs-Williams-and-Hawkings model.
define/models/acoustics/moving-receiver?Enables/disables the moving receiver option.
define/models/acoustics/off?Enables/disables the acoustics model.
define/models/acoustics/read-compute-writeReads acoustic source data files and computes sound pressure.
define/models/acoustics/receiversSets acoustic receivers.
define/models/acoustics/sourcesSets acoustic sources.
define/models/acoustics/sources-fft/Enters 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.
define/models/acoustics/sources-fft/read-asd-filesReads ASD files to perform FFT of the pressure history field.
define/models/acoustics/sources-fft/compute-fft-fieldsComputes FFT of the read pressure histories. The computed spectra replace the pressure histories in memory.
define/models/acoustics/sources-fft/clean-up-storage-areaDe-allocates memory used to store the pressure histories and their Fourier spectra, as well as any created surface variables for the visualization.
define/models/acoustics/sources-fft/write-cgns-filesWrites surface pressure spectra in CGNS format, which can be used for one-way coupling with Ansys Mechanical in the frequency domain.
define/models/acoustics/sources-fft/fft-surface-variables/Enters the menu to create surface variables from the computed Fourier spectra for visualization.
define/models/acoustics/sources-fft/fft-surface-variables/create-constant-width-bandsSelects up to 20 constant width bands and creates either the surface pressures level (SPL) variables or the PSD of dp/dt variables for them.
define/models/acoustics/sources-fft/fft-surface-variables/create-octave-bandsCreates either the surface pressure level (SPL) variables or the PSD of dp/dt variables for 17 technical octaves.
define/models/acoustics/sources-fft/fft-surface-variables/create-third-bandsCreates either the surface pressure level (SPL) variables or the PSD of dp/dt variables for 54 technical thirds.
define/models/acoustics/sources-fft/fft-surface-variables/create-set-of-modesSelects up to 20 individual Fourier modes and create variable pairs for them, containing the real and the imaginary parts of the complex Fourier amplitudes.
define/models/acoustics/sources-fft/fft-surface-variables/remove-variablesRemoves all variables created in this menu.
define/models/acoustics/sponge-layers/Allows you to define sponge layers at boundary zones, so that the density is blended from the value calculated by the solver to user-specified far-field values. Such sponge layers can eliminate non-physical pressure wave reflections from boundary zones. This text command menu is only available in transient simulations of single-phase, compressible flows with the pressure-based solver.
define/models/acoustics/sponge-layers/activateActivates a sponge layer definition that you would like to use during the simulation.
define/models/acoustics/sponge-layers/addAdds a new sponge layer definition, which by default is set as active.
After being prompted for a name, you can enter the following to complete the definition:
boundary-zonesSpecifies all of the boundary zones on which the sponge layer is applied.
far-field-densitySpecifies a value of density that is used for blending with the solver value. It is recommended that you use the average density at the boundaries throughout the simulation.
nameSpecifies the name of the sponge layer definition.
ramping-distanceSpecifies a distance over which the density changes from the solver value to the far-field value. It is recommended that this length is 80–100% of the
total-thickness.total-thicknessSpecifies the total thickness of the sponge layer, a distance from the selected boundaries to the interior boundary of the sponge layer. It is recommended that this thickness is at least twice the wavelength of the expected pressure waves.
Enter
qwhen the definition is complete to return to the text command menu.define/models/acoustics/sponge-layers/deactivateDeactivates an active sponge layer, so that it is not used during the simulation.
define/models/acoustics/sponge-layers/deleteDeletes an existing sponge layer definition.
define/models/acoustics/sponge-layers/editEdits an existing sponge layer. You can revise the fields listed previously for the
define/models/acoustics/sponge-layers/addtext command.define/models/acoustics/sponge-layers/listPrints a list of the existing sponge layers in the console.
define/models/acoustics/sponge-layers/list-activePrints the names of the active sponge layer definitions in the console.
define/models/acoustics/sponge-layers/list-propertiesPrints the properties of an existing sponge layer of your choice in the console.
define/models/acoustics/wave-equation?Enables/disables the wave equation model.
define/models/acoustics/wave-equation-options/Enters the menu to define the acoustics wave equation model options.
define/models/acoustics/wave-equation-options/basic-shapes/Enters the menu to define the geometry of the source mask and sponge layer using the basic shapes, represented by the cell registers of the type "Region".
define/models/acoustics/wave-equation-options/basic-shapes/add-source-mask-shapeAdds a basic shape to the definition of the source mask geometry.
define/models/acoustics/wave-equation-options/basic-shapes/add-sponge-layer-shapeAdds a basic shape to the definition of the sponge layer geometry.
define/models/acoustics/wave-equation-options/basic-shapes/list-source-mask-shapesList basic shapes, which are currently used in the definition of the source mask geometry.
define/models/acoustics/wave-equation-options/basic-shapes/list-sponge-layer-shapesList basic shapes, which are currently used in the definition of the sponge layer geometry.
define/models/acoustics/wave-equation-options/basic-shapes/list-region-registersList all available cell registers of the type "Region".
define/models/acoustics/wave-equation-options/basic-shapes/remove-source-mask-shapeRemove a basic shape from the definition of the source mask geometry.
define/models/acoustics/wave-equation-options/basic-shapes/remove-sponge-layer-shapeRemove a basic shape from the definition of the sponge layer geometry.
define/models/acoustics/wave-equation-options/remote-receivers-options/Enters the menu to define remote receivers for the Kirchhoff integral model.
define/models/acoustics/wave-equation-options/remote-receivers-options/integration-surfaceSelects the integration surface for the Kirchhoff model.
define/models/acoustics/wave-equation-options/remote-receivers-options/write-signalsWrites the computed receiver signals to the ASCII files.
define/models/acoustics/wave-equation-options/remote-receivers?Enables/disables the Kirchhoff integral model.
define/models/acoustics/wave-equation-options/source-mask-udfSpecifies the name of a user-defined function, which defines geometry of the source mask.
define/models/acoustics/wave-equation-options/sponge-layer-base-valueSpecifies the base value of the artificial viscosity coefficient.
define/models/acoustics/wave-equation-options/sponge-layer-factorSpecifies the factor of the artificial viscosity coefficient.
define/models/acoustics/wave-equation-options/sponge-layer-udfSpecifies the name of a user-defined function, which defines geometry of the sponge layer.
define/models/acoustics/wave-equation-options/time-filter-source?Enables/disables a time filter for the sound source.
define/models/acoustics/write-acoustic-signalsWrites on-the-fly sound pressure.
define/models/acoustics/write-centroid-infoWrites centroid info.
define/models/addon-moduleLoads addon module.
define/models/axisymmetric?Specifies whether or not the domain is axisymmetric.
define/models/battery-modelEnables the dual potential MSMD battery model. For text commands that become available when the battery model is enabled, refer to Battery Model Text Commands.
define/models/cht/Enters the cht (conjugate heat transfer) menu.
define/models/cht/implicit-coupling?Enables the implicit mapping scheme for any fluid-solid pair with a mapped mesh interface (only required for cases set up in version 19.2 or earlier).
define/models/cht/explicit-time-averaged-couplingEnters the explicit time averaged thermal coupling menu.
define/models/cht/explicit-time-averaged-coupling/conformal-coupled-wallsSpecify explicit coupling controls for coupled conformal walls. Note this operation will slit the coupled wall pair.
define/models/cht/explicit-time-averaged-coupling/coupling-controlsSpecifies the number of time steps per coupling iteration.
define/models/cht/explicit-time-averaged-coupling/fuse-explicit-cht-zonesFuses slitted conformal coupled walls marked for transient explicit thermal coupling.
define/models/crevice-model?Enables/disables the crevice model.
define/models/crevice-model-controls/Enters the crevice model controls menu.
define/models/dpm/Enters the dispersed phase model menu.
define/models/dpm/clear-particles-from-domainRemoves/keeps all particles currently in the domain.
define/models/dpm/collisions/Enters the DEM collisions menu.
define/models/dpm/collisions/collision-meshInput for the collision mesh.
define/models/dpm/collisions/collision-pair-settings/Supplies settings for collisions to a pair of collision partners. You will be prompted to specify the
Impact collision partnerand theTarget collision partner.define/models/dpm/collisions/collision-pair-settings/contact-force-normalSets the normal contact force law for this pair of collision partners.
define/models/dpm/collisions/collision-pair-settings/contact-force-tangentialSets the tangential contact force law for this pair of collision partners.
define/models/dpm/collisions/collision-pair-settings/list-pair-settingsLists the current settings for this pair of collision partners.
define/models/dpm/collisions/collision-partners/Manages collision partners.
define/models/dpm/collisions/collision-partners/copyCopies a collision partner.
define/models/dpm/collisions/collision-partners/createCreates a collision partner.
define/models/dpm/collisions/collision-partners/deleteDeletes a collision partner.
define/models/dpm/collisions/collision-partners/listLists all known collision partners.
define/models/dpm/collisions/collision-partners/renameRenames a collision partner.
define/models/dpm/collisions/dem-collisions?Enables/disables the DEM collision model.
define/models/dpm/collisions/list-all-pair-settingsFor each pair of collision partners, lists the collision laws and their parameters.
define/models/dpm/collisions/max-particle-velocitySets the maximum particle velocity that may arise from collisions.
define/models/dpm/erosion-dynamic-mesh/Enters the menu to enable/configure/run the erosion-dynamic mesh interaction.
define/models/dpm/erosion-dynamic-mesh/enable-erosion-dynamic-mesh-coupling?Enables mesh deformation due to wall erosion.
define/models/dpm/erosion-dynamic-mesh/general-parameters/Enters the menu for setting erosion coupling with dynamic mesh.
define/models/dpm/erosion-dynamic-mesh/general-parameters/dynamic-mesh-settingsSets parameters for dynamic mesh calculations.
define/models/dpm/erosion-dynamic-mesh/general-parameters/erosion-settingsSets parameters for erosion calculations.
define/models/dpm/erosion-dynamic-mesh/general-parameters/participating-wallsSpecifies all participating walls.
define/models/dpm/erosion-dynamic-mesh/run-parameters/Manages erosion-dynamic mesh run settings.
define/models/dpm/erosion-dynamic-mesh/run-parameters/autosave-filesSets the iteration increment and filename to save data files.
define/models/dpm/erosion-dynamic-mesh/run-parameters/autosave-graphicsSets the iteration increment to save graphics files.
define/models/dpm/erosion-dynamic-mesh/run-parameters/flow-simulation-controlSets the number of iterations per flow simulation step.
define/models/dpm/erosion-dynamic-mesh/run-parameters/mesh-motion-time-stepSets the mesh motion time stepping parameters and method.
define/models/dpm/erosion-dynamic-mesh/run-parameters/simulation-terminationSets the total time of erosion.
define/models/dpm/erosion-dynamic-mesh/run-simulationPerforms a coupled erosion-dynamic mesh simulation.
define/models/dpm/injections/Enters the injections menu.
define/models/dpm/injections/create-injectionCreates an injection.
define/models/dpm/injections/delete-injectionDeletes an injection.
define/models/dpm/injections/injection-properties/Enters the menu to set or display properties for one or more injections.
define/models/dpm/injections/injection-properties/file/Enters the menu to specify file injection settings.
define/models/dpm/injections/injection-properties/file/filenameSpecifies the name for the injection file.
define/models/dpm/injections/injection-properties/file/repeat-interval-in-filePuts the unsteady file injection into a time-periodic mode. For more information, see User Input for File Injections in the Fluent User's Guide.
define/models/dpm/injections/injection-properties/file/start-flow-time-in-fileSpecifies the flow-time in the unsteady injection file from which Ansys Fluent starts reading the injection file. For more information, see User Input for File Injections in the Fluent User's Guide.
define/models/dpm/injections/injection-properties/list/Enters the menu to display the current properties for one or more injections.
define/models/dpm/injections/injection-properties/list/list-picked-injectionsLists the injections that have been selected for display using
pick-injections-to-list.define/models/dpm/injections/injection-properties/list/list-picked-properties-to-listLists the properties that have been selected for display using
pick-properties-to-list.define/models/dpm/injections/injection-properties/list/list-property-valuesLists the settings for the properties selected with
pick-properties-to-list. This text command is only available when a single injection has been selected withpick-injections-to-list. This option is available if at least two injections have been selected.define/models/dpm/injections/injection-properties/list/list-uniform-valuesLists the settings for properties selected with
pick-properties-to-listthat have uniform values for all of the injections selected withpick-injections-to-list. This option is available if at least two injections have been selected.define/models/dpm/injections/injection-properties/list/list-values-per-injectionFor each injection selected with
pick-injections-to-list, lists the values for properties selected withpick-properties-to-list. This option is available if at least two injections ave been selected.define/models/dpm/injections/injection-properties/list/list-values-per-propertyFor each property selected with
pick-properties-to-list, lists the values for the injections selected withpick-injections-to-list. This option is available if at least two injections have been selected.define/models/dpm/injections/injection-properties/list/pick-injections-to-listSelects the injection or injections for which property values will be displayed. The use of asterisks (
*) as wildcards is supported.define/models/dpm/injections/injection-properties/list/pick-properties-to-listSelects the property or properties for which values will be displayed. The use of asterisks (
*) as wildcards is supported.
define/models/dpm/injections/injection-properties/set/Enters the menu to set physical models such as drag and breakup for one or more injections.
define/models/dpm/injections/injection-properties/set/list-picked-injectionsLists the injections selected for setting with
pick-injections-to-set.define/models/dpm/injections/injection-properties/set/location/Enters the injection location settings menu.
define/models/dpm/injections/injection-properties/set/general-settings/Enters the menu for general settings. This option is available only if at least one injection has been selected using
define/injections/properties/set/pick-injections-to-set.define/models/dpm/injections/injection-properties/set/general-settings/inject-wall-film-particles?Enables the injection of wall-film particles.
define/models/dpm/injections/injection-properties/set/general-settings/particle-reinjection/Enters the menu for setting particle reinjection options. This item is available for unsteady particle tracking only.
define/models/dpm/injections/injection-properties/set/general-settings/particle-reinjection/use-inj-for-reinjection?Specifies whether the injection is used only for reinjecting particles.
define/models/dpm/injections/injection-properties/set/general-settings/particle-reinjection/reinjection-time-delaySpecifies a time delay for particle reinjection, thus accounting for a residence time of the particle outside the CFD mesh domain. This item is available only when the
use-inj-for-reinjection?text option or the Reinjection Only GUI option is enabled.
define/models/dpm/injections/injection-properties/set/general-settings/reference-frameSets the reference frame for injection point properties. You can choose either
global(default) or one of the local reference frames that you created. This option is available only if at least one injection has been selected usingdefine/injections/properties/set/pick-injections-to-set.
define/models/dpm/injections/injection-properties/set/location/spatial-staggering/Enters the injection spatial-staggering settings menu.
define/models/dpm/injections/injection-properties/set/location/spatial-staggering/stagger-in-injection-plane?Enables/disables spatial staggering of the hollow cone injection in the injection plane. This option is available only if a hollow cone injection has been selected using
define/injections/properties/set/pick-injections-to-set.define/models/dpm/injections/injection-properties/set/location/spatial-staggering/stagger-atomizer-positions?Enables 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.define/models/dpm/injections/injection-properties/set/location/spatial-staggering/stagger-radiusSpecifies 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.define/models/dpm/injections/injection-properties/set/location/spatial-staggering/stagger-std-inj-positions?Enables 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.
define/models/dpm/injections/injection-properties/set/physical-models/Enters 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-settext command.define/models/dpm/injections/injection-properties/set/physical-models/brownian-motionEnables Brownian motion effects for the currently selected injection(s).
define/models/dpm/injections/injection-properties/set/physical-models/drag-parametersSets the drag law and corresponding parameters for the currently selected injection(s).
define/models/dpm/injections/injection-properties/set/physical-models/heat-exchangeEnters the menu for setting the heat exchange with the continuous phase. This item is available only for cases with inert or combusting particles, or with multicomponent particles that do not contain evaporating species.
define/models/dpm/injections/injection-properties/set/physical-models/heat-exchange/heat-transfer-coefficientAllows you to choose the heat transfer coefficient correlation. The options include
constant-HTC,Nusselt-number,Ranz-Marshall(default),Hughmark,Tomiyama, andGunn.
define/models/dpm/injections/injection-properties/set/physical-models/particle-rotationEnters the menu to set-up rotation related models.
define/models/dpm/injections/injection-properties/set/physical-models/particle-rotation/enable-rotationEnables/disables solution of ODE for the angular acceleration of particles.
define/models/dpm/injections/injection-properties/set/physical-models/particle-rotation/magnus-lift-lawSets the law for the rotational lift coefficient used in the formulation of Magnus lift force.
define/models/dpm/injections/injection-properties/set/physical-models/particle-rotation/rotational-drag-lawSets the law for the rotational drag coefficient.
define/models/dpm/injections/injection-properties/set/physical-models/rough-wall-modelEnables/disables the rough wall model.
define/models/dpm/injections/injection-properties/set/physical-models/spray-secondary-breakupEnters 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.
define/models/dpm/injections/injection-properties/set/pick-injections-to-setSelects the injection or injections for which properties will be set. The use of asterisks (
*) as wildcards is supported.define/models/dpm/injections/injection-properties/set/point-properties/Enters the menu for setting the initial conditions for the injection selected using
define/injections/properties/set/pick-injections-to-set. See Setting Initial Conditions for the Discrete Phase in the Fluent User's Guide for a list of point properties for the specific injection type.define/models/dpm/injections/injection-properties/set/size-distribution/Enters the menu for linking the size distribution variables to the tabulated distribution data. This item is available only with surface, cone and volume injections. Prior to using this menu, you must read a table into your case using the
file/table-manager/read-matrix-data-filetext command.define/models/dpm/injections/injection-properties/set/size-distribution/enable-tabulated-size-distribution?Enables/disables the use of the tabulated size distribution for your injection.
define/models/dpm/injections/injection-properties/set/size-distribution/set-diam-column-nameSelects the column name where data for the reference diameters is stored. Note that you must first select the table name using the
define/models/dpm/injections/injection-properties/set/size-distribution/table-nametext command.define/models/dpm/injections/injection-properties/set/size-distribution/set-mass-frac-column-nameSelects the column name where data for the mass fractions is stored. Note that you must first select the table name using the
define/models/dpm/injections/injection-properties/set/size-distribution/table-nametext command.define/models/dpm/injections/injection-properties/set/size-distribution/set-num-frac-column-nameSelects the column name where data for the number fractions is stored. Note that you must first select the table name using the
define/models/dpm/injections/injection-properties/set/size-distribution/table-nametext command.define/models/dpm/injections/injection-properties/set/size-distribution/table-nameSpecify the name of the table containing discrete diameter distribution data.
define/models/dpm/injections/injection-properties/set/size-distribution/use-diameter-interpolation-between-classes?Enables/disables linear interpolation of particle diameters between neighboring diameter classes.
define/models/dpm/injections/injection-properties/set/size-distribution/use-randomized-diameter-sampling?Enables/disables the use of the randomized diameter sampling for the tabulated size distribution. When this text option is disabled, particles from each tabulated diameter class are injected from each particle starting position.
define/models/dpm/injections/list-injection-propertiesLists properties of the selected injection(s) in the console window.
define/models/dpm/injections/list-particlesLists particle streams in an injection.
define/models/dpm/injections/modify-all-injections/Enters the menu to set properties for all injections.
define/models/dpm/injections/modify-all-injections/injection-typeDefines injection type.
define/models/dpm/injections/modify-all-injections/number-of-triesSets the number of stochastic tries.
define/models/dpm/injections/modify-all-injections/random-eddy-lifetime?Turns enable/disable a random eddy lifetime.
define/models/dpm/injections/modify-all-injections/stochastic-tracking?Turns enable/disable stochastic tracking.
define/models/dpm/injections/modify-all-injections/time-scale-constantSets the time scale constant.
define/models/dpm/injections/rename-injectionRenames an injection.
define/models/dpm/injections/set-injection-propertiesSets injection properties.
Important: Drag and breakup model parameters for each injection are set instead in
/define/models/dpm/injections/injection-properties.
define/models/dpm/interaction/Sets parameters for coupled discrete phase calculations.
define/models/dpm/interaction/coupled-calculations?Selects whether or not to couple continuous and discrete phase calculations.
define/models/dpm/interaction/ddpm-energy-coupling-via-source-term?Enables/disables the energy coupling between the discrete phases (DDPM) and the primary phase via the source term. Note that when this option is enabled, the Total Heat Transfer Rate flux report for the mixture currently generates inaccurate results.
define/models/dpm/interaction/ddpm-enhanced-inter-phase-exchange?Enables/disables the enhanced Eulerian inter-phase exchange. This option is available only for cases with the energy equation enabled and is recommended for simulations with poly-dispersed particles.
define/models/dpm/interaction/dpm-iteration-intervalSets the frequency with which the particle trajectory calculations are introduced.
define/models/dpm/interaction/enhanced-source-term-linearization-enabled?When enabled, uses an enhanced source-term linearization method for the discrete phase. The method can improve solution convergence in some cases. This command is available only when the
define/models/dpm/interaction/linearized-dpm-source-terms?option is enabled.define/models/dpm/interaction/enable-flow-blocking-by-particles?Enables/disables the inclusion of DPM volume fraction in continuous flow.
define/models/dpm/interaction/implicit-momentum-coupling?Enables/disables implicit treatment for the DPM momentum source terms.
define/models/dpm/interaction/implicit-source-term-coupling?Enables/disables implicit treatment for all DPM source terms.
define/models/dpm/interaction/linear-growth-of-dpm-source-term?Enables/disables the linear ramping up of the DPM source terms at every DPM iteration.
define/models/dpm/interaction/linearized-dpm-mixture-fraction-source-terms?Enables/disables linearization of mixture fraction source terms. This command is available only for non- or partially-premixed combustion cases.
define/models/dpm/interaction/linearized-dpm-source-terms?Enables/disables linearization of source terms for the discrete phase.
define/models/dpm/interaction/linearized-dpm-species-source-terms?Enables/disables the linearization of the species source terms for the discrete phase. This item is available with the species transport model.
define/models/dpm/interaction/max-vf-allowed-for-blockingSets the maximum DPM volume fraction in the continuous flow. This item is available only when the
define/models/dpm/interaction/enable-flow-blocking-by-particles?option is enabled.define/models/dpm/interaction/replace-dpm-mass-source-by-mixture-fraction?When enabled, recalculates the mixture fraction source terms as a function of the primary mixture fraction. This command is available for non- or partially-premixed combustion cases only.
define/models/dpm/interaction/reset-sources-at-timestep?Enables/disables flush of DPM source terms at beginning of every time step.
define/models/dpm/interaction/second-order-time-accurate-sources-enabled?When enabled, uses the second-order accurate formulation for transient DPM source terms. The method may improve the solution accuracy. The command is available only for the pressure-based solver when the
define/models/unsteady-2nd-order?option is enabled.define/models/dpm/interaction/underrelaxation-factorSets the under-relaxation factor for the discrete phase sources.
define/models/dpm/interaction/update-dpm-sources-every-flow-iteration?Enables/disables the update of DPM source terms every flow iteration (if this option is not enabled, the terms will be updated every DPM iteration).
define/models/dpm/numerics/Enters the numerics menu to set numerical solution parameters.
define/models/dpm/numerics/automated-scheme-selection?Enables/disables the adaptation of integration step length based on a maximum error.
define/models/dpm/numerics/average-DDPM-variables?Enables/disables mesh node averaging of DDPM quantities.
define/models/dpm/numerics/average-each-step?Enables/disables mesh node averaging during integration time step.
define/models/dpm/numerics/average-kernelSpecifies the averaging kernel to use for mesh node averaging.
define/models/dpm/numerics/average-source-terms?Enables/disables mesh node averaging of DPM source terms.
define/models/dpm/numerics/coupled-heat-mass-updateEnables/disables coupled heat and mass update.
define/models/dpm/numerics/drag-lawSets the drag law.
define/models/dpm/numerics/dynamic-interaction?Enable/disable the dynamic interaction range. This option can be helpful for cases where the particle diameter may be too large compared to the local mesh cell size. See Using the Dynamic Interaction Range in the Fluent User's Guide for more information. This option is available only with high-resolution tracking.
define/models/dpm/numerics/enable-node-based-averaging?Enables/disables mesh node averaging of DPM quantities.
define/models/dpm/numerics/enhanced-packing-limit-numerics?Enables/disables enhanced packing limit numerics to avoid exceeding the packing limit for granular phases. This item is available only when the DDPM model is used.
define/models/dpm/numerics/error-control?Adapts integration step length based on a maximum error.
define/models/dpm/numerics/gaussian-factorSpecifies the Gaussian constant when using thegaussian kernel for mesh node averaging.
define/models/dpm/numerics/high-resolution-tracking/Enters the high resolution tracking menu. See Tracking Settings for the Discrete Phase Model in the Fluent User's Guide for more information about these options.
-
define/models/dpm/numerics/high-resolution-tracking/always-use-face-centroid-with-periodics? When enabled, Ansys Fluent uses quad face centroids when creating subtets in cases with periodic boundaries.
define/models/dpm/numerics/high-resolution-tracking/barycentric-interpolation/Enter the barycentric interpolation menu.
define/models/dpm/numerics/high-resolution-tracking/barycentric-interpolation/interpolate-flow-cp?Enables/disables the barycentric interpolation of specific heat to the particle position. This option is recommended when the specific heat varies with position to avoid discontinuities in the interpolated variable at cell boundaries. For flows with constant specific heat, this option is unnecessary.
define/models/dpm/numerics/high-resolution-tracking/barycentric-interpolation/interpolate-flow-density?Enables/disables the barycentric interpolation of the flow density. This option is recommended when the density varies with position to avoid discontinuities in the interpolated variable at cell boundaries. For constant density flows, this option is unnecessary.
define/models/dpm/numerics/high-resolution-tracking/barycentric-interpolation/interpolate-flow-solution-gradients?When enabled, flow solution gradients are interpolated to the particle position. This can be useful when using physical models that depend on these gradients (for example, the thermophoretic force, pressure-gradient force, or virtual mass force). Interpolating the gradients also improves the accuracy and robustness of the trapezoidal numerics scheme, which is the default method for pathlines.
define/models/dpm/numerics/high-resolution-tracking/barycentric-interpolation/interpolate-flow-viscosity?Enables/disables the barycentric interpolation of flow viscosity to the particle position. This option is recommended when the flow viscosity varies with position to avoid discontinuities in the interpolated variable at cell boundaries. For flows with constant viscosity, this option is unnecessary.
define/models/dpm/numerics/high-resolution-tracking/barycentric-interpolation/interpolate-temperature?Enables/disables the barycentric interpolation of temperature to the particle position. The cell temperature is used by default in calculations of heat transfer to/from the particle.
-
define/models/dpm/numerics/high-resolution-tracking/barycentric-interpolation/interpolate-wallfilm-properties? When enabled, the wall film properties (film height, film mass, and wall shear) are interpolated to the particle position.
-
define/models/dpm/numerics/high-resolution-tracking/barycentric-interpolation/precompute-pdf-species? When this option is enabled for premixed or non-premixed combustion simulations, the species composition in each cell is precomputed prior to tracking particles. This approach may improve performance for cases with many particles and relatively few cells. By default, this option is set to
no, and Ansys Fluent calculates the species composition during particle tracking. The solution results will be identical for both methods.-
define/models/dpm/numerics/high-resolution-tracking/barycentric-interpolation/user-interpolation-function Provides a hook for the
DEFINE_DPM_INTERPOLATIONuser-defined function (UDF) used to interpolate cell UDM to the particle position when using high-resolution particle tracking. SeeDEFINE_DPM_BODY_FORCEin the Fluent Customization Manual for more information about this UDF.define/models/dpm/numerics/high-resolution-tracking/barycentric-interpolation/zero-nodal-velocity-on-walls?When enabled, sets the velocity at wall nodes to zero. (By default, the nodal velocities on walls are first reconstructed from cell and face values and then corrected to ensure that there are no velocity components directed towards the walls). This may be useful if you want to consider particle impingement on the walls. Note that enabling this option will more likely produce incomplete particles as some particles may settle on the walls.
define/models/dpm/numerics/high-resolution-tracking/boundary-layer-tracking?Enables/disables the calculation of the particle time step that considers both the cell aspect ratio and the particle trajectory. This method improves the accuracy of the predictions in boundary layer cells, particularly in layers where flow gradients are large.
define/models/dpm/numerics/high-resolution-tracking/check-subtet-validity?When enabled, checks the validity of a subtet when the particle first enters it. If the subtet is found to be degenerate, the tracking algorithm modifies to accommodate it.
define/models/dpm/numerics/high-resolution-tracking/enable-automatic-intersection-tolerance?Enables/disables the automatic calculation of intersection tolerance. By default, the tolerance used in intersection calculations is scaled by the residence time of the particle in the cell to improve robustness. For most cases, the scaled tolerance is sufficient to identify all intersections of the particle trajectory and the subtet faces. You can set the intersection tolerance manually using the
set-subtet-intersection-tolerancetext command.define/models/dpm/numerics/high-resolution-tracking/enable-barycentric-intersections?Enables/disables an alternative method of calculating intersections with cell boundaries. Barycentric intersections are linear calculations and are faster than the default intersection algorithm. The default intersection algorithm is second-order for stationary meshes; therefore, using the barycentric intersection may sacrifice accuracy. You must verify that the barycentric intersections provide comparable results to the default intersection method. This option is available only for 3D stationary meshes and the double precision solver.
define/models/dpm/numerics/high-resolution-tracking/enable-high-resolution-tracking?Enables/disables high resolution tracking.
define/models/dpm/numerics/high-resolution-tracking/particle-relocation/Enters the particle relocation menu.
define/models/dpm/numerics/high-resolution-tracking/particle-relocation/enhanced-cell-relocation-method?When enabled, Ansys Fluent uses a more rigorous method of locating the cell in which the particle is currently contained. This approach is computationally more expensive than the default method; however, it is recommended for cases when Fluent reports that particles are lost after the mesh has been changed due to MDM, dynamic adaption, or repartitioning.
define/models/dpm/numerics/high-resolution-tracking/particle-relocation/enhanced-wallfilm-location-method?When enabled, Ansys Fluent uses a more robust method of locating the wall film particles on the film zone after the domain has been remeshed either due to dynamic mesh movement or automatic adaption. The improved robustness involves a performance penalty. This method is recommended for cases when Fluent reports that wall film particles are lost during relocation.
define/models/dpm/numerics/high-resolution-tracking/particle-relocation/load-legacy-particles?Allows you to use a Fluent data file containing particles that were tracked without the high-resolution tracking option. When this option is enabled, the particles that are found outside the associated cells in the data file will be moved inside these cells prior to tracking. Neither the mesh nor the partitioning should be modified prior to the first time the particles are tracked. If you need to perform manual or dynamic mesh adaption, you must first disable this option. This option can be enabled before or after reading the data file into Ansys Fluent.
define/models/dpm/numerics/high-resolution-tracking/particle-relocation/overset-relocation-robustness-levelSets the performance/robustness trade-off when relocating particles in overset meshes. The default value is 1, which corresponds to a more robust algorithm. Performance may be improved by setting the value to 0; however, this may result in particle loss, particularly if the mesh is moving. You need to make sure that no particle loss occurs.
define/models/dpm/numerics/high-resolution-tracking/particle-relocation/use-legacy-particle-location-method?Provides the ability to use the legacy particle location method with high-resolution tracking to improve performance. This option allows the faster but less accurate particle location method to be used with high-resolution tracking. This option is useful when tracking in polyhedral meshes, particularly when unsteady particles that evaporate quickly are injected frequently (for example, gas turbine combustors). Note that it does not improve the particle tracking speed, only the time it takes to inject the particles.
define/models/dpm/numerics/high-resolution-tracking/particle-relocation/wallfilm-relocation-tolerance-scale-factorSets a scaling factor to modify the tolerance for locating Lagrangian wall film (LWF) particles on a film face during the relocation. The default value is 1.0. Increasing the tolerance may help when Ansys Fluent fails to locate LWF particles in such cases.
define/models/dpm/numerics/high-resolution-tracking/project-wall-film-particles-to-film?Enables/disables projecting existing particles to Lagrangian wall film to track using high-resolution tracking.
When reading in a data file that contains wall film particles previously tracked with the existing Ansys Fluent tracking method, you need to either clear the particles from the domain or project their positions to the wall film surface using the
project-wall-film-particles-to-film?text command prior to using the high-resolution tracking method. After tracking the particles for one timestep, this option can be disabled to improve performance.-
define/models/dpm/numerics/high-resolution-tracking/set-film-spreading-parameter Provides the ability to add a random component to the Lagrangian wall-film particle acceleration to reduce streaking that may result from tracking particles on faceted geometry. As small variations in face normals can produce streaks in the wall-film appearance, this parameter makes the film look smoother. The value of this parameter should range between 0 and 1.0. The default value of 0 prevents any artificial smoothing.
define/models/dpm/numerics/high-resolution-tracking/set-subtet-intersection-toleranceSpecifies the tolerance used in intersection calculations. This tolerance will be scaled by the characteristic cell crossing time of the particle if the
enable-automatic-intersection-tolerance?text command is enabled. If that option is disabled, the specified tolerance will be used without scaling. The default intersection tolerance is 10-5.-
define/models/dpm/numerics/high-resolution-tracking/sliding-interface-crossover-fraction Specifies the fraction of the distance to the subtet center to move the particle.
At non-conformal interfaces, the nodes used for the barycentric interpolation are different on either side of the interface. This may result in incomplete particles due to discontinuities in the variable interpolation. The number of incomplete particles may be reduced by moving the particles slightly off of the sliding interface. Recommended values range between 0 and 0.5.
define/models/dpm/numerics/high-resolution-tracking/use-barycentric-sampling?When enabled, this option provides improved accuracy and parallel consistency when sampling particles at planes. This item is available only with the 3D solver. Using the double-precision solver and bounded planes is recommended.
define/models/dpm/numerics/high-resolution-tracking/use-quad-face-centroid?Enables/disables using quad face centroids when creating subtets. This option changes the way hexahedral cells are decomposed to avoid creating degenerate subtets.
-
define/models/dpm/numerics/high-resolution-tracking/use-particle-timestep-for-intersection-tolerance? Enables/disables the use of the particle timestep for the subtet intersection tolerance with axisymmetric grids (default: enabled). If disabled, the tolerance will be calculated in the same manner as non-axisymmetric meshes (a scaled value of the tolerance which is set using the
define/models/dpm/numerics/high-resolution-tracking/set-subtet-intersection-tolerancetext command).-
define/models/dpm/numerics/high-resolution-tracking/use-velocity-based-error-control? Enables/disables an alternative method of timestep adaption. By default, Ansys Fluent uses the half-step method of timestep adaption with particle integration. This alternative method of controlling the integration timestep based upon velocity changes is faster; however, you need to ensure that the accuracy is comparable for your specific application.
-
define/models/dpm/numerics/minimum-liquid-fractionA droplet evaporates completely when the remaining mass is below this fraction of the initial droplet mass.
define/models/dpm/numerics/re-randomize-every-iteration?Determines whether or not the initial particle positions will vary from iteration to iteration.
define/models/dpm/numerics/re-randomize-every-timestep?Determines whether or not the initial particle positions will vary from time step to time step.
define/models/dpm/numerics/tracking-parametersSets parameters for the (initial) tracking step length.
define/models/dpm/numerics/tracking-schemeSpecifies a tracking scheme.
define/models/dpm/numerics/tracking-statisticsControls the format of the one-line tracking statistics to be printed after every DPM tracking pass. A value of
0(the default) prints only fates with non-zero values. A value of1prints all fates, including fates with zero values.define/models/dpm/numerics/underrelax-film-heightSets the under-relaxation factor for the film height calculation. The recommended values range between 0.5 (default) and 0.9.
define/models/dpm/numerics/vaporization-limiting-factorsSets the Vaporization Fractional Change Limits.
define/models/dpm/options/Enters the options menu to set optional models.
define/models/dpm/options/allow-supercritical-pressure-vaporization?Enforces 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 whenPressure Dependent Boiling is enabled in the Physical Models tab of the Discrete Phase Models dialog box. For more details, see Considering Pressure Dependence in Boiling in the Fluent User's Guide.define/models/dpm/options/brownian-motionEnables/disables Brownian motion of particles.
define/models/dpm/options/current-positions-in-sample-file-format?When enabled, generates a file containing particle current positions (step-by-step history report for unsteady tracking) in the sampling file format.
define/models/dpm/options/convective-film-heat-transfer?Enables/disables the convective wall-film heat transfer model. See Film Boiling Model with Convective Heat Transfer Model in the Fluent Theory Guide for more information about this model.
define/models/dpm/options/enable-contour-plotsEnables computation of mean and/or RMS values of additional discrete phase variables for postprocessing.
define/models/dpm/options/erosion-accretionEnables/disables erosion/accretion.
define/models/dpm/options/include-lwf-particles-in-dpm-concentration?When enabled, the mass of the Lagrangian wall film particles is included in the calculation of the concentration. This option is disabled by default.
define/models/dpm/options/init-erosion-accretion-rateInitializes the erosion/accretion rates with zero.
define/models/dpm/options/maximum-udf-speciesSpecifies 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.
define/models/dpm/options/particle-radiationEnables/disables particle radiation.
define/models/dpm/options/pressure-gradient-forceEnables/disables inclusion of pressure gradient effects in the particle force balance.
define/models/dpm/options/remove-wall-film-temperature-limiter?Answering
yesat the first prompt removes the wall temperature limiter for walls with the Lagrangian wall-film boundary condition. If you enterno(default), then you will be prompted for the temperature difference above the boiling point. You will be also prompted whether you want to enable the reporting of the Leidenfrost temperature on the wall faces.define/models/dpm/options/set-minimumparticle- diameterSets the minimum particle diameter permitted during tracking. By default, Ansys Fluent limits the smallest particle diameter to 10 nm. Evaporating and reacting particles that are smaller than this limit will be removed. If inert particles are injected with diameters below this limit, the results may be inaccurate. When tracking smaller particles, you can use this text command to reduce the minimum particle diameter.
define/models/dpm/options/scr-urea-deposition/Enters the menu for setting up options for urea deposition in Selective Catalytic Reduction (SCR) simulations. For more information about risk for solids deposit formation for the SCR process, see Assessing the Risk for Solids Deposit Formation During Selective Catalytic Reduction Process in the Fluent User's Guide.
define/models/dpm/options/scr-urea-deposition/cryst-depo-weightSets the weighting factor for crystallization reactions risk.
define/models/dpm/options/scr-urea-deposition/cryst-max-tempSets maximum temperature for urea crystallization.
define/models/dpm/options/scr-urea-deposition/cryst-min-mass-fractSets the minimum urea mass fraction for crystallization.
define/models/dpm/options/scr-urea-deposition/cryst-min-tempSets minimum temperature for urea crystallization.
define/models/dpm/options/scr-urea-deposition/enable-risk-analysis?Enables/disables the SCR urea deposition risk analysis.
define/models/dpm/options/scr-urea-deposition/heat-flux-based-risk-weightSets the weighting factor for heat flux-based component within hydrodynamic risk.
define/models/dpm/options/scr-urea-deposition/hydrodynamic-risk-weightSets the weighting factor for all hydrodynamic deposition risk.
define/models/dpm/options/scr-urea-deposition/seco-rx-max-tempSets maximum temperature for secondary reactions.
define/models/dpm/options/scr-urea-deposition/seco-rx-min-hncoSets the minimum HNCO mass fraction in the gas phase above the film for secondary reactions.
define/models/dpm/options/scr-urea-deposition/seco-rx-min-tempSets minimum temperature for secondary reactions.
define/models/dpm/options/scr-urea-deposition/set-liquid-propertiesSpecifies viscosity and surface tension of the deposited urea-liquid by-products.
define/models/dpm/options/scr-urea-deposition/velocity-based-risk-weightSets the weighting factor for velocity-based component within hydrodynamic risk.
define/models/dpm/options/scr-urea-deposition/wall-face-zonesLists the selected wall zones and allows you to modify the selection list.
define/models/dpm/options/set-thermolysis-limitSets the limit for the thermolysis model.
define/models/dpm/options/stagger-spatially-atomizer-injections?Enables/disables spatial staggering for atomizer and solid-cone injections.
define/models/dpm/options/stagger-spatially-standard-injections?Enables/disables spatial staggering for standard (non-atomizer and non-solid-cone) injections.
define/models/dpm/options/stagger-temporally?Enables/disables temporal staggering.
define/models/dpm/options/staggering-factorControls the percentage of every particle's initial time step that will be sampled.
define/models/dpm/options/saffman-lift-forceEnables/disables Saffman lift force.
define/models/dpm/options/stagger-radiusSpecifies the region over which to spatially stagger particles when particle-staggering is enabled for non-atomizer injections.
define/models/dpm/options/step-report-sig-figuresSets significant figures in the step-by-step report.
define/models/dpm/options/thermophoretic-forceEnables/disables thermophoretic force.
define/models/dpm/options/track-in-absolute-frameEnables/disables tracking in absolute frame.
define/models/dpm/options/two-step-devolatilization-limitSets the limit for the two-step devolatilization reaction.
define/models/dpm/options/treat-multicomponent-saturation-temperature-failure?Enables/disables dumping multicomponent particle mass into the continuous phase if the saturation temperature calculation fails.
define/models/dpm/options/two-way-couplingEnables/disables calculation of DPM sources in TKE equation.
define/models/dpm/options/uniform-mass-distribution-for-injections?Specifies 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.
define/models/dpm/options/use-absolute-pressure-for-vaporization?Determines whether the absolute pressure or constant operating pressure (specified in
define/operating-conditions/operating-pressure) will be used in vaporization rates calculations.define/models/dpm/options/vaporization-heat-transfer-averagingEnables averaging of the Spalding heat transfer term for the convection/diffusion-controlled model.
define/models/dpm/options/vaporization-optionsSets Vaporization options.
define/models/dpm/options/virtual-mass-forceEnables/disables inclusion of the virtual mass force in the particle force balance.
define/models/dpm/parallel/Enters the parallel menu to set parameters for parallel DPM calculations.
define/models/dpm/parallel/enable-workpile?Turns on/off particle workpile algorithm. This option is only available when the
define/models/dpm/parallel/use-shared-memoryoption is selected.define/models/dpm/parallel/expert/Enters the menu for expert DPM parallel text commands.
define/models/dpm/parallel/expert/partition-method-hybrid-2domainEnables/disables a partitioning method that is more granular and can yield faster calculations (especially for cases that are running on a low to moderate number of processors). This partitioning method is only applied when you use the DPM domain for the hybrid parallel DPM tracking mode (that is, when you have enabled the
define/models/dpm/parallel/hybrid-2domain?text command).
define/models/dpm/parallel/fix-source-term-accumulation-order?Enables/disables the deterministic tracking order of particles. This option is available only for fully coupled DPM cases that involve the hybrid parallel method.
define/models/dpm/parallel/hybrid-2domain?Enables/disables the use of a second domain for DPM particle tracking.
define/models/dpm/parallel/n-threadsSets the number of processors to use for DPM. This option is only available when the
define/models/dpm/parallel/enable-workpile?option is enabled.define/models/dpm/parallel/reportPrints particle workpile statistics. This option is only available when the
define/models/dpm/parallel/enable-workpile?option is enabled.define/models/dpm/parallel/use-hybridSpecifies that the calculations are performed using multicore cluster computing or shared-memory machines. This option works in conjunction with
openmpifor a dynamic load balancing without migration of cells.define/models/dpm/parallel/use-message-passingSpecifies 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.
define/models/dpm/parallel/use-shared-memorySpecifies that the calculations are performed on shared-memory multiprocessor machines.
define/models/dpm/splash-options/Enters the splash option menu.
define/models/dpm/splash-options/orourke-splash-fractionEnables/disables 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.
define/models/dpm/splash-options/splash-pdf-limitingSets 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.
define/models/dpm/spray-model/Enters the spray model menu. This command is available only if the breakup model enabled globally.
define/models/dpm/spray-model/breakup-model-summaryCurrent spray model settings.
define/models/dpm/spray-model/consider-children-in-the-same-tracking-step?Enables/disables collecting and tracking new generated child droplets within the same time step.
define/models/dpm/spray-model/droplet-coalescence?Enables/disables droplet coalescence when using the stochastic collision model. This option is available if all injections have been selected and the DEM model is disabled.
define/models/dpm/spray-model/droplet-collision?Enables/disables droplet collision model.
define/models/dpm/spray-model/enable-breakup?Enables/disables breakup globally, but does not alter injection settings other than enable/disable.
define/models/dpm/spray-model/khrt-modelSets the KHRT breakup model.
define/models/dpm/spray-model/madabhushi-modelSets the Madabhushi breakup model.
define/models/dpm/spray-model/no-breakupDisables 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.
define/models/dpm/spray-model/schmehl-modelSets the Schmehl breakup model.
define/models/dpm/spray-model/set-breakupEnables/disables breakup model globally and uniformly specifies injection breakup parameters.
define/models/dpm/spray-model/ssd-modelSets the SSD breakup model.
define/models/dpm/spray-model/tab-modelSets the TAB breakup model.
define/models/dpm/spray-model/tab-number-of-breakup-parcelsSets the number of parcels to break up a droplet in the TAB model.
define/models/dpm/spray-model/tab-randomize-breakup-parcel-diameter?Enables sampling of diameter for each TAB breakup parcel from a Rosin-Rammler distribution using a random number.
define/models/dpm/spray-model/wave-allow-rayleigh-growth?Allows 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.
define/models/dpm/spray-model/wave-mass-cutoffSets the minimum percentage of parent parcel mass shed before new parcel creation. This option is available only if the WAVE model is enabled.
define/models/dpm/spray-model/wave-modelSets the WAVE breakup model.
define/models/dpm/spray-model/wave-spray-angle-constantSets 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.
define/models/dpm/stripping-options/Enters the stripping options menu.
define/models/dpm/stripping-options/diameter-coefficientSets the diameter coefficient (
in Equation 17–20
in the Theory Guide)define/models/dpm/stripping-options/mass-coefficientSets the mass coefficient (
in Equation 17–21
in the Theory Guide)
define/models/dpm/unsteady-trackingEnables/disables unsteady particle tracking.
define/models/dpm/user-definedSets DPM user-defined functions.
define/models/electrolysis-setup/Enter the electrolysis and H2 pump model setup menu. This item is only available if the electrolysis and H2 pump model is enabled using the
define/models/potential-and-li-ion-battery?text command.define/models/electrolysis-setup/advanced-setup/Enter the advanced setup menu.
define/models/electrolysis-setup/advanced-setup/contact-resistivitySpecifies contact-resistivity for the specified zones.
define/models/electrolysis-setup/anode-setup/Enter the anode setup menu.
-
define/models/electrolysis-setup/anode-setup/catalyst-layer Specifies the settings for the catalyst layer.
-
define/models/electrolysis-setup/anode-setup/current-collector Specifies the settings for current collector.
-
define/models/electrolysis-setup/anode-setup/flow-channel Specifies the settings for the flow channel.
-
define/models/electrolysis-setup/anode-setup/porous-layer Specifies the settings for the porous-layer.
-
define/models/electrolysis-setup/cathode-setup/Enter the cathode setup menu.
-
define/models/electrolysis-setup/cathode-setup/catalyst-layer Specifies the settings for the catalyst layer.
-
define/models/electrolysis-setup/cathode-setup/current-collector Specifies the settings for current collector.
-
define/models/electrolysis-setup/cathode-setup/flow-channel Specifiesthe settings for the flow channel.
-
define/models/electrolysis-setup/cathode-setup/porous-layer Specifies the settings for the porous-layer.
-
define/models/electrolysis-setup/customizationAllows you to hook up your
DEFINE_ELECTROLYSIS_ECHEM_RATEandDEFINE_ELECTROLYSIS_RELATIVE_PERMEABILITYuser-defined functions only if you previously compiled and loaded UDF library. SeeDEFINE_ELECTROLYSIS_ECHEM_RATEandDEFINE_ELECTROLYSIS_RELATIVE_PERMEABILITYin the Fluent Customization Manual for more information.define/models/electrolysis-setup/membrane-setup/Enters the menu for setting electrolyte/membrane.
define/models/electrolysis-setup/membrane-setup/electrolyteSpecifies the electrolyte/membrane settings.
-
define/models/electrolysis-setup/model-options Sets the electrolysis and H2 pump model options.
-
define/models/electrolysis-setup/model-parameters Sets the electrolysis and H2 pump model parameters.
define/models/energyEnables/disables the energy model.
define/models/eulerian-wallfilm/Enters the Eulerian wall film model menu.
define/models/eulerian-wallfilm/coupled-solution/Enters the Coupled-Solution menu.
define/models/eulerian-wallfilm/coupled-solution/enable-coupled-solution?Enables/disables the coupled solution method.
define/models/eulerian-wallfilm/coupled-solution/enable-curvature-smoothing?Enables/disables the film curvature smoothing option and sets the smoothing parameters.
define/models/eulerian-wallfilm/enable-film-vof-transition-messageEnables/disables messages showing the Film/VOF transition criteria on the selected film walls. This command is available only when the Film/VOF Transition & Criteria has been enabled in the Wall dialog box (VOF Interaction tab).
define/models/eulerian-wallfilm/enable-wallfilm-model?Enables/disables Eulerian Wall Film Model.
define/models/eulerian-wallfilm/film-materialSets Film Material and Properties.
define/models/eulerian-wallfilm/initialize-wallfilm-modelInitializes Eulerian wall film model.
define/models/eulerian-wallfilm/list-film-wallsLists names and IDs of all walls where the Eulerian wall film model is enabled.
define/models/eulerian-wallfilm/model-optionsSets Eulerian Wall Film Model Options.
define/models/eulerian-wallfilm/solution-optionsSets Eulerian Wall Film Model Solution Options.
define/models/eulerian-wallfilm/solve-wallfilm-equation?Activates Eulerian Wall Film Equations.
define/models/frozen-flux?Enables/disables frozen flux formulation for transient flows.
define/models/heat-exchanger/Enters the heat exchanger menu.
define/models/heat-exchanger/dual-cell-model/Enters the dual cell model menu.
define/models/heat-exchanger/dual-cell-model/add-heat-exchangerAdds heat-exchanger.
define/models/heat-exchanger/dual-cell-model/alternative-formulation?Enables/disables alternative formulation for heat transfer calculations.
define/models/heat-exchanger/dual-cell-model/delete-heat-exchangerDeletes heat-exchanger.
define/models/heat-exchanger/dual-cell-model/heat-exchanger?Enables/disables the dual cell heat-exchanger model.
define/models/heat-exchanger/dual-cell-model/modify-heat-exchangerModifies heat-exchanger.
define/models/heat-exchanger/dual-cell-model/plot-NTUPlots NTU vs. primary mass flow rate for each auxiliary mass flow rate.
define/models/heat-exchanger/dual-cell-model/write-NTUWrites NTU vs. primary mass flow rate for each auxiliary mass flow rate.
define/models/heat-exchanger/macro-model/Enters the heat macro-model menu.
define/models/heat-exchanger/macro-model/delete-heat-exchanger-groupDeletes heat-exchanger group.
define/models/heat-exchanger/macro-model/heat-exchanger?Enables/disables heat-exchanger model.
define/models/heat-exchanger/macro-model/heat-exchanger-groupDefines heat-exchanger group.
define/models/heat-exchanger/macro-model/heat-exchanger-macro-reportReports the computed values of heat rejection, outlet temperature, and inlet temperature for the macroscopic cells (macros) in a heat exchanger.
define/models/heat-exchanger/macro-model/heat-exchanger-modelDefines heat-exchanger core model.
define/models/heat-exchanger/macro-model/heat-exchanger-reportReports the computed values of total heat rejection, outlet temperature, and inlet temperature for a specified heat-exchanger core.
define/models/heat-exchanger/macro-model/heat-exchanger-zoneSpecifies the zone that represents the heat exchanger, the dimensions of the heat exchanger, the macro grid, and the coolant direction and properties.
define/models/heat-exchanger/macro-model/plot-NTUPlots NTU vs. primary mass flow rate for each auxiliary mass flow rate.
define/models/heat-exchanger/macro-model/write-NTUWrites NTU vs. primary mass flow rate for each auxiliary mass flow rate.
define/models/multiphase/Enters the multiphase model menu.
define/models/multiphase/body-force-formulationSpecifies body force formulation.
define/models/multiphase/coupled-level-setEnables coupled level set interface tracking method.
define/models/multiphase/explicit-expert-options/Enters the menu to set explicit VOF expert options.
define/models/multiphase/explicit-expert-options/solve-vof-every-iter?If you enter
yes, the volume fraction equations will be solved every iteration. By default, the volume fraction equations will be solved only once per time step.define/models/multiphase/explicit-expert-options/sub-time-step-methodSelects the sub-time step method.
define/models/multiphase/explicit-expert-options/volume-fraction-filtering/Enters the volume fraction filtering menu.
define/models/multiphase/explicit-expert-options/volume-fraction-filtering/enable?Enables/disables the volume fraction filtering treatment.
define/models/multiphase/explicit-expert-options/volume-fraction-filtering/filtering-optionsSelects the volume fraction filtering method. This command becomes available once the
define/models/multiphase/explicit-expert-options/volume-fraction-filtering/enable?text option has been set toyes.
define/models/multiphase/explicit-expert-options/volume-fraction-filtering/vol-frac-cutoffSpecifies a cut-off value for the volume fraction filtering. This command becomes available after you select the node averaged cutoff method using the
define/models/multiphase/explicit-expert-options/volume-fraction-filtering/filtering-optionstext command.
define/models/multiphase/flow-regime-modelingEnters the flow regime modeling menu. See Algebraic Interfacial Area Density Method for Flow Regime Blending in the Fluent Theory Guide for details about the below parameters.
define/models/multiphase/flow-regime-modeling/aiad-parameters/Enters the menu for setting the AIAD parameters. This item is available only when the flow regime modeling is enabled.
define/models/multiphase/flow-regime-modeling/aiad-parameters/critical-vfSpecifies the critical volume fraction of either gas or liquid for calculating the blending factors for the bubbly and droplet flows (
and 
in Equation 14–178 in the Fluent Theory Guide).define/models/multiphase/flow-regime-modeling/aiad-parameters/delta-gradSpecifies the critical gradient fraction for determining the intermediate transition width for the free surface blending factor (
in Equation 14–183 in the Fluent Theory Guide).define/models/multiphase/flow-regime-modeling/aiad-parameters/delta-vfSpecifies the volume fraction width for the intermediate transition (
in Equation 14–178 in the Fluent Theory Guide).define/models/multiphase/flow-regime-modeling/aiad-parameters/ncells-fsSpecifies the cell number across the interface for determining the interfacial width for free surface flow (
in Equation 14–182 in the Fluent Theory Guide).
define/models/multiphase/flow-regime-modeling/enable?Enables/disables the flow regime modeling.
define/models/multiphase/hybrid-models/Enters the menu for selecting the hybrid model.
define/models/multiphase/hybrid-models/ddpm?Enables/disables the dense discrete phase model.
define/models/multiphase/hybrid-models/multi-fluid-vof?Enables/disables the multi-fluid VOF model.
define/models/multiphase/interface-modeling-optionsSpecifies interface modeling options.
define/models/multiphase/mixture-parametersSpecifies mixture parameters.
define/models/multiphase/modelSpecifies multiphase model.
define/models/multiphase/number-of-phasesSpecifies the number of phases.
define/models/multiphase/population-balance/Enters the population balance models menu.
define/models/multiphase/population-balance/expert/Enters the population balance expert menu.
define/models/multiphase/population-balance/expert/qmom/Enter the menu for the quadrature method of moments (QMOM).
define/models/multiphase/population-balance/expert/qmom/retain-qmom-sources-for-low-vof?If enabled, retains the QMOM sources for the low volume fraction of the secondary phase.
define/models/multiphase/population-balance/includeexpansion?Allows you to account for bubble expansion due to large changes in hydrostatic pressure in compressible flows. This option is available with the inhomogeneous discrete method.
define/models/multiphase/population-balance/modelAllows you to select the population balance model and set its parameters.
define/models/multiphase/population-balance/phenomena/Enters the phenomena menu for population balance.
define/models/multiphase/population-balance/phenomena/aggregationSets the aggregation kernel.
define/models/multiphase/population-balance/phenomena/aggregation-factorSpecifies a factor that controls the intensity of the selected aggregation kernel.
define/models/multiphase/population-balance/phenomena/breakageSets the breakage kernel.
define/models/multiphase/population-balance/phenomena/breakage-aggregation-vof-cutoffspecifies a cutoff limit for the volume fraction values for the breakage and aggregation kernels.
define/models/multiphase/population-balance/phenomena/breakage-factorSpecifies a factor that controls the intensity of the selected breakage kernel.
define/models/multiphase/population-balance/phenomena/growthSpecifies the growth rate.
define/models/multiphase/population-balance/phenomena/nucleationSpecifies the nucleation rate.
define/models/multiphase/population-balance/size-calculatorGives you recommendations for appropriate bubble sizes and/or droplet size limits.
define/models/multiphase/regime-transition-modelingenables the Algebraic Interfacial Area Density (AIAD) model and sets the AIAD secondary continuous phase and the secondary entrained phase. Entering
0as a phase ID cancels any previous phase selection. Note that you must define the phases in your simulation using thedefine/phases/text command prior to using theregime-transition-modelingtext command. This option is available only with the Eulerian multiphase model.define/models/multiphase/sub-models/Enters the sub-model menu.
define/models/multiphase/sub-models/boiling?Enables/disables the boiling model.
define/models/multiphase/sub-models/boiling-options/Enters the boiling model options menu.
define/models/multiphase/sub-models/boiling-options/nlbf-modelEnables/disables the non-local boundary field (NLBF) model.
define/models/multiphase/sub-models/boiling-options/optionsAllows you to choose the boiling model option (RPI boiling model, non-equilibrium boiling, or critical heat flux).
define/models/multiphase/vof-sub-modelsEnables the Open Channel sub-model and/or the Open Channel Wave Boundary Condition sub-model.
define/models/multiphase/volume-fraction-parameters/Enters the menu for setting the volume fraction parameters.
define/models/multiphase/volume-fraction-parameters/courant-numberSpecifies the maximum Courant number allowed near the free surface. This item is available with the explicit formulation for the volume fraction.
define/models/multiphase/volume-fraction-parameters/formulationAllows you to choose the volume tracking formulation (implicit or explicit).
define/models/multiphase/volume-fraction-parameters/volume-fraction-cutoffSpecifies a cutoff limit for the volume fraction values. This item is available with the explicit formulation for the volume fraction.
define/models/multiphase/wet-steam/Enters the wet steam model menu.
define/models/multiphase/wet-steam/compile-user-defined-wetsteam-functionsCompiles user-defined wet steam library.
define/models/multiphase/wet-steam/enable?Enables/disables the wet steam model.
define/models/multiphase/wet-steam/load-unload-user-defined-wetsteam-libraryLoads or unloads user-defined wet steam library.
define/models/multiphase/wet-steam/set/Enters the set menu for setting wet steam model options.
define/models/multiphase/wet-steam/set/droplet-growth-rateSets the droplet growth rate to either Young's formulation (default) or Hill's.
define/models/multiphase/wet-steam/set/rgp-tablesSets the RGP (real gas property) table to be used with the Wet Steam model.
define/models/multiphase/wet-steam/set/virial-equationSets the equation of state for steam to either Vukalovich formulation (default) or Young formulation.
define/models/multiphase/wet-steam/set/max-liquid-mass-fractionSets the maximum limit on the condensed liquid-phase mass-fraction to prevent divergence.
define/models/multiphase/wet-steam/set/stagnation-conditionsComputes stagnation conditions using either gas phase only, or mixture. For details, see Computing Stagnation Conditions for the Wet Steam Model in the Fluent Theory Guide.
define/models/multiphase/wet-steam/set/zonal-phase-changeSwitches off the phase change model in specific cell zones.
define/models/noniterative-time-advance?Enables/disables noniterative time advancement scheme.
define/models/nox?Enables/disables the NOx model.
define/models/nox-parameters/Enters the NOx parameters menu.
define/models/nox-parameters/inlet-diffusion?Enables/disables inclusion of diffusion at inlets.
define/models/nox-parameters/nox-chemistrySelects NOx chemistry model.
define/models/nox-parameters/nox-expertSelects additional NOx equations.
define/models/nox-parameters/nox-turbulence-interactionSets NOx turbulence interaction model.
define/models/potential-and-li-ion-battery?Contains options to enable/disable potential models (electric potential, li-ion battery model, and electrolysis and H2 pump model) and include Joule heating in the energy equation.
define/models/radiation/Enters the radiation models menu.
define/models/radiation/apply-full-solar-irradiation?Enables/disables the application of the complete solar load to the first wavelength band only, reverting to the pre-2019 R1 behavior of the Solar Load and Discrete Ordinates models.
define/models/radiation/blending-factorSets numeric option for Discrete Ordinate model. Make sure thatSecond Order Upwind is selected for the Discrete Ordinates spatial discretization for the
blending-factoroption to appear in the text command list.define/models/radiation/discrete-ordinates?Enables/disables discrete ordinates radiation model.
define/models/radiation/discrete-transfer?Enables/disables discrete transfer radiation model.
define/models/radiation/do-acceleration?Enables/disables the acceleration of the discrete ordinates (DO) radiation model calculations. The acceleration is provided by NVIDIA GPGPUs in offload mode or the CPU cores.
define/models/radiation/do-coupling?Enables/disables DO/energy coupling.
define/models/radiation/solar-irradiation?Enables/disables the solar irradiation model.
define/models/radiation/dtrm-parameters/Enters the dtrm parameters menu.
define/models/radiation/dtrm-parameters/check-ray-fileReads DTRM rays file.
define/models/radiation/dtrm-parameters/controlsSets dtrm solution controls.
define/models/radiation/dtrm-parameters/make-globsMakes globs (coarser mesh) for radiation.
define/models/radiation/dtrm-parameters/ray-traceCreates DTRM rays for radiation.
define/models/radiation/fast-second-order-discrete-ordinate?Enables/disables the fast-second-order option for Discrete Ordinate Model.
define/models/radiation/mc-model-parametersSpecifies Monte Carlo model parameters. This text command is available only when the Monte Carlo model is enabled.
define/models/radiation/mc-under-relaxationSets the under-relaxation factor for Monte Carlo radiation sources used in the energy equation.
define/models/radiation/method-partially-specular-wallSets the method for partially specular wall with discrete ordinate model.
define/models/radiation/montecarlo?Enables/disables the Monte Carlo radiation model.
define/models/radiation/non-gray-model-parametersSets parameters for non-gray model.
define/models/radiation/p1?Enables/disables P1 radiation model.
define/models/radiation/radiation-iteration-parametersSets iteration parameters for radiation models.
define/models/radiation/radiation-model-parametersSets parameters for radiation models.
define/models/radiation/rosseland?Enables/disables Rosseland radiation model.
define/models/radiation/s2s?Enables/disables S2S radiation model.
define/models/radiation/s2s-parameters/Enters the S2S parameters menu.
define/models/radiation/s2s-parameters/compute-clusters-and-vf-acceleratedEnables/disables the accelerated computation/writing/reading of a file with the surface cluster information and view factors for the surface to surface (S2S) radiation model, using MPI/OpenMP/OpenCL models and/or GPGPUs in offload mode. Note that this text command is not available with the hemicube method if the face to face basis is selected.
define/models/radiation/s2s-parameters/compute-fpsc-valuesComputes only fpsc values based on current settings
define/models/radiation/s2s-parameters/compute-vf-onlyComputes/writes view factors only.
define/models/radiation/s2s-parameters/compute-write-vfComputes/writes surface clusters and view factors for S2S radiation model.
define/models/radiation/s2s-parameters/enable-mesh-interface-clustering?enables surface clusters on mesh interfaces.
define/models/radiation/s2s-parameters/non-participating-boundary-zones-temperatureSets temperature for the non-participating boundary zones.
define/models/radiation/s2s-parameters/print-thread-clustersPrints the following for all boundary threads: thread-id, number of faces, faces per surface cluster, and the number of surface clusters.
define/models/radiation/s2s-parameters/print-zonewise-radiationPrints the zonewise incoming radiation, viewfactors, and average temperature.
define/models/radiation/s2s-parameters/read-vf-fileReads S2S file.
define/models/radiation/s2s-parameters/set-global-faces-per-surface-clusterSets global value of faces per surface cluster for all boundary zones.
define/models/radiation/s2s-parameters/set-vf-parametersSets the parameters needed for the viewfactor calculations.
define/models/radiation/s2s-parameters/split-angleSets split angle for the clustering algorithm.
define/models/radiation/s2s-parameters/use-new-cluster-algorithmUses the new surface clustering algorithm.
define/models/radiation/s2s-parameters/use-old-cluster-algorithmUses the old surface clustering algorithm.
define/models/radiation/solar?Enables/disables solar model.
define/models/radiation/solar-calculatorCalculates sun direction and intensity.
define/models/radiation/solar-parameters/Enters the solar parameters menu.
define/models/radiation/solar-parameters/autoread-solar-dataSets autoread solar data parameters.
define/models/radiation/solar-parameters/autosave-solar-dataSets autosave solar data parameters. Note this command is only available on Linux in serial mode -t0.
define/models/radiation/solar-parameters/ground-reflectivitySets ground reflectivity parameters.
define/models/radiation/solar-parameters/illumination-parametersSets illumination parameters.
define/models/radiation/solar-parameters/iteration-parametersSets update parameters.
define/models/radiation/solar-parameters/quad-tree-parametersSets quad-tree refinement parameters.
define/models/radiation/solar-parameters/scattering-fractionSets scattering fraction parameters.
define/models/radiation/solar-parameters/solar-thread-controlSets 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 andSolar Ray Tracing is enabled.
define/models/radiation/solar-parameters/sol-adjacent-fluidcellsSets solar load on for adjacent fluid cells.
define/models/radiation/solar-parameters/sol-camera-posSets camera position based on sun direction vector.
define/models/radiation/solar-parameters/sol-on-demandSets solar load on demand.
define/models/radiation/solar-parameters/sun-direction-vectorSets sun direction vector.
define/models/radiation/solar-parameters/use-direction-from-sol-calcSets direction computed from solar calculator.
define/models/radiation/solution-method-for-do-couplingEnables/disables the solution method for DO/energy coupling.
define/models/radiation/target-cells-per-volume-clusterSets the amount of coarsening of the radiation mesh for the Monte Carlo radiation model. A number greater than one implies coarsening, whereas equal to one implies no coarsening.
define/models/radiation/wsggm-cell-basedEnables/disables WSGGM cell based method. Note that when enabled, the wsggm-cell-based option will become available in theAbsorption Coefficient drop-down list in the Create/Edit Materials dialog box.
define/models/shell-conduction/Enters the shell conduction models menu.
define/models/shell-conduction/enhanced-encapsulation?Enables/disables 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.
define/models/shell-conduction/multi-layer-shell?Enables/disables 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.
define/models/shell-conduction/read-csvDefines the shell conduction settings by reading a CSV file.
define/models/shell-conduction/save-shell-zones?Enables the saving of shell zones to case files.
define/models/shell-conduction/settingsEnables shell conduction and defines the settings for any wall or group of walls by manually entering the number and properties of the layers.
define/models/shell-conduction/write-csvWrites your saved shell conduction settings to a CSV file.
define/models/solidification-melting?Enables/disables the solidification and melting model.
define/models/solver/Enters the menu to select the solver.
define/models/solver/density-based-explicitEnables/disables the density-based-explicit solver.
define/models/solver/density-based-implicitEnables/disables the density-based-implicit solver.
define/models/solver/pressure-basedEnables/disables the pressure-based solver.
define/models/soot?Enables/disables the soot model.
define/models/soot-parameters/Enters the soot parameters menu.
define/models/soot-parameters/inlet-diffusion?Enables/disables inclusion of diffusion at inlets.
define/models/soot-parameters/modify-schmidt-number?Changes the turbulent Schmidt number for soot/nuclei equations.
define/models/soot-parameters/soot-model-parametersSelects soot model parameters.
define/models/soot-parameters/soot-process-parametersSelects soot process parameters.
define/models/soot-parameters/soot-radiation-interactionEnables/disables the soot-radiation interaction model.
define/models/soot-parameters/soot-turbulence-interactionSets soot-turbulence interaction model.
define/models/species/Enters the species models menu.
define/models/species/CHEMKIN-CFD?Enables/disables the Ansys CHEMKIN-CFD solver.
define/models/species/CHEMKIN-CFD-parameters/Enters the expert CHEMKIN-CFD parameters menu.
define/models/species/CHEMKIN-CFD-parameters/add-cell-monitorMonitors cell for debug output.
define/models/species/CHEMKIN-CFD-parameters/advanced-optionsSets advanced parameter options.
define/models/species/CHEMKIN-CFD-parameters/basic-optionsSets basic parameter options.
define/models/species/CHEMKIN-CFD-parameters/delete-cell-monitorsDeletes cell monitors.
define/models/species/CHEMKIN-CFD-parameters/list-cell-monitorsLists cell monitors.
define/models/species/clear-isat-tableClears ISAT table.
define/models/species/coal-calculatorSets up coal modeling inputs.
define/models/species/combustion-expertEnables import of the CHEMKIN mechanism transport data. When this option is enabled, you will be prompted for importing CHEMKIN transport property database when setting your combustion case.
define/models/species/combustion-numericsApplies optimal solver settings automatically to provide a faster solution time. This command is available only for transient non-premixed and partially premixed combustion models.
define/models/species/decoupled-detailed-chemistry?Enables/disables the Decoupled Detailed Chemistry model.
define/models/species/diffusion-energy-source?Enables/disables diffusion energy source.
define/models/species/electro-chemical-surface-reactions?Enables/disables electrochemical surface reactions.
define/models/species/epdf-energy?Enables/disables EPDF energy option.
define/models/species/flamelet-expertSets flamelet expert parameters.
define/models/species/full-tabulation?Enables/disables building of a full 2-mixture fraction table
define/models/species/heat-of-surface-reactions?Enables/disables heat of surface reactions.
define/models/species/ignition-model?Enables/disables the ignition model.
define/models/species/ignition-model-controlsSets ignition model parameters.
define/models/species/import-flamelet-for-restartImports Flamelet File for Restart.
define/models/species/inert-transport-controlsSets inert transport model parameters.
define/models/species/inert-transport-model?Enables/disables the inert transport model.
define/models/species/inlet-diffusion?Enables/disables inclusion of diffusion at inlets.
define/models/species/integration-parametersSets chemistry ODE integrator parameters. Enables/disables stiff chemistry acceleration methods and set their parameters.
define/models/species/init-unsteady-flamelet-probInitializes Unsteady Flamelet Probability.
define/models/species/liquid-micro-mixing?Enables/disables liquid micro mixing.
define/models/species/mass-deposition-source?Enables/disables mass deposition source due to surface reactions.
define/models/species/mixing-modelSets PDF Transport mixing model.
define/models/species/multicomponent-diffusion?Enables/disables multicomponent diffusion.
define/models/species/non-premixed-combustion?Enables/disables non-premixed combustion model.
define/models/species/non-premixed-combustion-expertSets PDF expert parameters.
define/models/species/non-premixed-combustion-parametersSets PDF parameters.
define/models/species/off?Enables/disables solution of species models.
define/models/species/partially-premixed-combustion?Enables/disables partially premixed combustion model.
define/models/species/partially-premixed-combustion-expertSets PDF expert parameters.
define/models/species/partially-premixed-combustion-gridsSets values for the grid distribution for PDF table or flamelet parameter. This text command is available only for partially premixed combustion cases with FGM.
define/models/species/partially-premixed-combustion-parametersSets PDF parameters.
define/models/species/partially-premixed-propertiesSets/changes partially-premixed mixture properties. This command is only available when
partially-premixed-combustion?is enabled.define/models/species/particle-reactions?Enables/disables particle reactions.
define/models/species/pdf-transport?Enables/disables the composition PDF transport combustion model.
define/models/species/pdf-transport-expert?Enables/disables PDF Transport expert user.
define/models/species/premixed-modelSets premixed combustion model.
define/models/species/premixed-combustion?Enables/disables premixed combustion model.
define/models/species/re-cacl-par-premix-propsRe-calculates partially-premixed properties. This command is only available when
partially-premixed-combustion?is enabled.define/models/species/reaction-diffusion-balance?Enables/disables reaction diffusion balance at reacting surface for surface reactions.
define/models/species/reacting-channel-model?Enables/disables the Reacting Channel Model.
define/models/species/reacting-channel-model-optionsSets Reacting Channel Model parameters.
define/models/species/reactor-network-model?Enables/disables the Reactor Network Model.
define/models/species/relax-to-equil?Enables/disables the Relaxation to Chemical Equilibrium model.
define/models/species/save-gradients?Enables/disables storage of species mass fraction gradients.
define/models/species/set-premixed-combustionSets premixed combustion parameters.
define/models/species/set-turb-chem-interactionSets EDC model constants.
define/models/species/spark-modelSwitches between the R15 and R14.5 spark models and sets spark model parameters.
define/models/species/species-migration?Includes species migration in electric field. This command is available only when the electrochemical surface reactions are enabled.
define/models/species/species-transport-expert/Sets the convergence acceleration expert parameters. This command is only available when the species transport model is enabled.
define/models/species/species-transport-expert/useconvergence acceleration method?Answering
yesat the prompt, uses a combination of different convergence acceleration techniques. If you enterno(default), additional options will be displayed in the console.define/models/species/species-transport-expert/Usespecies clipping?Enables/disables the explicit clipping of species between 0 and 1.
define/models/species/species-transport-expert/Linearize higher order convection sources?Enables/disables linearization of higher order convection sources.
define/models/species/species-transport-expert/Linearizesecondary diffusion sources?Enables/disables linearization of species secondary diffusion sources.
define/models/species/species-transport-expert/Enable mesh quality based first-second order species blending?Enables/disables skewness-based blending of first and second order convection.
define/models/species/species-transport-expert/Minimum cell quality threshold for blendingSpecifies the minimum cell orthogonal quality for blending.
define/models/species/species-transport?Enables/disables the species transport model.
define/models/species/stiff-chemistry?Enables/disables stiff chemistry option.
define/models/species/surf-reaction-aggressiveness-factor?Sets the surface reaction aggressiveness factor.
define/models/species/surf-reaction-netm-paramsSets the surface reaction parameters for the Non-Equilibrium Thermal Model.
define/models/species/thermal-diffusion?Enables/disables thermal diffusion.
define/models/species/thickened-flame-model?Enables/disables the Relaxation to Chemical Equilibrium model
define/models/species/volumetric-reactions?Enables/disables volumetric reactions.
define/models/species/wall-surface-reactions?Enables/disables wall surface reactions.
define/models/species/water-corrosion-preSets up and computes water chemistry and creates a corrosion material. This item is available only for the Species Transport model with electrochemical reactions.
define/models/steady?Enables/disables the steady solution model.
define/models/structure/Enters the structure model menu.
define/models/structure/controlsEnters the structure controls menu.
define/models/structure/controls/amg-stabilizationSets the algebraic multigrid (AMG) stabilization method for the structural model calculations.
define/models/structure/controls/max-iterSets the maximum number of iterations for the structural model calculations.
define/models/structure/controls/numerical-damping-factor?Sets the damping factor for the structural model (that is, the amplitude decay factor
in Equation 16–16 in the Theory Guide).
define/models/structure/expert/Enters the structure expert menu.
define/models/structure/expert/explicit-fsi-force?Enables/disables an explicit fluid-structure interaction force.
define/models/structure/expert/include-pop-in-fsi-force?Enables/disables the inclusion of operating pressure into the fluid-structure interaction force.
define/models/structure/expert/include-viscous-fsi-force?Enables/disables the inclusion of a viscous fluid-structure interaction force.
define/models/structure/expert/starting-t-re-initialization?Re-assigns the starting temperature as a temperature field from a previous calculation, then re-initializes the new starting temperature field.
define/models/structure/linear-elasticity?Enables the linear elasticity model.
define/models/structure/structure-off?Disables the structural model.
define/models/swirl?Enables/disables axisymmetric swirl velocity.
define/models/system-coupling-settings/Enters the system coupling menu.
define/models/system-coupling-settings/user-defined-coupling-variables-via-udmEnables a previously defined UDM to be specified as a data transfer variable for use in System Coupling.
define/models/system-coupling-settings/use-face-or-element-based-data-transfer?Answering
yesat the prompt enables Fluent to use element data for mapping surface conservative quantities such as surface forces and heat flows.
define/models/two-temperatureEnters the Two-Temperature model menu.
define/models/two-temperature/enable?Enables/disables the Two-Temperature model.
define/models/two-temperature/robustness-enhancement?Enables/disables the robustness enhancement, which is on by default.
define/models/two-temperature/set-verbosity?Specifies the level of detail printed in the console about the Two-Temperature model. For a verbosity of one, Fluent will print the number of cells that reach the temperature limit, have an excessive temperature change, or get a negative temperature.
define/models/two-temperature/translational-vibrational-energy-relaxationEnters the two-temperature translational-vibrational energy relaxation model menu.
define/models/two-temperature/translational-vibrational-energy-relaxation/modelSpecifies the model for translational-vibrational energy relaxation. The available options are Millikan-White or Park, with Park set as the default option.
define/models/two-temperature/translational-vibrational-energy-relaxation/expertEnters the expert menu for Park’s model.
define/models/two-temperature/translational-vibrational-energy-relaxation/expert/number-of-objectsSpecifies the number of collisions for Park’s model.
define/models/two-temperature/translational-vibrational-energy-relaxation/expert/list-allLists the vibrational constants for all collisions.
define/models/two-temperature/translational-vibrational-energy-relaxation/expert/list-propertiesLists the vibrational constants for the specified collision.
define/models/two-temperature/translational-vibrational-energy-relaxation/expert/editEdits the vibrational constants for the specified collision.
define/models/two-temperature/translational-vibrational-energy-relaxation/expert/deleteDeletes the vibrational constants for the specified collision.
define/models/unsteady-1st-order?Selects the first-order implicit formulation for transient simulations.
define/models/unsteady-2nd-order-bounded?Selects the bounded second-order implicit formulation for transient simulations.
define/models/unsteady-2nd-order?Selects the second-order implicit formulation for transient simulations.
define/models/unsteady-global-time?Selects the explicit transient formulation. This text command is only available for unsteady cases that use the density-based solver with the explicit formulation.
define/models/unsteady-structure-euler?Selects the backward Euler method for the direct time integration of the finite element semi-discrete equation of motion. This text command is only available for transient simulations that use the structural model.
define/models/unsteady-structure-newmark?Selects the Newmark method for the direct time integration of the finite element semi-discrete equation of motion. This text command is only available for transient simulations that use the structural model.
define/models/virtual-blade-modelEnters the VBM menu.
define/models/virtual-blade-model/enable?Enable/disable VBM.
define/models/virtual-blade-model/modeSelects VBM / mode.
define/models/virtual-blade-model/applyReads and applys VBM setting.
define/models/virtual-blade-model/rotorEnters the main menu to define a rotor disk.
define/models/virtual-blade-model/rotor/newCreates a new rotor object. You are prompted to provide the name of the rotor object that you wish to create. All properties of the rotor object are set using default values and you can change them using the
editcommand later.
define/models/virtual-blade-model/rotor/deleteDeletes a rotor object. You are prompted to provide the name of the existing rotor that you wish to delete.
define/models/virtual-blade-model/rotor/duplicateCreates a copy of a specified rotor object. You are prompted to provide the name of the existing rotor that you wish to copy.
define/models/virtual-blade-model/rotor/renameRenames an existing rotor object. You are prompted to provide the name of the existing rotor that you wish to rename.
define/models/virtual-blade-model/rotor/listPrints the names of the existing rotor objects to the console.
define/models/virtual-blade-model/rotor/list-propertiesPrints the properties of a rotor object to the console. You are prompted to provide the name of the existing rotor that you wish to see its properties.
define/models/virtual-blade-model/rotor/editEdits an existing rotor object. You are prompted to provide the name of the existing rotor that you wish to edit.
Note: You have three subgroups to set up when editing a rotor object:
General
Geometry
Trimming
When you set up any subgroup properties of each rotor object using journal file, add a space between
editandobject-nameand another space betweenobject-nameand subgroup setup. In this case, RotorName represents the rotor object name that you wish to edit.define/models/virtual-blade-model/rotor/edit “RotorName” generalEnters the menu to define the rotor's general information.
define/models/virtual-blade-model/rotor/edit “RotorName” general/basic-info/Enters the menu to define the rotor's basic information.
define/models/virtual-blade-model/rotor/edit “RotorName” general/basic-info/Enters the menu to define the
basic-infosubmenu under thegeneralsubmenu.define/models/virtual-blade-model/rotor/edit “RotorName” general/basic-info/number-of-bladesSets the number of blades.
define/models/virtual-blade-model/rotor/edit “RotorName” general/basic-info/rotor-speedSets rotor speed.
define/models/virtual-blade-model/rotor/edit “RotorName” general/basic-info/tip-radiusSets rotor blade’s tip radius.
define/models/virtual-blade-model/rotor/edit “RotorName” general/basic-info/root-radiusSets rotor blade’s root radius.
define/models/virtual-blade-model/rotor/edit “RotorName” general/blade-flap-angles/Enters the menu to define the rotor flapping angles.
define/models/virtual-blade-model/rotor/edit “RotorName” general/blade-flap-angles/blade-flapping-coneSet the blade’s cone angle.
define/models/virtual-blade-model/rotor/edit “RotorName” general/blade-flap-angles/blade-flapping-cyclic-cosSets the cosine of the blade's cyclic flapping angle.
define/models/virtual-blade-model/rotor/edit “RotorName” general/blade-flap-angles/blade-flapping-cyclic-sinSets the sine of the blade's cyclic flapping angle.
define/models/virtual-blade-model/rotor/edit “RotorName” general/blade-pitch-angles/Enters the menu to define the rotor pitch angles.
define/models/virtual-blade-model/rotor/edit “RotorName” general/blade-flap-angles/blade-pitch-collectiveSets blade’s collective pitch angle.
define/models/virtual-blade-model/rotor/edit “RotorName” general/blade-flap-angles/blade-pitch-cyclic-cosSets the cosine of the blade's cyclic pitch angle.
define/models/virtual-blade-mode/rotor/edit “RotorName” general/blade-flap-angles/blade-pitch-cyclic-sinSets the sine component of the blade's cyclic pitch angle.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-idEnters the menu to define the disk face/surface name.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-id/embedded-face-zoneSets embedded face zone. This command is available when Embedded Disk mode is enabled.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-id/create-floating-diskCreates a floating disk. This command is available when Floating Disk mode is enabled.
Note: Note that disk-origin and blade’s tip and root radius should be set up in advance.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-id/floating-surface-nameSets the floating disk name. This command is available when Floating Disk mode is enabled.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-orientation/Enters the menu to define the rotor disk orientation.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-orientation/terminologySelects the terminology to define rotor disk orientation. Enter
0if using Rotor Disk Angles. Enter1if using .
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-orientation/disk-pitch-angleSets the pitch angle of the rotor disk.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-orientation/disk-bank-angleSets the bank angle of the rotor disk.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-orientation/disk-normal-xSets the x-component of the rotor disk normal vector.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-orientation/disk-normal-ySets the y-component of the rotor disk normal vector.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-orientation/disk-normal-zSets the z-component of the rotor disk normal vector.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-originEnters the menu to define coordinates of the rotor disk center if using mode, and rotor zone center if using mode.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-origin/disk-origin-xSets the x-coordinate of the disk origin.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-origin/disk-origin-ySets the y-coordinate of the disk origin.
define/models/virtual-blade-model/rotor/edit “RotorName” general/disk-origin/disk-origin-zSets the z-coordinate of the disk origin.
define/models/virtual-blade-model/rotor/edit “RotorName” general/tip-lossEnters the menu to define the tip loss model.
define/models/virtual-blade-model/rotor/edit “RotorName” general/tip-loss/model-tip-lossSelects the Tip Loss Function model. Enter
1if using model, and enter2if using the modified model.
define/models/virtual-blade-model/rotor/edit “RotorName” general/tip-loss/tip-loss-limitSets Tip Loss Limit (%R) if using tip loss model.
define/models/virtual-blade-model/rotor/edit “RotorName” general/tip-loss/prandtl-tuning-coefficientSets the tuning coefficient if using modified Prandtl Tip Loss Function model. Select a number equal to or larger than
1.
define/models/virtual-blade-model/rotor/edit “RotorName” geometryEnters the menu to set up rotor blade geometry by defining blade sections along its span. A blade section is a named-object and you can create/rename/delete/duplicate/edit it in this menu.
define/models/virtual-blade-model/rotor/edit “RotorName” geometry/newCreates a new section object. You are prompted to provide the name of the section object that you wish to create. All properties of the section object are set using default values and you can change them using edit command after.
define/models/virtual-blade-model/rotor/edit “RotorName” geometry/deleteDeletes a section object. You are prompted to provide the name of the existing section that you wish to delete.
define/models/virtual-blade-model/rotor/edit “RotorName” geometry/duplicateCreates a copy of a specified section object. You are prompted to provide the name of the existing section that you wish to copy.
define/models/virtual-blade-model/rotor/edit “RotorName” geometry/renameRenames an existing section object. You are prompted to provide the name of the existing section that you wish to rename.
define/models/virtual-blade-model/rotor/edit “RotorName” geometry/listPrints the names of the existing sections to the console.
define/models/virtual-blade-model/rotor/edit “RotorName” geometry/list-propertiesPrints the properties of a section object to the console. You are prompted to provide the name of the existing section that you wish to see its properties.
define/models/virtual-blade-model/rotor/edit “RotorName” geometry/editEdits an existing section object. You are prompted to provide the name of the existing section that you wish to edit.
Note: When you set up any properties of each section object using journal file, you should put a space between
editandobject-nameand another space betweenobject-nameandproperty name. The followingSecNamerepresents the section object name that you wish to edit.
define/models/virtual-blade-model/rotor/edit “RotorName” geometry/edit “SecName” radius-ratioSets the section's radius (distance between the center of rotor and the location of the current section) as a fraction of blade tip radius (r/R).
define/models/virtual-blade-model/rotor/edit “RotorName” geometry/edit “SecName” chordSets the section’s chord length.
define/models/virtual-blade-model/rotor/edit “RotorName” geometry/edit “SecName” airfoil-data-fileSets the name of the section’s airfoil-data-file.
define/models/virtual-blade-model/rotor/edit “RotorName” geometry/edit “SecName” twistSets the section’s twist angle.
Note: The blade twist adds to the collective pitch to define the pitch angle at the current section. Therefore, the twist should be set based on the same reference point that the collective pitch angle is defined. For more information, see Blade Pitch in the Fluent User's Guide.
define/models/virtual-blade-model/rotor/edit “RotorName” trimmingEnters the menu to set up rotor trimming setup.
define/models/virtual-blade-model/rotor/edit “RotorName” trimming/trim-optionSelects Trimming option. You are prompted to provide a number that define rotor trim option.
define/models/virtual-blade-model/rotor/edit “RotorName” trimming/damping-factorSets trimming damping factor.
define/models/virtual-blade-model/rotor/edit “RotorName” trimming/update-frequencySets trimming update frequency.
define/models/virtual-blade-model/rotor/edit “RotorName” trimming/thrust-coefSets desired thrust coefficient of the rotor.
define/models/virtual-blade-model/rotor/edit “RotorName” trimming/roll-moment-coefSets desired roll moment coefficient of the rotor.
define/models/virtual-blade-model/rotor/edit “RotorName” trimming/pitch-moment-coefSets desired pitch moment coefficient of the rotor.
define/models/viscous/Enters the Viscous model menu.
define/models/viscous/add-transition-modelSets Transition model to account for transitional effects. The default is
none, however you can selectgamma-algebraicorgamma-transport-eqn.After a transition model has been enabled, you have additional options in the submenu
transition-model-options.define/models/viscous/corner-flow-correction-ccornerSets the strength of the quadratic term of the corner flow correction. The default value is 1. This is available after the
corner-flow-correction?option is enabled.define/models/viscous/corner-flow-correction?Enables/disables the corner flow correction.
define/models/viscous/curvature-correction-ccurvSets the strength of the curvature correction term. The default value is 1. This is available after the
curvature-correction?option is enabled.define/models/viscous/curvature-correction?Enables/disables the curvature correction.
define/models/viscous/des-limiter-optionSelects the DES limiter option (none, F1, F2, Delayed DES, or Improved Delayed DES).
define/models/viscous/geko-options/Enters the GEKO model menu..
define/models/viscous/geko-options/csepSets
csep, the parameter to optimize flow separation from smooth surfaces.define/models/viscous/geko-options/cnwSets
cnw, the parameter to optimize flow in non-equilibrium near wall regions.define/models/viscous/geko-options/cmixSets
cmix, the parameter to optimize strength of mixing in free shear flows.define/models/viscous/geko-options/cjetSets
cjet, the parameter to optimize free shear layer mixing (optimize free jets independent of mixing layer).define/models/viscous/geko-options/blending-functionSets the blending function, which deactivates
cmixandcjetinside boundary layers.define/models/viscous/geko-options/crealSets
creal, a realizability limiter that ensures positive normal stresses in the entire domain.define/models/viscous/geko-options/cnw_subSets
cnw_sub, which allows the adjustment of log-layer and cf.define/models/viscous/geko-options/cjet_auxSets
cjet_aux, which allows fine-tuning of the parameter to optimize free jets.define/models/viscous/geko-options/cbf_turSets
cbf_tur, a factor for the main blending factor, controlling the thickness of the layer near walls.define/models/viscous/geko-options/cbf_lamSets
cbf_lam, a part of the blending function and shields the laminar boundary layer.define/models/viscous/geko-options/geko-defaultsRestores the defaults of all GEKO parameters.
define/models/viscous/geko-options/wall-distance-free?Enables/disables the wall distance free version of the GEKO model.
define/models/viscous/detached-eddy-simulation?Enables/disables detached eddy simulation.
define/models/viscous/inviscid?Enables/disables inviscid flow model.
define/models/viscous/ke-easm?Enables/disables the EASM
-
turbulence model.define/models/viscous/ke-realizable?Enables/disables the realizable
-
turbulence model.define/models/viscous/ke-rng?Enables/disables the RNG
-
turbulence model.define/models/viscous/ke-standard?Enables/disables the standard
-
turbulence model.define/models/viscous/k-kl-w?Enables/disables the k-kl-
turbulence model.define/models/viscous/kw-easm?Enables/disables the EASM
-
turbulence model.define/models/viscous/kw-low-re-correction?Enables/disables the
-
low Re option.define/models/viscous/kw-shear-correction?Enables/disables the
-
shear-flow correction option. This
text command is only available for the standard
-
model and the stress-omega RSM
model.define/models/viscous/kw-bsl?Enables/disables the baseline (BSL)
-
turbulence model.define/models/viscous/kw-geko?Enables/disables the generalized
- (GEKO) turbulence model.define/models/viscous/kw-sst?Enables/disables the SST
-
turbulence model.define/models/viscous/kw-standard?Enables/disables the standard
-
turbulence model.define/models/viscous/kw-wj-bsl-earsm?Enables/disables the WJ-BSL-EARSM
- turbulence model.define/models/viscous/laminar?Enables/disables laminar flow model.
define/models/viscous/large-eddy-simulation?Enables/disables large eddy simulation.
define/models/viscous/les-dynamic-energy-flux?Enables/disables the dynamic sub-grid scale turbulent Prandtl Number.
define/models/viscous/les-dynamic-scalar-flux?Enables/disables the dynamic sub-grid scale turbulent Schmidt Number.
define/models/viscous/les-subgrid-dynamic-fvar?Enables/disables the dynamic subgrid-scale mixture fraction variance model.
define/models/viscous/les-subgrid-smagorinsky?Enables/disables the Smagorinsky-Lilly subgrid-scale model.
define/models/viscous/les-subgrid-tke?Enables/disables kinetic energy transport subgrid-scale model.
define/models/viscous/les-subgrid-wale?Enables/disables WALE subgrid-scale model.
define/models/viscous/les-subgrid-wmles-s_minus_omega?Enables/disables the WMLES
-
subgrid-scale model.define/models/viscous/les-subgrid-wmles?Enables/disables the WMLES subgrid-scale model.
define/models/viscous/low-pressure-boundary-slip?Enables/disables the slip boundary formulation for low-pressure gas systems.
define/models/viscous/mixing-length?Enables/disables mixing-length (algebraic) turbulence model.
define/models/viscous/multiphase-turbulence/Enters the multiphase turbulence menu.
define/models/viscous/multiphase-turbulence/multiphase-optionsEnables/disables multiphase options.
define/models/viscous/multiphase-turbulence/rsm-multiphase-modelsSelects Reynolds Stress multiphase model.
define/models/viscous/multiphase-turbulence/turbulence-multiphase-modelsSelects
-
multiphase model.
define/models/viscous/near-wall-treatment/Enters the near wall treatment menu.
define/models/viscous/near-wall-treatment/enhanced-wall-treatment?Enables/disables enhanced wall functions.
define/models/viscous/near-wall-treatment/harmonic-blend-rplus-wf?Enables/disables harmonic blended wall functions based on r+.
define/models/viscous/near-wall-treatment/menter-lechner?Enables/disables the Menter-Lechner near-wall treatment.
define/models/viscous/near-wall-treatment/non-equilibrium-wall-fn?Enables/disables non-equilibrium wall functions.
define/models/viscous/near-wall-treatment/scalable-wall-functions?Enables/disables scalable wall functions.
define/models/viscous/near-wall-treatment/standard-wall-fn?Enables/disables standard wall functions.
define/models/viscous/near-wall-treatment/user-defined-wall-functions?Enables/disables user-defined wall functions.
define/models/viscous/near-wall-treatment/wall-omega-treatmentSets the wall omega treatment.
define/models/viscous/near-wall-treatment/werner-wengle-wall-fn?Enables/disables Werner-Wengle wall functions.
define/models/viscous/near-wall-treatment/wf-pressure-gradient-effects?Enables/disables wall function pressure- gradient effects.
define/models/viscous/near-wall-treatment/wf-thermal-effects?Enables/disables wall function thermal effects.
define/models/viscous/reynolds-stress-model?Enables/disables the Reynolds-stress turbulence model.
define/models/viscous/rng-differential-visc?Enables/disables the differential-viscosity model.
define/models/viscous/rng-swirl-model?Enables/disables swirl corrections for rng-model.
define/models/viscous/rsm-bsl-based?Enables/disables the stress-BSL Reynolds stress model.
define/models/viscous/rsm-linear-pressure-strain?Enables/disables the linear pressure-strain model in RSM.
define/models/viscous/rsm-omega-based?Enables/disables the stress-omega Reynolds stress model.
define/models/viscous/rsm-or-earsm-geko-option?Enables/disables the RSM version of the GEKO model.
define/models/viscous/rsm-solve-tke?Enables/disables the solution of T.K.E. in RSM model.
define/models/viscous/rsm-ssg-pressure-strain?Enables/disables quadratic pressure-strain model in RSM.
define/models/viscous/rsm-wall-echo?Enables/disables wall-echo effects in RSM model.
define/models/viscous/sa-alternate-prod?Enables/disables strain/vorticity production in Spalart-Allmaras model.
define/models/viscous/sa-damping?Enables/disables full low-Reynolds number form of Spalart-Allmaras model.
Note: This option is only available if your response was
notosa-enhanced-wall-treatment?.define/models/viscous/sa-enhanced-wall-treatment?Enables/disables 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.
define/models/viscous/sas?Enables/disables Scale-Adaptive Simulation (SAS) in combination with the SST
-
turbulence model.define/models/viscous/spalart-allmaras?Enables/disables Spalart-Allmaras turbulence model.
define/models/viscous/transition-model-options/Enters the transition model options menu.
define/models/viscous/transition-model-options/capg-hightuSets the algebraic transition model coefficient CAPG_HIGHTU.
define/models/viscous/transition-model-options/capg-lowtuSets the algebraic transition model coefficient CAPG_LOWTU.
define/models/viscous/transition-model-options/cbubble-c1Sets the algebraic transition model coefficient CBUBBLE_C1.
define/models/viscous/transition-model-options/cbubble-c2Sets the algebraic transition model coefficient CBUBBLE_C2.
define/models/viscous/transition-model-options/cfpg-hightuSets the algebraic transition model coefficient CFPG_HIGHTU.
define/models/viscous/transition-model-options/cfpg-lowtuSets the algebraic transition model coefficient CFPG_LOWTU.
define/models/viscous/transition-model-options/clambda-scaleSets the algebraic transition model coefficient CLAMBDA_SCALE.
define/models/viscous/transition-model-options/critical-reynolds-number-correlationSets the critical Reynolds number correlation.
define/models/viscous/transition-model-options/ctu-hightuSets the algebraic transition model coefficient CTU_HIGHTU.
define/models/viscous/transition-model-options/ctu-lowtuSets the algebraic transition model coefficient CTU_LOWTU.
define/models/viscous/transition-model-options/rec-c1Sets the algebraic transition model coefficient REC_C1.
define/models/viscous/transition-model-options/rec-c2Sets the algebraic transition model coefficient REC_C2.
define/models/viscous/transition-model-options/rec-maxSets the algebraic transition model coefficient REC_MAX.
define/models/viscous/transition-model-options/rv1-switchSets the algebraic transition model coefficient RV1_SWITCH.
define/models/viscous/transition-model-options/crossflow-transition?Enables/disables the effects of crossflow instability.
define/models/viscous/transition-sst?Enables/disables the transition SST turbulence model.
define/models/viscous/trans-sst-roughness-correlation?Enables/disables the Transition-SST roughness correlation option.
define/models/viscous/turb-buoyancy-effects?Enables/disables effects of buoyancy on turbulence.
define/models/viscous/turb-compressibility?Enables/disables the compressibility correction option.
define/models/viscous/turbulence-expert/Enters the turbulence expert menu.
define/models/viscous/turbulence-expert/kato-launder-model?Enables/disables Kato-Launder modification.
define/models/viscous/turbulence-expert/kw-add-des?Enables/disables 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.define/models/viscous/turbulence-expert/kw-add-sas?Enables/disables Scale-Adaptive Simulation (SAS) in combination with the currently selected
-based URANS turbulence model.
This text command is only available for transient
cases.define/models/viscous/turbulence-expert/kw-vorticity-based-production?Enables/disables vorticity-based production.
define/models/viscous/turbulence-expert/low-re-ke?Enables/disables the low-Re
-
turbulence model.define/models/viscous/turbulence-expert/low-re-ke-indexSpecifies 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.
define/models/viscous/turbulence-expert/production-limiter?Enables/disables Production Limiter modification.
define/models/viscous/turbulence-expert/non-newtonian-modification?Enables/disables non-Newtonian modification for Lam-Bremhorst model.
define/models/viscous/turbulence-expert/restore-sst-v61?Enables/disables SST formulation of v6.1.
define/models/viscous/turbulence-expert/rke-cmu-rotation-term?Modifies 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.define/models/viscous/turbulence-expert/sbes-sdes-hybrid-modelSelects 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.
define/models/viscous/turbulence-expert/sbes-sgs-optionSelects the subgrid-scale model for the LES portion of your Stress-Blended Eddy Simulation (SBES).
define/models/viscous/turbulence-expert/sbes-update-interval-k-omegaSets the number of time steps between updates of the k-ω part of the SBES model.
define/models/viscous/turbulence-expert/thermal-p-function?Enables/disables Jayatilleke P function.
define/models/viscous/turbulence-expert/turb-add-sbes-sdes?Enables/disables the Stress-Blended Eddy Simulation (SBES) model or Shielded Detached Eddy Simulation (SDES) model.
define/models/viscous/turbulence-expert/turb-non-newtonian?Enables/disables turbulence for non-Newtonian fluids.
define/models/viscous/turbulence-expert/turbulence-damping?Enables/disables turbulence damping and sets turbulence damping parameters.
define/models/viscous/turbulence-expert/turb-pk-compressible?Enables/disables turbulent production due to compressible divergence.
define/models/viscous/user-definedSelects user-defined functions to define the turbulent viscosity and the turbulent Prandtl and Schmidt numbers.
define/models/viscous/user-defined-transitionSets user-defined transition correlations.
define/models/viscous/zero-equation-hvac?Enables/disables zero-equation HVAC turbulence model.
define/motion-definitions/Enters the motion definitions menu, where you can manage motion definitions.
define/motion-definitions/addAdds a new motion definition. After you enter a name for the definition, you can define the following settings:
nameThis allows you to revise the name of the definition.
ref-frameThis allows you to specify the reference frame for the definition. You can use the default
globalreference frame, or specify a local reference frame definition that you have previously set up using thedefine/reference-framestext command menu.rigid-body-motion-definitionThis provides the following settings that define the motion for a rigid body dynamic mesh zone.
rotationThis allows you to define the axis and speed of the rotation. For 3D cases, you can define the rotation axis components in the coordinate directions through the
x,y. andzsettings; for 2D cases, the axis direction is the positive Z direction. Then you can provide a value for thespeed, which is defined using the right-hand rule with respect to the defined axis. Each of these settings can be defined as a constant value, an expression, an input parameter, or a named expression.translationThis allows you to define the translation velocity components in the coordinate directions. You can define
x,y, and (for 3D cases)zcomponents. These settings can be defined as a constant value, an expression, an input parameter, or a named expression.
define/motion-definitions/deleteDeletes a specified motion definition.
define/motion-definitions/editEdits an existing motion definition. After you enter the name of the definition you want to edit, you can edit the following settings:
nameThis allows you to revise the name of the definition.
ref-frameThis allows you to specify the reference frame for the definition. You can use the default
globalreference frame, or specify a local reference frame definition that you have previously set up using thedefine/reference-framestext command menu.rigid-body-motion-definitionThis provides the following settings that define the motion for a rigid body dynamic mesh zone.
rotationThis allows you to define the axis and speed of the rotation. For 3D cases, you can define the rotation axis components in the coordinate directions through the
x,y. andzsettings; for 2D cases, the axis direction is the positive Z direction. Then you can provide a value for thespeed, which is defined using the right-hand rule with respect to the defined axis. Each of these settings can be defined as a constant value, an expression, an input parameter, or a named expression.translationThis allows you to define the translation velocity components in the coordinate directions. You can define
x,y, and (for 3D cases)zcomponents. These settings can be defined as a constant value, an expression, an input parameter, or a named expression.
define/motion-definitions/listLists all of the motion definitions in the console.
define/motion-definitions/list-propertiesLists the settings for a specified motion definition in the console.
define/named-expressions/Enters the named expressions menu.
define/named-expressions/addCreates a new named expression.
define/named-expressions/computeComputes and prints the value of an expression. This is only available for expressions that evaluate to a single value.
define/named-expressions/copyAllows you to copy an existing named expression.
define/named-expressions/deleteAllows you to delete a named expression, as long as it is not in use.
define/named-expressions/export-to-tsvExport one or more named expressions to a file in TSV format.
define/named-expressions/import-from-tsvImport one or more named expressions saved in TSV format.
define/named-expressions/editAllows you to edit the definition of a named expression.
define/named-expressions/listLists all of the currently defined named expressions.
define/named-expressions/list-propertiesLists the definition of a named expression.
define/operating-conditions/Enters the define operating conditions menu.
define/operating-conditions/gravitySets gravitational acceleration.
define/operating-conditions/gravity-mrf-behaviorEnables/disables the fixing of the gravity vector in the stationary reference frame. When enabled, the gravity vector rotates with respect to the moving reference frame such that the direction of gravity in the global stationary coordinates remains fixed. When disabled, the gravity vector is fixed in the moving reference frame. This item is available only for transient cases with moving reference frames and gravity enabled.
define/operating-conditions/operating-density?Enables/disables use of a specified operating density. This command is available only for single-phase flows.
define/operating-conditions/operating-density/Enters the operating density menu. This menu is available only for multiphase flows.
define/operating-conditions/operating-density/print-operating-densityPrints the operating density value.
define/operating-conditions/operating-density/set-operating-densityAllows you to select the operating density method in your simulation. You can choose from:
0 = minimum-phase-averaged1 = primary-phase-averaged2 = mixture-averaged3 = user-input
See Modeling Buoyancy-Driven Multiphase Flow in the Fluent User's Guide for more information about these options.
define/operating-conditions/operating-pressureSets the operating pressure.
define/operating-conditions/operating-temperatureSets the operating temperature for Boussinesq.
define/operating-conditions/reference-pressure-locationSets a location that determines the reference pressure cell or cells (depending on the selected reference pressure method). The pressure value in such cells can be used to adjust the gauge pressure field after each iteration to keep it from floating.
define/operating-conditions/reference-pressure-methodSpecifies the method used for adjusting the gauge pressure field after each iteration to keep it from floating: the method can assume that all of the cell zones are connected by internal boundary zones (such as interior zones), or can account for connected and disconnected cell zones. Such adjustment is only allowed for incompressible flows, and will be limited partially or entirely by the presence of a pressure boundary.
define/operating-conditions/set-stateSelects state for real gas EOS subcritical condition.
define/operating-conditions/used-ref-pressure-locationPrints the coordinates of the reference pressure cell or cells (depending on the selected reference pressure method). The pressure value in such cells can be used to adjust the gauge pressure field after each iteration to keep it from floating.
define/operating-conditions/use-inlet-temperature-for-operating-densityUses inlet temperature to calculate operating density.
define/overset-interfaces/Enters the overset interfaces menu.
define/overset-interfaces/adapt/Enters the overset adaption menu.
define/overset-interfaces/adapt/adapt-meshMarks and adapts the mesh to improve your overset mesh.
define/overset-interfaces/adapt/mark-adaptionMarks cells to identify those that can be adapted in order to improve your overset mesh.
define/overset-interfaces/adapt/set/Enters the overset adaption set menu.
define/overset-interfaces/adapt/set/adaption-sweepsSets the number of rounds of adaption applied during each adaption cycle.
define/overset-interfaces/adapt/set/automatic?Enables/disables the option to automatically adapt overset meshes during the calculation, to remove orphans, reduce size mismatches between donor and receptor cells, and/or increase the mesh resolution in gaps as needed (in order to prevent the creation of orphan cells). This option is disabled by default.
define/overset-interfaces/adapt/set/buffer-layersSets the number of cell layers marked in addition to the cells marked for orphan adaption.
define/overset-interfaces/adapt/set/gap-resolutionSets the target (minimum) gap resolution used when marking cells for gap adaption. This is set to 4 by default and is only available when
define/overset-interfaces/adapt/set/mark-gaps?is enabled.define/overset-interfaces/adapt/set/length-ratio-maxSets the length scale ratio threshold used to determine which cells are marked for adaption based on donor-receptor cell size differences. This is set to 3 by default and is only available when
define/overset-interfaces/adapt/set/mark-size?is enabled.define/overset-interfaces/adapt/set/mark-coarsening?Enables/disables the option to coarsen the mesh if mesh refinement is no longer needed. This option is enabled by default.
define/overset-interfaces/adapt/set/mark-fixed-orphans?Enables/disables the option to also adapt based on cells that are not actual orphans because they were fixed by accepting neighbor donors. This option is only available when
define/overset-interfaces/adapt/set/mark-orphans?is enabled.define/overset-interfaces/adapt/set/mark-gaps?Enables/disables the option to adapt under-resolved gaps in order to prevent the creation of orphan cells. This option is disabled by default.
define/overset-interfaces/adapt/set/mark-orphans?Enables/disables the option to adapt for orphan reduction.
define/overset-interfaces/adapt/set/mark-size?Enables/disables the option to adapt based on donor-receptor cell size differences.
define/overset-interfaces/adapt/set/maximum-refinement-levelSets the maximum level of refinement during overset adaption, in conjunction with the value set using the
mesh/adapt/set/maximum-refinement-leveltext command (the larger of the two values is used).define/overset-interfaces/adapt/set/prismatic?Enables/disables the option to use anisotropic refinement for the prismatic cells adapted as part of overset orphan adaption and/or overset gap adaption. Instead of being isotropically refined, these cells will not be split on particular edges, in order to reduce the resulting cell count. This anisotropic adaption option is available only for 3D cases and is applied only to prismatic cells that are deemed suitable. For orphan adaption, the goal is to produce cells that have a lower aspect ratio; for gap adaption, the goal is to produce a mesh resolution that is suitable for boundary layers near walls.
define/overset-interfaces/checkChecks the integrity of the overset interfaces. Reports orphan cells and errors in the domain connectivity.
define/overset-interfaces/clearClears the domain connectivity of an overset interface. This text command is only available when
define/overset-interfaces/options/expert?is set toyes.define/overset-interfaces/clear-allClears the domain connectivity of all overset interfaces. This text command is only available when
define/overset-interfaces/options/expert?is set toyes.define/overset-interfaces/createCreates an overset interface.
define/overset-interfaces/cut-control/Enters the overset hole cut control menu.
define/overset-interfaces/cut-control/addAdds a hole cut control, so that a boundary zone does not cut specified cell zones.
define/overset-interfaces/cut-control/cut-seeds/Enters the overset hole cut seeds menu.
define/overset-interfaces/cut-control/cut-seeds/cut-seeds-for-all-component-zones?Specifies whether all component zones get cut seeds, which cut pilot holes into the overlapping meshes that will then be enlarged during overlap minimization.
define/overset-interfaces/cut-control/deleteDeletes the hole cut control for a boundary zone.
define/overset-interfaces/cut-control/delete-allDeletes the hole cut controls for all boundary zones.
define/overset-interfaces/cut-control/listLists the defined hole cut controls.
define/overset-interfaces/debug-hole-cutDebugging tool to troubleshoot hole cutting of overset interfaces. This text command is only available when
define/overset-interfaces/options/expert?is set toyes.define/overset-interfaces/deleteDeletes an overset interface.
define/overset-interfaces/delete-allDeletes all overset interfaces in the domain.
define/overset-interfaces/display-cellsDisplays the overset cells marked using the text command
define/overset-interfaces/mark-cells.define/overset-interfaces/grid-prioritiesAllows you to specify grid priorities on background and component meshes, used in the overlap minimization of an overset interface.
define/overset-interfaces/intersectExecutes 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 toyes.define/overset-interfaces/intersect-allExecutes hole cutting for all overset interfaces in the domain. This text command is only available when
define/overset-interfaces/options/expert?is set toyes.define/overset-interfaces/listLists information about the overset interfaces. The output depends on the overset verbosity setting.
define/overset-interfaces/mark-cell-changeMarks cells that have undergone a specified overset cell type change (from
solve,receptor, ordeadto 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 ifdefine/overset-interfaces/options/expert?is set toyes.define/overset-interfaces/mark-cellsMarks the specified overset cells (solve, receptor, donor, orphan, or dead) and fills registers based on the markings. Display the marked cells via the text command
define/overset-interfaces/display-cells.define/overset-interfaces/options/Enters the overset interface options menu.
define/overset-interfaces/options/auto-create?Enables the automatic creation of a default overset interface during initialization or mesh motion update.
define/overset-interfaces/options/dead-cell-update?Enables/disables the updating of dead cells during the solution process, which may be helpful for some moving and dynamic mesh simulations (though at the cost of solver performance). You can enter the number of layers of dead cells adjacent to the receptor cells that you want updated, or enter
-1to request that all dead cells are updated. This text command is only available for transient simulations whendefine/overset-interfaces/options/expert?is set toyes.define/overset-interfaces/options/donor-priority-methodAllows 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.
define/overset-interfaces/options/expert?Enables / disables overset-related expert tools.
define/overset-interfaces/options/mesh-interfaces?Allows the inclusion of non-conformal mesh interfaces inside overset cell zones, as long as the mesh interfaces do not spatially overlap with the cells where the overset interfaces lie.
define/overset-interfaces/options/minimize-overlap?Allows you to disable overlap minimization during hole cutting.
define/overset-interfaces/options/modified-donor-search?Enables / disables modified donor search parameters. When enabled, these parameters result in a more extended donor search, which can be helpful for meshes with orphans. This text command is only available when
define/overset-interfaces/options/expert?is set toyes.define/overset-interfaces/options/modified-hole-cutting?Enables / disables modified hole cutting parameters. When enabled, the parameters used can help avoid dead cell zones that result from a hole cutting failure. This text command is only available when
define/overset-interfaces/options/expert?is set toyes.define/overset-interfaces/options/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 toyes.define/overset-interfaces/options/overlap-boundaries?Allows you to disable the detection of overlapping boundaries during hole cutting, in order to reduce the computational expense for cases that do not include such boundaries. When enabled, this text command also allows you to specify which boundary zones should be considered when detecting overlapping boundaries; this can be helpful when the default hole cutting process fails.
define/overset-interfaces/options/parallelAllows you to select the algorithm used for overset parallel processing. You can select from the default cell exchange model or the local cell zone replication model; the cell exchange model should require less memory and may result in faster calculations.
define/overset-interfaces/options/partial-cut-faces?Enables/disables enhanced hole cutting, where partially overlapping cut faces are decomposed into overlapping and non-overlapping fractions, and only the non-overlapping fractions participate in the hole cutting. This can help avoid the situation where a region or cell zone is erroneously identified as dead because of leakage during flood filling, even though it has overlapping boundaries that match well. When this text command is disabled, the partially overlapping faces are entirely protected from cutting.
define/overset-interfaces/options/render-receptor-cells?Allows you to enable visualization of receptor cells in contour and mesh displays.
define/overset-interfaces/options/solve-island-removalSets 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 toyes.define/overset-interfaces/options/transient-cachingSets 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 toyes.define/overset-interfaces/options/update-before-case-write?Enables/disables the updating of the overset interfaces before writing a case file in the Common Fluids Format (CFF). This text command is only available when
define/overset-interfaces/options/expert?is set toyes.define/overset-interfaces/options/verbositySpecifies the level of detail printed in the console about overset interfaces.
define/overset-interfaces/set-mark-boundsAllows you to set bounds so that any marking of cells is performed within a spherical region based on a specified origin and radius. This can be useful when diagnosing a local problem on a large mesh. This text command is only available if
define/overset-interfaces/options/expert?is set toyes. After defining the bounds, you can then mark the cells using thedefine/overset-interfaces/mark-cell-changeordefine/overset-interfaces/mark-cellstext command. To disable the bounds, enter a radius of0.
define/parameters/Enters the parameters menu.
define/parameters/enable-in-TUI?Enables/disables parameters in the text user interface.
define/parameters/input-parameters/Enters the input-parameters menu.
define/parameters/input-parameters/deleteDeletes an input parameter.
define/parameters/input-parameters/editEdits an input parameter.
define/parameters/output-parameters/Enters the output-parameters menu.
define/parameters/output-parameters/createCreates an output parameter.
define/parameters/output-parameters/deleteDeletes an output parameter.
define/parameters/output-parameters/editEdits an output parameter.
define/parameters/output-parameters/print-all-to-consoleDisplays all parameter values in the console.
define/parameters/output-parameters/print-to-consoleDisplays parameter value in the console.
define/parameters/output-parameters/renameRenames an output parameter.
define/parameters/output-parameters/write-all-to-fileWrites all parameter values to file.
define/parameters/output-parameters/write-to-fileWrites parameter value to file.
define/periodic-conditions/Enters the periodic conditions menu.
define/periodic-conditions/massflow-rate-specification?Enables/disables specification of mass flow rate at the periodic boundary.
define/periodic-conditions/pressure-gradient-specification?Enables/disables specification of pressure gradient at the periodic boundary.
define/phases/Enters the phases menu.
define/phases/iac-expert/Enters the IAC expert setting menu.
define/phases/iac-expert/hibiki-ishii-modelSets Hibiki-Ishii model coefficients.
define/phases/iac-expert/ishii-kim-modelSets Ishii-Kim model coefficients.
define/phases/iac-expert/yao-morel-modelSets Yao-Morel model coefficients.
define/phases/set-domain-properties/Enters the menu to set phase domain properties.
define/phases/set-domain-properties/change-phases-names?Allows you to change the names of all the phases in your simulation.
define/phases/set-domain-properties/interaction-domain/Enters the menu to set the interaction domain properties.
define/phases/set-domain-properties/interaction-domain/forces/Enters the menu to set interfacial forces models.
define/phases/set-domain-properties/interaction-domain/forces/dragSpecifies the drag function, drag modification, and drag factor for each pair of phases. This command is available only with the Eulerian and Mixture multiphase models.
define/phases/set-domain-properties/interaction-domain/forces/lift/Enters the menu to set the lift force. This item is available only with the Eulerian multiphase model.
define/phases/set-domain-properties/interaction-domain/forces/lift/liftSpecifies the lift function for each pair of phases.
define/phases/set-domain-properties/interaction-domain/forces/lift/lift-shaver-podowski?Enables/disables the Shaver-Podowski lift correction.
define/phases/set-domain-properties/interaction-domain/forces/restitutionSpecifies the restitution coefficient for collisions between each pair of granular phases, and for collisions between particles of the same granular phase. This command is available only for multiphase flows with two or more granular phases.
define/phases/set-domain-properties/interaction-domain/forces/slip-velocitySpecifies the slip velocity function for each secondary phase with respect to the primary phase. This command is available only for the Mixture multiphase model.
define/phases/set-domain-properties/interaction-domain/forces/surface-tension/Enters the menu to set surface tension models.
define/phases/set-domain-properties/interaction-domain/forces/surface-tension/jump-adhesion?Enables/disables the treatment of the contact angle specification at the porous jump boundary. This command is available only for the VOF multiphase model with the continuum surface stress model option and when
sfc-modeling?is enabled.define/phases/set-domain-properties/interaction-domain/forces/surface-tension/sfc-modeling?Allows you to include the effects of surface tension along the fluid-fluid interface. This option is only available for the VOF and Eulerian multiphase models.
define/phases/set-domain-properties/interaction-domain/forces/surface-tension/sfc-model-typeSelects the surface tension model. You can choose between the continuum surface force and continuum surface stress methods. This item is available only when
sfc-modeling?is enabled.define/phases/set-domain-properties/interaction-domain/forces/surface-tension/sfc-tension-coeffSpecifies the surface tension coefficient for each pair of phases.
define/phases/set-domain-properties/interaction-domain/forces/surface-tension/wall-adhesion?Enables/disables the specification for a wall adhesion angle. This item is available only when
sfc-modeling?is enabled.
define/phases/set-domain-properties/interaction-domain/forces/turbulent-dispersionSpecifies the turbulent dispersion model for each primary-secondary phase pair. This command is available only with the Eulerian multiphase model.
define/phases/set-domain-properties/interaction-domain/forces/turbulence-interactionSpecifies the turbulence interaction model for each primary-secondary phase pair. This command is available only with the Eulerian multiphase model.
define/phases/set-domain-properties/interaction-domain/forces/virtual-mass/Enters the menu to set virtual mass models.
define/phases/set-domain-properties/interaction-domain/forces/virtual-mass/virtual-mass?Allows you to include the virtual mass force effect that occurs when a secondary phase accelerates relative to the primary phase. This command is available only with the Eulerian multiphase model.
define/phases/set-domain-properties/interaction-domain/forces/virtual-mass/vmass-coeffSpecifies the virtual mass coefficient for each pair of phases. This option is available only if
virtual-mass?is enabled.define/phases/set-domain-properties/interaction-domain/forces/virtual-mass/vmass-implicit?Enables/disables the implicit method for the virtual mass force. This option can improve convergence in some cases. This option is available only if
virtual-mass?is enabled.define/phases/set-domain-properties/interaction-domain/forces/virtual-mass/vmass-implicit-optionsSpecifies what form of the implicit method to use (
default,option-2, oroption-3).defaultmodels the entire virtual mass force whileoption-2andoption-3model truncated expressions which may further improve convergence. This option is available only ifvmass-implicit?is enabled.
define/phases/set-domain-properties/interaction-domain/forces/wall-lubricationSpecifies the wall lubrication model for each primary-secondary phase pair. This command is available only with the Eulerian multiphase model.
define/phases/set-domain-properties/interaction-domain/heat-mass-reactions/Enters the menu to set heat, mass-transfer, and reaction models.
define/phases/set-domain-properties/interaction-domain/heat-mass-reactions/cavitation/Enters the menu to set cavitation models. This option is available only for the Mixture multiphase model with the Singhal-et-al cavitation model enabled via
solve/set/advanced/singhal-et-al-cavitation-model.define/phases/set-domain-properties/interaction-domain/heat-mass-reactions/cavitation/cavitation?Allows you to include the effects of cavitation. When the cavitation is enabled, you must specify vaporization pressure, surface tension coefficient, and non-condensable gas mass fraction using the
define/phases/set-domain-properties/interaction-domain/heat-mass-reactions/cavitation/caviationtext command. If multiple species are included in one or more secondary phases, or the heat transfer due to phase change is considered, the mass transfer mechanism must be defined before enabling the cavitation model.define/phases/set-domain-properties/interaction-domain/heat-mass-reactions/cavitation/cavitationSets the vaporization pressure, surface tension coefficient, and non-condensable gas mass fraction. This command is available only when
cavitation?is enabled.
define/phases/set-domain-properties/interaction-domain/heat-mass-reactions/heat-coeffSpecies the heat transfer coefficient function between each pair of phases (
constant-htc,nusselt-number,ranz-marshall,hughmark,tomiyama,fixed-to-sat-temp,two-resistance, oruser-defined). This command is enable only with the Eulerian multiphase model.define/phases/set-domain-properties/interaction-domain/heat-mass-reactions/mass-transferSets the mass transfer mechanisms.
define/phases/set-domain-properties/interaction-domain/heat-mass-reactions/reactionsAllows you to define multiple heterogeneous reactions and stoichiometry. This option is available only with the species model.
define/phases/set-domain-properties/interaction-domain/interfacial-area/Enters the menu to set interfacial area models. This menu is available only for the Mixture and Eulerian multiphase models.
define/phases/set-domain-properties/interaction-domain/interfacial-area/interfacial-areaSpecifies the interfacial area model for each pair of phases.
define/phases/set-domain-properties/interaction-domain/model-transition/Enters the menu to set model transition mechanisms.
define/phases/set-domain-properties/interaction-domain/model-transition/model-transitionSets the VOF-to-DPM model transition mechanism.
define/phases/set-domain-properties/interaction-domain/numerics/Enters the menu to set numerics models. This menu is available for multiphase models with the sharp-dispersed and phase localized discretization interface modeling options (set in
define/models/multiphase/interface-modeling-options).define/phases/set-domain-properties/interaction-domain/numerics/interphase-discretization/Enters the menu to set interphase discretization models.
define/phases/set-domain-properties/interaction-domain/numerics/interphase-discretization/interphase-discr?Enables/disables phase localized compressive scheme.
define/phases/set-domain-properties/interaction-domain/numerics/interphase-discretization/slope-limiterSpecifies the slope limiter to set a specific discretization scheme for each phase pair. A value of 0 corresponds to first order upwind, a value of 1 corresponds to second order upwind, a value of 2 applies the compressive scheme, and a value between 0 and 2 corresponds to a blended scheme. This option is available only when
interphase-discr?is enabled.
define/phases/set-domain-properties/phase-domains/Enters the menu to select a specific phase.
define/phases/set-domain-properties/phase-domains/phasename/Enters the menu for setting properties for the selected phase
phasename, wherephasenameis the name of the phase you selected using thephase-domains/text command.define/phases/set-domain-properties/phase-domains/diameterphasename/Sets the diameter of the particles of the selected phase
phasename. This text command is available for secondary phases only.define/phases/set-domain-properties/phase-domains/granular-properties/phasename/Enters the menu for setting properties for the granular phase. This text command is available only when the
granular?text command is enabled.define/phases/set-domain-properties/phase-domains/bulk-viscosityphasename/granular-properties/Sets the solids bulk viscosity (constant, lun-et-al, or user-defined).
define/phases/set-domain-properties/phase-domains/elasticity-modulusphasename/granular-properties/Specifies the elasticity modulus (derived or user-defined).
define/phases/set-domain-properties/phase-domains/friction-anglephasename/granular-properties/Sets the angle of internal friction (constant or user-defined). This text command is available only when
schaefferis selected as the friction viscosity model.define/phases/set-domain-properties/phase-domains/friction-packingphasename/granular-properties/Sets a threshold volume fraction at which the frictional regime becomes dominant (constant or user-defined). The default value is 0.61. This text command is available only when
schaefferis selected as the friction viscosity model.define/phases/set-domain-properties/phase-domains/friction-viscosityphasename/granular-properties/Specifies a shear viscosity based on the viscous-plastic flow (none, constant, schaeffer, or user-defined). By default, the frictional viscosity is neglected (
none).Note: When
schaefferis selected as the friction viscosity model, you must specifyfriction-angle,friction-packing,frictional-modulus, andfrictional-pressure.define/phases/set-domain-properties/phase-domains/frictional-modulusphasename/granular-properties/Sets the frictional modulus (derived or user-defined). This text command is available only when
schaefferis selected as the friction viscosity model.define/phases/set-domain-properties/phase-domains/frictional-pressurephasename/granular-properties/Sets the pressure gradient term in the granular-phase momentum equation (none, johnson-et-al, syamlal-et-al, based-ktgf, or user-defined). This text command is available only when
schaefferis selected as the friction viscosity model.define/phases/set-domain-properties/phase-domains/granular-conductivityphasename/granular-properties/Sets temperature for the solids phase (constant, syamlal-obrien, gidaspow, or user-defined). This text command is available only if the
pde-granular?text command is enabled.define/phases/set-domain-properties/phase-domains/granular-temperaturephasename/granular-properties/Sets temperature for the solids phase (algebraic, constant, dpm-averaged, or user-defined). The
dpm-averagedoption is available only when using the Dense Discrete Phase Model (DDPM). This text command is available only if thepde-granular?text command is disabled.define/phases/set-domain-properties/phase-domains/packed-bed?phasename/granular-properties/Enables/disables the packed bed model.
define/phases/set-domain-properties/phase-domains/packingphasename/granular-properties/Sets the maximum volume fraction for the granular phase (constant or user-defined). For monodispersed spheres the packing limit is about 0.63.
define/phases/set-domain-properties/phase-domains/pde-granular?phasename/granular-properties/Enables/disables the partial differential equation (PDE) model for granular temperature. When the PDE model is enabled, you must specify
granular-conductivity. Otherwise, you must specifygranular-temperature.define/phases/set-domain-properties/phase-domains/radial-distributionphasename/granular-properties/Sets a correction factor that modifies the probability of collisions between grains when the solid granular phase becomes dense (lun-et-al, syamlal-obrien, ma-ahmadi, arastoopour, or user-defined).
define/phases/set-domain-properties/phase-domains/solids-pressurephasename/granular-properties/Sets the pressure gradient term in the granular-phase momentum equation (lun-et-al, syamlal-obrien, ma-ahmadi, user-defined, or none).
define/phases/set-domain-properties/phase-domains/viscosityphasename/granular-properties/Sets the kinetic part of the granular viscosity of the particles (constant, syamlal-obrien, gidaspow, or user-defined).
define/phases/set-domain-properties/phase-domains/granular?phasename/Enables/disables the granular approach for the solid phase. This text command is available only for secondary phases in a Eulerian multiphase case. This approach is not compatible with the interfacial area concentration approach. For more details, see Defining a Granular Secondary Phase in the Fluent User's Guide.
define/phases/set-domain-properties/phase-domains/iac-properties/phasename/Enters the menu for setting model properties for the interfacial area concentration. This text command is available only when the
iac?text command is enabled.define/phases/set-domain-properties/phase-domains/iac-breakage-kernelphasename/iac-properties/Sets the breakage kernel (none, constant, hibiki-ishii, ishii-kim, yao-morel, or user-defined).
define/phases/set-domain-properties/phase-domains/iac-coalescence-kernelphasename/iac-properties/Sets the coalescence kernel (none, constant, hibiki-ishii, ishii-kim, yao-morel, or user-defined).
define/phases/set-domain-properties/phase-domains/iac-critical-weberphasename/iac-properties/Sets the critical Weber number. This value is required if you selected
yao-morelas the breakage kernel.define/phases/set-domain-properties/phase-domains/iac-dissipation-ratephasename/iac-properties/Allows you to choose the dissipation function (constant, wu-ishii-kim, fluent-ke, or user-defined).
define/phases/set-domain-properties/phase-domains/iac-hydraulic-diamphasename/iac-properties/Sets the hydraulic diameter. This value is required when you selected
wu-ishii-kimfor the IAC dissipation rate function.define/phases/set-domain-properties/phase-domains/iac-max-diameterphasename/iac-properties/Sets the maximum for the bubble diameters.
define/phases/set-domain-properties/phase-domains/iac-min-diameterphasename/iac-properties/Sets the minimum for the bubble diameters.
define/phases/set-domain-properties/phase-domains/iac-nucleation-kernelphasename/iac-properties/Sets the source term for the interfacial area concentration that models the rate of formation of the dispersed phase (none, constant, yao-morel, or user-defined).
define/phases/set-domain-properties/phase-domains/iac-surface-tensionphasename/iac-properties/Sets the attractive forces between the interfaces.
define/phases/set-domain-properties/phase-domains/iac?phasename/Enables/disables the interfacial area concentration (IAC) approach. This text command is available for secondary phases only. The IAC approach is not compatible with the granular approach. See Defining the Interfacial Area Concentration via the Transport Equation and Defining the Interfacial Area Concentration in the Fluent User's Guide for details about using the IAC approach for the Mixture and Eulerian multiphase flows.
define/phases/set-domain-properties/phase-domains/materialphasename/Sets a material for the selected phase.
define/profiles/Enters the boundary profiles menu.
define/profiles/deleteDeletes a profile.
define/profiles/delete-allDeletes all boundary-profiles.
define/profiles/display-profile-point-cloud-dataDisplay the profile and/or its fields as a cloud of points.
define/profiles/display-profile-surfaceDisplay the profile as a surface (this option is only available if the specified profile contains node-connectivity data).
define/profiles/interpolation-methodChooses the method for interpolation of profiles.
define/profiles/link-profile-to-reference-frameAttaches a profile to a reference frame so that the profile will rotate according to the reference frame.
define/profiles/list-profilesLists all profiles.
define/profiles/list-profile-fieldsLists the fields of a particular profile.
define/profiles/morphing?Enables/disables profile morphing options in Orient Profile panel.
define/profiles/orient-profileRe-orient an existing profile.
define/profiles/overlay-profile-point-cloud-dataPreview a profile as a cloud of points and overlay an existing mesh or contour graphics object in the same graphics window.
define/profiles/overlay-profile-surfacePreview a profile as a surface (only available for profiles with node-connectivity data) and overlay an existing mesh or contour graphics object in the same graphics window.
define/profiles/replicate-profilesCopy an existing profile.
define/profiles/set-preference-profile-point-cloud-dataSet the marker symbol, size, and color for previewing a profile as a point cloud.
define/profiles/update-intervalSets the number of iterations between updates of dynamic profiles that use user-defined functions (UDFs) or named expressions.
define/reference-frames/Enters the reference frames menu.
define/reference-frames/addCreates a new reference frame.
define/reference-frames/deleteDeletes the reference frame you specify.
define/reference-frames/displayDisplays the reference frame you specify.
define/reference-frames/editAllows you to edit a reference frame.
define/reference-frames/hideRemoves the specified reference frame from the graphics window.
define/reference-frames/listLists all of the reference frames.
define/reference-frames/list-propertiesLists the properties of the reference frame you specify.
define/set-unit-systemApplies a standard set of units to all quantities. The options include
default,si,british, andcgs.define/solution-strategy/Enters the automatic initialization and case modification strategy menu.
define/solution-strategy/automatic-case-modification/Enters the automatic case modification menu.
define/solution-strategy/automatic-case-modification/before-init-modificationSpecifies modification to be performed before initialization.
define/solution-strategy/automatic-case-modification/modificationsSpecifies modifications to be performed during solution.
define/solution-strategy/automatic-case-modification/original-settingsSpecifies modification to be performed after initialization to restore to original settings.
define/solution-strategy/automatic-initializationDefines how the case is to be automatically initialized.
define/solution-strategy/continue-strategy-executionContinues execution of the currently defined automatic initialization and case modification strategy.
define/solution-strategy/enable-strategy?Enables/disables automatic initialization and case modification.
define/solution-strategy/execute-strategyExecutes the currently defined automatic initialization and case modification strategy.
define/turbo-model/Enters the turbo menu.
define/turbo-model/blade-flutter-harmonics/Enters the blade flutter harmonics options menu.
define/turbo-model/blade-flutter-harmonics/enable-harmonic-postprocessing?Enables the computation of Fourier coefficients of pressure, velocity components, and temperature based on the blade flutter frequency of the simulation.
define/turbo-model/blade-flutter-harmonics/enable-harmonic-exports?Enables the computation of real and imaginary harmonic pressure loads on user-defined surfaces based on the blade flutter frequency of the simulation.
define/turbo-model/blade-flutter-harmonics/write-harmonic-exports?Writes a
.csvfile containing real and imaginary harmonic pressure loads that can be read into CFD-Post.
define/turbo-model/create-turbomachine-descriptionCreates a turbomachine description that describes basic information about the turbomachine being modeled.
define/turbo-model/delete-turbomachine-descriptionDeletes a previously defined turbomachinery description.
define/turbo-model/enable-turbo-model?Enables/disables turbo model menu.
define/turbo-model/export-boundary-meshExports boundary data for that can be imported into CFX-Pre or CFD-Post as a user surface, or used in System Coupling mapping.
define/turbo-model/general-turbo-interface-settings/Enters the General Turbo Interface options menu.
define/turbo-model/general-turbo-interface-settings/expert/Enters the expert settings menu related to General Turbo Interface.
define/turbo-model/general-turbo-interface-settings/expert/backwardcompatibility/Enters the backward compatibility menu related to General Turbo Interface.
define/turbo-model/general-turbo-interface-settings/expert/backwardcompatibility/pre-24r2-mp-discretizationReverts to pre-2024 R2 behavior for mixing plane discretization where turbulence quantities might hit certain system limits.
define/turbo-model/general-turbo-interface-settings/expert/enforce-flux-scaling?Scales fluxes across interfaces to improve conservation.
define/turbo-model/general-turbo-interface-settings/expert/list-settingsLists flux scaling settings for all defined General Turbo Interfaces.
define/turbo-model/general-turbo-interface-settings/expert/nps-minimize-po-lossMinimizes total pressure loss across a NPS interface with large pitch difference.
define/turbo-model/general-turbo-interface-settings/mixing-plane-model-settings/Defines settings for the mixing plane model.
define/turbo-model/general-turbo-interface-settings/mixing-plane-model-settings/bands-typeSpecifies the averaging bands for mixing as fixed or variable width. Variable width band are used to accommodate mesh boundary layers.
define/turbo-model/general-turbo-interface-settings/mixing-plane-model-settings/number-of-bandsSets the number of bands to be used for mixing.
define/turbo-model/general-turbo-interface-settings/mixing-plane-model-settings/list-mixing-planesLists all the mixing-plane interfaces and their settings.
define/turbo-model/legacy-models/Enters the submenu to access legacy models.
define/turbo-model/legacy-models/legacy-mixing-plane/Enters the mixing planes menu.
define/turbo-model/legacy-models/legacy-mixing-plane/createCreates a mixing plane.
define/turbo-model/legacy-models/legacy-mixing-plane/deleteDeletes a mixing plane.
define/turbo-model/legacy-models/legacy-mixing-plane/listLists defined mixing plane(s).
define/turbo-model/legacy-models/legacy-mixing-plane/mixing-plane-guiOpens the Mixing Planes dialog box.
define/turbo-model/legacy-models/legacy-mixing-plane/set/Sets global parameters relevant to mixing planes.
define/turbo-model/legacy-models/legacy-mixing-plane/set/averaging-methodSets the mixing plane profile averaging method.
define/turbo-model/legacy-models/legacy-mixing-plane/set/under-relaxationSets mixing plane under-relaxation factor.
define/turbo-model/legacy-models/legacy-mixing-plane/set/fix-pressure-levelSets fixed pressure level using value based on
define/reference-pressure-location.define/turbo-model/legacy-models/legacy-mixing-plane/set/conserve-swirl/Enters the menu to set swirl conservation in mixing plane menu.
define/turbo-model/legacy-models/legacy-mixing-plane/set/conserve-swirl/enable?Enables/disables swirl conservation in mixing plane.
define/turbo-model/legacy-models/legacy-mixing-plane/set/conserve-swirl/verbosity?Enables/disables verbosity in swirl conservation calculations.
define/turbo-model/legacy-models/legacy-mixing-plane/set/conserve-swirl/report-swirl-integrationReports swirl integration (Torque) on inflow and outflow zones.
define/turbo-model/legacy-models/legacy-mixing-plane/set/conserve-total-enthalpy/Enters the menu to set total enthalpy conservation in mixing plane menu.
define/turbo-model/legacy-models/legacy-mixing-plane/set/conserve-total-enthalpy/enable?Enables/disables total enthalpy conservation in mixing plane.
define/turbo-model/legacy-models/legacy-mixing-plane/set/conserve-total-enthalpy/verbosity?Enables/disables verbosity in total-enthalpy conservation calculations.
define/turbo-model/list-turbomachine-descriptionLists a previously defined turbomachinery description in the console.
define/turbo-model/performanceEvaluates various efficiencies and performance characteristics of a turbomachine.
define/turbo-model/turbo-createCreates a general turbo interface.
define/turbo-model/turbo-interface-checkChecks a general turbo interface and displays relevant information in the console.
define/turbo-model/turbo-interface-deleteDeletes one or more general turbo interfaces or standard tip-gap interfaces.
define/turbo-model/turbo-interface-editEdits the type of one or more general turbo interfaces. This text command also edits the name of a standard tip-gap or general turbo interface (to include the new type).
define/turbo-model/turbo-topology/Enters the turbo topology menu.
define/turbo-model/turbo-topology/define-topologyDefines a turbo topology.
define/turbo-model/turbo-topology/deleteDeletes a previously created turbo topology.
define/turbo-model/turbo-topology/mesh-methodSets turbo structured mesh generation method.
define/turbo-model/turbo-topology/projection-methodSets 2D projection method.
define/turbo-model/turbo-topology/search-methodSets search method for a topology.
define/unitsSets unit conversion factors.
define/user-defined/Enters the user-defined functions and scalars menu.
define/user-defined/1D-couplingLoads 1D library.
define/user-defined/compiled-functionsOpens user-defined function library.
define/user-defined/execute-on-demandExecutes UDFs on demand.
define/user-defined/fan-modelConfigures user-defined fan model.
define/user-defined/function-hooksHooks up user-defined functions.
define/user-defined/interpreted-functionsLoads interpreted user-defined functions.
define/user-defined/real-gas-models/Enters the real-gas menu to enable/configure real gas model.
define/user-defined/real-gas-models/nist-multispecies-real-gas-modelLoads the NIST real-gas library.
define/user-defined/real-gas-models/nist-real-gas-modelLoads the NIST real-gas library.
define/user-defined/real-gas-models/set-stateSelects the state for NIST real gas model.
define/user-defined/real-gas-models/user-defined-multispecies-real-gas-modelLoads a user-defined multispecies real-gas library.
define/user-defined/real-gas-models/user-defined-real-gas-modelLoads the user-defined real-gas library.
define/user-defined/use-built-in-compiler?Enables/disables the use of a built-in compiler (Clang) when the
define/user-defined/compiled-functionstext command is used. This text command / compiler is available for Windows only, and is provided as part of the Ansys Fluent installation. It is recommended that you enable this text command when the compiler you installed on your machine is an older version that is no longer supported. Note that the built-in compiler is used automatically if Fluent determines that you have not installed Microsoft Visual Studio or Clang on your computer, whether this text command is enabled or not.define/user-defined/use-contributed-cpp?Enables/disables use of the cpp utility included with the Ansys Fluent installation.
define/user-defined/use-zone-based-udmAllows you to allocate the user-defined memory to the specified zones, rather than the default of the entire domain.
define/user-defined/user-defined-memoryAllocates user-defined memory.
define/user-defined/user-defined-scalarsDefines user-defined scalars.