This section describes the features of the CPU-driven solution mode of Fluent that can be used with the Fluent GPU Solver. The features outlined in this section can be defined after you have read in a previously defined Fluent case file (see Reading Fluent Case Files Into the Fluent GPU Solver) or after reading in a mesh file (see Reading Mesh Files).
This section only covers those settings relevant to setting up your case and does not include information on calculating or postprocessing the GPU solver solution. The settings and procedure for defining calculation activities, calculating the solution, and postprocessing the solution within the Fluent GPU Solver is the same as that of the CPU-driven Fluent solver. Note that the supported features outlined in this section may contain limitations, which are detailed in Fluent GPU Solver Limitations.
Prior to setting up your case in the Fluent GPU Solver, note the following general requirements and capabilities:
The Fluent GPU Solver can only be used with either a single NVIDIA GPU or multiple NVIDIA GPUs with shared/distributed memory. For details on setting specifying GPUs to be used see Starting the Fluent GPU Solver Using the Fluent Launcher or Starting the Fluent GPU Solver from the Command Line.
The Fluent GPU Solver can be used in single precision or double precision.
Multiple CPU processes can be specified for setting up your case and postprocessing the GPU solver solution. See Using CPU Processes for Setup and Postprocessing for details.
Only 3D geometries are supported.
Mesh topologies with polyhedral, hexahedral, tetrahedral, pyramid, and prism cells, as well as meshes with hanging nodes are supported.
The settings that can be defined when setting up your case within the Fluent GPU Solver are detailed in the following sections:
The following physics modeling capabilities are supported with the Fluent GPU Solver:
Conjugate Heat Transfer (CHT) including for anisotropic solids as described in Conjugate Heat Transfer and Settings for Anisotropic Solid Zones.
Discrete Ordinates (DO) radiation model. See Setting Up the DO Model for details.
Species transport with Volumetric reactions or without reactions as outlined in Volumetric Reactions and Species Transport Without Reactions, respectively. Species transport models can be set up with the following settings:
Finite-Rate/No TCI and Eddy-Dissipation turbulence-chemistry interaction models.
Stiff Chemistry Solver and None - Direct Source chemistry solvers.
Compressible flows (see Compressible Flows for details).
The following turbulence models are supported:
Laminar
Standard and Realizable k-epsilon
k-omega, GEKO, and k-omega SST
Large Eddy Simulation (LES)
For the LES turbulence model, the following sub-grid scale models are supported:
Smagorinsky-Lilly
WALE
For the LES turbulence model, the following additional model options are available:
Near-Wall-RANS-Layer (WMLES)
When enabled, this option activated the Generic WMLES model (Generic WMLES Formulation in the Fluent Beta Features Manual), which uses LES for the bulk of the domain and the algebraic RANS model for the thin near-wall section of the boundary layer.
Optimized LES Numerics
When enabled, this option will automatically apply optimal solution controls to enhance stability of the solution.
Stress-Blended Eddy Simulation (SBES)
Only supported with any of the k-omega models.
For detailed information on setting up the turbulence models listed above see Modeling Turbulence.
Sponge layers acoustics model (see Sponge Layers for details).
Note that multiple sponge layers are not supported and only one sponge layer can be activated within the Manage Sponge Layers dialog box. If multiple sponge layers are activated, the GPU Solver will only simulate the first sponge layer listed and all other sponge layers will be ignored.
The Fluent GPU Solver supports the following material properties:
Density
piecewise-linear
piecewise-polynomial
polynomial
ideal-gas
incompressible-ideal-gas
boussinesq
constant
Cp:
constant
piecewise-linear
piecewise-polynomial
polynomial
kinetic-theory
Thermal Conductivity
constant
piecewise-linear
piecewise-polynomial
polynomial
kinetic-theory
cyl-orthotropic
orthotropic
anisotropic
The cyl-orthotropic, orthotropic, and anisotropic options listed above are available when simulating conjugate heat transfer with anisotropic/orthotropic conductivity for solids. For details see Anisotropic Thermal Conductivity for Solids.
Viscosity
constant
piecewise-linear
piecewise-polynomial
polynomial
kinetic-theory
sutherland
Molecular Weight, Standard State Enthalpy, Standard State Entropy, and Reference Temperature can be defined as:
constant
For more details on setting up material properties for your simulation see Physical Properties.
The Fluent GPU solver supports the pressure based solver with absolute velocity formulation for both transient and steady-state calculations. Pressure-velocity coupling can be specified as Coupled (steady state only), or segregated with the SIMPLE and SIMPLEC schemes. The GPU solver supports the Least Squares Cell Based gradient and both second-order and first-order discretization schemes for the flow equations. Additionally, the Bounded Central Differencing scheme is available when the Large Eddy Simulation (LES) or Stress-Blended Eddy Simulation (SBES) turbulence models are enabled. For incompressible time-dependant calculations, both first order and second order implicit are supported for the Transient Formulation (see Inputs for Time-Dependent Problems). Additionally, the Flow Courant Number is supported for the Coupled solver when Pseudo Time Method is set to Off.
For poor quality meshes, you can incorporate poor mesh numerics by entering the following TUI command, which will delete any cells with left-handed faces:
/solve/set/poor-mesh-robustness/poor-mesh-removal yes
For steady-state cases, Data sampling for Steady Statistics is supported within the Run Calculation task page.
For additional information on specifying the above solver settings, see Choosing the Spatial Discretization Scheme.
The Fluent GPU solver supports updating parametric studies sequentially for variations in supported parameters. For more information on performing a sequential parametric study see Performing Parametric Studies.
This section describes the cell zone and boundary conditions that can be defined when using the Fluent GPU Solver.
The boundary conditions listed below can be defined as constant or as input parameters. Additionally, certain boundary condition settings can also be defined using a steady-state profile, as described in Profiles. Note that input parameters and steady-state profiles are not supported for Mass Flow Rate and Speed for rotational wall motion.
The following boundary conditions are supported:
Wall
Stationary Wall and Moving Wall, including Rotational wall motion. See Wall Boundary Conditions for details.
Thermal conditions. See Thermal Boundary Conditions at Walls for details.
Symmetry. See Symmetry Boundary Conditions for details.
Rotational Periodic boundary conditions. See Periodic Boundary Conditions for details.
Translational Periodic boundary condition with or without a non-conformal mesh interface. See Periodic Boundary Conditions for details.
Inlet
Velocity-inlet. See Defining the Velocity for details.
Pressure-inlet. See Pressure Inlet Boundary Conditions for details.
Mass-flow-inlet. See Mass-Flow Inlet Boundary Conditions for details.
Intake Fan. See Intake Fan Boundary Conditions for details.
Outlet
Pressure-outlet. See Pressure Outlet Boundary Conditions for details.
Mass-flow-outlet. See Mass-Flow Outlet Boundary Conditions for details.
Pressure-far-field
Outlet Vent. See Outlet Vent Boundary Conditions for details.
Porous Jump. See Porous Jump Boundary Conditions for details.
The following boundary conditions can be defined for both incompressible and compressible flows:
Velocity-inlet
Mass-flow-inlet
Mass-flow-outlet
The following settings can be specified for fluid cell zone conditions:
Frame Motion for Moving reference frames (MRF). See Modeling Flows with Moving Reference Frames for details.
Mesh Motion. See Defining Zone Motion for details.
Porous Zone. See Porous Media Conditions for details.
Source Terms for heat, momentum, and species are supported, as outlined in Defining Mass, Momentum, Energy, and Other Sources, and can be defined as constant or using a steady-state profile.
Reaction mechanisms for species transport with reactions. See Specifying a Reaction Mechanism for details.
The Fluent GPU Solver supports sliding meshes with both conformal and non-conformal mesh interfaces as outlined in Using Sliding Meshes. For details on defining non-conformal mesh interfaces see Using a Non-Conformal Mesh in Ansys Fluent.
This section describes the solution monitors that are supported by the Fluent GPU Solver.
Note: Solution monitors can not be created on the following user defined surfaces:
Iso-surfaces
Iso-clips
Zone surfaces
Quadric-surfaces
The report definitions listed below can be created on an existing surface (boundary condition) or on a Point..., Plane..., or Line... surface.
Force
For details on defining the following force reports see Force and Moment Report Definitions.
Drag...
Lift...
Moment...
Force...
Flux
For details on defining the following flux reports see Flux Report Definition.
Mass Flow Rate...
Total Heat Transfer Rate...
Surface
For details on defining the following surface reports see Surface Report Definitions.
Area...
Area-Weighted Average...
Facet Average...
Facet Maximum...
Facet Minimum...
Integral...
Mass Flow Rate...
Volume Flow Rate...
Mass-Weighted Average...
Sum...
Standard Deviation...
Uniformity Index - Mass Weighted...
Uniformity Index - Area Weighted...
Volume
For details on defining the following volume reports see Volume Report Definitions.
Mass-Average...
Mass Integral...
Mass...
Max...
Min...
Volume...
Volume-Average...
Volume Integral...
Sum...