Set file and path options using the General Options tab in Fluent Launcher.

Figure 4.1: The General Options Tab of Fluent Launcher

Both single-precision and double-precision versions of Ansys Fluent are available on all computer platforms. For most cases, the single-precision solver will be sufficiently accurate, but certain types of problems may benefit from the use of a double-precision version. Several examples are listed below:

The Parallel Settings tab allows you to specify settings for running Ansys Fluent in parallel.

Figure 4.2: The Parallel Settings Tab of Fluent Launcher

Refer to Parallel Processing for details on parallel processing using Fluent and Starting Parallel Ansys Fluent Using Fluent Launcher for additional details parallel process configuration options on this tab.

The Remote tab (Figure 4.3: The Remote Tab of Fluent Launcher) allows you to specify settings for running Ansys Fluent parallel simulations on Linux clusters, via the Windows interface.

Figure 4.3: The Remote Tab of Fluent Launcher

For additional information about this tab, see Setting Additional Options When Running on Remote Linux Machines.

Enable Use Job Scheduler in the Scheduler tab (Figure 4.4: The Scheduler Tab of Fluent Launcher (Windows Version)) to specify settings for running Ansys Fluent with various job schedulers (for example, the Microsoft Job Scheduler for Windows, or LSF, SGE, PBS Pro, and Slurm on Linux).

Figure 4.4: The Scheduler Tab of Fluent Launcher (Windows Version)

For additional information about this tab, see Setting Parallel Scheduler Options in Fluent Launcher.

The Environment tab (Figure 4.5: The Environment Tab of Fluent Launcher) allows you to specify compiler settings for compiling user-defined functions (UDFs) with Ansys Fluent (Windows only). The Environment tab also allows you to specify environment variable settings for running Ansys Fluent.

Figure 4.5: The Environment Tab of Fluent Launcher

Specify a batch file that contains UDF compilation environment settings by selecting the Set up Compilation Environment for UDF check box (enabled by default). Once selected, you can then enter a batch file name in the text field. By default, Fluent Launcher uses the udf.bat file that is located in the directory where Ansys Fluent is installed. It is recommended that you keep the default batch file, which is tested with MS Visual Studio C++ and Clang compilers (for supported versions, see Compiler Requirements for Windows Systems), as well as the built-in compiler (Clang) included with the Fluent installation. For more information about compiling UDFs, see the separate Fluent Customization Manual.

Under Other Environment Variables, enter or edit license file or environment variable information in the text field. For example, FLUENT_AFFINITY=<x> specifies the process binding (affinity) setting, in the same manner as the -affinity=<x> command line option (see Parallel Options for details). Using the Default button resets the default value(s).

fluent -act loads Ansys ACT at Fluent startup. For additional information about ACT in Fluent, see Customizing Fluent.

fluent -app=flremote launches either the Fluent Launcher or the specified dimension of Fluent (for example, 3ddp), along with the Fluent Remote Visualization Client. For additional information about the Fluent Remote Visualization Client, refer to Remote Visualization and Accessing Fluent Remotely in the Fluent Workspaces User's Guide.

fluent -appscript, allows you to specify a script that will run in the specified application (-appscript must be used in conjunction with -app).

fluent -driver allows you to specify the graphics driver to be used in the session. When enabling graphics display, you have various options: on Linux, the available drivers include fluent -driver opengl2, fluent -driver opengl, and fluent -driver x11; on Windows, the available drivers include fluent -driver opengl2, fluent -driver opengl, fluent -driver dx11, and fluent -driver msw (the latter instructs Ansys Fluent to use the Operating Systems Windows driver). For both Linux and Windows, you can disable graphics display using fluent -driver null. For a comprehensive list of the drivers available to you, open a Fluent session, enter the display/set/rendering-options/driver text command, and then press the Enter key at the driver> prompt. For more details about using the driver options, see Hiding the Graphics Window Display.

fluent -gui_machine=<hostname> will run Cortex on a specified machine (<hostname>) rather than automatically on the same machine as that used for compute node 0. If you just include -gui_machine (without =<hostname>), Cortex is run on the same machine used to submit the fluent command. This option is only available when running on Linux, and may be needed to ensure optimal graphics performance when running Fluent under a scheduler / load manager (using the -scheduler=<scheduler> option, as described in Scheduler Options).

fluent -g will run Cortex without graphics and without the graphical user interface. This option is useful if want to submit a batch job.

fluent -gr will run Cortex without graphics. This option can be used in conjunction with the -i <journal> option to run a job in "background" mode.

fluent -gu will run Cortex without the graphical user interface but will open graphics windows and display graphics objects. You cannot interact with the displayed graphics objects.

To start Fluent and immediately read a journal file, type fluent -i <journal>, replacing <journal> with the name of the journal file you want to read.

To start Fluent and immediately read a case file, type fluent <dimensions and precision> -case <path to case>, replacing <path to case> with the path to and name of the case file you want to read.

To start Fluent and immediately read a case and data file, type fluent <dimensions and precision> -case <path to case> -data, replacing <path to case> with the path to and name of the case file you want to read. The data file must be in the same directory as the case file and its name must exactly match that of the case file (except for the .dat file extension).

To start Fluent at a specific capability level (licensing level), type fluent <dimensions and precision> -license=<enterprise or premium>.

fluent -h<heap size> will update the heap space for Cortex processes to the specified size. For example, fluent 3ddp -h50000000. The default heap size is 18000000. Increasing the heap size will also increase Fluent's memory usage, which could negatively impact machine performance. Note that you cannot decrease the heap size below the default value of 18000000.

fluent -nm will run Cortex without displaying the mesh in the graphics window.

fluent -meshing specifies that Fluent opens in meshing mode rather than the default solution mode. See Introduction to Meshing Mode in Fluent for further details about the meshing mode.

-cflush specifies that memory is allocated in such a way as to ensure that all of the associated file cache buffers are flushed. This may resolve processing performance issues. For more details, see Clearing the Linux File Cache Buffers.

-platform=<x> loads a binary that is specially ported for a particular platform. When <x>=intel, an AVX2 optimized binary is used that enhances performance when running on processors that support the AVX2 instruction set (available only on Linux).

-stream prints the memory bandwidth, using a variant of the STREAM benchmark. This information can be helpful in determining if your memory is set up in an optimal manner.

These options are used in association with the parallel solver.

-affinity=<x> specifies the process binding (affinity) settings. The default behavior is optimized for the respective run scenarios. The available choices for this option depends upon the platform on which you are running:

-ccp <x> (where <x> is the name of the head node) runs the parallel job through the Microsoft Job Scheduler as described in Starting Parallel Ansys Fluent with the Microsoft Job Scheduler.

-cnf=<x> (where <x> is the name of a hosts file or a list of Linux machines) spawns a compute node on each of the specified machines. For details, see Starting Parallel Ansys Fluent on a Windows System Using Command Line Options or Starting Parallel Ansys Fluent on a Linux System Using Command Line Options.

-gpgpu=<n> specifies the number of general purpose graphics processing units (GPGPUs) per machine to be used in offload mode for AMG acceleration and/or DO acceleration. For more information, see Using General Purpose Graphics Processing Units (GPGPUs) With the Algebraic Multigrid (AMG) Solver and Accelerating Discrete Ordinates (DO) Radiation Calculations, respectively.

-gpu[=<n>} specifies that the native GPU Solver is run, and you can specify which graphics processing units to use as needed; for example, -gpu=1,2,4. For further details, see Starting the Fluent GPU Solver from the Command Line.

-host_ip=<host:ip> specifies the IP interface to be used by the host process.

-mpi=<mpi> specifies that <mpi> is to be used for the MPI. You can skip this flag if you choose to use the default MPI.

-mpiopt=<x> allows you to specify any additional MPI flags (<x>) to be included in the run (Linux only).

-mpitest runs the mpitest program instead of Ansys Fluent to test the network.

-p<ic> specifies the use of parallel interconnect <ic>, where <ic> can be any of the interconnects listed in Starting Parallel Ansys Fluent on a Windows System Using Command Line Options or Starting Parallel Ansys Fluent on a Linux System Using Command Line Options.

-pcheck checks the network connections before spawning compute nodes (Linux only).

By default, the mpirun command (which launches the node processes) is executed on the compute node where the host process is spawned. You can use -remote_node=<hostname> to specify a different machine for the execution of this command. If =<hostname> is omitted, the first node in the hosts file will be used. (Linux only)

-ssh specifies that SSH should be used to spawn remote processes. (Beginning with Ansys Fluent R16.0, SSH is used by default. This option is included primarily for backward compatibility with existing launch scripts, etc.)

-t<x> specifies that <x> processors are to be used. For more information about starting the parallel version of Ansys Fluent, see Starting Parallel Ansys Fluent on a Windows System or Starting Parallel Ansys Fluent on a Linux System.

-tm<x> specifies that <x> processors are to be used for meshing. This value must be less than or equal to the number of processes specified with -t<x>.

fluent -post will run a version of Fluent that allows you to set up a problem or perform postprocessing, but will not allow you to perform calculations. Running Ansys Fluent for pre- and postprocessing requires you to use the -post flag on startup. To use this option on Linux, launch Ansys Fluent by adding the -post flag after the version number, for example,

fluent 3d -post

To use this same feature from the graphical interface on Windows or Linux, select the Pre/Post Only option in the General Options tab of Fluent Launcher, as described in Starting Ansys Fluent Using Fluent Launcher.

The -sifile=<name>.txt option starts Ansys Fluent and the server that is necessary for running the remote visualization client. For additional information on remote visualization, refer to Remote Visualization and Accessing Fluent Remotely.

The -scheduler=<scheduler> option allows you to specify that your Linux session is run under a scheduler / load manager, where <scheduler> can be one of the following:

If you use custom scheduler scripts instead of relying on the standard Fluent option (-scheduler=<scheduler>), your environment variables related to the job scheduler will not be used unless you include the -scheduler_custom_script option with the Fluent options in your script.

Other options are available when you use a scheduler:

The -command="<TUI command>" option allows you to specify that a single text command (<TUI command>) is executed at Fluent startup. The text command must be complete, that is, it cannot rely on further user input in the console after launching. Up to 10 instances of this option can be included, and the text commands will be executed in the order they are entered. When this option is used along with the -i <journal> option, the text commands are executed before the journal.

For example, you could enter the following to read a case and start a calculation: fluent 3d -command="file/read-case file_name.cas" -command="solve/initialize/initialize-flow" -command="sol iter 10".

Typing fluent <version> -r, replacing <version> with the desired version (2d or 3d, or for double precision, fluent or 3ddp), will list all releases of the specified version.

fluent -r<x> will run release <x> of Ansys Fluent.

Typing fluent <version> -env, replacing <version> with the desired version, will list all environment variables before running Ansys Fluent.

Including the -setenv="<var>=<value>" option sets the environment variable <var> explicitly to <value> before launching Ansys Fluent. Note that you can include as many instances of this option as you need to set all of the relevant environment variables. You can also unset an environment variable by entering -setenv="<var>=".

The following command line options (in either Windows or Linux) can be used when Ansys Fluent is involved in a system coupling simulation.

-schost="<x>" (where <x> is the name of the host machine, in quotes) specifies the host machine on which the coupling service is running (to which the co-simulation participant/solver must connect).

-scport=<y> (where <y> is the port number) specifies the port on the host machine upon which the coupling service is listening for connections from co-simulation participants.

-scname="<z>" (where <z> is the name of the participant, in quotes) specifies the unique name used by the co-simulation participant to identify itself to the coupling service (see Server File in the System Coupling User's Guide for more information).

The general syntax for invoking Ansys Fluent for system coupling is:

fluent 3d –schost=host name in quotes –scport=port number –scname=name of the solver in quotes

For instance:

fluent 3d –schost="machine1.domain.com" –scport=1234 –scname="Solution1"

Once Ansys Fluent loads the case, initialize the solution using the following command:

s i i

Once your case is initialized, start the system coupling by typing the following command in the Ansys Fluent text user interface (TUI):

(sc-solve)

For more information, see Performing System Coupling Simulations Using Fluent, as well as the System Coupling User's Guide.

There are other startup options that are not listed when you type the fluent -help command. These options can be used to customize your graphical user interface. For example, to change the Ansys Fluent window size and position you can either modify the .Xdefaults file described in Customizing the Graphical User Interface, or you can simply type the following command at startup:

fluent <version> -geometry <XX>x<YY>+<xx>-<yy> 

where <XX> and <YY> are the width and height in pixels, respectively, and +<xx>-<yy> is the position of the window.

Therefore, typing fluent 3d -geometry 700x500+20-400 will start the 3D version of Ansys Fluent, sizing the Ansys Fluent console to 700x500 pixels and positioning it on your monitor screen at +20-400.

There are additional Qt command line startup options for modifying the graphical stylesheet and more, which can be found in Qt documentation.