Physical models and settings which are unavailable for the GPU solver are either hidden from the GUI or have ‘Unsupported’ added to the option name. To support journal compatibility between the CPU-based solver and the GPU solver, unsupported models and settings can be set using the TUI. Unsupported models activated using the TUI will be listed as either ignored, converted, or unsupported. Similarly, case files developed on the CPU-based solver will typically run on the GPU solver, with any unsupported models or features highlighted as ignored, converted, or unsupported.

The following limitations apply to using the DO radiation model with the GPU solver:

The GPU solver is not available in the Ansys Workbench environment.

For the GPU Solver, the interval specified for report definitions will be a multiple of the reporting interval. For example, with a reporting interval of 5, and an export frequency of 3 time steps, new data will be received by the monitor only every 15 time steps. Therefore, larger reporting intervals for residuals and monitors is recommended for comparing the performance of the GPU solver to the CPU-driven Fluent solution. A reporting interval of 20 is recommended and can be specified with the following TUI command:

/solve set report-interval 20

Profiles in cylindrical coordinate systems, which includes those used for swirl inlets, are not supported.

Monitors and report definitions must be defined prior to solution initialization or before calculating the solution. Additionally, if the solver settings are changed from steady to transient, it may be necessary to redefine report definitions.

When monitoring mass flow rate at a non-conformal mesh interface where the fluxes are collected from intersected faces to the parent faces, the printed result will have the wrong sign (e.g., -1 instead of 1).

When monitoring Dynamic Pressure (Pressure... category) at a stationary wall boundary, the resulting value will be zero as expected. However, results computed using a report (as outlined in Creating Output Parameters) will show an incorrect non-zero value.

The Turbulent Viscosity Ratio is clipped to 10e5 in the same manner as the CPU-driven Fluent solver, however the GPU solver will not provide feedback to the transcript or console.

When thermal effects are defined for your case as outlined in Modeling Thermal Energy, using a steady-state solution to initialize a transient case does not work correctly when solving the energy equation. This limitation can be resolved by performing the procedure outlined in Transitioning from a Steady-State Solution to a Transient Calculation.

For cases using hybrid initialization with far-field pressure boundary conditions, the initialization procedure may not converge or may produce unphysical initial velocity values at outflow faces. In such cases please use standard initialization instead. If this occurs, standard initialization should be used.

With the CPU-based Fluent solver, when modeling supersonic flow at a pressure inlet or velocity inlet all flow characteristics enter into the flow domain and the flow state must be fully specified. Similarly, when there is supersonic flow at a pressure outlet, all flow characteristics exit the domain and the specified pressure will be ignored by the solver. However, when modeling supersonic flow with the GPU solver, the flow will not be discretized correctly at pressure inlets, velocity inlets, and pressure outlets and the flow will be treated as subsonic at these boundary types. Supersonic static pressure at inlets will therefore be ignored, leading to an under-specified state which may produce an unreliable solution. Additionally, the specified static pressure on pressure outlets will still be enforced, which may lead to inconsistencies in the solution directly adjacent to the boundary.

For specified shear walls, the GPU solver currently supports only a specified shear stress of zero. The GPU solver also automatically removes the effects of turbulence wall functions at the specified shear walls, similar to when the solve/set/advanced/specified-zero-shear-alternative-treatment? text command is enabled for the CPU-based Fluent solver.

With the CPU-based Fluent solver, if a fluid region is closed (has no pressure boundaries) and the flow is not compressible and not transient, the solver will set the pressure to zero at the cell closest to the pressure reference location ((0,0,0) by default). The GPU solver will instead constrain the pressure level by preserving the volume average of the initial condition for pressure. Therefore, there will be an offset in pressure between the CPU-based and GPU solver solutions. Additionally, since the pressure level is arbitrary for such flows, this offset will have no other effect on the solution but may affect force integrals on bodies which are not closed surfaces.

When restarting a simulation using second-order transient, the solver uses the first-order Backward Euler scheme on the first time step after restarting.

Restarting a GPU Solver solution on the CPU-driven Fluent solver will not restart correctly if the energy equation with a compressible material is calculated in the GPU Solver solution.

The Linear pressure scheme for the GPU Solver differs from the CPU-based Fluent solver. The face pressure still depends only on the adjacent cell pressures only, but is more accurate when the mesh spacing is nonuniform.

The expressions used with the GPU solver are explicit in nature, because they use the previously solved field variables.