Defines new animation.

Changes animation monitor attributes.

Specifies a keyframe number and adds a frame to the keyframe animation.

Deletes all defined keyframes.

Allows for the deletion of a single keyframe.

Plays the defined keyframe animation.

Allows for the reading of a animation file.

Contains options for setting how the keyframes are played as an animation.

Saves the keyframe animation with the provided name in the specified format.

Clears solution animation object history.

Copies solution animation object.

Creates new solution animation object.

Deletes solution animation object.

Edits solution animation object.

Deletes animation sequence.

Plays the selected animation.

Reads new animation from file or already defined animations.

Specify a custom start frame, increment, and end frame for video export.

Plays the 3D animation sequence using the view stored in the sequence.

Enters the video menu.

Writes animation sequence to the file.

Enter the pulse hardcopy menu.

Set whether the pulse is a single pulse or continuous.

Enters the pulse video menu.

Select a pathline or particle track graphics object, specify whether you want to write a video file or picture files, and enter the destination directory for the files. Continuous pulse animations result in a 5 second video. Single pulse animations run for a full cycle.

Creates a new convergence condition.

Deletes a convergence condition.

Edits a convergence condition.

Lists all of the report definition-based convergence conditions.

Lists the properties of the specified convergence condition.

Initializes the flow field with the default values.

You can select the type of zone from which you want to compute these values. The types of zones available are:

Enables/disables localized initialization of turbulent flow variables.

Sets values for the turbulent intensity and turbulent viscosity ratio for localized initialization.

Resets FMG controls to default values.

Sets value for the turbulent viscosity ratio used during FMG initialization.

Enables/disables volumetric reactions during FMG initialization.

Enables/disables the inclusion of viscous terms during FMG initialization.

Enters the general settings menu.

Enters the turbulence settings menu.

Enters the species-settings menu.

Performs volumetric smoothing for volume fraction.

Sets options for patching and smoothing volume fraction.

Chooses which currently monitored residuals should be checked for convergence.

Sets convergence criteria for residuals that are currently being both monitored and checked.

Sets convergence criterion type.

Enables/disables an enhanced formulation for the local scaling of the continuity residuals with the pressure-based solver, so that the absolute mass flow rate at each cell is used. This text command is only available when the computing of the local scale is enabled through the solve/monitors/residual/scale-by-coefficient? text command.

Chooses which residuals to monitor as printed and/or plotted output.

Sets the number of most recent residuals to display in plots.

Sets the number of iterations through which normalization factors will be maximized.

Sets normalization factors for currently monitored residuals (if normalize? is set to yes).

Chooses whether to normalize residuals in printed and plotted output.

Sets number of residuals to be saved with data. History is automatically compacted when buffer becomes full.

Chooses whether residuals will be plotted during iteration.

Chooses whether residuals will be printed during iteration.

Sets relative convergence criteria for residuals that are currently being both monitored and checked.

Re-normalize residuals by maximum values.

Chooses whether to delete the residual history and reset iteration counter to 1.

Chooses whether to scale residuals by coefficient sum in printed and plotted output.

Specifies window in which residuals will be plotted during iteration.

Enters the menu to specify the expert parameters.

Specifies the maximum number if iterations, which will be performed by the acoustics wave equation solver in one timestep.

Specifies the iterations convergence criterion in terms of the residual norm drop.

Enables/disables an alternate formulation for wall temperatures.

Enters the anisotropic solid heat transfer menu, which provides text commands that affect the calculations in anisotropic solid zones. This text command menu is only available when using the pressure-based solver with the energy equation enabled and a solid zone with an anisotropic option (other than biaxial) selected for the thermal conductivity.

Specifies the BCD scheme parameter, which controls the boundedness strength of the BCD scheme in the pressure-based solver, as described in Bounded Central Differencing Scheme in the Fluent Theory Guide.

Enables/disables freezing of weighting coefficients of the central differencing and the upwind components of the BCD scheme. This dialog command requires the iteration number, after which the BCD scheme weights are to be frozen at each timestep. Freezing the BCD weighting coefficients may help to improve convergence of the timestep iterations as described in Bounded Central Differencing Scheme in the Fluent Theory Guide.

Enables/disables the use of the correction form of the discretized momentum equations when using the pressure-based solver, as described in Using the Correction Form of Momentum Discretization in the User's Guide. Note that this text command will be removed in a future release, so that the correction form is always used.

Enables/disables a filter to eliminate non-physical numerical noise in the energy field. Numerical noise can appear in solution fields where large variations in specific heat or combustion with phase change are present. Using the energy equation numerical noise filter increases robustness, but may make the solution slightly more diffusive. This text command is only available with the pressure-based solver.

Sets the explicit under-relaxation value for the density-based implicit solver.

Enables/disables the use of a linearized mass transfer user-defined function (that is, the DEFINE_LINEARIZED_MASS_TRANSFER macro), as opposed to a mass transfer user-defined function (that is, the DEFINE_MASS_TRANSFER macro).

Enables/disables the retention of cell residuals for postprocessing.

Enables/disables the retention of temporary solver memory, which retains gradient data and makes some advanced options available for postprocessing.

Note that this text command has the same effect as the Keep temporary solver memory from being freed? TUI option under solve/set/expert.

Enters the secondary gradient limiting menu. This menu is only available when the define/models/solver/pressure-based text command is enabled.

Enables/disables the availability of all applicable discretization schemes.

Enables/disables the availability of the Singhal et al. cavitation model option, which can then be enabled in the Multiphase Model dialog box or by using the following text command: define/phases/set-domain-properties/interaction-domain/heat-mass-reaction/cavitation/cavitation?.

Enables/disables an enhanced formulation for the skewness correction that computes the pressure-correction gradient. In a mesh with very skewed elements, the enhanced formulation should improve solver robustness (though in rare cases it may decrease stability). The enhanced skewness formulation is only used during the simulation when SIMPLEC or PISO is selected for the pressure-velocity coupling scheme with one or more active skewness correction iterations. This text command is only available with the pressure-based solver, when a segregated solver is selected.

Enters the turbomachinery-specific numerics menu. This text command menu is only available when the turbo model is enabled for a steady calculation with the pressure-based solver selected and the pseudo time method set to the global time step option.

Enables/disables the use of a version of the AMG solver that is optimized for high coarsening rates. This option is recommended if the AMG solver diverges with the default settings.

Enters the AMG GPGPU options menu, which contains text commands to enable / disable the use of GPGPUs in offload mode to accelerate the Algebraic Multigrid (AMG) solver for individual coupled or scalar equations. When using this text command menu, you must ensure that GPGPU acceleration is enabled for only coupled equations or only scalar equations, rather than a mix of both.

Enables/disables the use of conservative coarsening techniques for scalar and/or coupled equations that can improve parallel performance and/or convergence for some difficult cases.

Enables/disables Laplace coarsening for scalar and/or coupled equations.

The default is[no]. If you enter yes, and the flow leaving the pressure outlet is subsonic, then the total pressure and total temperature from the domain’s interior are extrapolated to the boundary and used with the imposed static pressure to determine the full thermodynamic state at the boundary.

The default is[no]. If you enter yes, then for cases with very low Mach number flow in the single-precision density-based solver, you can improve convergence by using pressure extrapolation instead of the default velocity extrapolation scheme.

The default is[yes]. If you choose the default, this means that the pressure-outlet boundary condition implementation in the density-based solver has an absorption behavior, as described in Calculation Procedure at Pressure Outlet Boundaries of the User’s Guide. To revert to pre-Ansys Fluent 6.3 boundary condition implementations, where the pressure on the faces of a pressure-outlet boundary is fixed to the specified value while the flow is subsonic, enter no.

The default is[yes].

The default is[no].

The default is[no].

Specify zone and quantity combinations for sampling of steady and unsteady flow statistics and set whether you want the minimum, maximum, mean, root-mean-square-error, and moving average collected.

Enters the menu for specifying runtime discrete Fourier transformation (DFT) datasets.

Lists the combinations of zones and quantities that are defined for sampling steady and unsteady flow statistics.

Specify which zone and quantity combinations to remove from the sampling of steady and unsteady flow statistics.

Selects the discretization scheme for the flow equations.

Selects the discretization scheme for the turbulent dissipation rate.

Selects the discretization scheme for the turbulent kinetic energy.

Selects the discretization scheme for momentum.

Selects which convective discretization scheme for volume fraction is to be used.

Selects the discretization scheme for pressure.

Selects the discretization scheme for energy.

Enables a divergence prevention option so that Fluent applies under-relaxation to the variables in select cells where the temperature and/or pressure values are approaching the minimum and/or maximum limits.

Allows you to enable the use of a two-stage Runge-Kutta scheme for time integration, or revert to the default multi-stage Runge-Kutta scheme. This text command is only available for transient cases that use the density-based explicit formulation.

Enables/disables High Order Term Relaxation (HOTR).

High Order Term Relaxation Options.

Enables/disables High Speed Numerics.

Sets the level of stabilization used to achieve fast convergence. Enter a number 0-5 corresponding to the Mach number range that best characterizes the flow.

Makes available the Pressure Discontinuity Sensor which is a binary identifier equal to 1 if a cell is in proximity of a pressure discontinuity.

Enters the menu for the stability controls for multiphase flows. For more information about the below option, see NITA Expert Options and Default and Stability Controls in the Fluent User's Guide.

Enters the menu for the multiphase boiling model parameters.

Enters the compressible multiphase flow numerics menu.

Enters the default controls menu. This menu is available only for multiphase flows.

Enters the energy controls menu for the multiphase model.

Enters the menu for the multiphase heat mass transfer parameters.

Enters the NITA controls menu.

Enters the porous media numerics menu.

Enters the solution-stabilization numerics menu. This item is available only for the VOF model.

Enters the viscous multiphase flow numerics menu.

Enables and sets hybrid NITA options. For more details, see User Inputs in the Fluent User's Guide.

Setting this to 1, enables the verbosity for NITA diagnostics. The default value of 0 disables verbosity output for NITA diagnostics.

Enables/disables coupling of the neighbor and skewness corrections.

Sets the buffer layer height.

Sets the open channel wave verbosity.

Specifies which open channel wave theory formulation Fluent uses.

Uses the pressure gradient of the donor cell in the interpolation of pressure for its receptor cell.

Selects the interpolation method for overset interfaces. Note that the least squares method is recommended for sliding mesh cases.

Enables/disables a numerical treatment that attempts to assign reasonable data values to orphan cells.

Enables/disables the application of poor mesh numerics on cells with an orthogonal quality that is equal to or less than the threshold defined by the solve/set/poor-mesh-numerics/set-quality-threshold text command (which by default is set to 0.05).

Enables/disables the application of poor mesh numerics on cells (those with an orthogonal quality of 0, as well as those identified by other enabled criteria), and defines whether the local solution correction is 0th, 1st, or 2nd order.

Enables/disables the detection and treatment of poor cells using a criterion based on the cell gradient quality. Poor mesh numerics are applied when the criterion value is equal to or less than a threshold value defined as part of this text command. This criterion is only available with the pressure-based solver, and is not supported for cases that have periodic boundaries.

Enables/disables the relocation of select cell centroids, to improve the orthogonality metrics and solution stability. It is applied to cells when the criterion value is equal to or less than a threshold value defined as part of the text command. Note that the enhanced metrics are only apparent when reporting the quality in the solution mode of Fluent, and not in the meshing mode.

Prints out a listing of the poor cells for each criterion: default, cell quality, and register-based, and (if enabled) cell gradient quality and solution and cell quality.

Enters the register-based menu, which provides text commands that allow you to specify that poor mesh numerics are applied to cells in specified cell registers. The cell registers can be marked manually at the start of the calculation and/or automatically at a specified interval during the calculation.

Resets the list of poor cells included by the default, cell quality, register-based, cell gradient quality, and solution and cell quality criteria.

Sets the orthogonal quality threshold used for applying poor mesh numerics when the solve/set/poor-mesh-numerics/cell-quality-based? text command is enabled. By default, cells with an orthogonal quality of 0.05 or lower are corrected.

Enables/disables the detection and treatment of poor cells using a criterion based on the solution and cell quality. Poor mesh numerics are applied when the criterion value is equal to or less than a threshold value defined as part of this text command, and at a specified frequency (of iterations or time steps). This criterion is only available with the pressure-based solver.

Enables a specific poor mesh numerics treatment for turbulence models. The shear production term is approximated by the destruction term in order to avoid zero turbulence shear production and thus improve the behavior on poor mesh cells. This treatment is available for the following two-equation turbulence models:

Allows you to undo enhancements introduced in version 2019 R1 of Ansys Fluent, including:

Allows you to undo enhancements introduced in version 2019 R3 of Ansys Fluent, including:

Allows you to undo enhancements introduced in version 2021 R1 of Ansys Fluent, including:

Allows you to undo the following enhancements introduced in version 2021 R2 of Ansys Fluent:

Allows you to undo the following enhancements introduced in version 2022 R1 of Ansys Fluent:

Allows you to undo enhancements introduced in release 2023 R1 of Ansys Fluent:

Allows you to undo the following enhancement introduced in release 2023 R2 of Ansys Fluent: the application of poor mesh numerics to the turbulence production term.

Allows you to undo the following enhancement introduced in release 2024 R1 of Ansys Fluent: the default change of the value of kappa used in the Spalart-Allmaras model for interior terms.

Allows you to undo enhancements introduced in version 19.0 of Ansys Fluent, including the treatment of symmetry boundary conditions and the treatment of walls with the specified shear condition, as well as an early protection scheme for the linear solver.

Enters the advanced options menu, which allows you to enable / disable the pseudo time method for individual equations and define their pseudo time scale factors or under-relaxation factors, respectively. These settings only apply when the global time step formulation is selected.

Selects the pseudo time step size formulation.

Defines the pseudo time settings for the calculation when the global time step formulation is selected.

Defines the pseudo time Courant number when the local time step formulation is selected.

Enters the relaxation factors menu, where you can set the pseudo time relaxation factors for individual equations.

Sets the verbosity of the messages related to the pseudo time method.

Selects the slope limiting direction. The available options are cell-to-face, cell-to-cell, and cell-to-node.

Enables/disables the slope limiter filter.

Selects the type of slope limiter. The available options are default, multi-dimensional, and differentiable.

Allows you to specify that an adaptive time stepping method is used in which the time step gets modified by Ansys Fluent as the calculation proceeds such that a version of the Courant–Friedrichs–Lewy (CFL) condition is satisfied, using the specified Courant number.

Allows you to specify the following advanced settings for the CFL-based time stepping:

Sets the method by which you will specify the duration of the calculation. The duration can be defined by the total time, the total number of time steps, the incremental time, or the number of incremental time steps. In this context, "total" indicates that Fluent will consider the amount of time / steps that have already been solved and stop appropriately, whereas "incremental" indicates that the solution will proceed for a specified amount of time / steps regardless of what has previously been calculated. This text command is only available when the time stepping is adaptive or based on a user-defined function.

Allows you to specify that an adaptive time stepping method is used in which the time step gets modified by Ansys Fluent  based on the specified truncation error tolerance.

Enters the extrapolation menu.

Applies a predictor algorithm for computing initial conditions at time step n+1. The predictor algorithm is a computation that sets a better initial condition for the time step.

Allows you to specify that a fixed time stepping method is used in which a specified period or frequency is the basis for determining the time step size and number of time steps.

Allows you to specify that a fixed time stepping method is used in which you directly specify the time step size and number of time steps.

Enters the menu for setting multiphase-specific time constraints.

Sets the amount of incremental (that is, additional) time to run the simulation, regardless of how much time has already been run in previous calculations. This text command is only available when the solve/set/transient-controls/duration-specification-method is set to3.

Sets the maximum flow time.

Sets the number of time steps for a transient simulation.

Allows you to specify that an adaptive time stepping method is used in which the time step gets modified by Ansys Fluent  based on the convective time scale (global Courant number): the time-step-size calculation depends on the mesh density and velocity in interfacial cells. This method is available for all multiphase models using the implicit or explicit volume fraction formulation, except for the wet steam model.

Sets the number of time steps for a transient simulation without starting the calculation.

Applies a predictor algorithm for computing the next time step. The predictor algorithm is a computation that sets a better initial condition for the time step. It uses the rate of change between the prediction and the correction as an indicator for whether the next time step should be larger, smaller, or the same as the current one.

Enables / disables an option that allows for better prediction of the flow field in rotating fluid zones at every time step, in order to speed up the calculation. This text command is only available for transient simulations.

Allows you to specify that the time step size used for solid zones is independent from that used for fluid zones. This text command is only available when both a solid zone exists and energy is enabled.

Allows you to open theSimulation Status dialog box, which reports details about the simulation.

Specifies whether to define the transient advancement either directly by entering a time step size / period / frequency (using the text commands available in thesolve/set/transient-controls menu) or indirectly by entering a Courant number value (using the solve/set/courant-number text command). This text command is only available for the density-based solver when both the explicit formulation and explicit transient formulation are used.

Sets the magnitude of the (physical) time step. This text command is only available when the solve/set/transient-controls/fixed-user-specified text command is set toyes.

Specifies the time interval for acoustic data sampling. This text command is only available when both the Ffowcs Williams and Hawkings model is selected and the density-based solver is used with the explicit formulation and explicit transient formulation.

Sets the total number of time steps that the simulation will run (which includes any time steps that have already been run in previous calculations). This text command is only available when the solve/set/transient-controls/duration-specification-method is set to1.

Sets the total amount of time that the simulation will be run (which includes any time that has already been run in previous calculations). This text command is only available when the solve/set/transient-controls/duration-specification-method is set to2.

Allows you to specify that the time step size is defined by a user-defined function (UDF) that uses theDEFINE_DELTAT macro.

When enabled, if the truncation error within a time step exceeds the specified tolerance Fluent will automatically undo the current calculation and make another attempt with the time step reduced by 1/2. This will be attempted up to 5 times after which Fluent will accept the result and proceed to the next time step.

Enables/disables gradient enhancement computations and specifies whether Fluent uses fast or memory saving mode.