For 4K monitors with a resolution higher than 1920x1080, when invoking field-level user assistance (“?”) in the Fluent Meshing workflows, the help window cannot be automatically resized, causing the text to be cut off and scroll bars to be added. (1006416)

(Linux only) ANSYS Fluent does not support AMD Radeon Pro graphics cards and the Fluent session may close unexpectedly. (348500)

Dragging the ANSYS Fluent application between 4K and non-4K displays may result in the application not scaling correctly. As a workaround, restart ANSYS Fluent after relocating it to a new screen to make it appear as expected. (345352)

ANSYS Fluent may hang unexpectedly if you have a non-default layout, such as tabbing the console and the graphics window, and you force the MSW graphics driver, either by using HOOPS_PICTURE=msw/win or by launching with the -driver msw option. (269471)

(Windows on 4K monitors) You may need to adjust your display scaling and layout settings to optimize the fit of the Fluent application on your monitor.

(Linux Only) Automatic scaling of the Ansys Fluent application window and graphics window interactivity are not compatible when viewed on a 4K monitor. If the application is scaled properly, interactions in the graphics window may not behave as expected. Set QT_AUTO_SCREEN_SCALE_FACTOR equal to 1 to have the application scale properly. (143229)

(Red Hat 8.8 only) Avoid the import/export of CGNS files as CGNS is not supported on Red Hat and it will cause the Fluent session to close unexpectedly. (882695)

(1-way Fluent to Mechanical data transfer using the legacy .dat or .dat.gz file formats) For Fluent multiphase cases, pressure values may not appear in Ansys Mechanical. As a workaround, use the following steps:

For some cases with wall/wall-shadow pairs, the variables exported on these surfaces to Common Fluids Format - Post (CFF-Post) may be incorrectly populated with zero-values when, in reality, the variable does not have a value at this location (for example, wall shear stress on a coupled wall shadow). This can lead to differences when comparing postprocessing images and values between Fluent and other postprocessors such as EnSight or CFD-Post. In such comparisons, the postprocessing values seen in Fluent results should be the ones considered as correct. (419385)

You cannot read a default CFF case file (.cas.h5) when creating a bounded-by-surfaces design condition (as part of the adjoint design tool) or when creating an imprinted surface. Workaround: Legacy case files (.cas) can be read in these circumstances, so you can save your .cas.h5 file as a .cas file by opening it in a Fluent session and disabling the writing of CFF files (by entering the following text command: file/cff-files? no). (199821)

(Windows only) You cannot export files larger than 2GB to CGNS format. As a workaround, use a Linux machine to export files larger than 2GB to CGNS format. (259220)

Surfaces exported to EnSight format may contain a surface with an ID of zero. This is OK for importing into EnSight, but it will cause an error if you are importing into a non-ANSYS third-party postprocessing software, such as Paraview. As a workaround, create a zone surface for the surface with an ID of zero and export the newly created surface instead of the original. (254966)

CGNS files exported from TurboGrid 2019 R3 cannot be read into ANSYS Fluent unless the Split Blade Faces By Geometry option is disabled in TurboGrid before you export the CGNS files. You can disable this option in TurboGrid by right-clicking 3D Mesh in the Mesh tab, selecting Edit in Command Editor and setting Split Blade Faces By Geometry to false. (121053)

If you change the File Storage Options settings in the Autosave dialog box, the solution history will be lost.

When exporting EnSight Case Gold files for transient simulations, the solver cannot be switched between serial and parallel, and the number of compute nodes cannot be changed for a given parallel run. Otherwise, the exported EnSight Case Gold files for each time step will not be compatible.

EnSight export with topology changes is not supported.

To properly view Fieldview Unstructured (.fvuns) results from a serial or parallel Ansys Fluent simulation:

Tecplot file import does not support the Tecplot360 file format.

The maximum number of profiles that can be read into a single Fluent session is 50.

The PARALLEL INDEPENDENT mode for Common Fluids File (CFF) file I/O is known to exhibit slow write performance. On parallel file systems, consider using the PARALLEL COLLECTIVE mode when writing CFF files. On other network file systems, consider using the HOST or NODE0 mode.

If you are accessing a file using a Universal Naming Convention (UNC) path, you must ensure that you have permission to access to all of the folders in the path or you will not be able to open the file.

(Windows only) The file filter available in the Select File dialog box may not work as expected, requiring you to manually select the desired file(s) without filtering aid. (174291)

Files written by Ansys products do not support synchronization with Microsoft's OneDrive file hosting service. (187717 / 74067)

When slitting a coupled wall, Fluent will terminate abnormally if the coupled wall includes a node that is also shared by two or more periodic boundary zone pairs. Note that a slitting operation is performed not only when you use the mesh/modify-zones/slit-face-zone text command, but also when you specify a time-averaged explicit thermal coupling (for example, by using the define/models/cht/explicit-time-averaged-coupling/conformal-coupled-walls text command). Workaround: decouple all of the periodic pairs that share the node (for example, by using the define/boundary-conditions/modify-zones/slit-periodic text command) before you slit the coupled wall. (528636)

When using the gap model with a flow-blocking gap region or when using contact detection in a dynamic mesh with the contact marks method selected for flow control, you must ensure that none of the cells that are marked as part of the blocked region are adjacent to a periodic boundary zone, as this will result in Fluent reporting an error during initialization or the calculation. (498569)

If your license preferences are set to Share a single license between applications when possible (under Tools>License Preferences...) and you have a Fluent Meshing session open, then you open the Fluent Solution workspace, Fluent Meshing hangs without a chance for you to save your session. As a workaround, change your license preference to Use a separate license for each application, which will prevent you from opening another Fluent session if there is already one open. (147834)

Hover-over highlighting and Boundary Markers are not available in Meshing Mode. (241447)

Boundary zone extrusion is not possible from faces that have hanging nodes.

For simulations that involve the Fluent, Mechanical, and Meshing applications, meshing problems can arise in instances where there are multiple regions and contacts between them. In Fluent, a zone can only exist in a single contact region. The Mechanical and Meshing applications both use a different approach concerning contact regions when compared to Fluent.

Ansys Fluent does not support FSI data mapping of edges and, therefore, it is not supported in 2D.

At non-conformal interfaces, the Matching option is no longer allowed with the Mapped option. When opening a case set up in a previous release with both options enabled, you will be prompted to recreate the interface without the Matching option.

If your mesh topology has a step-wise prism mesh near the walls, do not use node-based gradients with MUSCL.

Mass-Weighted Average report definitions are not supported for reduced order models because the ROM only has data available on cell face centers and cell centers. Instead, use Area-Weighted Average, Facet Average, Facet Minimum, or Facet Maximum report definitions. (281540)

The physical velocity porous formulation may produce non-physical flow fields and poor convergence when porous resistance (Inertial or Viscous) values are less than or comparable to the change in the dynamic pressure across the porous interface (interior face zone separating the porous and non-porous cell zone). Switching the porous interface zone to a porous jump boundary is an effective way to overcome this issue. (61773)

Ansys Fluent supports the Chemkin II format for Oppdif flamelet import only.

The surface-to-surface (S2S) radiation model does not work with moving/deforming meshes.

The DPM work pile algorithm is not compatible with the wall film boundary condition.

For transient Lagrangian multiphase analysis with DPM unsteady particle tracking, atomizer or cone injections will release particles from the same position rather than from random positions in one of the following cases:

To use random starting points for the particles, enter the following scheme commands in the Ansys Fluent console:

(rpsetvar 'dpm/random/seed-timestep-corrected? #t)

(dpm-parameters-changed)

Note that this change will also affect particle trajectories if stochastic tracking, particle breakup, or other mechanisms that involve random numbers are used. (176638)

The shell conduction model is not applicable on moving walls.

The heat exchanger model is not compatible with mesh adaption.

The Fluent/Ansys Reaction Design KINetics coupling is not available on the win64 platform.

DO-Energy coupling is recommended for large optical thickness cases (> 10) only.

FMG initialization is not available with the shell conduction model.

FMG initialization is not compatible with the unsteady solver.

The MHD module is not compatible with Eulerian multiphase models.

Bounded 2nd order discretization in time is not compatible with moving and deforming meshes.

When simulating porous media, the value of the Porosity (defined in the Fluid dialog box) cannot be 0 or 1 (that is, it must be in between these values) if the non-equilibrium thermal model is enabled.

When simulating porous media, the non-equilibrium thermal model is not supported with radiation and/or multiphase models.

For porous media simulations, the relative velocity resistance formulation is not supported with axisymmetric-swirl when there are non-zero swirl resistances.

The junction of a wall with shell conduction enabled and a non-conformal coupled wall is not supported. Such a junction will not be thermally connected, that is, there will be no heat transfer between the shell and the mesh interface wall.

After you enable the Eulerian Wall Film model, Fluent will not allow you to save the mesh modifications, such as separating cells, extruding face zones, and changing the cell zones type. If you want to modify the mesh in Fluent, be sure to complete all mesh operations prior to enabling the Eulerian Wall Film model.

The Transition SST model (also known as the γ-Re_θ model) is not Galilean invariant and should therefore not be applied to surfaces that move relative to the coordinate system for which the velocity field is computed; for such cases, the Intermittency Transition model (also known as the γ model) should be used instead.

User-defined wall functions are not compatible with the Eulerian multiphase formulation and cannot be used.

The view factor files generated as part of a surface-to-surface radiation model calculation for version 16.0 or 16.1 of Fluent may not be compatible with newer versions if the Matching option was enabled for a mapped interface. For any case file with such a setup, you must recompute the view factors in the newer version to ensure correct results.

Since saved journals are designed to be run in a new Fluent session and not in a session where a parametric study is initialized, journals saved as part of a parametric study (using the Save Journal button in the Parametric ribbon) may cause errors. Contact technical support for a workaround. (932695)

The discrete transfer radiation model (DTRM) is unavailable in the parallel solver.

Note that on systems using large pages for memory allocation, the virtual memory usage reported by Fluent may be much higher than actual memory used. In this case resident memory (also reported by Fluent) is a more reliable guide.

The Eulerian Wall-film model is not compatible with the DPM Domain option of the hybrid parallel DPM tracking. For such model combination, the Use DPM Domain option must be disabled in the Parallel tab of the Discrete Phase Model dialog box.

Starting in version 18.0, Ansys Fluent will require approximately 60 MB more memory per node process compared to version 17.0–17.2.

If you have OpenSSH inside C:\windows\system32 and want to run a mixed Windows-Linux simulation, Fluent may not be able to locate and execute the ssh command, and the following warning will be printed:

'ssh' is not recognized as an internal or external command, operable program or batch file.

You must specify the path of the actual ssh to be used: launching from the command line, use the -rsh option (for example, -rsh=c:\cygwin64\bin\ssh.exe); using Fluent Launcher, select Other from the Remote Spawn Control list in the Remote tab and enter the path in the text box (for example, c:\cygwin64\bin\ssh.exe).

In addition, you should add the location of ssh executable to the beginning of the PATH environment variable. (184255/176971)

Memory usage may increase compared to previous releases for parallel simulations that use the InfiniBand interconnect. This can be particularly problematic for large cases that are run on a cluster, as you may run out of memory. The memory usage increase is more prominent during intensive input/output (I/O), such as the frequent writing of CFF data files (.dat.h5). Workaround: use the ethernet interconnect, or if that is not possible, reduce the frequency of I/O operations during the solution and/or stop the calculation when the memory starts to increase and then restart. For details on changing the interconnect see Starting Parallel Ansys Fluent Using Fluent Launcher, Starting Parallel Ansys Fluent on a Windows System Using Command Line Options, and/or Starting Parallel Ansys Fluent on a Linux System Using Command Line Options. (597320 / 610518)

Using dynamic process spawning requires that you manually specify the interconnect as -pethernet for shared memory or distributed memory without InfiniBand, and -pib.ofed for distributed memory over InfiniBand.

For certain Mellanox OFED driver versions or UCX versions, users may need to specify -pib.ofed instead of just -pib to run Fluent with Infiniband. Most users will not require this workaround.

The IBM MPI has been discontinued by the vendor, and is no longer available in the standard installation of Fluent. The Intel MPI is now the default MPI for Windows (with less than 64 logical cores) and Linux, and is known to have the following limitations:

On Windows Server OS, Ansys Fluent supports only MS MPI for parallel runs. Installing the Intel MPI library will result in conflicts.

On Windows 7 and later, installing Ansys Fluent on any drive other than C: may result in issues arising from spaces in the pathname not getting converted to short file names. This is the result of a change in the default value for NtfsDisable8dot3NameCreation starting with Windows 7. If you need to install Ansys Fluent on any drive other than C: you must run the following command prior to installing Ansys Fluent:

fsutil 8dot3name set <driveletter> 0

where <driveletter> is the target drive letter including the colon (for example, D:).

The minimum OS requirements for Linux are SLES 11 SP2 or RHEL 6. Note that SLES 12.5 is not supported.

The pathname length to the cpropep.so library (including the lib name) is limited to 80 characters. (Linux Opteron cluster using Infiniband interconnect only.)

On Linux platforms, including a space character in the current working directory path is not supported.

If you are installing Ansys Fluent 2024 R2 on a Windows machine that already has one or more previous versions of Ansys Fluent, then after installing the Intel MPI library from the prerequisites, make sure to delete the environment variable I_MPI_ROOT. Otherwise there will be a conflict while running previous Ansys Fluent versions in parallel mode.

Remote Solver Facility (RSF) is no longer supported in Ansys Fluent.

Itanium platform (lnia64) is no longer supported.

Ansys Fluent uses several TCP/IP ports for communications and error handling. Port conflicts with other programs trying to use the same ports are handled by Ansys Fluent and generate warnings similar to the following:

428: mpt_accept: warning: incorrect exercise message "GET /" from 10.1.0.188 on port 56564

Long running large sessions are more prone to generating such warnings, but these are generally safe for you to ignore.

If you lock the computer screen before the Fluent graphics are initialized, the Fluent session will not launch if you are using the OpenGL graphics driver. To avoid this issue with the OpenGL driver, you can use the alternative drivers x11 or null for Linux/unix and msw or null for Windows. You can specify an alternate graphics driver either by defining it in the HOOPS_PICTURE environment variable or using the -driver Fluent command line option.

Fluent may terminate abnormally during launch when running on Community Enterprise OS (CentOS) 7.3 or Red Hat Enterprise Linux (RHEL) 7.3 when DISPLAY is set to a Virtual Network Computing (VNC) session. To attempt to resolve this, verify that you are using a supported graphics card and update the graphics card drivers (directly from the graphics card vendor website). If the issue persists, you can do one of the following: set the DISPLAY to a local machine; set the LD_PRELOAD environment variable to /usr/lib64/libstdc++.so.6; or use the alternative drivers x11 or null (either by defining it in the HOOPS_PICTURE environment variable or using the -driver Fluent command line option).

Running Ansys Fluent on an accelerated remote display (including but not limited to DCV and EOD) with the OpenGL2 graphics driver may result in Fluent closing unexpectedly. If you experience this issue, change to the OpenGL1 graphics driver (display/set/rendering-options/driver/opengl). (283643)

Connecting or disconnecting a VPN network while running a Fluent simulation will result in a failure because of changes to the network interface.

If you experience an abnormal termination when running Fluent via a remote display, check you graphics card to ensure that you have a modern professional graphics card that is up-to-date (that is, the latest updated driver for that card, which is available on the company's website). If your system does not meet the graphics card requirements, launch Fluent using a completely software-based driver, such as MSW (Windows) or X11 (Linux).

(Exceed onDemand and VNC Viewer) The Num Lock number keys and arrows may not function in the graphical user interface or console. As a workaround, you can define the XKB_DEFAULT_RULES environment variable set equal to base, which resolves the arrow keys' functionality. Number entries must still be completed using the number keys at the top of the standard keyboard. (172528)

(Linux only) When running Ansys Fluent using the Virtual Network Computing (VNC), Nice DCV, or Exceed on Demand (EoD) applications, you may experience unexpected error messages due to a 3rd party issue. To resolve these errors, install the following packages: (185796)

(Linux only) On some clusters without accelerated graphics, Fluent may not accept keyboard inputs. If you encounter this behavior, set the QT_XKB_CONFIG_ROOT environment variable equal to /usr/share/X11/xkb.

A reference frame is always displayed at its initial state (position and orientation) when displayed from the Reference Frame dialog box. While running a transient simulation for multiple time steps, a reference frame is displayed at its current state. After the calculation is completed, if you open the Reference Frame dialog box and display it, the reference frame triad will move back to its initial state. (184248)

Clicking OK within the Reference Frame dialog box will reset a reference frame to its initial state. If you do not intend to make changes to a reference frame, leave the dialog box by clicking Cancel. (184248)

Note that Mesh Motion doesn't work with 6DOF. If you want to have relative motion with respect to a six DOF zone you need to create a Rigid body dynamic zone.

Fluid zones designated as 3D fan zones cannot have non-conformal interfaces.

When using the standard CPU-driven solver, you may get erroneous results for cases that have both compressible and incompressible flow zones. Affected field variables include temperature and velocity. Workaround: Use the Fluent native GPU solver instead. (892103)

If you have enabled the application of poor mesh numerics using criteria based on the cell gradient quality, the number of cells to which it is applied may vary when performing single-precision calculations with different numbers of processes. Workaround: Use the double-precision solver. (362753)

The absolute and relative velocity formulations may yield different results in cases where a strong reversal of flow exists at a pressure outlet boundary.

The non-iterative time advancement (NITA) solver is applicable with only a limited set of models. See the Ansys Fluent User's Guide for more details.

NITA (using fractional time step method) is not compatible with porous media.

The following models are not available for the density-based solvers:

The pressure-based coupled solver is not available with the following features:

On some Linux platforms, pressing Ctrl+C will not interrupt the solution. A suggested workaround is to use the checkpoint mechanism in Fluent to save files and/or exit Fluent. (Checkpointing an Ansys Fluent Simulation in the Fluent User's Guide)

In certain cases with tetrahedral or hybrid meshes, the use of the Least-Squares Cell Based gradient method in combination with the cell-to-cell limiter may cause divergence. If this is observed, it is recommended that you either change the gradient method to Green-Gauss Node Based or change the limiter type to the cell-to-face limiter.

Beginning in version 17.0, the warped-face gradient correction (WFGC) is not supported with shell conduction if the ability to define multi-layer shells has been disabled through the define/models/shell-conduction/multi-layer-shell text command.

For transient and time-dependent cases, the solution advances to the next time step based on various inputs including time step size and convergence criteria, but it is not directly dependent on the flow time interval specified when 'flow-time' is selected for monitoring (report definitions, autosaving, transient export and so on). For these flow time dependent operations, the action will occur when the flow time meets or exceeds the specified flow time interval.

Note the following issues affecting residuals:

These issues can occasionally impact the residual history of long transient simulations (such as those that use the LES, SRS, or SBES model) when the solutions for each time step are not deeply converged.

For case files created in Release 19.2 or earlier and are steady, single phase, and use the pressure-based solver, the Density explicit relaxation factor in the Solution Controls task page is set to 1 in the following circumstances, even though it should be set to 0.25 (in order to match how a case file created in Release 2019 R1 would behave):

Work-around: Manually enter 0.25 for Density in the Solution Controls task page. (182453)

The following text command works appropriately for setting limits to default values, but fails to take action on solution controls and AMG controls:

> solve/set/set-controls-to-default
Set solution controls to default? [no] yes
Set AMG Controls to default? [no] yes
Set limits to default values? [no] yes

Work-around: Click the Default button in the Solution Controls task page and the Multigrid tab of the Advanced Solution Controls dialog box, respectively. As noted previously, for older steady-state, single-phase cases that use the pressure-based solver and involve reacting flow and/or species transport with a pseudo time method selected, you must also manually set the Density explicit relaxation factor to 0.25 in the Solution Controls task page. (183926)

The use of Fractional Step pressure-velocity coupling scheme with dynamic mesh layering is not supported. To run this combination, enter the following Scheme command before running the calculation: (rpsetvar 'dynamesh/layering/layering-before-move? #t). (125886)

If the specified frequency for the profile update interval is higher than the number of maximum iterations per time step for transient cases, the profile (that is, the user-defined function or named expression used to define a boundary condition) will not be updated every time step. If the profile must be updated every time step, then the profile update interval should retain the default value of 1. (882920)

When using the standard CPU-driven solver, you may get erroneous results for cases that have both compressible and incompressible flow zones. Affected field variables include temperature and velocity. Workaround: Use the Fluent native GPU solver instead. (892103)

For expressions evaluated for zone motion (moving reference frame or moving mesh), "Time" evaluates to the previous time step's flow time, whereas the "Time" argument of a DEFINE_TRANSIENT_PROFILE used for zone motion will have the current time step's flow time. (147162)

When you use curly brackets "{}" to specify the name of a defined object, such as a report definition or a cell register, automatic suggestions are disabled and you must provide the display name of that object. (118322)

Expressions defined for fields in the Fixed Values tab of the Fluid and Solid cell zone dialog boxes cannot include units in the expression definition. (146295)

Any scripts or journals that attempt to add menu items to Fluent pull-down menus (which have been replaced with the Fluent ribbon) will no longer work. You must create separate user-defined menus to house all user-defined menu items. For additional information about user-defined menus, see Adding Menus to the Right of the Ribbon in the Fluent Customization Manual.

Interpreted UDFs cannot be used with an Infiniband interconnect. The compiled UDF approach must be used instead.

The Visual Studio Express 2015 for Windows installer on Windows 10 installs libraries in non-standard locations. To ensure the use of Microsoft Visual Studio for UDF compiling (rather than the built-in compiler provided with the Fluent installation), you must instead use the Visual Studio Express 2015 for Desktop installer, or manually set the library path based on your local installation (for example, LIB="C:\Program Files (x86)\Microsoft Visual Studio 14.0\VC\lib\onecore\amd64";%LIB%).

(Postprocessing application, Linux only) Updates to the location of user-defined surfaces (such as lines) may not show if you only redisplay the scene containing the surface(s). Redisplay the surface(s) after modifying them to ensure they are displayed correctly in all containing graphics objects. (450062)

Data files do not store derived quantities, such as pressure gradients, so reading a data file and immediately displaying pressure gradients results will incorrectly show zeros. Run the solver for an iteration and redisplay to see the correct values. (774389)

(Parallel only) In some instances, the location selected using the mouse-probe in the graphics window may vary substantially from the location the code selects as the corresponding surface vertex. To make the mouse-probe and corresponding surface vertex match more closely, as they do when running with a single processor, disable the Remove Partition Lines option in the Graphics branch of Preferences (File > Preferences...). (458754)

(Linux only) Postprocessing objects displayed with the Node Values option disabled may not show all of the selected surfaces due to a third-party issue. As a workaround, use the OpenGL graphics driver. (347474)

Results visualized on bounded plane surfaces or on iso-clips of a plane may incorrectly imply that some hex mesh cells are triangles, when they are not. This is not known to impact results displayed on these surfaces. Planes created with the Bounded option disabled do not experience this issue. (380979)

If holes or unexpected dark spots appear when postprocessing on plane surfaces (such as displaying a contour plot), you can create an iso-surface to display the desired quantity. Refer to Iso-surfaces for additional information on creating iso-surfaces.

(Linux only) Ansys Fluent does not support AMD Radeon Pro graphics cards and the Fluent session may close unexpectedly. (348500)

(Linux only) Contour lines are not displayed when dynamic shadows are enabled. To make the contour lines display, you can disabled dynamic shadows either in the graphics window toolbar or in Preferences. (343770)

Keyframe Scene Animations of pathlines are only available for the non-persistent/"global" version of the Pathlines dialog box that does not have a Name field. This version of the dialog box is opened as described below: (269934)

Unsteady statistics mean and rms values for custom field functions defined for dp/dt may show as zero. Contact support for a workaround. (199006)

(2D Only) Box select is only working for selecting surfaces if you drag from right-to-left. However, you can enable Edges or Faces in the Mesh Display dialog box to restore left-to-right box selection. You can also enable Show model edges in the Appearance branch of Preferences (accessed via File>Preferences...) to change the default mesh display behavior. (259419)

When you use curly brackets "{}" to specify the name of a defined object, such as another report definition, automatic suggestions are disabled and you must provide the display name of that object. (118322)

When exporting a filled contour with contour lines to AVZ format, the contour lines will not be visible in the Ansys Viewer. As a workaround, you can create a scene containing 2 duplicate contour plots—one with filled contours, one with just contour lines (not filled). You can also disable the colormap for one of the plots so the plot only contains a single colormap. (137138)

Monitors may continue to print/plot values, even if the zones on which they are defined are deactivated.

If you are autosaving multiple scenes on a Windows machine, the Headlight lighting effect may inconsistently change its state (on/off). This can be avoided by rendering each scene in a separate graphics window.

Mean and root-mean-squared-error (RMSE) quantities of custom field functions are only available for mixtures. In previous releases it was possible to specify these quantities for phases, which was an incorrect behavior. This behavior is no longer allowed in R16.0 or later releases. If you are running a pre-R16.0 case set to output such quantities in R2024 R2, you may get a segmentation error. To avoid the error, redefine the previously defined monitors reporting mean or RMSE quantities of phases.

The mouse-annotate feature is no longer available. Annotations can still be created using the Annotate dialog box (see Annotate Dialog Box in the Fluent User's Guide for additional information).

Beginning in version 15.0, if a flux report for the heat transfer rate is generated on the wall of a moving solid, the reported values will include the convective heat flux due to the motion of the solid. Depending on the mesh and quality of the geometry representation, this may present flux values that are different than the flux specified in the boundary condition definition (for example, a non-zero flux may be reported for an adiabatic wall).

If you import a case file that was created prior to Release 18.0 and that contains multiple monitors plotting in the same window, you must review the setup to ensure each report plot is assigned to a different window before running the calculation. If the plot windows are not reassigned, then plots assigned to the same window will be lost.

It is possible to use text commands to create contour, vector, mesh, pathline, particle track, XY plot, and scene graphics objects with spaces in the name (for example, through the display/objects/create text command); however, objects with such names cannot be displayed using the display/objects/display text command, and attempting to do so will only result in the printing of an error. As a workaround, you can create graphics objects without spaces in the name or use the graphical user interface to display graphics objects with spaces in the name.

In rare cases, the Curve Length X Axis Function for XY plots may not plot correctly, even if the curvilinear surface is piecewise linear and appears to be a single closed curve. A workaround is to use the Direction Vector X Axis Function.

Transient statistics (Mean and RMS) reported for Fluent quantities that are nonlinear functions of the underlying solution variables represent evaluations of those quantities using the Mean or RMS values of the underlying solution variables. For instance, Mean Velocity Magnitude is computed as the magnitude of a vector constructed from the mean velocity components, and Mean Pressure Coefficient is computed as the pressure coefficient computed using the mean pressure. To construct the true Mean and/or RMS values of such quantities, you can define a custom field function and collect transient statistics of the custom field function. For example, define a custom field function vmag_cff = sqrt (Vx ^ 2 + Vy ^ 2 + Vz ^ 2), and report Mean and RMS of vmag_cff.

Scene animations created using Key Frames in the Animate dialog box are not compatible with graphics displays on isosurfaces (contours, vectors, pathlines, particle tracks). Pathlines are not compatible with scene animations, regardless of the selected surface(s).

When meshes contain a large number of cells (for example, ~150 million cells or higher), the meshing mode of Fluent may report an incorrect number of skewed cells, based on an incorrect inverse orthoskew (IOS) value. As a workaround, you can use the (tgapi-util-set-number-of-parallel-compute-threads 1) command. (168453)

If you create an XY plot for display on a rake surface and you use the savable XY plot graphics object, accessed by clicking New... in the ribbon or outline view, then the results may not be displayed immediately. If they do not appear, click Curves... in the XY Plot dialog box and select a Symbol from the drop-down list in the Marker Style group box, click Apply, then redisplay the XY plot. (180547)

If you are viewing cell values (Node Values disabled) on an XY plot of a rake surface and the points are being shown as a continuous line, then you can change the Pattern to "empty" in the Curves - Solution XY Plot dialog box (Line Style group box). (180547)

The transform operation in the Transform Surface dialog box is not available for user-created surfaces such as lines, points, iso-surfaces, and so on. To create a transformed line, point, iso-surface, or other user-created surface, you must manually translate the input point(s) and create a new line/point/iso-surface in the respective dialog box (Line/Rake, Point Surface, Iso-Surface, and so on).

Density contour plots that include a solid region in the display will include the solid zone(s) in any range calculations and will show a density for the solid that does not reflect the actual case setup. Fluid zone densities are still displayed correctly. Selecting Density... and Density All in the Contours of drop-down lists will correctly display density values for solids and fluids. (155346)

Special characters (/^*%@,<>{}()?&~!=) should not be used in object names: they can affect how an object is rendered in the graphics display, and may make it so the object does not appear at all. (157473)

Having special characters in object names can also lead to inconsistent report file names, causing validation issues when you attempt to start a calculation, therefore you should avoid using special characters for objects. (531947)

For annotations, the foreground and background color options for text are not in sync with those specified in Preferences, but are instead controlled using the display/set/colors/foreground and display/set/colors/background text commands, respectively.

For any meshing mode or solution mode session that displays graphics in the graphics window (including when running a batch job with the -gu command line option) and/or saves picture files, the rendering / saving speed will be significantly slower if you do not follow all of the following best practices:

In a Workbench project, if your Fluent case and data files are in the default common fluids format (CFF) and you also export a .cdat file, you may get an error message if you attempt to postprocess the results using CFD-Post. This is because when a .cdat file is exported, a legacy case file (.cas) is also written as the latest case, and so paired with the CFF data file (.dat.h5), and it is not possible to use a combination of legacy and CFF files in CFD-Post. Workaround: Manually write a new .cas.h5 and .dat.h5 file after the .cdat file is exported. (310992)

When using Fluent in Workbench, importing Fluent Case and Data into a Fluent system will cause project updates to fail if Submit to Design Point Service is chosen for Update Option. As a workaround, you can right-click the Solution cell and chooseRefresh prior to the project update, or select RSM under Update Option in the Project Schematic Properties. Projects that use the Import Fluent Case functionality only (without importing Data) or that start from Geometry/Mesh without Case file import are unaffected by this limitation. (277667)

The Automatic Skip option for colormaps is not functioning as intended. As a workaround, you can manually specify the skip value. (273989)

Fluent cases with either of:

may fail if updated in Workbench with the following message: "Update failed for the Solution component in Fluent. Value cannot be null. Parameter name: fileName". To avoid this issue you can first read the case into Fluent and either 1) delete the report file or 2) specify a valid filename for the report file. (146221)

Coupling between Fluent and HFSS or Q3D Extractor is not supported.

For two-way coupling between Maxwell and Fluent, by default Fluent uses the following zones: when mapping volumetric losses, the same list of zones that you selected for receiving volumetric losses in Fluent's Maxwell Mapping Volumetric dialog box are used; and when mapping surface losses, all cell zones are used. To change the zones that are used for feedback mapping, you can use a Scheme command, shown in the following example. This example specifies that only cell zone ID 1 and 2 are used: (em-set-feedback-map-cell-zone '(1 2)). Note that you can only specify the IDs of the cell zones as the arguments.

In a Fluent analysis system, the Clear Generated Data option for the Solution cell will not clear the files associated with animations. To have the Clear Generated Data option clear the animation files as well, you must define the FLUENT_WB_REMOVE ALL_GENERATE_FILES as a system environment variable on your local machine, prior to opening Workbench.

Fluent design point studies using the Remote Solve Manager may not completely update due to errors. Should this happen, you can rerun the affected design points and they will update as expected (you may have to rerun failed design points multiple times). (350696, 385734, 553033)

(Ubuntu systems only) The following help links in the Fluent Launcher and Fluent Solution workspace are not working and the correct location for these links is provided. As a workaround, you can define the LD_PRELOAD environment set equal to /usr/lib/x86-64-linux-gnu/libstdc++.so.6 prior to starting Fluent: (736116)

Do not use inf as the name for any boundaries, cell zones, or objects (report definitions, graphics objects, and so on) due to the conflict of 'inf' representing "infinity" in the Python language.

In some cases, you may see a warning when accessing Preferences after loading ACT at startup. As a workaround to open Preferences, close Fluent, disable Load ACT in the Fluent Launcher and start Fluent. Once Fluent is running you can modify Preferences and click OK to save your changes. (462205)

Performance on a Windows high performance computing (HPC) cluster may suffer due to poor affinity handling by Microsoft HPC Pack. Workaround: You can try running with the Microsoft HPC affinity management disabled, by selecting No jobs from the Affinity Type list in the Affinity tab of the Job Scheduler Configuration. (395881 / 400841)

The following combination is not supported: Open MPI + Infiniband + Mellanox OFED 5.1. Workaround: Either use the Intel MPI or upgrade to Mellanox OFED 5.2. (444933)

Images of embedded graphics windows captured using the Save Picture dialog box are saved without borders on the embedded windows, regardless of the setting specified in Preferences. (336851)

(Operating under the Pro license) While the user-defined specification method is available for some fields, such as material properties, you cannot load user-defined functions, as they are not supported at the Pro capability level. (321331)

Exports of Common Fluids Format - Post files from Fluent may incorrectly specify the pressure gradient as zero. Contact support for a workaround. (239127, 243318)

If the network connection is lost during a serial or parallel calculation, the Fluent session may terminate abnormally.

The IRIS Image and HPGL hard copy formats are no longer supported in Ansys Fluent.

When using Ansys Fluent with the Remote Solve Manager (RSM):

The turbo-averaged contour plot in turbomachinery postprocessing may give an unexpected contour region in a selected topology.

The Inverse Distance and Least Squares profile interpolation methods are not applicable when a profile is attached to cell zones.

When opening Ansys Help from Fluent in Linux, you may receive an error message in the Linux console. This can result when another user has created the installation and run Fluent, thus creating a registry file; if you then run this same installation, there will be a permissions conflict. As a workaround, remove the registry file:

path/ansys_inc/v242/Tools/mono/Linux64/etc/mono/registry

(where path is the directory in which you have placed the release directory). Then change the permissions for the Mono platform in order to remove write access from the directory:

path/ansys_inc/v242/Tools/mono/Linux64/etc/mono

On Windows, mesh reading into a serial Ansys Fluent session may fail if you use more than 20 million cells per core.

Fluent does not support non-ASCII characters in the names of files, zones, and boundaries.

When exiting a Fluent session on Linux that was started with the Load ACT option, Fluent may become unresponsive. If this occurs, the Fluent process must be manually terminated. In the console, the error message specifies that a corrupted double-linked list is responsible for the error. Because this unexpected shutdown occurs after the project has been saved, no data is lost.

When Fluent is run on Linux with the Load ACT option, Fluent may repeatedly issue the following warning during solution iteration:

Unexpected error checking licensing server.

This warning is harmless and does not impact Fluent or ACT usage.

When running a stand-alone instance of Fluent in a mixed Windows / Linux configuration or from a remote Windows installation, ACT does not open. To correct the problem, you must set the AWP_ROOT242 environment variable to point to the Ansys installation directory.

ACT with Ansys Fluent is disabled on Linux systems starting in Release 19.2. To use ACT with Ansys Fluent, use Release 19.2 or later on Windows or use Release 19.1 on Linux. (177173)

If the network connection is lost during a serial or parallel calculation, the Ansys Fluent session may terminate abnormally.

Ansys Fluent uses several TCP/IP ports for communications and error handling. Port conflicts with other programs trying to use the same ports are handled by Ansys Fluent and generate warnings similar to the following

428: mpt_accept: warning: incorrect exercise message "GET /" from 10.1.0.188 on port 56564

Long running large sessions are more prone to generating such warnings, but these are generally save for you to ignore.

When running ANSYS Fluent utilizing VirtualGL vglrun or EOD ssrun, Fluent may hang when writing image files. As a workaround, disable Use hardware acceleration under Save Picture Settings in the Graphics branch of Preferences (accessed via File>Preferences...). (252910)

For a client session with multiple connected servers, only one server can receive commands through the Send Command to Server dialog box—that server is whichever one you send a command to first using this dialog box. As a workaround, you can use the Python console to control the other connected servers. (177632)

When using previous versions of Fluent Meshing (version 2024 R2 or earlier), if an overlap in the display of the workflow tree/outline view and the graphics window occurs, simply remove the .cxlayout.ini file located in the home directory.

Limitations related to the Fluent guided meshing workflows are documented separately. See Limitations of the Fluent Guided Workflows for details.

When creating a rapid octree mesh, while creating a new mesh object is available in the graphical user interface, you are only able to perform the same operation in the text user interface using the following command(s):

/parallel/auto-partition? no
/parallel/agglomerate yes
/objects/create

When using the Fault-tolerant Meshing workflow, Fluent Meshing may encounter problems when reading mesh files while using large machine configurations, for example, 256 core machines or larger.

Performing a mesh check on a polyhexcore mesh may not yield satisfactory results if there are any isolated cells present. Isolated cells can be removed using the (%tg-delete-isolated-cells (get-cell-zones-of-filter '*))command in the console window.

Before importing SpaceClaim files (.scdoc) into Fluent Meshing, you need to first enable the Set as the alternative license preference license preference option in SpaceClaim in order to uphold licensing preferences.

Using journal (*.jou) or workflow (*.wft) files from previous releases may slow or even halt the volume mesh generation process. Workaround: For journal files, make sure that you add version-specific information to the beginning of your journal files (for example: /file/set-tui-version "19.5"). For workflow files, make sure that you have the Quality Warning Limit property in the Create Volume Mesh task set to a value closer to 0 (such as 0.05) instead of a value near 1. (163320)

While writing case files in the CFF format (.cas.h5) in a mixed Windows/Linux environment, Fluent Meshing will only write files on the Linux nodes. To write such case files properly, you have to assign a mapped driver on the Windows side as the working directory, and then assign the remote working directory to the same path, where the mapped driver path is derived from.

(Linux only) Geometries imported from Ansys Mechanical, Ansys DesignModeler, and Ansys Meshing depend on the Linux xmessage command. The following RedHat package managers should be installed before runtime:

Meshes generated from Ansys Meshing that are then imported into Fluent Meshing may not include all interior faces. Workaround: In Ansys Meshing, ensure that all interior surfaces are assigned to be internal faces (that is, put into a Named Selection that includes the name "internal") before generating the mesh, such that all internal surfaces will then be accounted for when the mesh is imported into Fluent Meshing.

After Ansys Fluent 19.2, you can no longer have multiple interior zones defined in a single cell zone. If your case file has such zones, they will not appear as available zones. Workaround: Read the mesh file into Ansys Fluent 19.2, and set the type for the interior zones to be 'wall' in order to restore the missing zones. (143347)

For example, to read files created in an older version of Ansys Fluent Meshing (or even Workbench), perform the following:

Meshing>file read-options
Enforce mesh topology [no]
Check read deata [no]
Correct Interiors? [yes] no

After reading the mesh, change the problematic boundary's type to 'internal' and save the mesh file.